Star CCM Tut

CCM TUTORIALS STAR-CD VERSION 4.02

CONFIDENTIAL — FOR AUTHORISED USERS ONLY

© 2006 CD-adapco

TABLE OF CONTENTS INTRODUCTION Tutorial Structure ..........................................................................................................1 Basic Definitions ..........................................................................................................1 Running a Tutorial ........................................................................................................2 Working with commands ................................................................................ 1-2 Using tutorial command files .......................................................................... 1-3 Tutorial 1 - FLOW IN A MIXING PIPE Physical Problem Description ......................................................................... 1-1 Tutorial 1.1 PRE-PROCESSING AND CFD SOLUTION ...................................... 1-3 Pre-Processing ................................................................................................. 1-3 CFD Analysis ................................................................................................ 1-15 Tutorial 1.1 POST-PROCESSING ......................................................................... 1-17 Post-Processing ............................................................................................. 1-17 Tutorial 2 - EVALUATION OF MESH EFFECTS Physical Problem Description ......................................................................... 2-1 Tutorial 2.1 HEXAHEDRAL MESH ANALYSIS .................................................. 2-3 Pre-Processing ................................................................................................. 2-3 CFD Analysis .................................................................................................. 2-7 Post-Processing ............................................................................................... 2-7 Tutorial 2.2 TETRAHEDRAL MESH ANALYSIS .............................................. 2-19 Pre-Processing ............................................................................................... 2-19 CFD Analysis ................................................................................................ 2-22 Post-Processing ............................................................................................. 2-23 Tutorial 2.3 POLYHEDRAL MESH ANALYSIS ................................................. 2-33 Pre-Processing ............................................................................................... 2-33 CFD Analysis ................................................................................................ 2-36 Post-Processing ............................................................................................. 2-36 Tutorial 3 - POROUS MEDIA FLOW Tutorial 3.1 FLOW IN AN ISOTROPIC, HIGHLY POROUS MEDIUM .............. 3-2 Physical Problem Description ......................................................................... 3-2 Modelling Strategy .......................................................................................... 3-2 Pre-Processing ................................................................................................. 3-2 CFD Analysis .................................................................................................. 3-7 Post-Processing ............................................................................................... 3-7 Version 4.02

i

Tutorial 3.2 FLOW IN AN ORTHOTROPIC, HIGHLY POROUS MEDIUM .... 3-17 Physical Problem Description ....................................................................... 3-17 Modelling Strategy ........................................................................................ 3-17 Pre-Processing ............................................................................................... 3-17 CFD Analysis ................................................................................................ 3-19 Post-Processing ............................................................................................. 3-19 Tutorial 3.3 FLOW IN A MEDIUM WITH ISOTROPIC FLOW RESISTANCE 3-27 Physical Problem Description ....................................................................... 3-27 Modelling Strategy ........................................................................................ 3-27 Pre-Processing ............................................................................................... 3-27 User Subroutine ............................................................................................. 3-29 CFD Analysis ................................................................................................ 3-31 Post-Processing ............................................................................................. 3-31 Tutorial 4 - FREE-SURFACE AND CAVITATION Tutorial 4.1 GRAVITY-DRIVEN FLOW WITH A FREE SURFACE ................... 4-2 Physical Problem Description ......................................................................... 4-2 Modelling Strategy .......................................................................................... 4-2 Pre-Processing ................................................................................................. 4-2 CFD Analysis .................................................................................................. 4-7 Post-Processing ............................................................................................... 4-7 Tutorial 4.2 FORCED FREE-SURFACE FLOW WITH CAPILLARY EFFECTS 4-11 Physical Problem Description ....................................................................... 4-11 Pre-Processing ............................................................................................... 4-11 CFD Analysis ................................................................................................ 4-15 Post-Processing ............................................................................................. 4-15 Tutorial 4.3 FORCED FREE-SURFACE FLOW WITH CAVITATION ............. 4-19 Physical Problem Description ....................................................................... 4-19 Pre-Processing ............................................................................................... 4-19 CFD Analysis ................................................................................................ 4-24 Post-Processing ............................................................................................. 4-24 Tutorial 5 - TURBULENT FLUID STREAM MIXING Physical Problem Description ......................................................................... 5-1 Tutorial 5.1 STEADY 3-D FLOW ........................................................................... 5-2 Pre-Processing ................................................................................................. 5-2 CFD Analysis .................................................................................................. 5-8 Post-Processing ............................................................................................... 5-8 Tutorial 5.2 TRANSIENT 3-D FLOW ................................................................... 5-13 ii

Version 4.02

Pre-Processing ............................................................................................... 5-13 CFD Analysis ................................................................................................ 5-17 Post-Processing ............................................................................................. 5-17 Tutorial 6 - SUPERSONIC AND TRANSONIC FLOWS Tutorial 6.1 ADAPTIVE MESH REFINEMENT FOR SUPERSONIC FLOW ..... 6-2 Physical Problem Description ......................................................................... 6-2 Pre-Processing ................................................................................................. 6-2 CFD Analysis - Coarse Mesh .......................................................................... 6-5 Mesh Refinement ............................................................................................ 6-6 CFD Analysis - Refined Mesh ........................................................................ 6-9 Post-Processing ............................................................................................. 6-11 Tutorial 7 - MULTIPLE ROTATING REFERENCE FRAMES Introduction ..................................................................................................... 7-1 Physical Problem Description ......................................................................... 7-1 Tutorial 7.1 ROTATING-FRAME FAN ANALYSIS ............................................. 7-2 Pre-Processing ................................................................................................. 7-2 CFD Analysis ................................................................................................ 7-14 Post-Processing ............................................................................................. 7-14 Tutorial 8 - LAGRANGIAN TWO-PHASE FLOW Tutorial 8.1 STEADY FLOW WITH FUEL SPRAY INJECTION ......................... 8-2 Physical Problem Description ......................................................................... 8-2 Pre-Processing ................................................................................................. 8-2 CFD Analysis .................................................................................................. 8-6 Post-Processing ............................................................................................... 8-7 Tutorial 8.2 TRANSIENT FLOW WITH FUEL SPRAY INJECTION ................ 8-13 Physical Problem Description ....................................................................... 8-13 Pre-Processing ............................................................................................... 8-13 CFD Analysis ................................................................................................ 8-15 Post-Processing ............................................................................................. 8-16 Tutorial 9 - COMBUSTION Physical Problem Description ......................................................................... 9-1 Tutorial 9.1 PROPANE COMBUSTION (ADIABATIC PPDF) ............................. 9-3 Pre-Processing ................................................................................................. 9-3 CFD Analysis ................................................................................................ 9-11 Post-Processing ............................................................................................. 9-11 Version 4.02

iii

Panel Definition ............................................................................................. 9-17 Tutorial 9.2 PROPANE COMBUSTION (THREE-STEP EDBR) ........................ 9-25 Additional Modelling Notes .......................................................................... 9-25 Numerical Considerations ............................................................................. 9-26 Pre-processing ............................................................................................... 9-26 CFD Analysis ................................................................................................ 9-34 Post-Processing ............................................................................................. 9-34 Tutorial 9.3 C7H8 DROPLET COMBUSTION (EDBR, RADIATION) ............... 9-39 Pre-processing ............................................................................................... 9-39 User Subroutines ........................................................................................... 9-50 CFD Analysis ................................................................................................ 9-54 Post-Processing ............................................................................................. 9-54 Tutorial 9.4 HYDROGEN COMBUSTION (LAMINAR FLAMELETS) ............ 9-61 Pre-Processing ............................................................................................... 9-61 CFD Analysis ................................................................................................ 9-68 Post-Processing ............................................................................................. 9-68 Tutorial 10 - BUOYANCY AND RADIATION EFFECTS Introduction ................................................................................................... 10-1 Material Properties ........................................................................................ 10-2 Tutorial 10.1 BUOYANCY DRIVEN FLOW AROUND A HEATED FIN ......... 10-3 Pre-Processing ............................................................................................... 10-3 CFD Analysis ................................................................................................ 10-9 Post-Processing ............................................................................................. 10-9 Tutorial 10.2 SURFACE-TO-SURFACE RADIATION ..................................... 10-15 Pre-Processing ............................................................................................. 10-15 CFD Analysis .............................................................................................. 10-20 Post-Processing ........................................................................................... 10-20 Tutorial 10.3 RADIATION THROUGH A TRANSPARENT SOLID ............... 10-25 Pre-Processing ............................................................................................. 10-25 CFD Analysis .............................................................................................. 10-29 Post-Processing ........................................................................................... 10-29 Tutorial 11 - MOVING GRIDS Tutorial 12 - EULERIAN TWO-PHASE FLOW Tutorial 12.1 TERMINAL VELOCITY OF BUBBLES ........................................ 12-2 Pre-Processing ............................................................................................... 12-3 CFD Analysis ................................................................................................ 12-7 iv

Version 4.02

Post-Processing ............................................................................................. 12-7 Suggestions for Further Exercises ................................................................. 12-8 Tutorial 12.2 AERATION TANK .......................................................................... 12-9 Pre-Processing ............................................................................................... 12-9 CFD Analysis .............................................................................................. 12-13 Post-Processing ........................................................................................... 12-13 Suggestions for Further Exercises ............................................................... 12-16 Tutorial 12.3 FLUIDISED BED RISER .............................................................. 12-17 Pre-Processing ............................................................................................. 12-17 User Subroutine ........................................................................................... 12-21 CFD Analysis .............................................................................................. 12-22 Post-Processing ........................................................................................... 12-23 Tutorial 12.4 BOILING SIMULATION .............................................................. 12-25 Pre-Processing ............................................................................................. 12-25 User Subroutines ......................................................................................... 12-29 CFD Analysis .............................................................................................. 12-35 Post-Processing ........................................................................................... 12-35 Discussion of Results .................................................................................. 12-39 Validation Check ......................................................................................... 12-39 Suggestions for Further Exercises ............................................................... 12-40 Tutorial 13 - AEROACOUSTIC ANALYSIS Introduction ................................................................................................... 13-1 Tutorial 13.1 STEADY FLOW AROUND A CYLINDER ................................... 13-2 Pre-Processing ............................................................................................... 13-2 CFD Analysis ................................................................................................ 13-5 Post-Processing ............................................................................................. 13-5 Tutorial 13.2 TRANSIENT FLOW AROUND A CYLINDER ........................... 13-11 Pre-Processing ............................................................................................. 13-12 User Subroutines ......................................................................................... 13-16 CFD Analysis .............................................................................................. 13-21 Post-Processing ........................................................................................... 13-21 Tutorial 14 - LIQUID FILM SIMULATION Tutorial 14.1 2D FILM FLOW DOWN A VERTICAL WALL ............................ 14-2 Physical Problem Description ....................................................................... 14-2 Pre-Processing ............................................................................................... 14-3 CFD Analysis ................................................................................................ 14-7 Post-Processing ............................................................................................. 14-8 Version 4.02

v

Suggestions for Further Exercises ............................................................... 14-11 Tutorial 14.2 SPRAY IMPINGEMENT ON A WALL ....................................... 14-13 Problem Description .................................................................................... 14-13 Pre-Processing ............................................................................................. 14-13 CFD Analysis .............................................................................................. 14-21 Post-Processing ........................................................................................... 14-21 Tutorial 15 - COAL COMBUSTION Physical Problem Description ....................................................................... 15-1 Modelling Strategy ........................................................................................ 15-1 Tutorial 15.1 ISOTHERMAL, NON-REACTING FLOW .................................... 15-3 Pre-Processing ............................................................................................... 15-3 CFD Analysis ................................................................................................ 15-7 Post-Processing ............................................................................................. 15-7 Tutorial 15.2 CONSTANT RATE DEVOLATILISATION ................................ 15-11 Pre-Processing ............................................................................................. 15-11 CFD Analysis .............................................................................................. 15-19 Post-Processing ........................................................................................... 15-19 Tutorial 15.3 TWO-COMPETING-STEPS DEVOLATILISATION .................. 15-25 Pre-Processing ............................................................................................. 15-25 CFD Analysis .............................................................................................. 15-27 Post-Processing ........................................................................................... 15-27 Tutorial 16 - LARGE EDDY SIMULATION OF FULLY-DEVELOPED CHANNEL FLOW Physical Problem Description ....................................................................... 16-1 Modelling Strategy ........................................................................................ 16-2 Tutorial 16.1 STEADY-STATE ANALYSIS ........................................................ 16-3 Pre-processing ............................................................................................... 16-3 CFD Analysis ................................................................................................ 16-3 Post-Processing ............................................................................................. 16-4 Macro ............................................................................................................ 16-8 Tutorial 16.2 LARGE EDDY SIMULATION ..................................................... 16-11 Pre-Processing ............................................................................................. 16-11 User Subroutine ........................................................................................... 16-14 CFD Analysis .............................................................................................. 16-15 Post-Processing ........................................................................................... 16-15 Bibliography ................................................................................................ 16-22 Macros ......................................................................................................... 16-22

vi

Version 4.02

INTRODUCTION Tutorial Structure This document contains examples of applying STAR-CD to a variety of tutorial problems, thus demonstrating some of its features and illustrating their use. However, for a detailed description of STAR-CD’s overall capabilities, you are advised to consult the Computational Continuum Mechanics (CCM) and Post-Processing User Guides in addition to this document. Each tutorial starts with a brief description of the physical problem, followed by a description of GUI operations and typed STAR-CD commands needed to set up the corresponding model, perform a CCM analysis and display the results. In those instances where graphical output is generated, selected screen plot images are also included in the description. This enables you to check that you have followed the tutorial correctly up to that point. The tutorials are structured in such a way that, for a given physical feature distinguishing a particular problem, a number of different variants are analysed to illustrate different options. The tutorial numbering system reflects this structure.

Basic Definitions Throughout this volume, it is assumed that you will be using STAR-CD’s Graphical User Interface facilities whenever possible. Therefore, the discussion is in terms of GUI operations (e.g. selecting items from a screen menu, clicking option buttons in a dialog box, etc.) unless the required action can only be performed by typing a command in pro-STAR’s I/O window. Most GUI facilities are incorporated in a special window called STAR GUIde that opens directly from pro-STAR and enables you to build models for most commonly-occurring CFD problems in a systematic and user-friendly way. The on-screen placement of pro-STAR windows and dialog boxes while working on a tutorial is entirely at your discretion. However, the arrangement shown below is recommended for greatest ease of use. This consists of: •

•

•

Version 4.02

The STAR GUIde window on the left — this displays the Navigation Centre tree structure for finding your way around the system, plus various panels for detailed specification of a particular operation. The main pro-STAR window on the right — this enables you to display your current model as well as manipulate various aspects of its on-screen appearance. The latter is achieved via several buttons and pop-up menus along the top and down the left-hand side of the window. Some of the less obvious buttons are labelled in the illustration shown overleaf. The I/O window at the bottom — this confirms the action taken by pro-STAR in response to a GUI operation. It also enables you to type instructions in command form for cases where no equivalent GUI operation is available.

1

Working with commands

Show STAR GUIde window Plot with legend Reset buttons Plot four views Turn mesh plotting on / off Turn edge plotting on / off Orientation slider controls Turn light shading on / off Quick Draw option Plot orientation cube Select a cell set Select a vertex set Select a spline set Select a block set Select a boundary set Select a couple set Select a droplet set Store/recall set, surface or view Display the cell table Display coordinate systems Display/edit a user table

Throughout the document, “>” signs denote successive mouse clicks on menu names, menu list items, dialog box buttons, etc. For example Tools > Cell Tool > Edit Types means click Tools on the main pro-STAR window’s menu bar, then click the Cell Tool item in the drop-down list, then click the Edit Types button on the displayed Cell dialog box. Detailed instructions on how to perform a STAR-CD analysis from start to finish are given in the CCM User Guide (Chapter 2, “Running a STAR-CD Analysis”). These instructions should also be followed in running the tutorials, together with any specific guidance given for each individual tutorial.

Running a Tutorial Working with commands If you wish to run through any of the tutorials by working in command mode, you can: 1. Type in just the desired command name. This will cause pro-STAR to prompt you for the required parameters and will also show you the system defaults. 2. Replace any number of commands with your own abbreviation, defined via command *ABBREVIATE. This substitute can be used repeatedly throughout 2

Version 4.02

Using tutorial command files

the session in place of the original commands. A comprehensive discussion of the various facilities for customising or abbreviating command-mode input is given in Chapter 1 of the Commands volume (section on “pro-STAR Commands”). 3. Repeat all commands in a single action, by making use of the tutorial command files supplied in your STAR-CD installation CD-ROM (see the STAR-CD Installation and Systems Guide for information on where these files may be found). The files are written in separate sub-directories for each tutorial and are called either prep.inp (for pre-processing) or post.inp (for post-processing). Also included are auxiliary files needed by particular cases, e.g. user-defined subroutines, cgrid files containing grid-changing commands, etc. Using tutorial command files The usual procedure for repeating the pre- or post-processing part of a tutorial via the supplied tutorial command files is as follows: 1. Create a directory for the tutorial and copy the prep.inp, post.inp and auxiliary files (e.g. user subroutines) to it. 2. If the tutorial involves a restart from a previous case, copy all STAR-CD generated files (e.g. tut.mdl, tut.ccm, etc.) from their current location to the new directory. 3. For a pre-processing session, start up pro-STAR in the usual way, supply a tutorial name (e.g. tut) and then type the following command in the I/O window: ifile prep.inp Important Note: When running tutorials involving use of the screen cursor, make sure that both the main pro-STAR window and the graphics area within it remain at their normal (default) sizes. Altering these in any way will invalidate the screen coordinate information stored in file prep.inp and the tutorial will fail. 4. Following the automatic execution of all commands, terminate the pro-STAR session by typing. quit, save 5. The procedure for a post-processing session is identical to the above, except that the file name supplied is now post.inp and the run is terminated by typing quit, nosave

Version 4.02

3

Physical Problem Description

Tutorial 1 FLOW IN A MIXING PIPE This tutorial describes in detail how to set up, run and post-process a simple CFD problem involving flow through a mixing pipe. The problem geometry is shown below:

Figure T1.0-1

Mixing pipe geometry

Physical Problem Description The assembly has two inlet pipes, located on the left and centre of the above figure, through which air at different temperatures flows into the interior. There is also an outlet pipe on the right-hand side through which the fluid exits. The air stream entering the solution domain at each inlet has a specified velocity, temperature, density, turbulence intensity and turbulence length scale. These properties vary throughout the pipe as the two streams mix. Adiabatic and no-slip conditions are assumed at the pipe walls. The mesh used to describe the problem geometry is shown below. Users wishing to generate the mesh used in this case from scratch should first complete Tutorial 1.1 and 1.2 of the Meshing Tutorials volume. Alternatively, they may continue with this tutorial using files provided in the STAR-CD installation directory.

Version 4.02

1-1


Figure T1.0-2

1-2

Mixing pipe mesh

Version 4.02

Tutorial 1.1

PRE-PROCESSING AND CFD SOLUTION

Pre-Processing Preliminaries

Tutorial 1.1


This part of the tutorial gives a detailed account of how to: • • • • •

Initiate a pro-STAR pre-processing session that builds a CFD model for a simple problem Alter fluid properties Specify turbulence and thermal models Apply boundary conditions Perform a CFD analysis using the STAR-CD solver

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut1-1. If you have completed Tutorial 1.1 and 1.2 of the Meshing Tutorials volume, copy the model file created at the end of Meshing Tutorial 1.2 (mixing_pipe.mdl) into this directory. Alternatively, copy the coded files mixing_pipe.cel, mixing_pipe.vrt, mixing_pipe.bnd and mixing_pipe.inp supplied with the STAR-CD installation into it. • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (mixing_pipe) in the Casename text box

If you have chosen to restart from the model file mixing_pipe.mdl: • •

Check that the Resume existing .mdl file option is selected Click Continue

If you have chosen to start from the coded files provided with STAR-CD: • •

Click Continue Select File > Read File... in the main pro-STAR window, as shown below:

•

In the Input Coded Command File dialog check that the File Name is mixing_pipe.inp Click Apply Click Close

• • Version 4.02

1-3

Tutorial 1.1


Pre-Processing Mesh Checking

The next step is to give the model a name: • •

In the main window, select File > Model Title In the Title text box type: FLOW IN A MIXING PIPE

• Mesh Checking

Click Apply

A simple, but often effective, method of checking the mesh is to display it on screen and examine it visually: •

Select C > All

The I/O window states that the mesh contains 82,339 cells. Rotating the mesh by holding the left mouse button whilst dragging the cursor across the display window should not reveal any malformed or irregular cells on the mesh surface. Once you are satisfied there are no problems there, reset the view and check the interior mesh structure:

1-4

•

Select Plot > Up Axis > Z

•

Select View > Isometric > -1,-1,1 Version 4.02

Tutorial 1.1



•

Click the button at the bottom of the rotate slider to reset the view angle

• •

Click Zoom Off Turn on light shading by clicking the ‘light’ button, . Light shading enhances the 3D effect of the mesh visualisation. Click Cell Plot to display the mesh shown in Figure T1.0-2 above Select a Clipped Hidden plot type to display Figure T1.1-1

• •

The varying size of cells within the trimmed mesh is clearly shown.

Version 4.02

1-5

Tutorial 1.1


Pre-Processing Basic Problem Settings

Figure T1.1-1

Basic Problem Settings

Clipped hidden view of mixing pipe mesh interior

Most pre-processing operations are performed using various panels of the STAR GUIde window. The first panel to check is Select Analysis Features at the top of the STAR GUIde folder tree: •

Open the Select Analysis Features panel

This case is a steady-state problem and includes none of the other analysis features listed here, so no changes are required.

1-6

Version 4.02

Tutorial 1.1


Pre-Processing Material Properties

Material Properties

Before any boundary conditions can be applied, appropriate fluid properties must be specified. The panel to check for this is Molecular Properties, located inside the Thermophysical Models and Properties and Liquids and Gases folders: • • •

Select the Thermophysical Models and Properties folder Select the Liquids and Gases sub-folder Open the Molecular Properties panel

The default fluid material is air so this does not need changing. However, since the air temperature (and hence density) of each inlet stream is different, the Density option must be re-specified: •

Select Ideal-f(T,P) from the Density list

The rest of this panel’s options are suitable for the analysis so: •

Click Apply

The next set of parameters requiring attention are those describing the application of a turbulence model: • • Version 4.02

Open the Turbulence Models panel Turn On turbulence modelling 1-7

Tutorial 1.1


Pre-Processing Boundary Locations

•

Under the Turbulence tab, select the k-Epsilon/High Reynolds Number model. This is the default k-ε model in STAR-CD and will be used in most of the tutorials provided.

All default parameter settings are suitable for this model so: •

Click Apply

Since the problem in hand is non-isothermal, the energy equation must be activated: • • •

Open the Thermal Models panel Turn On the temperature calculation Click Apply

This completes the specification of physical properties and models for the fluid. The next step is to locate the boundary regions and specify boundary conditions. Boundary Locations

Meshes such as this one created using pro-STAR’s Automated Meshing module automatically include boundary definitions on all mesh surfaces. To display these boundaries: • •

Select B > All in the pro-STAR window Click Bound in the Cell Plot Display Options area of this window to display Figure T1.1-2

Observe that there is one boundary for every cell face on the mesh surface. Depending on the features of that surface, these boundaries are split into different regions; in this case there are nine such regions numbered 14 — 22.

1-8

Version 4.02

Tutorial 1.1



Figure T1.1-2

Default boundaries displayed on a clipped hidden view of the mesh

Most of these regions correspond to parts of the mixing pipe wall and are redundant for the purposes of this tutorial. They may therefore be combined into a single region and assigned the appropriate wall boundary conditions. In doing this, one can take advantage of a useful pro-STAR feature that (a) assigns all cell faces on the mesh surface for which no boundaries have been specified to a default region (known as region no. 0) and (b) sets up a default set of boundary conditions (adiabatic, no-slip, stationary, smooth wall) to it. In this case, the default conditions are appropriate to the pipe wall and they may therefore be applied indirectly simply by deleting most of the boundaries shown in Figure T1.1-2. To start this process, first remove the boundaries on the inlet and outlet faces from the current boundary set: • •

Version 4.02

Select B > Unselect > Region (Cursor Select)... Using the screen cursor, click on any boundary lying on the pipe’s first inlet plane, as shown in Figure T1.1-3. The information displayed on the I/O window will indicate that the region number corresponding to this inlet is 14.

1-9

Tutorial 1.1



Select a boundary here

Figure T1.1-3

• • •

Selecting a boundary on the first inlet

Select View > Isometric > 1,-1,1 to change the view Select B > Unselect > Region (Cursor Select)... Using the screen cursor, click on any boundary lying on the pipe’s second inlet plane, as shown in Figure T1.1-4. The information displayed on the I/O window will indicate that the region number corresponding to this inlet is 22.


Figure T1.1-4

1-10

Selecting a boundary on the second inlet

Version 4.02

Tutorial 1.1



• •

Select B > Unselect > Region (Cursor Select)... Using the screen cursor, click on any boundary lying on the pipe’s outlet plane, as shown in Figure T1.1-5. The information displayed on the I/O window will indicate that the region number corresponding to the outlet is 19.


Figure T1.1-5

Selecting a boundary on the outlet

To verify that the above operations have been performed correctly: •

Enter the following command in the I/O window: COUNT BOUNDARY

The resulting I/O window output should be as shown below, indicating that all inlet/outlet boundaries have been excluded; hence all those remaining in the set are the (redundant) wall boundaries created by the AutoMesh Module.

To delete these boundaries: •

Enter the following command in the I/O window: BDEL BSET

Version 4.02

1-11

Tutorial 1.1


Pre-Processing Boundary Conditions

Display the remaining boundaries: • • •

Select B > All Change back to a Hidden Surface plot Select View > Isometric > -1,-1,1 to display Figure T1.1-6

Figure T1.1-6

Boundary Conditions

Specify boundary conditions at the inlets and outlet as follows: • • • • • •

1-12

Boundary display with a single (default) wall boundary region

Select the Define Boundary Conditions folder in the STAR GUIde window Open the Define Boundary Regions panel In the boundary regions list, select Reg# 0 (the default boundary region) and note that it is defined as a stationary, no-slip, adiabatic wall, as required Select Reg# 14, the first inlet, from the boundary regions list Choose Inlet from the Region Type drop-down menu Enter boundary conditions as shown below:

Version 4.02

Tutorial 1.1



• • • •

Version 4.02

Click Apply Select Reg# 22, the second inlet, from the boundary regions list Choose Inlet from the Region Type drop-down menu Enter boundary conditions as shown below:

1-13

Tutorial 1.1



• • • • •

1-14

Click Apply Select Reg# 19, the outlet, from the boundary regions list Choose Outlet from the Region Type drop-down menu The boundary condition defaults shown on the panel are appropriate for this case, so click Apply to confirm Click Replot to produce the mesh plot shown in Figure T1.1-7, which now includes a graphical representation of the boundary conditions applied above. Check that the yellow arrows indicating the inlet velocities point in the correct direction and are perpendicular to the inlet boundary planes.

Version 4.02

Tutorial 1.1


CFD Analysis Set Run Time Controls

Figure T1.1-7

Boundary conditions shown on mesh plot

This completes the boundary condition setup. •

Turn off the Bound Cell Plot Display Option

Set Run Time Before the analysis can be run in STAR-CD, the maximum number of iterations to Controls be performed and the maximum residual tolerance acceptable for convergence need to be specified: • • • •

In the STAR GUIde window, select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Change the Number of Iterations to 300 The default Max. Residual Tolerance of 0.001 is acceptable so click Apply

The pre-processing task is now complete. The next section details how to prepare and run the analysis in STAR-CD. CFD Analysis There are two ways of running a STAR-CD analysis: 1. Save the geometry and problem files in pro-STAR, then quit pro-STAR and run the STAR solver from the command line 2. Run STAR interactively from within pro-STAR using STAR GUIde Both of these are described below.

Version 4.02

1-15

Tutorial 1.1


CFD Analysis Running From The Command Line

Running From The Command Line

Begin by writing the geometry and problem files, save the model file and then quit pro-STAR: • • • • • •

In the pro-STAR window, select File > Write Geometry File to open the Geometry File Write dialog The geometry was created in centimetres so set the Scale Factor to 0.01 Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

At the command line enter the following: star The analysis will start and the results will be displayed in your session’s window. Once it is complete, pro-STAR may be restarted and the results post-processed as described in the second part of this tutorial. Running Interactively

STAR GUIde’s Run Analysis Interactively panel activates the STAR solver through the pro-STAR interface: • •

Open the Run Analysis Interactively panel Click Start New Analysis

The geometry and problem files will be written automatically and the analysis will run in the window that pro-STAR was started from. Once complete, you can continue by post-processing the results in pro-STAR as described in the next section.

1-16

Version 4.02

Tutorial 1.1

POST-PROCESSING

Post-Processing Preliminaries

Tutorial 1.1

POST-PROCESSING

This part of the tutorial gives a detailed account of how to: • • • •

Initiate a pro-STAR post-processing session for evaluating the solution results produced by STAR-CD for a simple problem Create simple vector and contour plots Produce plots of particle tracks Combine particle tracks with vector or contour plots

Post-Processing Preliminaries Begin by checking that the model file, mixing_pipe.mdl, and the results file, mixing_pipe.ccm, generated during the first part of this tutorial exist in your current working directory. • • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Check that the case name (mixing_pipe) is displayed in the Casename text box and that the Resume existing .mdl file option is selected Click Continue

Read in the results of the analysis: • • •

Contour Plots

The first plot to be drawn is a contour plot of temperature on the surface of the mixing pipe: • • •

Version 4.02

Select the Post-Processing folder Open the Load Data panel to display the File(s) tab Click Open Post File

Select the Data tab in the Load Data panel Turn On the Smooth Option Select item Temperature from the Scalar Data list

1-17

Tutorial 1.1

POST-PROCESSING

Post-Processing Contour Plots

1-18

• •

Click Get Data Select Go To > Create Plots to open the Create Plots panel

•

Under the 3-D Surface tab, select options Contour (filled) and Edge

•

Click Plot To Screen to display Figure T1.1-8

Version 4.02

Tutorial 1.1

POST-PROCESSING


Figure T1.1-8

Temperature contours on the mesh surface

Now plot contours of velocity magnitude on an x-z plane passing through the origin: • • • • • •

Version 4.02

Click Go To Load Data to return to the Load Data panel Select item Velocity Magnitude from the Calculated Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select options Contour (filled) and Edge Change the Normal coordinates to 0, 1, 0

1-19

Tutorial 1.1

POST-PROCESSING


• •

Click Apply Click Plot to Screen to display Figure T1.1-9

Figure T1.1-9

1-20

Velocity magnitude contours on an x-z plane through the origin

Version 4.02

Tutorial 1.1

POST-PROCESSING

Post-Processing Velocity Vector Plots

Velocity Vector Plots

Velocity vectors will first be plotted on the mesh surface: • • • • • •

Click Go To Load Data Select Velocity Components UVW from the Vector Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, select options Vector and Edge Click Plot to Screen to display Figure T1.1-10

Figure T1.1-10

Velocity vectors displayed on the mesh surface

It can be seen that the flow field pattern cannot be seen very clearly as Figure T1.1-10 displays far too many vectors. Therefore, the following measures may be taken to thin out the vectors and generally improve the clarity of the plot: • • • •

Version 4.02

Select the Vectors tab in the Create Plots panel Adjust the Thin Vectors slider so that it is at approximately 0.25 Change the Scale Factor to 0.7 to make each vector arrow shorter Change the Fraction Length of Arrow Head to 0.3 to make each arrow head larger

1-21

Tutorial 1.1

POST-PROCESSING


• •

Click Apply Click Replot in the pro-STAR window to display Figure T1.1-11

Figure T1.1-11

Thinned out velocity vectors displayed on the mesh surface

The revised plot now clearly shows the flow swirling through the mixing pipe. Next, plot velocity vectors on the plane that was previously used for the velocity magnitude contour plot:

1-22

Version 4.02

Tutorial 1.1

POST-PROCESSING


• • •

Select the Section Clipped tab in the Create Plots panel Select options Vector and Edge Click Plot to Screen to display Figure T1.1-12

Figure T1.1-12

Velocity vectors displayed on an x-z plane

The vectors shown in Figure T1.1-12 are too thinly spaced near the centre of the model geometry. However, this is not the case near the walls where the presence of a finer mesh results in more vectors being displayed. A plot with evenly distributed vectors across the plane can be achieved using the Presentation Grid facility: • • •

•

Version 4.02

Select the Vectors tab in the Create Plots panel Turn On the Presentation Grid facility The presentation grid is defined by the number of grid points in each direction across the entire plot window. For this case, specify the number of points in the x- and y- directions as 75 and 66, respectively. Move the Thin Vectors slider back to 1.0

1-23

Tutorial 1.1

POST-PROCESSING

Post-Processing Particle Tracks

• •

Click Apply Click Replot in the pro-STAR window to display Figure T1.1-13

Figure T1.1-13

Particle Tracks

1-24

Velocity vectors displayed on an x-z plane using a presentation grid

An effective way of visualising a flow pattern is to draw tracks of imaginary massless particles introduced into to the flow at specified points. Here we will draw tracks of particles introduced at the smaller inlet:

Version 4.02

Tutorial 1.1

POST-PROCESSING


• • • •

In the Post-Processing folder, select sub-folder Particle Tracks Open the Create Particle Tracks panel Select Boundary Faces for the Particle Location Type Select Bset from the drop-down menu that appears underneath

Before continuing, it is necessary to collect the inlet boundary faces from which particles will originate into a boundary set: • •

In the pro-STAR window, select a Geometry Plot and Hidden Surface plot type Click Bound in Cell Plot Display Options section

• • •

Hold the middle mouse button and drag to zoom in on the smaller inlet Select B > New > Cursor Select... Select 6 inlet boundary faces as indicated below:

Select boundaries here

Figure T1.1-14


Selecting boundary faces on the smaller inlet

Click the Done button at the top right of the screen to end cursor selection Click Replot to display a plot similar to that shown in Figure T1.1-15. Note 1-25

Tutorial 1.1

POST-PROCESSING


that the exact boundaries chosen is not important in this case

Figure T1.1-15

• • • •

Click Apply in the Create Particle Tracks panel Select the Generation tab Click Generate Tracks Select Go To > Plot Particle Tracks. The Plot Droplets/Particle Tracks panel should appear

•

In the Particle Tracks tab of this panel, change the Display Option to Continuous Click Plot Tracks Click Zoom Off in the pro-STAR window to display Figure T1.1-16

• •

1-26

Boundaries selected as starting points for particle tracks

Version 4.02

Tutorial 1.1

POST-PROCESSING


Figure T1.1-16

Tracks of particles introduced at the smaller inlet

Figure T1.1-16 illustrates very clearly the swirling nature of the flow. Particle tracks can also be plotted together with vectors or contours by producing such a plot after displaying the particle tracks: • • • • • • •

Version 4.02

Return to the Load Data STAR GUIde panel Select Data Type Cell & Wall/Bound (Smooth) Select Temperature from the Scalar Data list Click Get Data Select Go To > Create Plots In the Section Clipped tab of the Create Plots panel select options Contour (filled) and Edge Click Plot to Screen to display Figure T1.1-17

1-27

Tutorial 1.1

POST-PROCESSING


Figure T1.1-17

Particle tracks displayed with a temperature contour plot

Note that in order to produce further plots of vectors or contours without the particle tracks, you will need to return to the Create Droplets/Particle Tracks panel and click the Clear Tracks button at the bottom of the Particle Tracks tab. This completes the post-processing part of this tutorial. Descriptions of more complex post-processing operations may be found in some of the other tutorials in this volume.

1-28

Version 4.02


Tutorial 2 EVALUATION OF MESH EFFECTS Physical Problem Description The problem considered is steady airflow over an obstacle mounted at the bottom wall of a three-dimensional channel. The geometry is shown in Figure T2.0-1. This case is based on an investigation conducted by the Danish Maritime Institute whose experimental data are compared with the STAR-CD predictions. In the experimental set-up, the flow velocity and turbulence characteristics were non-uniform across the inlet section. However, to simplify the modelling procedure, the case presented here is based on a parabolic inlet velocity profile with fixed turbulence characteristics. The boundaries consist of an inlet, an outlet, a symmetry plane on one of the two ‘side’ faces (parallel to the plane of the paper in Figure T2.0-1) and default no-slip walls for the remaining boundaries. The fluid is air and its physical properties are assumed constant and equal to the STAR-CD default values: 1.205 kg/m3 1.81 × 10–5 Pa s

Density Molecular viscosity

The fluid enters the solution domain at standard pressure and temperature (1 bar and 293 K) with a velocity of 1.17 m/s. Based on the height of the obstacle, the Reynolds number is 3,115. The turbulent kinetic energy and dissipation rate at the inlet are set to 0.024 m2/s2 and 0.07 m2/s3, respectively; these values having been derived from experimental data. All fluid mass entering the solution domain exits through the outlet. The flow is isothermal, incompressible and turbulent and turbulence is simulated using the standard linear k-ε model combined with the Wolfstein two-layer model. Wall

300 Inlet

Outlet

40 320

Wall 870

10 All units in mm. The depth of the solution domain is 300 mm throughout.

Figure T2.0-1

Problem geometry

The same problem is modelled using three different meshes: a hexahedral, a tetrahedral and a polyhedral mesh. All three are based on the same initial shell surface defining the problem geometry but each mesh was produced using different Version 4.02

2-1


methods. Comparisons are then drawn between the accuracy and speed of each type of mesh.

2-2

Version 4.02

Tutorial 2.1

HEXAHEDRAL MESH ANALYSIS


Tutorial 2.1


This tutorial will show the user how to: • • • • •

Model a 3D flow using a simple hexahedral mesh Apply, and verify the use of, a two-layer turbulence model Use a pre-defined table to describe a boundary condition Produce contour plots of wall data Produce and customize graphs of cell and wall data

Pre-Processing Preliminaries Begin by creating a directory for this tutorial (called tut2-1) and copy the cell, vertex and boundary files supplied with STAR-CD (hex.cel, hex.vrt and hex.bnd) into it. Also copy the table file inlet.tbl and the text file exp230.xy. The table describes the inlet velocity profile while the text file contains the experimental data and is used for comparing them to the analysis results. Start up pro-STAR in this directory: • • • • • • •

Type prostar at the command line Specify the graphics driver (xm, mesa or glm) Type hex in the Casename text box Click Continue In the main pro-STAR window, select File > Model Title In the Title text box type AIR FLOW OVER AN OBSTACLE (HEXAHEDRAL MESH) Click Apply

Make sure that the STAR-GUIde window is displayed on your screen, next to the main pro-STAR window. If not, activate it by clicking the special ‘Show STAR-GUIde’ button shown below:

• • • •

Select folder Create and Import Grids and then open the Import Grids panel Select pro-STAR as the file Format Check that the default cell and vertex files are hex.cel and hex.vrt, respectively, and that both are of File Type Coded Click Import Grid

The I/O window should tell you that 74,985 vertices and 67,699 cells have been imported. Ignore the warnings regarding non-existent cell table numbers as new ones are created during import. To display the grid: • • Version 4.02

In the main pro-STAR window, choose C > All Select View > Isometric > -1,1,1 2-3

Tutorial 2.1



•

Click Cell Plot to display Figure T2.1-1

Figure T2.1-1

Hexahedral mesh

There are currently no boundaries attached to the grid as only the cell and vertex data have been imported. To import boundary definitions from the boundary file: • • •

Select folder Locate Boundaries in STAR-GUIde and open the Import Boundaries panel The boundary file is hex.bnd. This should be displayed in the File Name box Click Apply

Now the boundaries can be displayed: • •

In the main pro-STAR window, choose B > All Click Replot

Hide the boundary regions again: • Material Properties

Click off Bound in the Cell Plot Display Options area of the window

Check the default fluid property settings. The only property data needed for an isothermal and incompressible flow are fluid density and molecular viscosity. • • •

Select folder Thermophysical Models and Properties in STAR-GUIde Select sub-folder Liquids and Gases Open the Molecular Properties panel

Given that the default property values are those of air at standard temperature and pressure, no change is necessary. Turn on the standard k-ε turbulence model: • 2-4

Open the Turbulence Models panel Version 4.02

Tutorial 2.1



• • •

Click On to select turbulence modelling Select option K-Epsilon/High Reynolds Number from the Turbulence menu Click Apply

A two-layer model is to be used to account for turbulence near the walls. The near-wall layer thickness should be large enough to fully encompass the boundary layer (but not too large, as the computational time will increase unnecessarily). To define the two-layer model: • • • • •

Select the Near-Wall Treatment tab Turn On the Standard Two-Layer model Select option Wolfstein from the Two-Layer Model menu Change the Near-Wall Layer Thickness to 0.04 m. The suitability of this value will be checked in the “Post-Processing” section Click Apply

Choose a cell just above the obstacle (say cell no. 801) as the monitoring location. • • • • Boundary Conditions

Open the Monitoring and Reference Data panel Type 29772 in the Monitoring cell number box Type 93 in the Reference Pressure Cell Number box. This is a cell on the wall near to the inlet. Click Apply

Having imported the boundary location definitions and their associated region numbers, boundary conditions are specified as follows: For the wall (region 0): • • • • •

Select folder Define Boundary Conditions Open the Define Boundary Regions panel Select region no. 0 in the region scroll list Select Active from the Two-Layer drop-down menu Click Apply

For region 1, the inlet velocity profile will be specified by a table: • • •

Select region no. 1 in the region scroll list Select Table from the Options menu Click the file browser button shown below and select the table file inlet.tbl

• • •

Click OK to exit from the file browser Select option k/Epsilon from the Turb. Switch menu Type inlet values for the turbulence parameters; 0.024 m2/s2 in the k box and 0.07 m2/s3 in the Epsilon box. Click Apply

•

For the outlet (region 2): • Version 4.02

Check that the Flow Split is set to 1 2-5

Tutorial 2.1


Pre-Processing Analysis Controls

•

Click Apply

No user input is required for the last (symmetry plane) boundary region. Check the model by displaying some key parameters in the I/O window (number of cells and cell types, boundary regions, etc.) and then save the model data. • • Analysis Controls

In the main pro-STAR window, select Utility > Count > All Select File > Save Model

Use of a second-order differencing scheme can significantly increase the accuracy of the solution. Select MARS as the differencing scheme for this analysis: • • • •

Select folder Analysis Controls in STAR GUIde followed by sub-folder Solution Controls Select the Equation Behaviour sub-folder and open the Primary Variables panel Under the Differencing Schemes tab, select MARS as the momentum and turbulence Differencing Scheme Click Apply

Set the frequency of outputting data to the solution (post-processing) file and specify that wall data (shear force coefficients and y+ values) are to be stored in it. Also specify the maximum number of iterations: • • • • • • • • • Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data for the hexahedral mesh, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

2-6

Select sub-folder Output Controls in STAR-GUIde and then open the Analysis Output panel In the Solution File Setup section, type 10 in the Output Frequency box Go to the Additional Output Data section and select item Shear Force in the Wall Data scroll list Click option button Post Repeat the above process for item Yplus Click Show selected to display a summary of the chosen items Click Apply Go to the Analysis Preparation/Running folder and open the Set Run Time Controls panel Change the Number of Iterations to 200

In the main pro-STAR window, select File > Write Geometry File Type 0.001 in the Scale Factor text box to convert the geometry units from millimetres to metres Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit Version 4.02

Tutorial 2.1


CFD Analysis Preliminaries

CFD Analysis To perform the analysis interactively, proceed as follows: • • • •

Select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that the units in which the model was built are correctly selected (option button millimetres). Leave all other settings at their default values. Click Start New Analysis

The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file hex.ccm: • • • Basic Plots

Select the cell-based velocity vectors for plotting. Also scale down the vector size and switch on the edge display mode: • • • • • • • • • • • • • •

Version 4.02

Select folder Post-Processing Open the Load Data panel and display the File(s) tab Click Open Post File

Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW In the Scalar Data list, check that the default setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel In the Section Clipped tab, choose Vector from the Option menu and Edge from the Edge/Mesh menu Set the Normal parameter to 0, 0, 1 and the Point parameter to 0, 0, 0 Go to the Vectors tab and type 0.5 in the Scale Factor box Click Apply Go to the Options tab and select User from the Range menu Enter a range of 0 to 1.7 Click Apply Under the Section Clipped tab, click Plot to Screen Display Figure T2.1-2 by clicking the small button at the bottom right of the orientation cube, as shown below:

2-7

Tutorial 2.1


Post-Processing Basic Plots

Figure T2.1-2

Velocity vector plot on the symmetry plane

As expected, a recirculation zone is observed downstream of the obstacle. Zoom in using the mouse to examine it more closely. Now examine the pressure distribution: • • • • • • • •

2-8

Click Go To Load Data In the Data tab, select Cell & Wall/Bound (Smooth) from the Data Type menu In the Scalar Data list, select item Pressure and then click Get Data Select Go To > Create Plots to display the Create Plots panel In the Section Clipped tab choose Contour (filled) from the Option menu and Edge from the Edge/Mesh menu In the Options tab, enter a Range of -1.9 to 0.6 Click Apply Under the Section Clipped tab, click Plot to Screen to display Figure T2.1-3

Version 4.02

Tutorial 2.1



Figure T2.1-3

Filled contour plot of pressure on the symmetry plane

Plot the vertex-based turbulence kinetic energy and dissipation rate: • • • • • • • • •

In the Options tab select User from the Range list and enter values 0 to 0.2 Click Apply Click Go To Load Data Select item Turb. Kinetic Energy from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T2.1-4 Select item Dissipation Rate from the Scalar Data list Click Get Data In the main window, click Replot

The plot is almost entirely blue. This is because the dissipation rate is very high just above the obstruction. To apply a more suitable scale to the plot: • • • •

Version 4.02

Click Go To > Create Plots In the Options tab select User from the Range list and enter values 0 to 2 Click Apply In the main window, click Replot to display Figure T2.1-5

2-9

Tutorial 2.1


Post-Processing Validation of Results

Figure T2.1-4

Contour plot of turbulence kinetic energy on the symmetry plane S

Figure T2.1-5

Validation of Results

2-10

Contour plot of turbulence dissipation rate on the symmetry plane

In Tutorial 2.2 and 2.3, tetrahedral and polyhedral cells will be used to mesh the same problem. In order to ensure that the three meshes are comparable, the distribution of y+ values at the wall boundaries will be noted for each of them.

Version 4.02

Tutorial 2.1



• • • • • •

Go to the Options tab in the Create Plots panel Choose Auto for Range and click Apply In the Load Data panel, select option Wall from the Data Type menu Turn Smooth Option Off Select item YPLUS from the Scalar Data list Click Get Data

Since wall data are stored in specially created shells at the wall surfaces (cell type no. 5), it is necessary to assemble a new cell set that contains only these shells: • • • • • • • •

Change the plot type to a Hidden Surface plot Select View > Axis > +Y Turn off edge and mesh plotting by clicking the ‘edge’ and ‘mesh’ buttons in the main pro-STAR window Select Plot > Wall Plot Select C > New > Type... and click anywhere on the visible surface Select Post > Caverage > Cset Select Plot > Wall Plot Type VIEW -0.5 0.5 -1.0

•

in the I/O window Click Replot to display Figure T2.1-6

Figure T2.1-6

y+ values plotted on the walls

This plot shows that the y+ values never exceed 6.1 and that for the vast majority of the flow regime they are below 3.0, the maximum value considered acceptable for a rigorous examination of wall data. Version 4.02

2-11

Tutorial 2.1


Post-Processing Graph Plotting

To check whether the near-wall layer thickness in the turbulence model (see page 2-5) was given a reasonable value: • • • • • • • • • •

In the Load Data panel, select Data Type Cell Turn the Smooth option Off Choose Two Layer from the Scalar Data list Click Get Data Choose Go To > Create Plots In the 3D Surface tab select Contour (filled) and None Change the plot type to a Section (Surface) plot Click Plot to Screen Select C > All Click Cell Plot and reset the view by clicking the small button at the bottom left of the orientation cube to display Figure T2.1-7.

The red region in this plot represents cells in the boundary layer, the green region cells that are outside the boundary layer but still inside the near-wall layer and the blue region cells outside the near-wall layer. The plot shows that the two-layer model has been implemented correctly as there are no places at which the blue and red regions are in contact. In other words, the near-wall layer encompasses the whole boundary layer, as required. The green region also has minimal thickness, hence the computational cost is minimal.

Figure T2.1-7

Graph Plotting

2-12

Plot demonstrating correct application of two-layer model

It is sometimes useful to display the results of the analysis as x-y graphs, bar charts or pie charts. When combined with various data manipulation functions (e.g. OPERATE or ROPERATE), such pro-STAR facilities constitute powerful tools for display and analysis. Some of the code’s x-y graph plotting capabilities are demonstrated in this part of the tutorial. Version 4.02

Tutorial 2.1


Post-Processing Simple Graphs

The following operations are normally necessary for producing an x-y graph: • • • • • •

Extract and prepare the data to be plotted Store the data in graph registers Create graphs by plotting the contents of any register against those of another register Combine several graphs into pro-STAR’s basic graph entity, called a ‘frame’ Define essential information for each frame, such as axis scaling, legends and graph labels Display the frame

One does not need to follow the entire procedure outlined above. Default settings can often be used, as shown in the examples below. Simple Graphs

The first requirement is to assemble a set of U velocity magnitude values along a line on the symmetry plane located at x = 230 mm. The graph will plot the U velocity (the abscissa) against the y-coordinate (the ordinate). To do this, and produce a default graph, proceed as follows: •

• • • • • •

Not all the graph specification options are available when a section plot is displayed. To avoid this, select a Hidden Surface plot using the drop-down menu in the main pro-STAR window. In the STAR GUIde window, select sub-folder Graphs followed by sub-folder Extract/Graph Data Open the Field Data panel Click Graph Reset at the bottom of the panel and choose Yes Select option Line from the menu at the top of the Define Locations section Enter 300 as the Total number of data points To increase the number of allowed data points, type MEMORY MAXPRB 1000

• • • • • • • • • •

Version 4.02

in the I/O window Choose Line defined by End points Specify these end points to be 230, 0, 0 and 230, 300, 0 In the Data Type tab, choose Post 4 as the post register number in which to load field data and then click Go To Load Data In the Load Data panel, select option Cell from the Data Type menu Turn On the Smooth Option Select item Velocity Component U from the Scalar Data list Click Get Data Select Go To > Field Data. The Field Data panel display will confirm that the U velocity component (SU) is now loaded in post register no. 4 In the Graph Data section, choose to plot the graph data against the Y-axis Click Create Graph to see a default graph of the data, as shown in Figure T2.1-8

2-13

Tutorial 2.1


Post-Processing Customizing Graphs

Figure T2.1-8

Customizing Graphs

It is clear that the default graph is not exactly what is required. To swap the axes and adjust their scales: • • • • • • • • • • • • •

• • • • 2-14

Default graph of U velocity on the symmetry plane at x = 230 mm

Click Go To Customize Graph In the Customize Graphs panel, go to the Pairs tab Click Clear at the bottom of the Register Pairs list to remove the existing graph Choose SU (which should be Reg# 9) from the X-Axis Register list Choose Y LOCATION (which should be Reg# 4) from the Y-Axis Register list Click Add Register Pair and Apply Click Draw All Frames Go to the Axis tab In the X-Axis Parameters sub-tab, change the Title to U - m/s Change the axis end-points by entering 0 and 1.4 in the Xmin, Xmax boxes, respectively Change the axis annotations by entering 0.1, the required segment length for major tick marks, in the Xmajor box Click Apply In the Y-Axis Parameters sub-tab, change the Title to Y - mm. Also, change the axis end-points by entering 0 and 300 in the Ymin, Ymax boxes, respectively Change the format for Numbers to Integer Click Apply Go to the Options sub-tab In the Additional Graph Labels section, select label no. 1 in the scroll list and Version 4.02

Tutorial 2.1



• • •

then enter the desired label, U velocity profile at x = 230 mm, in the text box underneath. Specify the label’s location by entering coordinates (3.5, 9.0) in the Sx and Sy boxes Click Apply In the main window, click Redraw to display the modified graph

Experimental results are provided in a coded (text) file. To plot these on the same graph and hence check the validity of the numerical results: • • • •

Select Go To > External Data The required File name is exp230.xy. Find it using pro-STAR’s built-in file manager Select xyxyxy from the Establish x-y pairs list Click Create Graph

The External Data panel can also be used to save graph register data to an external file. To save the data displayed in Figure T2.1-8: • • • •

Change the File name to hex230.xy Choose to Specify the Starting register to write data as 4 Change the Increment in register to write data to 5 Click Save Registers

Unfortunately, the colours of the two graphs are the same. To change one of them and add a legend: • • • • • • • • • • •

Version 4.02

Click Go To Customize Graph In the Display tab select the Legend sub-tab Specify the Location as X1 = 7.35, Y1 = 8.85, X2 = 9.85, Y2 =9.85 Click Apply Select the Registers tab Click on Reg# 4 in the Registers list and change its label to Numerical Click Apply Click on Reg# 11 in the Registers list and change its label to Experimental Change the Color under Line Parameters to number 7, i.e. yellow Click Apply Click Redraw in the main pro-STAR window to display Figure T2.1-9

2-15

Tutorial 2.1


Post-Processing Wall Shear Force

Figure T2.1-9

Comparison of U velocity profile with experimental results

The numerical results are within 10% of the experimental results in the region in which the experiment was carried out (0 < Y (mm) < 180). Wall Shear Force

In this case, wall shear force is a useful quantity for judging the length of the circulation zone; i.e. the re-attachment point of the recirculation zone can be determined by finding the point on the ‘bottom’ wall at which the wall shear force is zero. This may be determined approximately by using a wall plot, as in Figure T2.1-6, but a more accurate method is to plot a graph. The x-component of the wall shear force is by far the greatest, so it can be used in place of the total wall shear force scalar. The former is a more suitable choice because its sign also indicates the flow direction. On the other hand, the total wall shear force scalar is positive everywhere and so a minimum value would need to be used to estimate the re-attachment point instead of a zero value. To produce such a graph: • • • • • • • • • •

Click Graph Reset and then Yes to remove the existing graph data Select Go To > Field Data Change the Total number of data points to 175 Choose to Select data along a Line and Specify the End points as 330, 0, 0 and 1200, 0, 0 Select Post 4 from the Post data to load menu and click Go To Load Data Select Data Type Wall and Smooth Option On Select Shear Force (X-Dir) from the Scalar Data list and click Get Data Select Go To > Field Data Choose to plot the graph data against the X-axis Click Create Graph

To customize the graph: 2-16

Version 4.02

Tutorial 2.1


Post-Processing Final Operations

• • • • • • • • • • • •

• •

Click Go To Customize Graph In the Axis tab, choose the X-Axis Parameters sub-tab Change Xmin and Xmax to 330 and 1200, respectively Change the Title to X - mm and the Numbers type to Integer Click Apply Under the Display tab, Specify the graph Location as having parameters X1 = 2.0, X2 = 9.0, Y1 = 2.35, Y2 = 8.65 Click Apply Under the Y-Axis Parameters tab, change the Title to Shear Force - N Change the Title Location to 0.5, 6.8 Click Apply Go to the Options tab In the Additional Graph Labels section, select label no. 1 in the scroll list and then enter the desired label, Wall Shear Force at y = 0, downstream of obstruction, in the text box underneath. Specify the label’s location by entering coordinates (2.5, 9.0) in the Sx and Sy boxes Click Apply then Draw All Frames to display Figure T2.1-10

Figure T2.1-10

Graph of wall shear force along the ‘bottom’ wall

The recirculation zone extends roughly 800 mm downstream of the obstacle. Final Operations

Version 4.02

This tutorial is now complete. Exit pro-STAR by selecting: •

File > Quit > Quit, Nosave

2-17

Tutorial 2.2

TETRAHEDRAL MESH ANALYSIS

Tutorial 2.2

Pre-Processing


This tutorial tackles exactly the same problem as Tutorial 2.1 except that, in this case, a tetrahedral mesh is used instead of a hexahedral one. The dimensions of individual cells are approximately the same as in the hexahedral mesh. Particular care is also taken to ensure that the near-wall cells are of the same thickness. This tutorial will show the user how to: • • • •

Model a 3D flow using a simple tetrahedral mesh Apply, and verify the use of, a two-layer turbulence model Produce contour plots of wall data Produce and customize graphs of cell and wall data

Pre-Processing Create a directory for this tutorial (called tut2-2) and copy the coded files provided supplied with the STAR-CD installation (tet.cel, tet.vrt and tet.bnd) into it. Also copy the table file inlet.tbl and the text file exp230.xy., containing the inlet velocity profile and experimental data. Start up pro-STAR in this directory: • • • • • • •

Type prostar at the command line Choose the graphics driver (mesa, glm or xm) Type tet in the Casename box Click Continue Select File > Model Title In the Title text box type AIR FLOW OVER AN OBSTACLE (TETRAHEDRAL MESH) Click Apply

Now, import the grid into pro-STAR using STAR-GUIde: • • • •

In the STAR-GUIde window, select folder Create and Import Grids and then open the Import Grids panel Select pro-STAR as the file Format Check that the default cell and vertex files are tet.cel and tet.vrt, respectively, and that both are of File Type Coded Click Import Grid

The I/O window should show that 52,663 vertices and 140,141 cells have been imported. Ignore the warnings regarding non-existent cell table numbers as new ones are created during import. Boundary data must also be imported, as follows: • • •

Select folder Locate Boundaries and open the Import Boundaries panel The boundary file is tet.bnd. This should be displayed in the File Name text box Click Apply

To display the grid: • Version 4.02

In the main pro-STAR window, select C > All 2-19

Tutorial 2.2



• •

Select View > Isometric > -1,1,1 Click Cell Plot to display Figure T2.2-1

Figure T2.2-1

Tetrahedral mesh

To display the boundaries: • • •

Select B > All Click Bound in the Cell Plot Display Options area of the window Check visually that all boundaries are appropriate to the case and then click off the Bound Cell Plot Display Option

Whenever a grid is imported from files other than a complete model (.mdl) file, it is always advisable to check that the mesh is connected and has no cracks in it. To check the mesh connectivity: • • •

Choose Tools > Check Tool from the pro-STAR window menu Select Connectivity from the Check Option list Click Apply

In this case, the cells are all connected and belong to one group so the mesh is OK. Material Properties

The default fluid property values are those of air at standard temperature and pressure. No change to these is necessary. Turn on the standard k-ε turbulence model: • • • • •

2-20

Select folder Thermophysical Models and Properties in STAR-GUIde Select sub-folder Liquids and Gases Open the Turbulence Models panel Click On to select turbulence modelling Select option K-Epsilon/High Reynolds Number from the Turbulence menu Version 4.02

Tutorial 2.2



•

Click Apply

A two-layer model is to be used to account for turbulence near the walls. The near-wall layer thickness should be large enough to fully encompass the boundary layer. To define the two-layer model: • • • • •

Select the Near-Wall Treatment tab Turn On the Standard Two-Layer model Select option Wolfstein as the Two-Layer Model Change the Near-Wall Layer Thickness to 0.035 m. The suitability of this value will be checked in the “Post-Processing” section Click Apply

Choose a fluid cell just above the obstacle (say cell no. 69732) as the monitoring location: • • • • Boundary Conditions

Open the Monitoring and Reference Data panel Type 66638 in the Monitoring cell number box Type 158 in the Pressure Reference Cell Number box. This cell is in the same position as the one specified in Tutorial 2.1 Click Apply

Having imported the boundary location definitions and their associated region numbers, boundary conditions are imposed as follows: For the wall (region 0): • • • • •

Select folder Define Boundary Conditions Open the Define Boundary Regions panel Select region no. 0 in the region scroll list Select Active from the Two-Layer pull-down menu Click Apply

For the inlet (region 1): • • • • • • •

Select region no. 1 in the region scroll list Select Table from the Options menu Click the file browser button and select the table file inlet.tbl Click OK to exit from the file browser Select option k/Epsilon from the Turb. Switch menu Type inlet values for the turbulence parameters; 0.024 in the K box and 0.07 in the Epsilon box. Click Apply

For the outlet (region 2): • •

Check that the Flow Split is set to 1 Click Apply

No user input is required for the last (symmetry plane) boundary region. Analysis Controls

Use of a second-order differencing scheme can significantly increase the accuracy of the solution. Select MARS as the differencing scheme for this analysis:

Version 4.02

2-21

Tutorial 2.2


CFD Analysis Final Operations

• • • •


Set the frequency of data output to the solution file and specify that wall data, specifically shear force coefficients and y+ values, are to be stored in it: • • • • • • •

Select sub-folder Output Controls and then open the Analysis Output panel In the Solution File Setup section, type 10 in the Output Frequency box Go to the Additional Output Data section and select item Shear Force in the Wall Data scroll list Click option button Post Repeat the above process for item Yplus Click Show selected to display a summary of the chosen items Click Apply

Specify the maximum number of iterations: • • •

Go to the Analysis Preparation/Running folder and open the Set Run Time Controls panel Change the Number of Iterations to 200 Click Apply

Check the model: • • Final Operations

In the Check Model Setup folder select the Check Everything panel Click All

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data for the tetrahedral mesh, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

In the main pro-STAR window, select File > Write Geometry File Enter 0.001 for the Geometry Scale Factor Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis To perform the analysis interactively, proceed as follows: • • 2-22

Select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Version 4.02

Tutorial 2.2



• •

Check that the units in which the model was built are correctly selected (option button millimetres). Leave all other settings at their default values. Click Start New Analysis

The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file tet.ccm: • • • Basic Plots

The plots shown in this section are similar to those in Tutorial 2.1, thus enabling the user to draw comparisons between the two cases. The first of these is a velocity vector plot: • • • • • • • • • • • • •

Version 4.02


Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW Click Get Data Select Go To > Create Plots to open the Create Plots panel In the Section Clipped tab, choose Vector from the Option menu and Edge from the Edge/Mesh menu Set the Normal parameter to 0, 0, 1 and the Point parameter to 0, 0, 0 Go to the Vectors tab and enter a Scale Factor of 0.5 Click Apply Go to the Options tab and select User from the Range list. Enter a range of 0 to 1.7 Click Apply Under the Section Clipped tab, click Plot to Screen Display Figure T2.2-2 by selecting View > Axis > +Z

2-23

Tutorial 2.2



Figure T2.2-2

Plot of velocity vectors on the symmetry plane

The plot shows very few differences to that in Figure T2.1-2, the most obvious being a slightly smaller recirculation zone. Now examine the pressure distribution: • • • • • • • •

2-24

Click Go To Load Data In the Data tab, select Cell & Wall/Bound (Smooth) from the Data Type menu In the Scalar Data list, select item Pressure and then click Get Data Select Go To > Create Plots to display the Create Plots panel In the Section Clipped tab choose options Contour (filled) and Edge In the Options tab, enter a Range of -1.9 to 0.6 Click Apply Under the Section Clipped tab, click Plot to Screen to display Figure T2.2-3

Version 4.02

Tutorial 2.2



Figure T2.2-3

Plot of pressure contours on the symmetry plane

The most obvious differences between Figure T2.2-3 and Figure T2.1-3 occur far downstream of the obstruction. Plot the vertex-based turbulence kinetic energy and dissipation rate: • • • • • • • • • • • •

Version 4.02

In the Options tab select User from the Range list and enter values 0 to 0.2 Click Apply Click Go To Load Data Select item Turb. Kinetic Energy from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T2.2-4 Select item Dissipation Rate from the Scalar Data list Click Get Data Click Go To > Create Plots In the Options tab select User from the Range list and enter values 0 to 2 Click Apply In the main window, click Replot to display Figure T2.2-5

2-25

Tutorial 2.2




Figure T2.2-4

Contours of turbulence kinetic energy on the symmetry plane

Figure T2.2-5

Contours of turbulence dissipation rate on the symmetry plane

Plot the y+ values at the wall boundaries to help verify the suitability of the mesh for the turbulence model employed: •

2-26

Go to the Options tab in the Create Plots panel Version 4.02

Tutorial 2.2



• • • • •

Choose Auto Range and click Apply In the Load Data panel, select option Wall from the Data Type menu Turn Smooth Option Off Select item YPLUS from the Scalar Data list Click Get Data

Since wall data are stored in specially created shells at the wall surfaces (cell type no. 5), it is necessary to assemble a new cell set that contains only these shells: • • • • • • • •

Change the plot type to a Hidden Surface plot Select View > Axis > +Y Turn off edge and mesh plotting by clicking the ‘edge’ and ‘mesh’ buttons in the main pro-STAR window Select Plot > Wall Plot Select C > New > Type... and click anywhere on the visible surface Select Post > Caverage > Cset Select Plot > Wall Plot Type VIEW -0.5 0.5 -1.0

•

in the I/O window Click Replot to display Figure T2.2-6

Figure T2.2-6


Note that the y+ values are roughly comparable to those shown for the hexahedral mesh (Figure T2.1-6). This is what we would expect because the thickness of the cell layer next to the wall is the same for both meshes. To check whether the near-wall layer thickness in the turbulence model (see page Version 4.02

2-27

Tutorial 2.2


Post-Processing Simple Graphs

2-21) was given a reasonable value: • • • • • • • • • • •

In the Load Data panel, select Data Type Cell Turn the Smooth option Off Choose Two Layer from the Scalar Data list Click Get Data Choose Go To > Create Plots In the Section Clipped tab select Contour (filled) and None Change the plot type to a Section (Surface) plot Click Plot to Screen Select C > All Click Cell Plot Display Figure T2.2-7 by clicking the small button at the bottom left of the orientation cube, as shown below:

The plot shows that the two-layer model has been implemented correctly. In addition, the tetrahedral mesh has permitted the use of a smaller near-wall layer thickness compared to that in Tutorial 2.1. This saves some computational time, though the greater number of cells in the tetrahedral model is a much more significant factor.

Figure T2.2-7

Simple Graphs 2-28


Graphs similar to those in Tutorial 2.1 will be created next. The first requirement is to assemble a set of U velocity magnitude values along a line located at x = 230 mm, z = 0 mm. The graph will plot the U velocity (the abscissa) against the y-coordinate Version 4.02

Tutorial 2.2



(the ordinate). To do this, and produce a default graph, proceed as follows: •

• • • • • • • • • • • • • • •

Not all the graph specification options are available when a section plot is displayed. To avoid this, select a Hidden Surface plot using the drop-down menu in the main pro-STAR window. In the STAR GUIde window, select sub-folder Graphs followed by sub-folder Extract/Graph Data Open the Field Data panel Click Graph Reset at the bottom of the panel and choose Yes Select option Line from the menu at the top of the Define Locations section Enter 300 as the Total number of data points Choose Line defined by End points Specify these end points to be 230, 0, 0 and 230, 300, 0 In the Data Type tab, choose Post 4 as the post register number in which to load field data and then click Go To Load Data In the Load Data panel, select option Cell from the Data Type menu Turn On the Smooth Option Select item Velocity Component U from the Scalar Data list Click Get Data Select Go To > Field Data. The Field Data panel display will confirm that the U velocity component (SU) is now loaded in post register no. 4 In the Graph Data section, choose to plot the graph data against the Y-axis Type MEMORY MAXPRB 1000

•

Customizing Graphs

The default graph in not very well presented at this stage. To rectify this we can swap the axes and adjust their scales: • • • • • • • • • • • • •

Version 4.02

in the I/O window to increase the number of sensors (data points) allowed Back on the Field Data panel, click Create Graph to see a default graph of the data

Click Go To Customize Graph In the Customize Graphs panel, go to the Pairs tab Click Clear at the bottom of the Register Pairs list to remove the existing graph Choose SU (which should be Reg# 9) from the X-Axis Register list Choose Y LOCATION (which should be Reg# 4) from the Y-Axis Register list Click Add Register Pair and Apply Go to the Axis tab In the X-Axis Parameters sub-tab, change the Title to U - m/s Enter 0 and 1.4 in the Xmin, Xmax boxes, respectively Enter 0.1 in the Xmajor box and click Apply In the Y-Axis Parameters sub-tab, change the Title to Y - mm. Also, enter 0 and 300 in the Ymin, Ymax boxes, respectively Select Integer as the Numbers format Click Apply 2-29

Tutorial 2.2



• • • • •

Go to the Options sub-tab In the Additional Graph Labels section, select label no. 1 in the scroll list and then enter U velocity profile at x = 230 mm in the text box underneath. Enter coordinates (3.5, 9.0) in the Sx and Sy boxes Click Apply In the main window, click Redraw to display the modified graph

Experimental results are provided in a coded (text) file. To plot these on the same graph and hence check the validity of the numerical results: • • • •

Select Go To > External Data The required File name is exp230.xy. Find it using pro-STAR’s built-in file manager Select xyxyxy from the Establish x-y pairs list Click Create Graph

The External Data panel can also be used to save graph register data to an external file. To save the data displayed in the graph: • • • •

Change the File name to tet230.xy Choose to Specify the Starting register to write data as 4 Change the Increment in register to write data to 5 Click Save Registers

To add a legend: • • • • • • • • • • •

2-30

Click Go To Customize Graph In the Display tab select the Legend sub-tab Specify the Location as X1 = 7.35, Y1 = 8.85, X2 = 9.85, Y2 =9.85 Click Apply Select the Registers tab Click on Reg# 4 in the Registers list and change its label to Numerical Click Apply Click on Reg# 11 in the Registers list and change its label to Experimental Change the Color under Line Parameters to number 7, i.e. yellow Click Apply Click Redraw in the main pro-STAR window to display Figure T2.2-8

Version 4.02

Tutorial 2.2


Post-Processing Wall Shear Force

Figure T2.2-8

Comparison of U velocity profile with experimental results

As with the hexahedral mesh, the numerical results are within 10% of the experimental results in the region in which the experiment was carried out (0 < Y (mm) < 180). Wall Shear Force

To produce a graph of wall shear force: • • • • • • • • • •

Click Graph Reset and then Yes to remove the existing graph data Select Go To > Field Data Change the Total number of data points to 175 Choose to Select data along a Line and Specify the End points as 330, 0, 0 and 1200, 0, 0 Select Post 4 from the Post data to load menu and click Go To Load Data Select Data Type Wall and Smooth Option On Select Shear Force (X-Dir) from the Scalar Data list and click Get Data Select Go To > Field Data Choose to plot the graph data against the X-axis Click Create Graph

To customize the graph: • • • • • • • • Version 4.02

Click Go To Customize Graph In the Axis tab, choose the X-Axis Parameters sub-tab Change Xmin and Xmax to 330 and 1200, respectively Change the Title to X - mm and the Numbers type to Integer Click Apply Under the Y-Axis Parameters tab, change the Title to Shear Force - N Change the Title Location to 0.5, 5.8 Click Apply 2-31

Tutorial 2.2



• •

• •

Go to the Options tab In the Additional Graph Labels section, select label no. 1 in the scroll list and then enter the desired label, Wall Shear Force at y = 0, downstream of obstruction, in the text box underneath. Specify the label’s location by entering coordinates (2.0, 9.0) in the Sx and Sy boxes Click Apply then Draw All Frames to display Figure T2.2-9

Figure T2.2-9

Graph of wall shear force along the ‘bottom’ wall

The irregularity of the tetrahedral mesh leads to a less smooth shear stress profile compared to that for the hexahedral mesh. Even so, the predicted recirculation zone length can easily be measured. Final Operations

2-32



Version 4.02

Tutorial 2.3

POLYHEDRAL MESH ANALYSIS

Tutorial 2.3

Pre-Processing


This tutorial will show the user how to: • • • • •

Model a 3D flow using a simple polyhedral mesh Apply, and verify the use of, a two-layer turbulence model Produce contour plots of wall data Produce and customize graphs of cell and wall data Draw comparisons between different mesh types

Pre-Processing Create a directory for this tutorial (called tut2-3) and copy the files provided with STAR-CD (poly.cel, poly.vrt and poly.bnd) into it. Also copy the table file inlet.tbl and the text files exp330.xy, hex330.xy, and tet330.xy, which will be used to draw comparisons between the results produced by the three meshes in this tutorial group. Start up pro-STAR in this directory: • • • • • • •

Type prostar at the command line Choose the graphics driver (mesa, glm or xm) Type poly in the Casename box Click Continue Select File > Model Title In the Title text box type AIR FLOW OVER AN OBSTACLE (POLYHEDRAL MESH) Click Apply

Import the cell, vertex and boundary data into pro-STAR using STAR-GUIde and display the grid and boundaries: • • • • • • • • • • • • • •

Version 4.02

In the STAR-GUIde window, select folder Create and Import Grids and then open the Import Grids panel Select pro-STAR as the file Format Check that the default cell and vertex files are poly.cel and poly.vrt, respectively, and that both are of File Type Coded Click Import Grid In the main pro-STAR window, select C > All Select View > Isometric > -1,1,1 Click Cell Plot to display Figure T2.3-1 In the STAR-GUIde window, select folder Locate Boundaries Open the Import Boundaries panel Check that poly.bnd is displayed in the File Name box Click Apply In the main pro-STAR window, select B > All Click Bound in the Cell Plot Display Options area of the window Check the boundary locations visually and then click off the Bound Cell Plot Display Option

2-33

Tutorial 2.3



Figure T2.3-1

Material Properties

Polyhedral Mesh

Turn on the two-layer turbulence model: • • • • • • • •

Select folder Thermophysical Models and Properties in STAR-GUIde Select sub-folder Liquids and Gases Open the Turbulence Models panel Turn On turbulence and select the k-Epsilon/High Reynolds Number model from the list Under the Near-Wall Treatment tab, turn On the Standard Two-Layer option Select Wolfstein from the list Enter a Near-Wall Layer Thickness of 0.05 m. The suitability of this value will be checked in the “Post-Processing” section. Click Apply

Set the monitoring and pressure reference cell locations to be equivalent to those chosen in the previous two tutorials: • • • Boundary Conditions

2-34

Select the Monitoring and Reference Data panel Change the Monitoring cell number to 27774 Change the Reference Pressure Cell Number to 9

Activate the two-layer turbulence model at all wall boundaries: • • • • •

Select folder Define Boundary Conditions Open the Define Boundary Regions panel Select Reg# 0 Wall from the list Change the Two-Layer option to Active Click Apply

Version 4.02

Tutorial 2.3



Specify conditions at the inlet and outlet: • • • • • • • • • • Analysis Controls

Select Reg# 1 Inlet from the list Select Table from the Options menu Click the file browser button and select the table file inlet.tbl Click OK to exit from the file browser Select option k/Epsilon from the Turb. Switch menu Specify k to be 0.024 m2/s2 and Epsilon to be 0.07 m2/s3 Click Apply Select Reg# 2 Outlet from the list Check that the Flow Split is set to 1 Click Apply

Select MARS as the differencing scheme for this analysis: • • • •


Set the frequency of data output to the solution file and specify that wall data are to be stored in it: • • • • • • • Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data for the polyhedral mesh, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

Version 4.02

Select sub-folder Output Controls and then open the Analysis Output panel In the Solution File Setup section, type 10 in the Output Frequency box Go to the Additional Output Data section and select item Shear Force in the Wall Data scroll list Click option button Post Repeat the above process for item Yplus Click Show selected to display a summary of the chosen items Click Apply

Select File > Write Geometry File Enter 0.001 as the Geometry Scale Factor Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

2-35

Tutorial 2.3




Select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that the units in which the model was built are correctly selected (option button millimetres). Leave all other settings at their default values. Click Start New Analysis

The analysis will then start automatically. Convergence will be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file poly.ccm: • • • Basic Plots

The plots drawn in this section are similar to those in Tutorial 2.1 and Tutorial 2.2 to enable the user to draw comparisons between them. The first of these is a velocity vector plot: • • • • • • • • • • • • •

2-36


Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW Click Get Data Select Go To > Create Plots to open the Create Plots panel In the Section Clipped tab, choose options Vector and None Set the Normal parameter to 0, 0, 1 and the Point parameter to 0, 0, 0 Go to the Vectors tab and then enter a Scale Factor of 0.5 Click Apply Go to the Options tab and select User from the Range list Enter a range of 0 to 1.7 Click Apply Click Plot to Screen Display Figure T2.3-2 by selecting View > Axis > +Z

Version 4.02

Tutorial 2.3



Figure T2.3-2

Velocity vector plot

The vector plot is, again, quite similar to those shown in Figure T2.1-2 and Figure T2.2-2. However, as with the tetrahedral mesh, the recirculation zone appears slightly shortened. Now examine the pressure distribution: • • • • • • • •

Version 4.02

Click Go To Load Data In the Data tab, select Cell & Wall/Bound (Smooth) from the Data Type menu In the Scalar Data list, select item Pressure and then click Get Data Select Go To > Create Plots to display the Create Plots panel In the Section Clipped tab choose options Contour (filled) and Edge In the Options tab, enter a Range of -1.9 to 0.6 Click Apply Click Plot to Screen to display Figure T2.3-3

2-37

Tutorial 2.3



Figure T2.3-3

Pressure contour plot

There are a few differences between Figure T2.1-3, Figure T2.2-3 and Figure T2.3-3, but all three plots are very similar. Plot the vertex-based turbulence kinetic energy and dissipation rate: • • • • • • • • • • • •

2-38

In the Options tab select User from the Range list and enter values 0 to 0.2 Click Apply Click Go To Load Data Select item Turb. Kinetic Energy from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T2.3-4 Select item Dissipation Rate from the Scalar Data list Click Get Data Click Go To > Create Plots In the Options tab select User from the Range list and enter values 0 to 2 Click Apply In the main window, click Replot to display Figure T2.3-5

Version 4.02

Tutorial 2.3




Figure T2.3-4

Contours of turbulence kinetic energy

Figure T2.3-5

Contours of turbulence dissipation rate

Plot the y+ values at the wall boundaries to help verify the suitability of the mesh for the turbulence model employed: •

Version 4.02

Go to the Options tab in the Create Plots panel 2-39

Tutorial 2.3



• • • • •

Choose Auto Range and click Apply In the Load Data panel, select option Wall from the Data Type menu Turn Smooth Option Off Select item YPLUS from the Scalar Data list Click Get Data

Since wall data are stored in specially created shells at the wall surfaces (cell type no. 5), it is necessary to assemble a new cell set that contains only these shells: •

Type VIEW -0.5 0.5 -1.0

• • • • • • •

in the I/O window In the main window, deselect the ‘edge’ button Deselect the ‘mesh’ button Select a Hidden Surface plot Select Plot > Wall Plot Select C > New > Type and click anywhere on the upper wall boundary Select Post > Caverage > Cset Select Plot > Wall Plot to display Figure T2.3-6

Figure T2.3-6


The y+ values are roughly comparable to those shown for the hexahedral and tetrahedral meshes (Figure T2.1-6 and Figure T2.2-6, respectively). This is what we would expect because the thickness of the cell layer next to the wall is the same for all three meshes. To check whether the near-wall layer thickness in the turbulence model (see page 2-34) was given a reasonable value: 2-40

Version 4.02

Tutorial 2.3


Post-Processing Comparative Graphs

• • • • • • • • • •

In the Load Data panel, select Data Type Cell Turn the Smooth option Off Choose Two Layer from the Scalar Data list Click Get Data Choose Go To > Create Plots Change the plot type to a Section (Surface) plot In the Section Clipped tab select Contour (filled) and None Click Plot to Screen Select C > All Click Cell Plot and reset the view by clicking the small button at the bottom left of the orientation cube to display Figure T2.3-7

The plot shows that the two-layer model has been implemented correctly.

Figure T2.3-7

Comparative Graphs

Instead of plotting graphs showing just the current results, as in Tutorial 2.1 and Tutorial 2.2, we will now plot graphs comparing results from all three meshes with each other and with the experimental data. Files containing experimental data and also those obtained in Tutorial 2.1 and Tutorial 2.2 should have been copied into the working directory at the beginning of this tutorial. Begin by plotting a graph of U velocity at x = 330mm, z = 0 mm against the y-coordinate: •



Not all the graph specification options are available when a section plot is displayed. To avoid this, select a Hidden Surface plot using the drop-down menu in the main pro-STAR window. In the STAR GUIde window, select sub-folder Graphs followed by sub-folder Extract/Graph Data Open the Field Data panel 2-41

Tutorial 2.3



• • • • • • • • • • • • •

Click Graph Reset at the bottom of the panel and choose Yes Select option Line from the menu at the top of the Define Locations section Enter 300 as the Total number of data points Choose Line defined by End points Specify these end points to be 330, 0, 0 and 330, 300, 0 In the Data Type tab, choose Post 4 as the post register number in which to load field data and then click Go To Load Data In the Load Data panel, select option Cell from the Data Type menu Turn On the Smooth Option Select item Velocity Component U from the Scalar Data list Click Get Data Select Go To > Field Data. The Field Data panel display will confirm that the U velocity component (SU) is now loaded in post register no. 4 In the Graph Data section, choose to plot the Graph data against the Y-axis Type MEMORY MAXPRB 1000

• • • • • • • • • • • • • • • • • • •

in the I/O window to increase the number of sensors (data points) allowed Back on the Field Data panel, click Create Graph to see a default graph of the data Click Go To Customize Graph In the Customize Graphs panel, go to the Pairs tab Click Clear at the bottom of the Register Pairs list to remove the existing graph Choose SU (which should be Reg# 9) from the X-Axis Register list Choose Y LOCATION (which should be Reg# 4) from the Y-Axis Register list Click Add Register Pair and Apply Go to the Axis tab In the X-Axis Parameters sub-tab, change the Title to U - m/s Enter -0.4 and 1.5 in the Xmin, Xmax boxes, respectively Enter 0.1 in the Xmajor box and click Apply In the Y-Axis Parameters sub-tab, change the Title to Y - mm. Also, enter 0 and 300 in the Ymin, Ymax boxes, respectively Select Integer as the Numbers format Click Apply Go to the Options sub-tab In the Additional Graph Labels section, select label no. 1 in the scroll list and then enter U velocity profile at x = 330 mm in the text box underneath. Enter coordinates (3.5, 9.0) in the Sx and Sy boxes Click Apply In the main window, click Redraw to display the modified graph

Now import the experimental data and the data sets from the previous two tutorials and plot them all on the same graph: • •

2-42

Select Go To > External Data The File containing data from the hexahedral mesh is hex330.xy. Find it using the file manager Version 4.02

Tutorial 2.3



• • • • • • • •

Select xyxyxy from the Establish x-y pairs list Click Create Graph The File containing data from the tetrahedral mesh is tet330.xy. Find it using the file manager Select xyxyxy from the Establish x-y pairs list Click Create Graph Select File exp330.xy using the file manager Select xyxyxy from the Establish x-y pairs list Click Create Graph to display Figure T2.3-8

Figure T2.3-8

Graph comparing U velocity data at x = 330 mm

Files containing data at x = 30 mm, x =230 mm and x = 380 mm are also available and graphs of these are shown below. These graphs have been generated in the same way as Figure T2.3-8.

Version 4.02

2-43

Tutorial 2.3



2-44

Figure T2.3-9


Figure T2.3-10


Version 4.02

Tutorial 2.3



Figure T2.3-11


The results from the three meshes show broad agreement with the experimental data, although all of them also show discrepancies, primarily in the recirculation zone. In this region in particular, the hexahedral mesh is marginally more accurate than the other two. However, examination of the model size and number of iterations and time required to reach convergence (shown in Table 1) shows that the polyhedral mesh may be preferable. Table 1:Comparison of run data Mesh

No. of cells

Hexahedral Tetrahedral Polyhedral

67699 140141 60838

No. of Time (s)a iterations 179 169 95

412 644 277

a.Run time will vary with computer speed

The polyhedral mesh fills the problem geometry much more efficiently, allowing fewer cells to be used and run times to be reduced without significantly degrading the solution accuracy. Conversely, a polyhedral mesh with as many cells as the tetrahedral mesh in Tutorial 2.2 would be expected to produce a significant increase in accuracy with little increase in run time. Final Operations

Version 4.02



2-45

Tutorial 3 POROUS MEDIA FLOW The next three tutorials (Tutorial 3.1 to Tutorial 3.3) are designed to familiarise users with STAR-CD’s capabilities for modelling porous media flow. A polyhedral mesh, based on the geometry used in Meshing Tutorial 6 (see the Meshing Tutorials volume) is provided. The tutorials demonstrate how to model flow in highly porous (isotropic and orthotropic) or moderately porous media.

Figure T3.0-1

Version 4.02

Mesh geometry

3-1

Tutorial 3.1

FLOW IN AN ISOTROPIC, HIGHLY POROUS MEDIUM

Physical Problem Description Preliminaries

Tutorial 3.1


This tutorial aims to demonstrate how to: • • • •

Model flow through an isotropic, highly porous medium Produce vector and contour plots Compute sums and averages of field data Check the validity of the porous model

Physical Problem Description The tutorial models an isotropic porous subdomain of length 0.03 m in the centre of the catalyst geometry. The pressure drop per unit length is given by the equation ∆p ------ = – ( αv + β )v L where v is the superficial velocity through the medium and α, β are coefficients defining the porous resistance. Values for the resistance coefficients can be measured experimentally or derived using various empirical relationships, depending on the exact nature of the problem (see Chapter 8 of the Methodology volume). In this case α = 25 and β = 1500. These values are roughly what would be expected from a porous catalyst. Modelling Strategy The following steps are taken to set up the model: • • • •

In the cell table list, define a porosity index for the porous medium Define porous properties pertaining to that porosity index Select a cell range for the porous medium Modify the cell type of the selected cell range

Pre-Processing Preliminaries Create a sub-directory for this tutorial called tut3-1. Copy the coded files catalyst.cel, catalyst.vrt, catalyst.bnd and catalyst.inp supplied with the STAR-CD installation into it. • • • • • • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (cat_iso) in the Casename text box Click Continue Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog, change the File Name to catalyst.inp Click Apply Click Close

This will read default problem settings from file catalyst.inp as well as problem geometry and boundary location definitions from the remaining three files. 3-2

Version 4.02

Tutorial 3.1



• •

In the main window, select File > Model Title In the Title text box type: 3D FLOW THROUGH AN ISOTROPIC HIGHLY POROUS CATALYST

• Mesh Checking

Click Apply

Verify that the mesh data are correct by selecting all cells and vertices and plotting the mesh in ‘Hidden Surface’ mode: • • • • • •

In the main window, select C > All. The I/O window tells you that the mesh read in has 29,108 cells. Select V > All. The I/O window tells you that the mesh has 103,488 vertices. Select Hidden Surface as the cell plot type Select Plot > Up Axis > Z Set the viewpoint by selecting View > Isometric > -1,1,1 Click Cell Plot

The mesh geometry is shown in Figure T3.0-1 Material Properties

This part of the model building is conveniently handled through a series of panels under the Thermophysical Models and Properties folder. • • •

Go to the Thermophysical Models and Properties folder to display the available facilities Select sub-folder Liquids and Gases Open the Molecular Properties panel

In this tutorial, the fluid is air at standard pressure and temperature and its temperature, density and viscosity are assumed to be constant. These conditions are also the pro-STAR defaults, so the properties shown on the panel are acceptable. • • • • •

Open the Turbulence Models panel Click On to set up a turbulent flow Select the desired turbulence model, K-Epsilon/High Reynolds Number, from the Turbulence menu Click Apply to save your settings Open the Monitoring and Reference Data panel to check the cell whose flow variable values will be sent to the solution monitoring file (cat_iso.run). The cell number appears in the Monitoring cell number box and can be left at its default value of 1. The displayed Reference Data defaults for pressure and reference pressure cell location are also acceptable.

Next, define the porous subdomain. In the cell table list, define cells of type 2 as belonging to a porous medium (called POR1 and identified by colour 3 and porosity index 1): • • • • • • Version 4.02

In the main window, click the CTAB button Select cell no. 2 in the Cell Table Editor’s scroll list Select Fluid from the Cell Type menu Change the value in the Porosity Index box to 1 Type POR1 in the Name box Click Apply and then Close 3-3

Tutorial 3.1



Specify the resistance coefficients in the global Cartesian directions: • • • • • • •

Go to the STAR GUIde window and select folder Thermophysical Models and Properties Select sub-folder Porosity Open the Resistance and Porosity Factor panel Select option By local coordinate system in the Define X1,X2,X3 menu and type 1 in the Local Coord. System box Type 25 in the AlphaX1, AlphaX2 and AlphaX3 boxes Type 1500 in the BetaX1, BetaX2 and BetaX3 boxes Click Apply

Collect all cells that will take on porous properties into a set: • • • • • •

•

Select View > Axis > -X Select C > Unselect > Type... and click on any of the blue extrusion-layer cells Click Cell Plot Select C > New > Zone Carefully draw a box enclosing only the central block of cells, i.e. those within the catalyst ring If any cells outside the ring are accidentally selected, they may be removed from the cell set by selecting C > Unselect > Zone and drawing a box around them Click Cell Plot

Some of the blue extrusion-layer cells are also part of the porous subdomain. To include these three layers, you will need to ‘grow’ the cell set three times: • • • • • • • •

3-4

Select V > New > Cell Set Select C > New > Vertex Set (Face) Select V > New > Cell Set Select C > New > Vertex Set (Face) Select V > New > Cell Set Select C > New > Vertex Set (Face) Click Cell Plot to display Figure T3.1-1 Change the viewpoint by selecting View > Isometric > -1, 1, 1

Version 4.02

Tutorial 3.1



Figure T3.1-1

Catalyst ring

Assign the selected cells to the currently active cell type (no. 2) and plot: • • • •

In the main window, select Tools > Cell Tool In the Cell Table scroll list, highlight cell type number 2 and then choose Modify Type > Cell Set Click Replot. You will see that the colour of the chosen cells is now green (colour 3), confirming the change to porous cells. Close the Cell Tool

Finally, select the whole mesh and display it as shown in Figure T3.1-2 to confirm visually that the correct cells have become porous. • •

Version 4.02

In the main window, select C > All Click Cell Plot

3-5

Tutorial 3.1


Pre-Processing Boundary conditions

Figure T3.1-2

Boundary conditions

Mesh geometry displaying porous subdomain

Specify boundary conditions for the inlet and outlet boundary regions: • • • •

Select folder Define Boundary Conditions and then open the Define Boundary Regions panel Select region no. 1 (the inlet) in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions as shown below:

• • •

Click Apply Select region no. 2 (the outlet) in the scroll list The default settings are acceptable, so click Apply

Check visually that the boundary conditions are applied correctly: 3-6

Version 4.02

Tutorial 3.1



• • • Final Operations

In the main window, click Bound from the Cell Plot Display Options button group Select B > All Click Cell Plot

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • • • •

In the main pro-STAR panel, select File > Write Geometry File Set the Scale Factor to 0.1. This gives the catalyst a realistic maximum diameter of 10cm Click Apply. Ignore the I/O window warning regarding the scale factor Click Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis To perform the analysis interactively, proceed as follows: • • •

In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Leave all settings at their default values and click Start New Analysis

The analysis will then start automatically. The solution should satisfy the convergence criteria within the specified maximum number of iterations. Check file cat_iso.info for error messages during the run. There should be none. Post-Processing Preliminaries Read in the results of the analysis: • • •

Select folder Post-Processing Open the Load Data panel to display the File(s) tab Click Open Post File

You are now ready to start the post-processing session. Postprocessing

Load the velocity vector components and then plot the vectors: • • • • • •

Version 4.02

Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW to load all three velocity components In the Scalar Data list, check that the default setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel In the Section Clipped tab, select Vector from the Option menu and Edge from the Edge/Mesh menu 3-7

Tutorial 3.1


Post-Processing Post- processing

• • • • •

Change the Normal Vector to -1, 0, 0 Click Apply Click Plot to Screen Click off Bound in Cell Plot Display Options Select View > SNORMAL to display Figure T3.1-3

Figure T3.1-3

Velocity vector plot on the y-z plane

To establish the approximate mean velocity magnitude in the porous subdomain: • • • •

3-8

Open the Cell Tool and select Cell Type number 2 Click Set Active Type Close the Cell Tool Select C > New > Type(Current) and then click Cell Plot to display Figure T3.1-4

Version 4.02

Tutorial 3.1



Figure T3.1-4

Velocity vectors on the y-z plane in the porous region

Note that the mean velocity magnitude through the porous cells is approximately 3.2 m/s. Now inspect the pressure variation throughout the model: • • • • • • • •

Version 4.02

Select C > All Go back to the Load Data panel by clicking Go To Load Data In the Data tab, select option Cell & Wall/Bound (Smooth) from the Data Type menu In the Scalar Data list, select item Pressure and then click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select plot options Contour (filled) and Edge Click Plot to Screen Click Cell Plot to display Figure T3.1-5

3-9

Tutorial 3.1


Post-Processing Analysis of Results

Figure T3.1-5

Analysis of Results

Figure T3.1-5 shows that the largest pressure drop occurs across the porous cells. To see the value of this drop more clearly, collect all cells within the porous region (porosity index 1) into a set and plot pressure contours on the surface of the porous medium. • • • •

3-10

Cell-averaged filled contour plot of pressure

In the main window, select C > New > Porosity When the cursor appears on your screen, click any cell in the porous region. The I/O window message should indicate that 9,621 cells have been selected Select View > Isometric > -1,1,1 Click Cell Plot to display Figure T3.1-6

Version 4.02

Tutorial 3.1



Figure T3.1-6

Filled contour plot of pressure on the surface of the porous medium

Figure T3.1-6 shows that the pressure across the upstream interface of the porous medium is non-uniform, so an average needs to be calculated. To do this, it is necessary to collect all cells on each of the porous interfaces into a set: • • • • • • • • • • •

Version 4.02

Select V > New > Cell Set Surface Select Tools > Cell Tool In the Cell Tool, select Table# 11 from the list and click Set Active Type Select C > New > Type(Current) Select V > Subset > Cell Set Surface Select C > New > Vertex Set (Face) Click Cell Plot Select View > Axis > -X Turn off ‘edge’ and ‘mesh’ plotting to display Figure T3.1-7 Select C > Subset > Zone... Draw a box around the left-hand (upstream) group of cells

3-11

Tutorial 3.1



Figure T3.1-7

Vertex set on the upstream boundary of the porous medium

The pressure values at the fluid cells adjacent to the porous medium can be reasonably used to approximate the pressure values on the upstream surface of the porous medium, given that the pressure drop across this medium is much greater than that in the unresisted flow. In addition, cell values are more suitable than surface vertex values since the latter are averages of cell values on either side of the surface separating the porous from the non-porous subdomain, and may lead to a possible underestimate of the pressure drop. This point is illustrated in Figure T3.1-8.

3-12

Version 4.02

Tutorial 3.1



Porous subdomain

Pressure

Actual surface value Values at adjacent cells

Vertex value

y-coordinate

Figure T3.1-8

Diagram illustrating the reason for choosing cell-centred pressure values

Load the pressure values and their corresponding cell volumes into pro-STAR’s post registers: • • • • • • •

Select Post > Operate Select Function > Load Cell Data > Pressure Select Register 5 using Relative Values Click Apply Select Function > Load Cell Data > Volume Select Register 6 Click Apply

The average pressure value should be accurately volume-weighted. If the cell values were averaged without volume-weighting, the small near-wall cells would be over-represented and the pressure magnitude would thus be underestimated. To calculate the pressure-volume product for each cell: • Version 4.02

Select Function > Multi-Register > Multiply 3-13

Tutorial 3.1



• •

Select Register 4 = Register 5 * Register 6 Click Apply then Close

Sum the pressure-volume product on the upstream surface of the porous medium: •

In the I/O window, type *get prs1 rtot 4. A value of 1.505 should be displayed.

Sum the cell volumes on the upstream surface of the porous medium: •

In the I/O window, type *get vol1 rtot 6. A value of 0.822e-2 should be displayed.

The volume-weighted average pressure across the upstream surface is the first of these parameters divided by the second, i.e. 183.09 Pa. The pressure across the downstream surface of the porous medium is also non-uniform, though to a much lesser degree. The average pressure across the non-porous cells on this surface can be calculated similarly and was found to be 33.88 Pa. The average pressure drop is therefore 149.21 Pa compared to a theoretical pressure drop of 151.68 Pa. Since the theoretical value assumes a constant superficial velocity of 3.2 m/s throughout the porous medium, while the calculated velocity varies, the 1.6% discrepancy between the theoretical and calculated pressure drops is acceptable. The turbulence parameters can be inspected by plotting the relevant contours: • • • • • • • • • • • •

3-14

Select C > All Select View > SNORMAL Go back to the Load Data panel by clicking Go To Load Data Select Data Type Cell & Wall/Bound (Smooth) Select item Turb Kinetic Energy from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select options Contour (filled) and Edge Click Plot To Screen to display Figure T3.1-9 In the Load Data panel, select item Dissipation Rate from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T3.1-10

Version 4.02

Tutorial 3.1



Figure T3.1-9

Turbulence kinetic energy contour plot

Figure T3.1-10

Dissipation rate contour plot

Turbulence parameters are fixed in the porous medium by assuming a turbulence intensity of 10% and length scale of 0.01 m. These correspond to values of 0.154 m2/s2 and 0.989 m2/s3 for the turbulence kinetic energy and dissipation rate, respectively. Fixing the turbulence parameters within the porous subdomain causes Version 4.02

3-15

Tutorial 3.1



the flow downstream of it to exhibit very little turbulence. Note that such settings may be changed via the Turbulence Properties panel within the Thermophysical Models and Properties > Porosity sub-folder in the STAR GUIde window. Finally, confirm that STAR-CD’s porous model has been used correctly by normalising the resistance coefficients as follows (again assuming a superficial through-flow velocity of 3.2 m/s): αL ------- = 0.622 ρ βL -------- = 11.67 ρV The simplified momentum equation employed within the porous medium is only valid if the sum of the normalised parameters is >> 1. This condition is satisfied here and the total resistance term is one order of magnitude greater than the convection term. Therefore, the use of the porosity model is justified. Quit the pro-STAR session by choosing: •

3-16


Version 4.02

Tutorial 3.2

FLOW IN AN ORTHOTROPIC, HIGHLY POROUS MEDIUM


Tutorial 3.2



Model flow through an orthotropic, highly porous medium Produce vector and contour plots Compute sums and averages of field data Check the validity of the porous model

Physical Problem Description In this tutorial, the isotropic, highly porous medium specified in Tutorial 3.1 is re-defined as an orthotropic porous medium. To this end, resistance coefficients are set up so as to prevent flow along the x- and z-directions of the global Cartesian coordinate system (see Figure T3.2-1). The values of these coefficients in the y-direction are the same as in Tutorial 3.1, i.e. αy = 25 and βy = 1500 Modelling Strategy The modelling steps used in setting up this case are identical to those described in Tutorial 3.1, except that the porous medium now has orthotropic properties. Pre-Processing Preliminaries A number of preliminary file-copying operations are needed for proper operation of this tutorial, as follows: • • •

Create a sub-directory for the tutorial called tut3-2 and copy the model file generated in Tutorial 3.1 (i.e. cat_iso.mdl) into it Rename this file cat_ortho.mdl Since the solution obtained in Tutorial 3.1 will act as the starting point of the current analysis, it is also necessary to copy the solution file for that case (cat_iso.ccm) to the current directory

Start up the pro-STAR interface: • • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Accept the default case name (cat_ortho) displayed in the Casename text box Select the Resume existing .mdl file option Deselect the Append to .echo file option Click Continue

The above reads the data in file cat_ortho.mdl and sets up the model as it was at the end of Tutorial 3.1. • • Version 4.02

In the main window, select File > Model Title In the Title text box, change the title to: 3-17

Tutorial 3.2



3D FLOW THROUGH AN ORTHOTROPIC HIGHLY POROUS CATALYST •

Click Apply

Check the model geometry retrieved from file cat_ortho.mdl • • •

Select C > All In the main window, click Cell Plot Turn off the Bound option in Cell Plot Display Options group to display Figure T3.2-1

Figure T3.2-1

Material Properties

Enter appropriate resistance coefficients for the porous medium in the Cartesian coordinate system: • • • • • • • • •

3-18

Mesh Geometry

Go to the STAR GUIde window and select folder Thermophysical Models and Properties Select sub-folder Porosity Open the Resistance and Porosity Factor panel Select option By local coordinate system from the Define X1,X2,X3 menu Enter 1 in the Local Coord. System box (or use the Select button to help locate the required coordinate system number) Type 1.0E6 in the AlphaX1 and BetaX1 boxes Type 25 in the AlphaX2 box and 1500 in the BetaX2 box Type 1.0E6 in the AlphaX3 and BetaX3 boxes Click Apply Version 4.02

Tutorial 3.2


CFD Analysis Run Time Controls

Run Time Controls

Set restart options so that the analysis will restart from the solution file of Tutorial 3.1: • • • •

Final Operations

Select folder Analysis Preparation/Running and open the Analysis (Re)Start panel Select Standard Restart from the Restart File Option list Click the browser button next to the Restart File box, select file cat_iso.ccm from the browser dialog and then click OK Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • • •

In the main pro-STAR panel, select File > Write Geometry File Accept the default value, 0.1, shown in the Scale Factor box Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit


In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Leave all settings at their default values and click Restart Analysis

The analysis will then start automatically. The solution should converge within the specified maximum number of iterations. Check file cat_ortho.info for error messages during the run. Post-Processing Preliminaries Read in the results of the analysis: • Select folder Post-Processing • Open the Load Data panel to display the File(s) tab • Click Open Post File You are now ready to start the post-processing session Postprocessing

Load the velocity vector components and plot the vectors: • • • • •

Version 4.02

Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW to load all three velocity components In the Scalar Data list, check that the default setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel 3-19

Tutorial 3.2



• • • • •

In the Section Clipped tab, select Vector from the Option menu and Edge from the Edge/Mesh menu Check that the Normal setting is -1, 0, 0 Click Apply Click Plot to Screen Select View > SNORMAL to display Figure T3.2-2

Figure T3.2-2

Velocity vectors on the y-z plane

Initial comparison of Figure T3.2-2 with the equivalent plot for the isotropic porous medium, Figure T3.1-3, reveals few apparent differences between them. To examine any variations more closely, a velocity magnitude plot in the porous subdomain is necessary: • • •

3-20

Open the Cell Tool and select Cell Type number 2 Select C > New > Type(Current) and click Cell Plot to display Figure T3.2-3 Close the Cell Tool

Version 4.02

Tutorial 3.2



Figure T3.2-3

Velocity vectors on the y-z plane in the porous subdomain

The significant difference between Figure T3.2-3 and the equivalent plot for the isotropic porous medium, Figure T3.1-4, is that the orthotropic property prevents the bulk of the fluid flowing through the centre of the model from spreading outwards and slowing down, as it does in the isotropic case. Note that the mean velocity magnitude in the porous subdomain is approximately 3.2 m/s. Now inspect the cell-based pressure variation: • • • • • • • • •

Version 4.02

Select C > All Go back to the Load Data panel by clicking Go To Load Data Select Data Type Cell & Wall/Bound (Smooth) In the Scalar Data list, select item Pressure Click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select plot options Contour (filled) and Edge Click Plot to Screen Click Cell Plot to display Figure T3.2-4

3-21

Tutorial 3.2



Figure T3.2-4

Cell-averaged pressure plot

Before calculating the pressure drop across the catalyst, plot the cell-centred pressure in the porous subdomain: • • •

3-22

Select C > New > Porosity and click anywhere inside the porous subdomain Select View > Isometric > -1,1,1 Click Cell Plot to display Figure T3.2-5

Version 4.02

Tutorial 3.2



Figure T3.2-5

Cell-averaged pressure plot in the porous subdomain

The pressure across the surfaces of the porous medium is clearly non-uniform, so averages should be calculated. For the downstream surface: • • • • • • • • • • • • • • • • • • • • • • Version 4.02

Select V > New > Cell Set Surface Select Tools > Cell Tool In the Cell Tool, select Table# 11 from the list and click Set Active Type Select C > New > Type(Current) Select V > Subset > Cell Set Surface Select C > New > Vertex Set (Face) Click Cell Plot Select View > Axis > -X Turn off ‘edge’ and ‘mesh’ plotting Select C > Subset > Zone... Draw a box around the right-hand (downstream) group of cells Select Post > Operate Select Function > Load Cell Data > Pressure Select Register 5 using Relative Values Click Apply Select Function > Load Cell Data > Volume Select Register 6 Click Apply Select Function > Multi-Register > Multiply Select Register 4 = Register 5 * Register 6 Click Apply then Close In the I/O window type *get prs2 rtot 4. A value of 0.280 should be 3-23

Tutorial 3.2



•

displayed. In the I/O window type *get vol2 rtot 6. A value of 0.841e-2 should be displayed.

The volume-weighted average pressure across the downstream surface is the first of these parameters divided by the second, i.e. 33.29 Pa. The pressure across the upstream surface of the porous subdomain can be calculated similarly and found to be 182.07 Pa. Analysis of Results

The above figures give an average pressure drop of 148.78 Pa. This may be compared with the expected pressure drop of 151.68 Pa, based on an average cell velocity of 3.2 m/s. The user can verify these calculations. The turbulence parameters may be inspected by plotting the relevant contours: • • • • • • • • • • • • •

3-24

Select C > All Select View > SNORMAL Go back to the Load Data panel by clicking Go To Load Data Select Data Type Cell & Wall/Bound (Smooth) Select item Turb Kinetic Energy from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select options Contour (filled) and Edge Click Plot To Screen Click Cell Plot to display Figure T3.2-6 In the Load Data panel, select item Dissipation Rate from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T3.2-7

Version 4.02

Tutorial 3.2



Version 4.02

Figure T3.2-6

Contour plot of turbulence kinetic energy

Figure T3.2-7

Contour plot of dissipation rate

3-25

Tutorial 3.2



Turbulence parameters are fixed in the porous medium by assuming a turbulence intensity of 10% and length scale of 0.01 m. Consequently, the values for turbulence kinetic energy and its dissipation rate should be roughly 0.154 m2/s2 and 0.989 m2/s3, respectively, based on a velocity magnitude of 3.2 m/s. As in Tutorial 3.1, fixing the turbulence parameters in this way causes the flow downstream of the porous medium to exhibit very little turbulence. The normalised resistance coefficients have the same values as those in Tutorial 3.1. Therefore, the same conclusions about the validity of using the STAR-CD porous model can be drawn in this case. Quit the pro-STAR session by choosing: •

3-26


Version 4.02

Tutorial 3.3

FLOW IN A MEDIUM WITH ISOTROPIC FLOW RESISTANCE


Tutorial 3.3


This tutorial aims to demonstrate how to: • • •

Model flow in a moderately porous region with isotropic flow resistance Introduce momentum source terms via user coding Produce vector and contour plots

Physical Problem Description In this tutorial, the properties of the porous medium defined in Tutorial 3.1 are modified in order to demonstrate the implementation of a flow resistance mechanism (momentum sink) via user coding. The porous region is assumed to be moderately porous and to exhibit the same flow resistance in all directions. The resultant pressure drop is assumed to depend on the superficial velocity in exactly the same way as in the standard STAR-CD porous media model (see Chapter 8 of the Methodology volume). The user specifies values for the resistance coefficients, α and β, which in this example are: α = β = 300.0 As intended, the above values do not satisfy the criteria for highly porous media under the problem’s flow conditions. Specifically, for L = 0.03 m, ρ = 1.205 kg/m3, U = 3.2 m/s, the normalised resistance coefficients are equal to 7.469 and 2.334, respectively, indicating that the resistance term is of the same order of magnitude as the convection term in the momentum equations. This simulation thus requires a more rigorous treatment of momentum transport than the STAR-CD porosity model can provide. Modelling Strategy The following steps are required to set up flow with a momentum sink: • • • • •

Define a unique cell identifier for the sink region Select the cells in the sink region Assign these to the cell type defined above Employ user coding to calculate momentum sources Supply a user subroutine to calculate the flow resistance

Pre-Processing Preliminaries The following file-copying operations are needed for proper operation of this tutorial, as follows: • •

Create a sub-directory for the tutorial called tut3-3 and copy the model file generated in Tutorial 3.1 (i.e. cat_iso.mdl) into it Rename this file cat_res.mdl

Start up the pro-STAR interface: Version 4.02

3-27

Tutorial 3.3



• • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Accept the default case name (cat_res) displayed in the Casename text box Select the Resume existing .mdl file option Deselect the Append to .echo file option Click Continue

The above reads the data in file cat_res.mdl and sets up the model as it was at the end of Tutorial 3.1. • •

In the main window, select File > Model Title In the Title text box, change the title to: 3D FLOW THROUGH A CATALYST WITH ISOTROPIC FLOW RESISTANCE

•

Click Apply

Perform a visual check of the mesh geometry retrieved: • • •

Select C > All In the main window, click Cell Plot Click off the Bound button in the Cell Plot Display Options group to display Figure T3.3-1

Figure T3.3-1

Material Properties

Most properties used in Tutorial 3.1 are acceptable for this tutorial. The one item requiring adjustment is a redefinition of the porous region so that it does not use the previously set parameters: •

3-28

Mesh geometry

In the main window, click the CTAB button Version 4.02

Tutorial 3.3


User Subroutine Run Time Controls

• • • •

Select cell index no. 2 in the Cell Table Editor’s scroll list Change the Porosity Index back to 0 Type POR2 in the Name box Click Apply and then Close

Signal to pro-STAR that momentum source terms will be supplied via user subroutine SORMOM and place a dummy version of this subroutine in subdirectory ufile. • • • • • • • Run Time Controls

In the main window, choose File > System Command Type ufiles in the text box, click Apply and then Close Open the STAR GUIde window and select folder Thermophysical Models and Properties Open sub-folder Sources Select Source Terms to open the corresponding panel and then select the Momentum tab Click On to activate momentum source calculations and then choose User Coding from the Define Source menu Click Apply and Define User Coding to write the default (dummy) version of subroutine SORMOM in sub-directory ufile, ready for editing

Check the status of the run time control parameters. • • •

Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 1e-4 for the maximum residual tolerance Click Apply

The boundary conditions remain the same so the pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the “CFD Analysis” section. • • • • • •

In the main pro-STAR panel, select File > Write Geometry File Accept the default value, 0.1, shown in the Scale Factor box Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

User Subroutine To introduce the coding needed for the extra source terms, use pro-STAR’s built-in editor to edit subroutine SORMOM (in file sormom.f within sub-directory ufile) as follows: • • • • Version 4.02

In the main pro-STAR panel, select File > Edit File In the pro-STAR Editor dialog, click File > Open In the File Selection dialog displayed, enter sub-directory ufile and select file sormom.f Click OK 3-29

Tutorial 3.3


User Subroutine Final Operations

• • •

Edit the contents of the subroutine by adding an extra 11 lines of code after the explanatory section, as shown below Click File > Save Click File > Quit to exit from the editor

C************************************************************************* SUBROUTINE SORMOM(S1U,S2U,S1V,S2V,S1W,S2W,POROS) C Source-term for momentum C************************************************************************* C--------------------------------------------------------------------------* C STAR-CD VERSION 4.02 C--------------------------------------------------------------------------* INCLUDE ’comdb.inc’ COMMON/USR001/INTFLG(100) INCLUDE ’usrdat.inc’ DIMENSION SCALAR(50) EQUIVALENCE( UDAT12(001), ICTID ) EQUIVALENCE( UDAT03(001), CON ) EQUIVALENCE( UDAT03(006), G1 ) EQUIVALENCE( UDAT03(007), G2 ) EQUIVALENCE( UDAT03(008), G3 ) EQUIVALENCE( UDAT03(019), VOLP ) EQUIVALENCE( UDAT04(001), CP ) EQUIVALENCE( UDAT04(002), DEN ) EQUIVALENCE( UDAT04(003), ED ) EQUIVALENCE( UDAT04(005), PR ) EQUIVALENCE( UDAT04(008), TE ) EQUIVALENCE( UDAT04(009), SCALAR(01) ) EQUIVALENCE( UDAT04(059), U ) EQUIVALENCE( UDAT04(060), V ) EQUIVALENCE( UDAT04(061), W ) EQUIVALENCE( UDAT04(062), VISM ) EQUIVALENCE( UDAT04(063), VIST ) EQUIVALENCE( UDAT04(007), T ) EQUIVALENCE( UDAT04(067), X ) EQUIVALENCE( UDAT04(068), Y ) EQUIVALENCE( UDAT04(069), Z ) C------------------------------------------------------------------------C This subroutine enables the user to specify the momentum source C term (per unit volume) in linearised form: C C Source in x direction = S1U-S2U*U, (N/m3) C Source in y direction = S1V-S2V*V, (N/m3) C Source in z direction = S1W-S2W*W, (N/m3) C C in an arbitray manner. C C ** Parameters to be returned to STAR: S1U,S2U,S1V,S2V,S1W,S2W, C POROS C C------------------------------------------------------------------------if (ictid.eq.2) then gvmag = sqrt(u**2+v**2+w**2) 3-30

Version 4.02

Tutorial 3.3



galpha = 300.0 gbeta = 300.0 s1u = 0.0 s1v = 0.0 s1w = 0.0 s2u = galpha*gvmag + gbeta s2v = galpha*gvmag + gbeta s2w = galpha*gvmag + gbeta endif C-------------------------------------------------------------------------C RETURN END


In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Leave all settings at their default values and click Start New Analysis

The analysis will then start automatically. The solution should converge within the specified maximum number of iterations. Check file cat_res.run for error messages. There should be none. Post-Processing Preliminaries Read in the results of the analysis: • • •


You are now ready to start the post-processing session Postprocessing

Load the velocity vector components and plot the vectors: • • • • • • • • •

Version 4.02

Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW to load all three velocity components In the Scalar Data list, check that the default setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel In the Section Clipped tab, select Vector from the Option menu and Edge from the Edge/Mesh menu Check that the Normal setting is -1,0,0 and then click Apply Click Plot to Screen Select View > SNORMAL to display Figure T3.3-2

3-31

Tutorial 3.3



Figure T3.3-2


To examine the velocity vectors in the region where the momentum sink is applied: • • •

Open the Cell Tool and select Cell Type number 2 Select C > New > Type(Current) and click Cell Plot to show Figure T3.3-3 Close the Cell Tool

Figure T3.3-3 3-32

Velocity vector plot in the porous region Version 4.02

Tutorial 3.3


Post-Processing Results analysis

Inspect the pressure variation throughout the model: • • • • • • • •

Go back to the Load Data panel by clicking Go To Load Data Select option Cell & Wall/Bound (Smooth) from the Data Type menu In the Scalar Data list, select item Pressure Click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select options Contour (filled) and Edge Click Plot to Screen Select C > All and click Cell Plot to display Figure T3.3-4

Figure T3.3-4

Results analysis

The pressure drop in the sink region is of comparable magnitude to the pressure variation elsewhere. To calculate the approximate total pressure drop across the porous block, select cells of type 2 and plot cell-centred (non-averaged) pressure contours: • • •

Version 4.02

Cell-averaged pressure contours on the model surface

In the main window, select C > New > Type(Current) Choose View > Isometric > -1,1,1 Click Cell Plot to display Figure T3.3-5

3-33

Tutorial 3.3



Figure T3.3-5

Cell-averaged pressure contours on the surface of the porous region

The average pressure values on the two surfaces can be calculated as in Tutorial 3.1 and Tutorial 3.2. The pressure variation across the porous medium is 121.34 Pa. To inspect the turbulence parameters: • • • • • • • • • • • • •

Select C > All Select View > SNORMAL Go back to the Load Data panel by clicking Go To Load Data Select Data Type Cell & Wall/Bound (Smooth) Select item Turb Kinetic Energy from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select options Contour (filled) and Edge Click Plot To Screen Click Cell Plot to display Figure T3.3-6 In the Load Data panel, select item Dissipation Rate from the Scalar Data list Click Get Data In the main window, click Replot to display Figure T3.3-7

Using the full momentum equations does not fix the turbulence parameters in the porous region, as was the case when the built-in porosity model was used. Therefore, the turbulence kinetic energy and dissipation rate in the porous region are calculated as in the rest of the flow field, leading to increased turbulence downstream of the porous region. Depending on the nature of the problem, this can be a limitation of using the full momentum equations with an added source term. In some problems, further user coding to fix the turbulence parameters may also be necessary. 3-34

Version 4.02

Tutorial 3.3



Figure T3.3-6

Turbulence kinetic energy contour plot

Figure T3.3-7

Dissipation rate contour plot

Quit the pro-STAR session •

Version 4.02


3-35

Tutorial 4 FREE-SURFACE AND CAVITATION The next three tutorials demonstrate how to set up and perform simulations of free-surface and cavitating flows. All three tutorials use the same ready-to-use polyhedral mesh, supplied in file gridfs.ccm and displayed in Figure T4.0-1. The mesh consists of a single layer of polygonal prisms, suitable for performing a planar, two-dimensional flow analysis. Examples of mesh generation are provided in the Meshing Tutorials volume.

Figure T4.0-1

Version 4.02

Geometry plot showing the mesh, distribution of cell types and generic boundary region names

4-1

Tutorial 4.1

GRAVITY-DRIVEN FLOW WITH A FREE SURFACE


Tutorial 4.1



Perform an unsteady flow simulation using the transient SIMPLE algorithm Activate STAR-CD’s interface-capturing method for free-surface flows Post-process the simulation results Create animations using a neutral plot file together with pro-STAR’s Animation utility

Physical Problem Description The tutorial simulates gravity-driven fluid flow through a channel connecting two chambers. The one on the left is represented by the green-coloured cells shown in Figure T4.0-1 and the one on the right by the red-coloured cells. Given that this is a 2D simulation, the front and back planes of Figure T4.0-1 are symmetry planes. All other boundaries are solid walls except for the horizontal top surfaces where a constant (atmospheric) static pressure is applied. Initially, the left chamber is filled with liquid and the right one is filled with air. Under the action of gravity, liquid flows into the right chamber under assumed turbulent conditions. At the same time, liquid also flows in through the top left boundary so as to maintain the fluid level constant. After some time, the free surface on the right chamber settles at the level of the top boundary in the left chamber. Modelling Strategy During mesh generation, the cells on the right vessel were assigned to cell type 1 and those on the left to cell type 2. This was done in order to facilitate definition of the initial liquid and air distribution within the model. Note that in some cases (e.g. when inlet boundary conditions are present), one may start with the whole solution domain filled by a single fluid phase. However, if pressure boundary conditions and gravity are used to drive the flow, both phases need to be present within the domain. Cell typing then offers a convenient way of assigning “heavy” and “light” fluid characteristics to cells and thus make for a simple initialization process. Pre-Processing Preliminaries Create a directory for the tutorial called tut4-1 and copy file gridfs.ccm supplied with the STAR-CD installation into it. In this directory: • • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (gravfs) in the Casename text box Click Continue

Define a transient simulation of a free surface flow and give the case a title: • • • 4-2

Open the Select Analysis Features panel in STAR GUIde Select Transient in the Time Domain section Select On in the Free Surface section Version 4.02

Tutorial 4.1


Pre-Processing Mesh Import & Checking

• • •

Click Apply In the main window, select File > Model Title In the Title text box type: GRAVITY-DRIVEN FREE SURFACE FLOW

• Mesh Import & Checking

Click Apply

To import and display the mesh: • • • • • • • • •

Select the Create and Import Grids folder in STAR GUIde Open the Import Grids panel Select the CCM button from the Format list Enter gridfs.ccm as the CCM File name Check that the State Name entry is set to default Click Import Grid In the main window, select C > All to put all cells into the current cell set Check that the Geometry Plot mode and Hidden Surface plot type are selected Click Cell Plot to display the grid shown in Figure T4.0-1

The generic names of all boundary regions are indicated in Figure T4.0-1. Their locations can be displayed on the grid plot via the following steps: • • • • Material Properties

Select the Locate Boundaries folder in STAR GUIde Open the Create Boundaries panel Select each region shown on the list in turn (except no. 0) and then click Plot Region to display its location Turn off the Bound Cell Plot Display Option

To examine the free-surface flow modelling options: • • • •

Select the Free Surface folder in Star GUIde Open the Controls panel to inspect the default settings and confirm that they are suitable for the current problem Open the Molecular Properties panel Note that, by default, the Light Fluid is AIR and the Heavy Fluid is H2O. Alternative fluids can be selected from the database, if required, but the defaults are suitable for this case.

To specify the magnitude and direction of the gravity force: • • • • •

Select the Thermophysical Models and Properties folder in STAR GUIde Open the Gravity panel Change the Acceleration due to gravity to 9.81 m/s2 Change the gravity Direction to (0, -1, 0) in coordinate system 1 Click Apply

The remaining material properties are specified using panels in the Liquids and Gases folder. These panels feature a Material # slider, enabling you to specify different properties for each fluid material used. For the heavy and light fluids defined in free surface problems, this functionality is not relevant since those properties specified for the light fluid (Material # 1) are also applied automatically Version 4.02

4-3

Tutorial 4.1


Pre-Processing Initialization

to the heavy fluid (Material # 2). Turn on turbulence modelling and select an appropriate model: • • • • •

Select the Liquids and Gases folder and open the Turbulence Models panel Check that the slider at the bottom of the panel is set to Material # 1 Turn On turbulence modelling Select the k-Epsilon/High Reynolds Number model from the list Click Apply

To select monitoring and pressure reference locations: • • •

• •

•

Open the Monitoring and Reference Data panel Click the mouse symbol in the Monitoring cell number section to select the monitoring location In the main pro-STAR window, select a cell just to the right of the narrow section. This location is chosen because large variations in field variable values are expected here. In the Reference Data section, click the mouse symbol to select the reference pressure cell number In the main pro-STAR window, click on a cell at the top right-hand corner. This location is chosen because this corner will always contain air and so the pressure variations are likely to be minimal. Click Apply

To turn on buoyancy: • • • Initialization

Initially, the left-hand vessel contains only water and the right-hand vessel only air. This initial distribution is specified by associating the two fluids with different cell types: • • • • • •

Boundary Conditions

Open the Buoyancy panel Turn On buoyancy The default values for Datum Location and Datum Density are suitable so click Apply

Click the CTAB button in the main pro-STAR window to open the Cell Table Editor Select Table# 1 in the list, i.e. the cell type of the red-coloured cells Check that the Initial Free Surface Material setting is Light Select Table# 2 in the list, i.e. the cell type of the green-coloured cells Select option Heavy from the Initial Free Surface Material menu Click Apply and then Close

First, define the wall boundary conditions: • • • •

Select the Define Boundary Conditions folder and open the Define Boundary Regions panel In the region list, select Reg#1 named Wall Change the Region Type to Wall and click Apply Repeat this operation for the regions named Left, Right, and Bottom

Next, define the pressure boundary conditions:

4-4

Version 4.02

Tutorial 4.1


Pre-Processing Scalar Boundaries

• • • • • • • Scalar Boundaries

All free surface analyses involve a scalar called VOF, representing the volume fraction of the heavy fluid. The values of this scalar at pressure boundaries must be specified as follows: • • •

• • •

• Analysis Controls

Select Reg#5 named TopRight Change the Region Type to Pressure Change the pressure Option to Static and set the Pressure value to 0 Pa Check that the Envir Press and Mean options are turned Off. These options are not applicable to free-surface flows. Click Apply Repeat this process for Reg#7 named TopLeft No action is needed for the regions named Back and Front as these are already defined as symmetry planes in the supplied mesh geometry file

Open the Scalar Boundaries panel and check that the currently selected Scalar is VOF Select Boundary Region 5 from the Boundary Region list Check that the Boundary Condition is set to Boundary Mass Fraction and that the Mass Fraction value is 0. This in effect enforces the condition that only air may enter the domain through this boundary. Note, however, that either fluid may leave through the boundary. Click Apply Select Boundary Region 7 from the Boundary Region list Check that the Boundary Condition is set to Boundary Mass Fraction and then set the Mass Fraction value to 1. This in effect enforces the condition that only water may enter the domain through this boundary. Click Apply

The transient SIMPLE solution algorithm must be used for free surface problems. This tutorial will also use the AMG solver, the recommended pressure-correction equation solver for all free surface problems. To specify these settings: • • • • •

Select the Analysis Controls folder Select the Solution Controls sub-folder and open the Solution Method panel In the Solution Setup section, change the Max. No. of Outer Iterations to 10 Change the Method menu setting to AMG and check that the Temporal Discretization option is set as Euler Implicit Click Apply

This tutorial involves a two-dimensional analysis so it is not necessary to solve for the momentum component in the z-direction. To turn this off and specify appropriate settings for the solver parameters and differencing schemes: • • • • •

Version 4.02

Select the Equation Behavior sub-folder and open the Primary Variables panel Under the Equation Status tab, deselect the W-Mom button Click Apply Under the Solver Parameters tab, set the Relaxation Factor for the momentum and turbulence equations to 0.8 Set the Relaxation Factor for the pressure equation to 0.4 (higher than the default because we are dealing with an unsteady flow and small time steps) 4-5

Tutorial 4.1


Pre-Processing Run Time Controls

•

• • • • • • •

In transient SIMPLE calculations, it is unnecessary to solve the pressure equation as accurately as in PISO calculations because the outer iterations within each time step control convergence. Therefore, set the Residual Tolerance for all variables to 0.01. Set the Number of Sweeps to 100 for all variables Click Apply Under the Differencing Schemes tab, check that the UD scheme is selected for all variables Click Apply Open the Additional Scalars panel Select Scalar 1 (VOF) and change the Under-Relaxation Factor to 0.8 Leave all other settings at their default values and click Apply

Specify what data should be written to the results (.ccm) file and the transient post data (.pstt) file: • • • • • • • Run Time Controls

Select the Output Controls folder and open the Analysis Output panel Under the Post tab, check that option Write final solution (restart) file is selected with an Output Frequency of 100 time steps Click Apply Under the Transient tab, choose to Write data every 0.25 seconds Select Turbulent Kinetic Energy as an output variable from the list and click Post Repeat for the VOF variable Click Apply

To specify the run time and time step size: • • • • • •

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel In the Run Time section, instruct the analysis to Run for 5 seconds Click Apply In the Time Step Option section, specify the Time Step for Period as 0.005 seconds. This means that the run will continue for 1,000 time steps. Click Set Period

Although you can run the simulation interactively from STAR GUIde, it is more common to run lengthy transient simulations from the command line. To write out the problem and geometry files and save the model file: • • • • • •

In the main pro-STAR window, select File > Write Geometry File In the Geometry File Write dialog, check that 1.0 is entered as the Geometry Scale Factor Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Save Model

You can stay within the current pro-STAR session by either moving pro-STAR into the background or by opening another terminal window to start up the STAR-CD solver. 4-6

Version 4.02

Tutorial 4.1



CFD Analysis Check that you are in the current working directory and then start the simulation by typing: star at the command line. The run should only take a few minutes. The screen output will show that, for some time steps, the residuals fail to converge to the specified tolerance within the specified maximum number of outer iterations. However, the monitored values do converge, so the maximum number of outer iterations need not be increased for this case. Post-Processing Preliminaries Start the post-processing session by opening the transient post data file: • • • • • •

In STAR-GUIde, select the Post-Processing folder and then open the Load Data panel Under the File(s) tab, select Transient as the Analysis option Select the first empty position, 1, in the Transient Post File(s) list Click Add File to List Select file gravfs.pstt from the Transient Post File(s) list Click Open Transient Post File

The following steps describe how to create static plots of flow variables at specified times and also how to create an animation from a sequence of static plots that show how the flow varies over time. Basic Plots

The first plot will show how the water front moves through the connecting channel into the right vessel, and how the free surface deforms during this process. The plot superimposes velocity vectors on a contour plot of the VOF scalar variable, the latter showing the distribution of air and water in the solution domain: • • • • • • • •

Version 4.02

Under the File(s) tab of the Load Data panel, select the first time step from the Select Time Step list and click Store Iter/Time to load the data. Under the Data tab, select Data Type Cell & Wall/Bound (Smooth) Select Velocity Components UV (2D vectors) from the Vector Data list Select VOF from the Scalar Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, use the Select Plot window’s slider to display the last available plot type (for edges, contours and vectors) and then select it Click Plot to Screen to display VOF contours and velocity vectors simultaneously, as computed after 50 time steps. This plot is shown in Figure T4.1-1

4-7

Tutorial 4.1



Figure T4.1-1

Volume fraction and velocity vectors after 50 time steps (0.25 s)

In some situations, usually when the mesh density varies significantly within the domain, it may be useful to use a presentation grid. This prevents overcrowding of velocity vectors in regions where the mesh is very fine. A description of how to do this is given in Tutorial 1.1. Figure T4.1-1 shows water flowing into the domain through the left pressure boundary (TopLeft) and moving towards the right chamber, displacing air through the right pressure boundary (TopRight) as it progresses. This is expected and, since the results look plausible, you may continue plotting contours of VOF alone, or in combination with vectors, or vectors alone for subsequent time steps. You may also plot other quantities such as pressure or turbulent kinetic energy, since these were also stored in the transient post data file. To do this, repeat the steps listed above changing the time step selected in the File(s) tab and the variables selected in the Data tab as desired. Pressure contours after 100, 600, and 1000 time steps are shown in Figure T4.1-2. This type of plot was created by selecting options Contour (filled) and Edge on the 3-D Surface tab.

4-8

Version 4.02

Tutorial 4.1


Post-Processing Animations

Figure T4.1-2

Pressure contours after 100 (top), 600 (middle) and 1000 (bottom) time steps

Note how, over time, the pressure profile becomes increasingly stratified. If the run duration is sufficiently extended, an equilibrium point will be reached at which the fluids become stationary and the pressure contours appear horizontal and evenly spaced. Animations

pro-STAR loops can be used to produce on-screen animations, as described in Tutorial 8.2 and Tutorial 12.3. However, animations can also be produced by writing data to a neutral plot file and using the Animation module to replay them. The advantage of this method is primarily in improved presentation, as an animation replayed from a neutral plot file will usually run faster and more smoothly than one created directly on screen. The animation created here uses contours of the VOF scalar variable, which must first be displayed as static contour plots: •

Version 4.02

Under the File(s) tab of the Load Data panel, select the first time step in the Select Time Step list 4-9

Tutorial 4.1



• • • •

Click Store Iter/Time Under the Data tab, select VOF from the Scalar Data list Click Get Data Click Replot in the main pro-STAR window to display a plot similar to Figure T4.1-1 but without the vectors. If such a plot does not appear, check that Contour Plot mode and Hidden Surface plot type are selected.

The Animation module is now used to set up, write and play back an animation sequence showing how the VOF scalar distribution changes during the analysis: • • • •

• • • • • • • •

In the main pro-STAR window, select Modules > Animation In the Animation module, change the Number of Frames in Sequence to 20 Select Edit Frame Definitions.. > First Frame... In the Animation Graphics Parameter Block dialog, select Copy > Current Plot. This makes the plotting options for the first animation frame the same as those of the current plot. Change the Time to 0.25 Click Apply Select the End of Animation Sequence radio button Select Copy > First Frame Change the Time to 5.0 Click Apply and then Close In the Animation module, click Edit Sequence Parameters Enter the following commands in the first two lines of the Post-Animation Sequence Commands box: STORE NEXT GETV CONC 1

• • • •

Change the Command For Initial Plot to Replot Click Close Click Record to store the animation into the neutral plot file Once the data have been written, click Play to view the result

The animation shows the free surface movement for the first 5 seconds. It will clearly take significantly longer for equilibrium to be reached. You may, if you wish, run the analysis for a longer period of time by: • • •

Increasing the Run Time specified in the Set Run Time Controls panel Writing a new problem file Running STAR again

The tutorial is now complete. To quit pro-STAR: •

4-10

Select File > Quit > Quit, Nosave

Version 4.02

Tutorial 4.2

FORCED FREE-SURFACE FLOW WITH CAPILLARY EFFECTS

Physical Problem Description Mesh Import & Checking

Tutorial 4.2


This tutorial aims to demonstrate: • •

How to simulate free-surface flow in which capillary effects are important The appearance of parasitic currents under certain conditions in such analyses

Physical Problem Description This tutorial simulates forced flow of liquid glycerine through a nozzle into an air-filled chamber at atmospheric pressure. The mesh used is the same as that of Tutorial 4.1 except that, in this instance, the problem’s physical dimensions are scaled down by a factor of 1,000. This gives a nozzle width of about 1 mm. The boundary region labelled “Left” in Figure T4.0-1 is now an inlet with fluid velocity of 1 mm/s and the boundary region labelled “Right” is at atmospheric pressure. The boundary regions labelled “Bottom”, “Front” and “Back” are symmetry planes, and all other regions are solid walls. Initially, the chamber behind the nozzle (cell type 2, coloured green in Figure T4.0-1) is filled with liquid and the remainder of the solution domain is filled with air. For the given geometry and inlet velocity, the flow can be assumed to be laminar. Gravity acts in the positive x-direction and so helps to drive the fluid flow through the nozzle. The shape of the free-surface that develops in the chamber downstream of the nozzle depends upon the contact angle between liquid and wall. Pre-Processing Create a directory for the tutorial called tut4-2 and copy file gridfs.ccm supplied with the STAR-CD installation into it. In this directory: • • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (forcfs) in the Casename text box Click Continue

Define a transient simulation of a free surface flow and give the case a title: • • • • • •

Open the Select Analysis Features panel in STAR GUIde Select Transient in the Time Domain section Select On in the Free Surface section Click Apply In the main window, select File > Model Title In the Title text box type: FORCED FREE-SURFACE FLOW WITH CAPILLARY EFFECTS


Version 4.02

Click Apply

To import and display the mesh: • •

Select the Create and Import Grids folder in STAR GUIde Open the Import Grids panel 4-11

Tutorial 4.2



• • • • • • • Material Properties

Select the CCM button from the Format list Enter gridfs.ccm as the CCM File name Check that the State Name entry is set to default Click Import Grid In the main window, select C > All to put all cells into the current cell set Check that the Geometry Plot mode and Hidden Surface plot type are selected Click Cell Plot to display the grid shown in Figure T4.0-1

Examine the free-surface flow modelling options and material property settings: • • • • • • • • • • • • •

Select the Free Surface folder in STAR GUIde Open the Controls panel Turn On Surface Tension Click Apply Open the Molecular Properties panel Select the Heavy Fluid tab Choose Select material from database from the drop-down menu at the top of the panel Select GLYCERINE(L) from the list that appears Click Select material Enter 45 for the Contact Angle at Wall Click Apply Select the Light Fluid tab The default fluid, AIR, is suitable for this case so click Apply

To select other physical models and initialize the flow variables: • • • • • •

Select the Thermophysical Models and Properties folder and open the Gravity panel Change the Acceleration value to 9.81 m/s2 Change the Direction of Gravity Force to (1, 0, 0) in coordinate system 1 Click Apply Select the Liquids and Gases folder and open the Turbulence Models panel Check that turbulence is switched Off so that the flow is treated as laminar


• •

•

4-12

Open the Monitoring and Reference Data panel Click the mouse symbol in the Monitoring cell number section to select the monitoring location In the main pro-STAR window, select a cell just to the right of the narrow section. This location is chosen because large variations in field variable values are expected here. In the Reference Data section, click the mouse symbol to select the reference pressure cell number In the main pro-STAR window, click on a cell at the top right-hand corner. This location is chosen because this corner will always contain air and so the pressure variations are likely to be minimal. Click Apply

Version 4.02

Tutorial 4.2



To turn on buoyancy: • • • Initialization

Initially, the left-hand vessel contains only glycerine and the right-hand vessel only air. This initial distribution is specified by associating the two fluids with different cell types: • • • • • •

Boundary Conditions

Open the Buoyancy panel Turn On buoyancy The default values for Datum Location and Datum Density are suitable so click Apply


To define boundary conditions for this simulation: • • • • • • • • • • • •

Select the Define Boundary Conditions folder and open the Define Boundary Regions panel In the region list, select Reg#1 named Wall Change the Region Type to Wall and click Apply Repeat this operation for the regions named TopLeft and TopRight Select Reg# 3, named Right, from the list Change the Region Type to Pressure Change the pressure Option to Static Click Apply Select Reg# 2, named Left Change the Region Type to Inlet Change the U velocity to 0.001 m/s Click Apply

No action is needed for the regions named “Back”, “Front” and “Bottom” as these are already defined as symmetry planes in the supplied mesh geometry file. Scalar boundary conditions must also be defined such that only glycerine enters through the inlet boundary and, in the case of backflow, only air enters through the pressure boundary: • • • • • • Analysis Controls Version 4.02

Open the Scalar Boundaries panel and check that the currently selected Scalar is VOF Select Boundary Region 2, Inlet from the Boundary Region list Check that the Boundary Condition is set to Boundary Mass Fraction Change the Mass Fraction value to 1 Click Apply The Mass Fraction for Boundary Region 3, Pressure is set to 0 by default so no change is required

The transient SIMPLE solution algorithm must be used for free surface problems. This tutorial will also use the AMG solver, the recommended pressure-correction 4-13

Tutorial 4.2



equation solver for all free surface problems. To specify these settings: • • • • •


This tutorial involves a two-dimensional analysis so it is not necessary to solve for the momentum component in the z-direction. To turn this off and specify appropriate settings for the solver parameters and differencing schemes: • • • • • •

• • • • • • •

Select the Equation Behavior sub-folder and open the Primary Variables panel Under the Equation Status tab, deselect the W-Mom button Click Apply Under the Solver Parameters tab, set the Relaxation Factor for the momentum equations to 0.8 Set the Relaxation Factor for the pressure equation to 0.4 (higher than the default because we are dealing with an unsteady flow and small time steps) In transient SIMPLE calculations, it is not necessary to solve the pressure equation as accurately as in PISO calculations because the outer iterations within each time step control convergence. Therefore, set the Residual Tolerance for all variables to 0.01. Set the Number of Sweeps to 100 for all variables Click Apply Under the Differencing Schemes tab, check that the UD scheme is selected for all variables Click Apply Open the Additional Scalars panel Select Scalar 1 (VOF) and change the Under-Relaxation Factor to 0.8 Leave all other settings at their default values and click Apply

Specify what data should be written to the results (.ccm) file and the transient post data (.pstt) file: • • • • • • Run Time Controls

4-14

Select the Output Controls folder and open the Analysis Output panel Under the Post tab, check that the analysis is set to Write final solution (restart) file with an Output Frequency of 100 time steps Click Apply Under the Transient tab, choose to Write data every 0.1 seconds Select VOF as an output variable from the list and click Post Click Apply

To specify the run time and time step size: • • • • •

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel In the Run Time section, instruct the analysis to Run for 2 seconds Click Apply In the Time Step Option section, change the Time Step for Period to 0.001 Version 4.02

Tutorial 4.2



•

seconds. This means that the run will continue for 2,000 time steps Click Set Period


In the main pro-STAR window, select File > Write Geometry File In the Geometry File Write dialog, change the Geometry Scale Factor to 0.001 to convert the model units to millimetres Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Save Model

You can stay within the current pro-STAR session by either moving pro-STAR into the background or by opening another terminal window to start up the STAR-CD solver. CFD Analysis Check that you are in the current working directory and then start the simulation by typing: star at the command line. The analysis should only take a few minutes. The output on the screen will show that the outer iterations are converging to the specified tolerance for each time step. Post-Processing Preliminaries Start the post-processing session by opening the transient post data file: • • • • • •

In STAR-GUIde, select the Post-Processing folder and then open the Load Data panel Under the File(s) tab, select Transient as the Analysis option Select the empty position, 1, in the Transient Post File(s) list Click Add File to List Select file forcfs.pstt from the Transient Post File(s) list Click Open Transient Post File

The remainder of this tutorial demonstrates how to create static plots of flow variables at specified times. Animated plots are not be produced here as the methods for creating them are described in detail in other tutorials, namely Tutorial 4.1, Tutorial 8.2 and Tutorial 12.3. Basic Plots

First, plot the VOF distribution and velocity vectors after 1,700 time steps: • •

Version 4.02

Under the File(s) tab of the Load Data panel, select step number 1700 from the Select Time Step list Click Store Iter/Time to load the data 4-15

Tutorial 4.2



• • • • • •

Under the Data tab, select Data Type Cell & Wall/Bound (Smooth) Select VOF from the Scalar Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, select options Contour (filled) and Edge Click Plot To Screen. Note that the angle the free surface makes with the wall is ~45o

To plot these contours in the same window as a velocity vector plot: •

Type the following command in the I/O window: CENTER 0.5 -0.1 0.0

• • •

Click Replot Select Plot > Display > Overlay Type the following command in the I/O window: CENTER 0.5 4.1 0.0

• • • • •

Under the Data tab of the Load Data panel, select Velocity Components UV (2D vectors) from the Vector Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, select options Vector and Edge Click Plot To Screen to display Figure T4.2-1

Figure T4.2-1

• 4-16

Distribution of volume fraction (upper) and velocity vectors (lower) for a contact angle of 45 degrees, after 1,700 time steps

Turn off the overlay mode by selecting Plot > Display > Overlay Version 4.02

Tutorial 4.2



The velocity vector plot shows high air velocities close to free surface. This is a numerical inaccuracy known as parasitic currents. These currents arise because the surface tension and pressure forces are much larger than all other terms in the momentum equations, and their balance on an irregular grid is difficult to achieve numerically due to the sensitivity of the curvature approximation. These parasitic currents become appreciable when the problem size is small and fluid velocity and viscosity are low. For cases where the free surface curvature is small (i.e. the radius is of the order of 10 mm or more) or where fluid flows at high speed (as in injection nozzles), these problems are not encountered. Since the artificial velocities are generated only within the air, their effect on the liquid flow (which is usually what we are trying to predict) is small. To examine how changing the contact angle affects the resulting free surface: • • • • •

Select the Free Surface folder in STAR GUIde and open the Molecular Properties panel Under the Heavy Fluid tab, change Contact Angle at Wall to 150 Click Apply Write the problem file and re-run the analysis Follow the procedure described above to plot contours of volume fraction and velocity vectors after 1,700 time steps. The resulting plot is shown in Figure T4.2-2

Figure T4.2-2

Distribution of volume fraction (upper) and velocity vectors (lower) for a contact angle of 150 degrees, after 1,700 time steps

The increase in contact angle means that the wall is now non-wetting, i.e. the liquid does not spread along the wall after passing through the nozzle, but instead continues to flow in the direction of the gravity force. If the solution domain was Version 4.02

4-17

Tutorial 4.2



extended further to the right and the analysis was run for longer, the droplet forming behind the nozzle would eventually detach from it. This would occur because gravity would cause the droplet to accelerate to a speed greater than that in the nozzle. In some applications, it may be necessary to specify different contact angles on different walls. This is not possible using current STAR GUIde facilities since the contact angle is specified as a heavy fluid property. However, this value can be over-ridden, where necessary, via user coding. The latter is activated by selecting User rather than Constant in the Additional Properties section of the Heavy Fluid tab. The relevant user subroutine, FSTEN, can then be modified, as required.

4-18

Version 4.02

Tutorial 4.3

FORCED FREE-SURFACE FLOW WITH CAVITATION


Tutorial 4.3


This tutorial aims to demonstrate how to: • • •

Perform a simulation of a free-surface flow in which cavitation takes place Display free-surface and cavitation data in the same plot Change the Post Colormap settings to improve the appearance of contour plots

Physical Problem Description This tutorial models the forced flow of water through a nozzle into an air-filled chamber at atmospheric pressure. The geometry, mesh and scale factor (0.001) are the same as those used in Tutorial 4.2. The boundary labelled “Left” in Figure T4.0-1 is at a static pressure of 500 bar and the boundary labelled “Right” is at atmospheric pressure. The boundaries labelled “Bottom”, “Front” and “Back” are symmetry planes, and all other boundaries are solid walls. Initially, the nozzle is filled with liquid (cell type 2) and the downstream chamber is filled with air (cell type 1). The sharp corner at the entrance into the narrow nozzle combined with the flow acceleration will produce a low pressure region in which cavitation will take place. Pre-Processing Preliminaries Create a directory for the tutorial called tut4-3 and copy file gridfs.ccm supplied with the STAR-CD installation into it. In this directory: • • • •

Start pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (cavit) in the Casename text box Click Continue

Define a transient simulation and activate the free surface and cavitation modelling options: • • • • •

Open the Select Analysis Features panel in STAR GUIde Select Transient in the Time Domain section Select On in the Free Surface section Select On in the Cavitation section Click Apply

Give the case a title: • •

In the main window, select File > Model Title In the Title text box type: FORCED FREE-SURFACE FLOW WITH CAVITATION

• Mesh Import & Checking Version 4.02

Click Apply

To import and display the mesh: •

Select the Create and Import Grids folder in STAR GUIde 4-19

Tutorial 4.3



• • • • • • • • Material Properties

Open the Import Grids panel Select the CCM button from the Format list Enter gridfs.ccm as the CCM File name Check that the State Name entry is set to default Click Import Grid In the main window, select C > All to put all cells into the current cell set Check that the Geometry Plot mode and Hidden Surface plot type are selected Click Cell Plot to display the grid shown in Figure T4.0-1

Examine the free-surface flow modelling options and material property settings: • • • • • •

Select the Free Surface folder in STAR GUIde Open the Controls panel Turn On Surface Tension Click Apply Open the Molecular Properties panel Both the default Light Fluid, AIR, and the default Heavy Fluid, H2O, are suitable for this case so no changes are needed

Examine the cavitation modelling options: • • •

Select the Cavitation folder Open the Cavitation Model panel The default options are all acceptable so click Apply. For a detailed description of the options in this panel, consult the corresponding pro-STAR on-line Help topic

The remaining material property settings are specified using panels in the Liquids and Gases folder. These panels feature a Material # slider, enabling you to specify different properties for each fluid material in the model. For the ‘heavy’ and ‘light’ fluids defined in free-surface problems, this functionality is not relevant since those properties specified for the ‘light’ fluid (Material # 1) are also applied automatically to the ‘heavy’ fluid (Material # 2). Turn on turbulence modelling and select an appropriate model: • • • • •

Select the Liquids and Gases folder and open the Turbulence Models panel Check that the slider at the bottom of the panel is set to Material # 1 Turn On turbulence modelling Select the k-Epsilon/High Reynolds Number model from the list Click Apply


•

4-20

Open the Monitoring and Reference Data panel Click the mouse symbol in the Monitoring cell number section to select the monitoring location In the main pro-STAR window, select a cell just to the right of the narrow section. This location is chosen because large variations in field variable values are expected here. In the Reference Data section, click the mouse symbol to select the reference pressure cell number Version 4.02

Tutorial 4.3



•

• Initialization

In the main pro-STAR window, click on a cell at the top right-hand corner. This location is chosen because this corner will always contain air and so the pressure variations are likely to be minimal. Click Apply

Initially, the left-hand vessel contains only water and the right-hand vessel only air. This initial distribution is specified by associating the two fluids with different cell types: • • • • • •


The initial turbulence parameters must also be set as follows: • • • •

• Scalars

Two scalars are defined for problems involving both free surfaces and cavitation. A passive scalar called VOF is defined as the volume fraction of the ‘heavy’ fluid. An active scalar named CAV stores the volume fraction of vapour generated during the cavitation process. • •

• • • • Boundary Conditions

Select the Additional Scalars folder and open the Molecular Properties (Scalar) panel Check that the slider at the bottom of the panel is set to Scalar # 1 and that the scalar’s Name is VOF. The properties of this scalar are defined by the choice of ‘heavy’ fluid so no changes are necessary in this panel. Move the slider to Scalar # 2, named CAV, which represents the ‘heavy’ fluid vapour The default properties are suitable so click Apply Open the Initialization panel Check that the Initial Mass Fraction of both VOF and CAV scalars is 0

To define boundary conditions for this problem: • • • • •

Version 4.02

Open the Initialization panel in STAR GUIde Under the Turbulence tab, check that option k-Epsilon is selected Change the Turbulent Energy to 1 Change Epsilon to 10000. Note that what is important here is not the actual values specified but rather their ratio, as this determines the initial turbulent viscosity. In this case, k and ε are chosen to give a turbulent viscosity of the order of 0.01 Click Apply

Select the Define Boundary Conditions folder and open the Define Boundary Regions panel In the region list, select Reg# 1 named Wall Change the Region Type to Wall and click Apply Repeat this operation for the regions named TopLeft and TopRight Select Reg# 3, named Right 4-21

Tutorial 4.3



• • • • • • • •

Change the Region Type to Pressure Change the pressure Option to Static Click Apply Select Reg# 2, named Left Change the Region Type to Pressure Change the pressure Option to Static Change the Pressure value to 5.0e7 Pa Click Apply

No action is needed for the regions named “Back”, “Front” and “Bottom” as these are already defined as symmetry planes in the supplied mesh geometry file. The values of VOF and CAV at the pressure boundaries must also be specified: • • • • • •

Open the Scalar Boundaries panel and check that the currently selected Scalar is VOF Select Boundary Region 2, Pressure from the Boundary Region list Check that the Boundary Condition is set to Boundary Mass Fraction Change the Mass Fraction value to 1 Click Apply The Mass Fraction for Boundary Region 3, Pressure is set to 0 by default so no change is required

No changes are required for the CAV scalar since its default setting of 0 volume fraction at all boundaries is appropriate for this problem. Analysis Controls

The transient SIMPLE solution algorithm must be used for free surface problems. This tutorial will also use the AMG solver, the recommended pressure-correction equation solver for all free surface problems. To specify these settings: • • • • •


This tutorial involves a two-dimensional analysis so it is not necessary to solve for the momentum component in the z-direction. To turn this off and specify appropriate settings for the solver parameters and differencing schemes: • • • • • •

4-22

Select the Equation Behavior sub-folder and open the Primary Variables panel Under the Equation Status tab, deselect the W-Mom button Click Apply Under the Solver Parameters tab, set the Relaxation Factor for the momentum and turbulence equations to 0.8 Set the Relaxation Factor for the pressure equation to 0.4 (higher than the default because we are dealing with an unsteady flow and small time steps) In transient SIMPLE calculations, it is not necessary to solve the pressure equation as accurately as in PISO calculations because the outer iterations within each time step control convergence. Therefore, set the Residual Version 4.02

Tutorial 4.3



• • • • • • • • •

Tolerance for all variables to 0.01. Set the Number of Sweeps to 100 for all variables Click Apply Under the Differencing Schemes tab, change the differencing scheme for the momentum equations to MARS Click Apply Open the Additional Scalars panel Select Scalar 1 (VOF) and check that the Under-Relaxation Factor is 0.8 Leave all other settings at their default values and click Apply Select Scalar 2 (CAV) and check that the Under-Relaxation Factor is 0.8 Leave all other settings at their default values and click Apply

Specify what data should be written to the results (.ccm) file and the transient post data (.pstt) file: • • • • • • • Run Time Controls

Select the Output Controls folder and open the Analysis Output panel Under the Post tab, check that the analysis is set to Write final solution (restart) file with an Output Frequency of 100 time steps Click Apply Under the Transient tab, choose to Write data every 1e-5 seconds Select VOF as an output variable from the list and click Post Repeat this for CAV Click Apply

To specify the run time and time step size: • • • • • •

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel In the Run Time section, instruct the analysis to Run for 5e-5 seconds Click Apply In the Time Step Option section, change the Time Step for Period to 1e-7 seconds. This means that the run will continue for 500 time steps Click Set Period


In the main pro-STAR window, select File > Write Geometry File In the Geometry File Write dialog, change the Geometry Scale Factor to 0.001 to convert the model units to millimetres Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Save Model

You can stay within the current pro-STAR session by either moving pro-STAR into the background or by opening another terminal window to start up the STAR-CD solver.

Version 4.02

4-23

Tutorial 4.3



CFD Analysis Check that you are in the current working directory and then start the simulation by typing: star at the command line. The analysis should only take a few minutes. The output on the screen will show that the outer iterations are converging to the specified tolerance for each time step. Post-Processing Preliminaries Start the post-processing session by opening the transient post data file: • • • • • •

In STAR-GUIde, select the Post-Processing folder and then open the Load Data panel Under the File(s) tab, select Transient as the Analysis option Select the empty position, 1, in the Transient Post File(s) list Click Add File to List Select file cavit.pstt from the Transient Post File(s) list Click Open Transient Post File

The remainder of this tutorial demonstrates how to create static plots of flow variables at specified times. Animated plots are not be produced here as the methods for creating them are described in detail in other tutorials, namely Tutorial 4.1, Tutorial 8.2 and Tutorial 12.3. Basic Plots

First, plot velocity vectors after 500 time steps: • • • • • •

4-24

Under the File(s) tab of the Load Data panel, select step number 500 from the Select Time Step list and click Store Iter/Time to load the data Under the Data tab of the Load Data panel, select Velocity Components UV (2D vectors) from the Vector Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, select options Vector and Edge Click Plot To Screen to display Figure T4.3-1

Version 4.02

Tutorial 4.3



Figure T4.3-1

Velocity vectors after 500 time steps

It is possible to create a contour plot that approximately shows both the CAV and VOF scalar distributions (i.e. both water vapour and liquid water) by using the OPERATE utility to manipulate the post data. First, put the VOF and CAV scalar data in post registers 5 and 6, respectively: •

Enter the following commands in the I/O window: OPERATE GETC CONC 5 1 OPERATE GETC CONC 6 2

• • • • • • • • •

• • • • • • Version 4.02

In the main pro-STAR window, select Post > Operate... to open the Post Register Operations dialog Select Function > Scalar/Vector > Multiply Choose Register 6 = 2 * Register 6 Click Apply Select Function > Multi-Register > Add Choose Register 4 = Register 5 + Register 6 Click Apply and then Close Select Post > Caverage > Cset Under the Options tab of the Create Plots panel, select RGB from the Colormap list. Note that the colours displayed under the pop-up menu change when you do this. Click Apply Change the Number of Color Indices to 12 Change the Range to User and enter minimum and maximum values 0 and 2 Click Apply Under the 3-D Surface tab, select options Contour (filled) and None Click Plot To Screen to display Figure T4.3-2 4-25

Tutorial 4.3



Figure T4.3-2

Contour plot showing VOF and CAV distributions after 500 time steps

To a reasonable approximation, the blue and turquoise regions are predominantly occupied by air, the green regions predominantly by liquid water and the yellow, orange and red regions predominantly by water vapour. As expected, cavitation occurs at the nozzle entrance as a result of the low pressure region produced by the sharp corner and the accelerating flow. Manipulating the results in this way provides a qualitative visual estimate of the extent of the different regions. However, the resulting plots are prone to inaccuracies in those places where air and water vapour occur together and also where the value of VOF is only slightly greater than that of CAV. In such a case, the latter leads to an overprediction of the size of the region of high water vapour concentration. The tutorial is now complete. To quit pro-STAR: •

4-26


Version 4.02


Tutorial 5 TURBULENT FLUID STREAM MIXING Physical Problem Description This tutorial deals with the mixing of air and methane gas in a dilution pipe, using the mesh shown in Figure T5.0-1, created in Tutorial 7.1 of the Meshing Tutorials volume. The problem geometry consists of two concentric pipes, with the inner pipe covering only one quarter of the total distance between inlet and outlet. An orifice plate protrudes from the outer wall half way along the pipe. Air at standard pressure and temperature (1 bar, 293 K), flows in through the outer annulus with a uniform velocity of 5 m/s. Methane gas (molecular weight 16 kg/kmole) at a temperature of 323 K flows in through the inner pipe at a uniform velocity of 10 m/s. The pipe walls (inner and outer) are assumed to be adiabatic and the orifice plate has negligible thermal resistance. The background fluid for this problem is air (constant pressure of 1 bar, temperature of 293 K); its physical properties are as follows: Molecular weight Density Molecular viscosity Specific heat Thermal conductivity

28.96 1.205 1.81 × 10–5 1006.0 2.637 × 10–2

kg/kmole kg/m3 Pa s J/kg K W/m K

The flow is three-dimensional and essentially symmetric, so only half of the problem geometry was considered in building the mesh. The tutorial is divided into two parts, one dealing with a steady-state and the other with a transient analysis.

Figure T5.0-1 Version 4.02

Mesh structure for the dilution pipe model (back elevation) 5-1

Tutorial 5.1

STEADY 3-D FLOW


Tutorial 5.1

STEADY 3-D FLOW

The primary task of this tutorial is to: • • •

Set up and analyse a turbulent, multi-species flow Define boundary conditions for both main flow variables and additional scalar variables representing species mass fractions Create multiple cross-sectional plots showing the analysis results as part of a single operation

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut5-1. The mesh for this problem has already been created in the Meshing Tutorials volume (Tutorial 7.1) and the relevant cell, vertex, boundary and problem setup files are already available (files dil_pipe.cel, dil_pipe.vrt, dil_pipe.bnd and dil_pipe.inp, respectively). Therefore, before starting the tutorial, make sure that the supplied files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, dil_pipe_ss) in the Casename text box Click Continue

Read in the available problem data: • • • •

Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is dil_pipe.inp Click Apply Click Close

This will read default problem settings from file dil_pipe.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: TURBULENT MIXING IN A DILUTION PIPE (STEADY)

• Mesh Checking

Verify that the mesh data are correct by selecting all cells and vertices and plotting the mesh in ‘Hidden Surface’ mode: • • • • •

5-2

Click Apply

In the main window, select C > All. The I/O window output shows that 2,080 cells were read in Select V > All. The I/O window output shows that 2,331 vertices were read in Check that Hidden Surface is the default cell plot type Click Cell Plot Change the viewpoint to approximately (-1, 0.5, -1) using the orientation Version 4.02

Tutorial 5.1

STEADY 3-D FLOW


cube’s slider controls to display Figure T5.1-1 It will be seen that the mesh is in fact the same as the one created in Meshing Tutorial 7.1.

Figure T5.1-1

Material Properties

Mesh geometry

Check the default fluid properties and then choose the ideal gas law for density variations, making it a function of temperature only (incompressible flow): • • • • •

In the STAR GUIde window, select folder Thermophysical Models and Properties Select sub-folder Liquids and Gases Open the Molecular Properties panel Choose option Ideal-f(T) from the Density menu Click Apply

Turn on the standard k-ε turbulence model: • • • •

Open the Turbulence Models panel Click On to switch on turbulence modelling Select K-Epsilon/High Reynolds Number from the drop-down menu Click Apply

Turn on the solution of the temperature equation: • • •

Open the Thermal Models panel Click the Temperature Calculation On button Click Apply

Set the monitoring point location: Version 4.02

5-3

Tutorial 5.1

STEADY 3-D FLOW

Pre-Processing Scalar Properties

• • • Scalar Properties

Open the Monitoring and Reference Data panel Type 11 in the Monitoring cell number text box Click Apply

Physical properties for scalar variables are specified next: •

Select the Additional Scalars folder and then open the Molecular Properties (Scalar) panel

It will be seen that no scalar entities have been defined yet. The required scalar is methane and its properties can be retrieved from the built-in property database. However, in this tutorial, methane is treated as a user-defined scalar and its properties are supplied manually for the purposes of illustration. •

•

Type the following property data in the corresponding dialog boxes: Name — CH4 Density — 0.669 Molecular Weight — 16 Molecular Viscosity — 1.175e-5 Specific Heat — 2230.0 Conductivity — 0.038 Heat of Formation — -4.68e6 Temp. of Formation — 298.15 Click Apply

The details of the scalar’s properties will be shown in the I/O window as follows: PROPERTIES FOR SCALAR NO. 1 NAMED CH4 INFLUENCE = ACTIVE SOLVER TURNED ON MOLECULAR WEIGHT = 16.0000 DENSITY = 0.669000 BETAM = 0. SPECIFIC HEAT = 2230.00 LAMINAR VISCOSITY = 0.117500E-04 THERMAL CONDUCTIVITY = 0.380000E-01 HEAT OF FORMATION = -4680000. TEMPERATURE OF FORMATION = 298.15 Note that the scalar’s ACTIVE designation signifies that its concentration at any point in the flow will influence the overall fluid density at that point. Save the model data entered so far: • Boundary Conditions

Specify boundary conditions for each region, including turbulence parameters at the two inlets in terms of turbulence intensity and length scale: • •

5-4

In the main window, select File > Save Model

Select folder Define Boundary Conditions and then open the Define Boundary Regions panel Select region no. 1 (the inner inlet) in the scroll list Version 4.02

Tutorial 5.1

STEADY 3-D FLOW


Version 4.02

• •

Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

•

Click Apply

• • •

Select region no. 2 in the scroll list Select option TI/Length in the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

•

Click Apply

• • •

Select region no. 3 in the Boundary Regions scroll list Select option TI/Length in the Turb. Switch menu Enter pressure boundary conditions in the appropriate boxes, as shown below:

5-5

Tutorial 5.1

STEADY 3-D FLOW


•

Click Apply

Specify boundary conditions for the scalar (CH4) mass fraction, ensuring that its value is 1.0 at the inner pipe inlet and 0.0 at all other boundaries. • • • •

Open the Scalar Boundaries panel Select region no. 1 (the inner pipe inlet) in the Boundary Region scroll list. CH4 is selected by default in the Scalar list. Enter the required boundary value, 1.0, in the Mass Fraction box and then click Apply Select region no. 2 (the outer pipe inlet) and then region no. 3 (the outflow boundary) in the list to confirm that the scalar mass fraction at both boundaries is 0.0

Check the boundary conditions graphically: • • • •

5-6

In the main window, select B > All Select B > Unselect > Symplane Select Cell Plot Display Option Bound Select cell plot type Quick Hidden Line to display Figure T5.1-2

Version 4.02

Tutorial 5.1

STEADY 3-D FLOW

Pre-Processing Control Parameters

Figure T5.1-2

Control Parameters

Inlet and outflow boundary condition display

Check the status of the control parameters: • •

Select folder Analysis Controls Select sub-folder Solution Controls followed by Equation Behavior

Check the scalar control parameters and then modify some of them: • • • •

Open the Additional Scalars panel Check that CH4 is selected in the Scalar scroll list and then type 0.95 in the Under-Relaxation Factor box Type 1.0e-4 in the Residual Tolerance box Click Apply

Make the residual error tolerances for the temperature and scalar equations the same. This ensures that both equations are solved to the same level of accuracy: • • • Run Time Controls

Check the status of the run time control parameters: • • •

Version 4.02

Open the Primary Variables panel Select the Solver Parameters tab and type 0.0001 in the Residual Tolerance box corresponding to the temperature (Temp.) equation Click Apply

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 200 for the maximum number of iterations Click Apply

5-7

Tutorial 5.1

STEADY 3-D FLOW


Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Remember that, for convenience, the model geometry units were specified in inches. This must be changed into meters by applying the appropriate conversion factor before writing data to the geometry file. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

In the main pro-STAR panel, select File > Write Geometry File In the Geometry File Write dialog, enter 0.0254 in the Scale Factor box Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit


In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that the units in which the model was built are correctly selected (option button inches). Leave all other settings at their default values Click Start New Analysis

The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file tut.ccm: • • • Postprocessing

Load velocity vector components for plotting and then display them on your screen using the ‘Quick Hidden Line’ mode: • • • • • • • •

5-8


Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Components UVW to load all three velocity components In the Scalar Data list, check that the default setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select Vector from the Option menu and Grid from the Edge/Mesh menu Click Plot to Screen In the main window, select cell plot type Quick Hidden Line to display Version 4.02

Tutorial 5.1

STEADY 3-D FLOW


Figure T5.1-3

Figure T5.1-3

Velocity magnitude plot

Load vertex-based pressure values, select the contour plotting option and plot in ‘Hidden Surface’ mode: • • • • • • •

Version 4.02

Go back to the Load Data panel by clicking Go To Load Data In the Data tab, select option Cell & Wall/Bound (Smooth) from the Data Type menu In the Vector Data list, check that the default setting is None In the Scalar Data list, select item Pressure and then click Get Data Select Go To > Create Plots to display the Create Plots panel In the 3-D Surface tab, select plot options Contour (filled) and Edge Click Plot to Screen to display Figure T5.1-4

5-9

Tutorial 5.1

STEADY 3-D FLOW


Figure T5.1-4

Pressure plot

Load vertex-based temperatures and plot: • • •

Go back to the Load Data panel by clicking Go To Load Data In the Scalar Data list, select item Temperature and then click Get Data In the main pro-STAR window, click Replot to display Figure T5.1-5

Figure T5.1-5 5-10

Temperature plot Version 4.02

Tutorial 5.1

STEADY 3-D FLOW


A multi-section plot of a variable can be made using the following procedure: • • • • • •

Select Go To > Create Plots Select tab Section Clipped Choose Contour (filled) from the Option menu and Edge from the Edge/Mesh menu Select the Multiple Plane Plot sub-tab The default number (10) of section planes to be plotted in succession is shown in the Increments box. Accept this value. Define the normal direction to these planes to be the direction of a coordinate axis, as follows: (a) Click the coordinate system selection button to display the Coordinate Systems dialog (b) Select the toroidal coordinate system (no. 4) and then click Close (c) Note that the entry in the Coordinate System box changes to show that system no. 4 has been selected. A pop-up menu (DIR) also appears, inviting you to choose the desired direction. (d) Select direction no. 2 (the θ- direction) from this menu and then click Apply

•

Click Sweep to see 10 section plots of temperature plotted in quick succession, starting at one end of the model and finishing at the other

Once the sections are defined, they can be re-used to produce plots of any other variable. For example, velocity magnitude plots can be generated as follows: • • • • • •

Click Go To Load Data In the Calculated Scalar Data list, select item Velocity Magnitude and then click Get Data Select Go To > Create Plots In the Section Clipped tab, choose Contour (filled) from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen to see the velocity magnitude distribution plotted on the model surface Click Sweep to see the same distribution plotted on a series of cross-sections through the model

To produce the best display of the calculated methane mass fraction distribution, load cell-based values and then average them at the vertex positions: • • • • • • •

Version 4.02

Click Go To Load Data In the Data tab, select Cell from the Data Type menu Select On from the Smooth Option menu In the Scalar Data list, select item CH4 and then click Get Data Select Go To > Create Plots Select the 3-D Surface tab and then choose Contour (filled) from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen to display Figure T5.1-6

5-11

Tutorial 5.1

STEADY 3-D FLOW


Figure T5.1-6

Final Operations

5-12

•

Methane mass fraction plot

In the main window, select File > Quit, Nosave

Version 4.02

Tutorial 5.2

TRANSIENT 3-D FLOW


Tutorial 5.2

TRANSIENT 3-D FLOW

The problem geometry and mesh for this tutorial is the same as for Tutorial 5.1. The model also has the same boundaries and boundary region definitions. The only difference is that transient boundary conditions are now imposed at the inlet planes. As shown in Figure T5.2-1, the air inlet velocity increases linearly from 5 m/s to 9 m/s over a period of 2 seconds. At the same time, the methane inlet velocity decreases from 10 m/s to 2 m/s, simulating the gradual shut down of an upstream valve. At the end of this tutorial it is expected that users will be able to: • • •

Set up a transient calculation Set up a table that defines the changing boundary conditions Perform some basic post-processing appropriate to transient calculations

Pre-Processing Preliminaries A number of initial file copying operations are needed for proper operation of this tutorial, as follows: • • •

Create a sub-directory for the tutorial called tut5-2 and copy the model file generated in Tutorial 5.1 (dil_pipe_ss.mdl) into it Rename this file as dil_pipe_tr.mdl Since the solution obtained in Tutorial 5.1 will act as the starting point of the present analysis, it is also necessary to copy the solution file for the steady-state case (dil_pipe_ss.ccm) to the current directory

Start up the pro-STAR interface: • • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Accept the default case name (dil_pipe_tr) displayed in the Casename text box Select the Resume existing .mdl file option Deselect the Append to .echo file option Click Continue

This will read all data in file dil_pipe_tr.mdl and will set up the model as it was at the end of Tutorial 5.1. • •

In the main window, select File > Model Title In the Title text box, change the title to: TURBULENT MIXING IN A DILUTION PIPE (TRANSIENT)

•

Click Apply

Check the geometry and boundary conditions visually to confirm that the model has been read in correctly: • •

Version 4.02

Select C > All Click Cell Plot

5-13

Tutorial 5.2

TRANSIENT 3-D FLOW

Pre-Processing Transient Solution Setting

Transient Solution Setting

The modifications needed to change to a transient analysis are as follows: 1. Select the transient solution mode 2. Define transient boundary conditions To set up the STAR GUIde environment for a transient simulation, proceed as follows: • •

Table Definition

Go to the STAR GUIde window and open the Select Analysis Features panel Select Transient from the Time Domain menu and then click Apply

As indicated in the tutorial’s introduction, the basic requirement of this case is to simulate a time variation in the inlet stream velocities, as shown in Figure T5.2-1 below:

Velocity (m/s)

10 Outer Inlet

9 8 7 6 5 4 3

Inner Inlet

2 1

Time (sec) 1

Figure T5.2-1

2

Velocity changes over a 2 sec. period at the two inlet planes

The above variation may be defined using pro-STAR tables and then applied to the two inlet boundaries. To set up a table for the inner inlet:

5-14

•

Click the Table Editor button in the main pro-STAR window

• •

In the Table Editor dialog, enter INNER_INLET in the Table Title box Click the Coordinate System button and then select system no. 1 (the global Cartesian coordinate system) in the scroll list, as velocities will be specified in Version 4.02

Tutorial 5.2

TRANSIENT 3-D FLOW

Pre-Processing Boundary Re-definition

• • • • • • • • • • • •

this system Click Close. The new coordinate system choice will appear on the Table Editor dialog. Select Extrapolate from the Out of bound value option menu Select the V component of velocity from the Dependent Variables scroll list Select TIME as the independent variable Click Setup Enter two values in the TIME column, 0.0 for the 1st time point and 2.0 for the 2nd time point Click the red FILL button. A warning message pops up asking you to confirm your choice of independent variable, so click Yes Enter two end-point values for the V-velocity, 10.0 and 2.0, corresponding to the two time points specified above Click Save Data to confirm your entries Enter a new name, in1.tbl, in the File Name box at the bottom of the panel Click Write Table to save the table data just entered in the above file Click Graph to display a graph of the inner inlet V-velocity variation, which should be as shown in Figure T5.2-1

Now set up a table for the outer inlet by editing the one currently on display: • • • • • • •

Enter a new name, OUTER_INLET, in the Table Title box Enter two new end-point values for the V-velocity, 5.0 and 9.0, corresponding to the previously defined time points of 0.0 and 2.0 Click Save Data to confirm your entries Enter a new name, in2.tbl, in the File Name box at the bottom of the panel Click Write Table to save the table data just entered in the above file Click Graph to display a graph of the outer inlet V-velocity variation, which should be as shown in Figure T5.2-1 Close the Table Editor dialog

Boundary Apply the time variation in velocity defined above to the inner inlet: Re-definition • Go to the STAR GUIde window and select folder Define Boundary Conditions • Open the Define Boundary Regions panel • Select region no. 1 (Inner_inlet) in the boundary regions scroll list • Select Table from the Options menu • Open the pro-STAR file browser by clicking the button next to the Table Name box, choose file in1.tbl from the file list and click OK. The selected file name will now be displayed inside the box. • Click Apply to instruct STAR to read V-velocity boundary values from this table Repeat for the outer inlet: • • •

Version 4.02

Select region no. 2 (Outer_inlet) in the boundary regions scroll list Select Table from the Options menu Open the pro-STAR file browser by clicking the button next to the Table Name box, choose file in2.tbl from the file list and click OK. The selected 5-15

Tutorial 5.2

TRANSIENT 3-D FLOW


•

Analysis Controls

Check the analysis controls status: • • • • • •

• Run Time Controls

file name will now be displayed inside the box. Click Apply to instruct STAR to read V-velocity boundary values from this table

Select folder Analysis Controls Select sub-folder Solution Controls and then open the Solution Method panel. It will be seen that the PISO algorithm has been selected automatically. Select sub-folder Output Controls and then open the Analysis Output (Transient) panel Go to the Transient tab Define an output period starting at time t = 0.0 s and a data output frequency of 0.5 s for the transient post file Note that, by default, the Velocity and Pressure variables are already selected for output in the upper scroll list. Choose a number of additional items for output, Turb Kinetic Energy, Dissipation, Turbulent Viscosity, Temperature, Density and scalar variable CH4, by selecting each one in turn and then clicking the Post button. Check the list display to verify your choices and then click Apply

Check the status of the run time controls and then specify the simulated elapsed time and the time step to be used: • • • • • •

Select folder Analysis Preparation/Running Open panel Set Run Time Controls Select option Run for and type 2 in the adjacent input box Click Apply Enter 0.0 in the Period Start Time box and 0.025 in the Time Step for Period box Click Set Period

Specify that the analysis is to start from the previously calculated steady-state solution: • • • • Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • •

5-16

Open the Analysis (Re)Start panel Select option Standard Restart from the Restart File Option menu Click the browser button next to the Restart File box, select file dil_pipe_ss.ccm from the browser dialog and then click OK Click Apply

In the main pro-STAR panel, select File > Write Geometry File In the Geometry File Write dialog, enter 0.0254 in the Scale Factor box Click Apply and then Close Version 4.02

Tutorial 5.2

TRANSIENT 3-D FLOW


• • •

Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis To perform the analysis interactively, proceed as follows: • • • • •

In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that the units in which the model was built are correctly selected (option button inches) Click Write New Geometry File Click Restart Analysis

The analysis will then start automatically and will stop after 80 time steps. Bear in mind that transient solutions can involve lengthy computer runs. Therefore, the analysis for this tutorial will take much longer than for Tutorial 5.1. Post-Processing Preliminaries Open the file containing the transient post data (dil_pipe_tr.pstt): • • • • • •

Postprocessing

In the STAR GUIde window, select folder Post-Processing Open the Load Data panel Select option Transient from the Analysis menu Check that file dil_pipe_tr.pstt is displayed in the File Name box and then select the first position in the Transient Post File(s) list Click Add File to List Select file dil_pipe_tr.pstt on the list again and then click Open Transient Post File; the time steps at which flow data were stored during the run should appear in the Select Time Step scroll list

The next step in transient post-processing is to identify the point in time at which results are to be manipulated and displayed. This is done as follows: •

In the Select Time Step list, select the required time (0.5 sec in this case) and then click Store Iter/Time. This loads results calculated after 20 time steps.

Load velocity vector components, select the cross-sectional plotting option and reduce the size of all vectors: • • • • • • • Version 4.02

Go to the Data tab and select item Velocity Components UVW in the Vector Data list Click Get Data Select Go To > Create Plots In the Create Plots panel, go to tab Section Clipped Accept the default section definition and then click Plot to Screen Go to the Vectors tab and then type 0.7 in the Scale Factor box Click Apply 5-17

Tutorial 5.2

TRANSIENT 3-D FLOW


Change the viewpoint and replot: •

In the main window, change the viewpoint to (0, 0, -1) by selecting View > Axis > -Z to display Figure T5.2-2

Figure T5.2-2

Velocity magnitude plot at t = 0.5 s

The methane mass fraction can be plotted as follows: • • • • • • •

5-18

In the Create Plots panel, click Go To Load Data Select On from the Smooth Option menu Select item CH4 in the Scalar Data list Click Get Data Select Go To > Create Plots In the Section Clipped tab, select Contour (filled) from the Option menu Click Plot to Screen to display Figure T5.2-3

Version 4.02

Tutorial 5.2

TRANSIENT 3-D FLOW


Figure T5.2-3

Methane mass fraction plot at t = 0.5 s

The results after 2.0 seconds (80 time steps) may be plotted in the same manner: • • • • • • • •

Version 4.02

Click Go To Load Data and then select the File(s) tab In the Select Time Step list, highlight the desired time (2.0 secs) and then click Store Iter/Time. This loads results calculated after 80 time steps. Go to the Data tab and select Smooth Option Off In the Vector Data list, select item Velocity Components UVW Click Get Data Select Go To > Create Plots In the Section Clipped tab, select Option Vector Click Plot to Screen to display Figure T5.2-4

5-19

Tutorial 5.2

TRANSIENT 3-D FLOW


Figure T5.2-4

• • • • • • •

5-20

Velocity magnitude plot at t = 2.0 s

Click Go To Load Data Select On from the Smooth Option menu Select item CH4 in the Scalar Data list Click Get Data Select Go To > Create Plots Select Contour (filled) from the Option menu Click Plot to Screen to display Figure T5.2-5

Version 4.02

Tutorial 5.2

TRANSIENT 3-D FLOW


Figure T5.2-5

Final Operations

Version 4.02

•

Methane mass fraction plot at t = 2.0 s


5-21

Tutorial 6 SUPERSONIC AND TRANSONIC FLOWS Tutorials in this section are designed to demonstrate the application of STAR-CD to compressible flow problems. Tutorial 6.1 involves flow over an idealised two-dimensional wing geometry, shown in Figure T6.0-1.

inflow

Figure T6.0-1

Version 4.02

5o

9 cm

Symmetrical diamond-shaped wedge used in supersonic flow tutorial

6-1

Tutorial 6.1

ADAPTIVE MESH REFINEMENT FOR SUPERSONIC FLOW


Tutorial 6.1


This tutorial aims to demonstrate: • • •

A method of adaptive mesh refinement How to set up a model of inviscid supersonic compressible flow How to calculate gradients of scalar post data

Physical Problem Description In this tutorial, the ‘wing’ geometry is a diamond wedge with major length 9 cm and half-angle 5° (see Figure T6.0-1). The inlet flow direction is parallel to the major length (zero angle of attack) so the flow is symmetrical. Therefore, a symmetry plane may be placed along the major length to reduce the computational cost of the simulation. The flow is assumed to be inviscid and the inlet velocity is set at Mach 1.893, which is sufficiently large to ensure that the flow is supersonic across the entire solution domain. For air at a temperature of 293 K, this is equivalent to a velocity of 650 m/s, as calculated from the equation below: u u M = --- = --------------c κRT where κ is the adiabatic index and R is the gas constant for air, taken as 1.402 and 287.05 Jkg-1K-1, respectively. Initially, the case is run with a simple, coarse mesh. This is then refined in the areas where the pressure gradient is greatest. This process is repeated until the mesh is sufficiently fine to give a reasonable resolution of the shock and expansion waves. Pre-Processing Preliminaries The two analyses described in this tutorial will be performed in separate directories. Create a sub-directory for the first analysis, called tut6-1a. The initial mesh for this problem has already been created and the relevant cell, vertex, boundary and problem setup files are provided with the STAR-CD installation (files super.cel, super.vrt, super.bnd and super.inp respectively). Therefore, before starting the tutorial, make sure these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name, super1, in the Casename text box Click Continue

Read in the available problem data: • •

6-2

Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is super.inp Version 4.02

Tutorial 6.1



•

Click Apply and then Close

This will read default problem settings from file super.inp as well as the problem geometry and boundary location definitions from the remaining three files. • • • •

In the main window, select File > Model Title Type ADAPTIVE MESH REFINEMENT FOR SUPERSONIC FLOW in the Title text box Click Apply Select C > All then Cell Plot to display the mesh shown in Figure T6.1-1

Figure T6.1-1

Coarse mesh geometry

The coarseness of the mesh leads to highly smeared shock waves in the first run but the refinement procedure will correct this. First though, a complete model for the problem must be set up. Material Properties

Since the flow is compressible, the fluid density will be modelled using the ideal gas law. The inviscid assumption also needs to be specified and the temperature calculation needs to be turned on: • • • • • • •

In the STAR-GUIde panel select the Thermophysical Models and Properties folder, followed by the Liquids and Gases sub-folder Open the Molecular Properties panel Change the Density setting to Ideal-f(T,P) Change the Molecular Viscosity setting to Inviscid Click Apply Go to the Thermal Models panel and turn Temperature Calculation On Click Apply

In order to obtain a solution as quickly as possible, it is advisable to specify a Version 4.02

6-3

Tutorial 6.1


Pre-Processing Boundary Locations and Types

suitable initial flow field. This can be particularly important in compressible flow simulations. A simple, but often effective, initialisation strategy is to assign the inlet conditions to the entire solution domain: • • • Boundary Locations and Types

Open the Initialization panel Set the U velocity to 650 m/s Click Apply

The boundary locations and types have already been specified in the coded file super.bnd. To display them on the screen: • • •

Select View > Isometric > -1,1,1 Select B > All Turn on Bound in Cell Plot Display Options to display Figure T6.1-2

Figure T6.1-2

Boundaries displayed on mesh geometry

Four boundary regions can be distinguished in Figure T6.1-2, each of a different type: 1. 2. 3. 4.

The red-coloured region on the left is an inlet The green-coloured region on the right is an outlet The turquoise-coloured region on the wing is a wall The fourth region, opposite the wing and coloured pale blue, is a free-stream boundary. This type of boundary allows shock waves produced by supersonic flows to be transmitted out of the domain without reflection. Free-stream boundaries can only be used in models involving supersonic free streams. The velocity at such boundaries is usually assumed to be the same as that at the inlet. All remaining external faces of the mesh are assigned to the default boundary region 6-4

Version 4.02

Tutorial 6.1


CFD Analysis - Coarse Mesh Boundary Conditions

0 which, in this case, is defined as a symmetry plane. The boundary types listed above constitute an appropriate boundary region combination for this problem. For further information about the suitability of various boundary region combinations for compressible flow applications see “Compressible Flow” on page -9 of the CCM User Guide. Boundary Conditions

To set the desired conditions for the inlet and free-stream regions: • • • • • • • •

In the Define Boundary Conditions folder open the Define Boundary Regions panel Select Inlet from the scroll list Change the U velocity to 650 m/s Change the Density to 1.189 kg/m3 Click Apply Select Free Stream from the scroll list Change the U velocity to 650 m/s Click Apply

The default settings are suitable for all other boundary regions. Analysis Controls

Solving the momentum equation in the z-direction is not necessary in this case as the model is two-dimensional. Therefore: • • • •

Final Operations

Select the Analysis Controls folder Select the Solution Controls sub-folder followed by the Equation Behaviour sub-folder and open the Primary Variables panel Under the Equation Status tab, turn off the solution of the z-momentum equation by unchecking the W-Mom tick box Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • •

Select File > Write Geometry File The geometry was created in centimetres, so set the Scale Factor to 0.01 Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close

CFD Analysis - Coarse Mesh To perform the analysis interactively, proceed as follows: • • •

File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Leave all settings at their default values and click Start New Analysis

The analysis will then start automatically. The solution should converge within the specified maximum number of iterations. Version 4.02

6-5

Tutorial 6.1


Mesh Refinement Preliminaries

Mesh Refinement Preliminaries In order to perform mesh refinement, the current analysis results need to be read into pro-STAR: • • •


Adaptive mesh refinement can be performed automatically using the Adaptive Refinement STAR GUIde panel or manually using the Cell Refine... option in the Cell Tool. Both methods will be demonstrated in this section. Cell set collection

Load the pressure data into pro-STAR using STAR GUIde: • • • • • • • •

In the Data tab select Data Type Cell and Smooth Option On Select Pressure from the Calculated Scalar Data list Click Get Data Select Go To > Create Plots In the 3-D Surface tab, select options Contour (filled) and None Click Plot to Screen Turn off the Bound Cell Plot Display Option Select View > SNORMAL to display Figure T6.1-3

Figure T6.1-3

Pressure contours obtained using coarse mesh

As expected, the coarse mesh results show a lot of smearing in the shock waves at the two wing tips and also in the fan-shaped expansion wave at the wing’s widest point. To improve the resolution of these flow features, the mesh will be refined in the regions exhibiting the greatest pressure gradients: • 6-6

Select the Analysis Preparation/Running folder and open the Adaptive Version 4.02

Tutorial 6.1


Mesh Refinement Cell set collection

• • • • •

Refinement panel Under the Gradient sub-tab of the Refinement Criteria tab, select the Top 40 Percent of Cells for refinement Select Pressure as the Variable to Apply Criteria Click New Set Turn on mesh plotting by clicking the ‘mesh’ button in the main pro-STAR window Click Cell Plot to display Figure T6.1-4

Figure T6.1-4

Cells to be refined and corresponding pressure gradient values

Not all cells shown in Figure T6.1-4 need to be refined in the same manner: the main body of cells should be refined in two directions (x and y) but the near-wall cells only need refinement in the direction perpendicular to the wall (x). For this reason, refinement has to be performed in two stages, starting with the main body of cells. Prior to this, the selected cell set should be stored so that it can be recalled for the second refinement: • • •

In the main pro-STAR window, select INFO > Store Set/Surface/View to open the Store Information dialog Under the Sets tab, type to_refine in the Set Name box Click Write and then Close the dialog

To refine the main body of cells: • • • • Version 4.02

Select C > Subset > Type... and click on one of the cells near the top of the window Go to STAR GUIde and select the Refine tab in the Adaptive Refinement panel Change the New Casename entry to super2 Click Refine/Update Model to refine the cells 6-7

Tutorial 6.1


Mesh Refinement Cell set collection

Now, to select the near-wall cell set due for refinement, read in the previously stored cell set and define a new subset: • • • • • • • •

In the main pro-STAR window, select INFO > Recall Set/Surface/View to open the Recall Information dialog Under the Sets tab, change the Set File entry to super1.set Click Refresh Select to_refine from the Select Entry list Click Recall Close the dialog Select the Geometry Plot option in the main window Click Cell Plot

Note that as a result of the refinement just completed, the original main-body cells in the set no longer exist so only the near-wall cells are now displayed. These are refined manually using the Cell Tool: • • • • • • • • •

Select Tools > Cell Tool In the Cell Tool window, click Cell Refine In the Cell Refine dialog, enter 2, 1 and 1 for the Number of divisions in the I, J and K directions, respectively Choose Cset as the Cells to Refine Choose Merge for the Vertex Merge Option Choose Couple for the Couple Option Click Apply and then Close In the main window, select C > All Click Cell Plot to display the refined mesh, shown in Figure T6.1-5

Figure T6.1-5 6-8

Geometry plot showing mesh after a single refinement Version 4.02

Tutorial 6.1


CFD Analysis - Refined Mesh Final Operations

Final Operations

Write the geometry and problem files and save the model file: • • • • •

Select File > Write Geometry File... In the Geometry File Write dialog click Apply then Close Select File > Write Problem File... In the Problem File Write dialog click Apply then Close Select File > Save Model

Run the case in STAR, either at the command line or interactively, as described previously. Examination of the analysis results in the post data file (super2.ccm) will show that the mesh is still too coarse to fully resolve the shock and expansion waves. A suitable mesh may be obtained by repeating the mesh refinement process described above until the position of the shock and expansion waves is clear. The rest of this tutorial will proceed with a mesh that has resulted from a total of four refinement cycles using this method. Some cells adjacent to the free-stream boundary have also been further refined manually. This is sometimes necessary because, as a result of the constant pressure defined on that boundary, the calculated pressure gradient in such cells is not sufficiently high to trigger their inclusion in the code-selected refinement set. You may perform all the refinement operations if desired and, once you are satisfied that you understand the process, save your refined mesh data and terminate the session as follows: • • •

Select File > Save As Coded... Click Apply and then Close Quit pro-STAR by selecting File > Quit > Quit, Nosave

Alternatively, you may terminate the session without saving any data and continue instead from the cell, vertex, boundary and problem setup files provided with the STAR-CD installation, as described in the next section. CFD Analysis - Refined Mesh Preliminaries For the second part of this tutorial, create a new subdirectory called tut6-1b. The cell, vertex, boundary and problem setup files for the final refined mesh are called super_ref.cel, super_ref.vrt, super_ref.bnd and super_ref.inp, respectively. Therefore, before starting this part of the tutorial, make sure these files are copied into the tut6-1b directory. Start up pro-STAR and enter the new case name and title: • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter case name super_ref Click Continue

Read in the available problem data: • •

Version 4.02

Select File > Read File... In the Input Coded Command File dialog check that the filename is super_ref.inp and then click Apply 6-9

Tutorial 6.1


CFD Analysis - Refined Mesh Final Operations

This will read all the current model settings from file super_ref.inp as well as the problem geometry and boundary location definitions from the remaining three files. • • • •

In the main window, select File > Model Title Type 2D SUPERSONIC FLOW OVER A DIAMOND WEDGE in the Title text box Click Apply Select C > All then Cell Plot to display the mesh shown in Figure T6.1-6. The latter also includes a magnification of the near-wall region so that the details of the mesh structure can be seen more clearly.

Figure T6.1-6

Mesh geometry, including magnification of the near-wall region

It can be seen that the mesh is very fine in places where shock waves are expected to occur. Refinement is used to a lesser extent near the wing surface and in the expansion wave region. The regions upstream and far downstream of the wing do not need to be finely meshed as the flow there will be relatively undisturbed. Final Operations

The model setup for this problem was described earlier in this tutorial and will not be repeated. All the information necessary to run the case is contained within the files provided, so it is only necessary to save the model data and write the problem and geometry files, as shown below. A description of how to run STAR interactively is also given below. Alternatively, you may exit from pro-STAR and run STAR from the command line. • • • •

6-10

Select File > Write Geometry File The geometry was created in centimetres, so set the Scale Factor to 0.01 Click Apply and then Close Select File > Write Problem File Version 4.02

Tutorial 6.1


Post-Processing Running the Analysis

• Running the Analysis

In the Problem File Write dialog, click Apply and then Close

To perform the analysis interactively, proceed as follows: • • •


The analysis will then start automatically. The solution should converge within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis: • • •


You are now ready to post-process the results. Postprocessing

Version 4.02

Display a contour plot of pressure: • • • • • •

In the Data tab select Data Type Cell and Smooth Option On Select Pressure from the Scalar Data list Click Get Data Select Go To > Create Plots In the 3-D Surface tab, select Contour (filled) and Edge Click Plot to Screen to display Figure T6.1-7

6-11

Tutorial 6.1



Figure T6.1-7

Pressure contour plot

The rapid changes in pressure that form shock waves at both wing tips and the fan-shaped expansion wave at the wing’s widest point are clearly visible in Figure T6.1-7. The resolution of these flow features is vastly superior to that produced with the unrefined mesh of Figure T6.1-3. The improved results may also be displayed as a Mach number plot: • • • •

6-12

Click Go To Load Data In the Data tab select Mach Number from the Calculated Scalar Data list Click Get Data Click Replot in the main pro-STAR window to display Figure T6.1-8

Version 4.02

Tutorial 6.1



Figure T6.1-8

Mach number contour plot

The extent of the solution accuracy improvement can be demonstrated by creating a graph of pressure on the wing and comparing it with similar data produced using the coarse mesh: • • • • • • • • • • •

In the Load Data panel, choose Data Type Boundary and Smooth Option On Select Pressure from the Scalar Data list Choose Absolute from the Press. Ref. list Click Get Data Select Go To > Field Data Click Graph Reset Choose Yes in the box that appears Choose Select data along Entire Cell Set In the Data Type tab, select Post 4 from the Post data to load pop-up menu In the Graph Data section, select Graph data vs. X-axis To isolate the wall shells, type the following in the I/O window: CSET NEWS TYPE 13

•

Also add some of the shells on the symmetry boundary to the set: CSET ADD GRAN -1.5 12.0 -0.01 0.01

•

In the Field Data panel, click Create Graph

The graph that now appears is not particularly useful. This is because data are sorted by cell number rather than by position. To sort the data by position on the x-axis and improve the plot appearance change the graph formatting as follows: • Version 4.02

Click Go To Customize Graph 6-13

Tutorial 6.1



• • • • • • •

Under the Registers tab, click Register Operations In the Graph Register Operations dialog, click Sort Data... Enter 3, 1, 9 and 1, in that order, in the four boxes of the Graph Sort dialog Click Apply and then Close Close the Graph Register Operations dialog Under the Axis tab, select the X-Axis Parameters sub-tab Enter appropriate values in the various text boxes, as shown below:

• •

Click Apply Select the Y-Axis Parameters tab and enter the details shown below:

•

Click Apply and then Redraw

The wall pressure data from the coarse mesh are stored in file coarse.xy. This is also provided with the STAR-CD installation and should be copied to your current directory. To plot both sets of data onto a single graph: • • • •

6-14

Select Go To > External Data Use the file browser at the top of the External Data panel to locate the coarse.xy file Choose xyxyxy for Establish x-y pairs Click Create Graph to display Figure T6.1-5

Version 4.02

Tutorial 6.1



Figure T6.1-9

Graph of wall pressure along the wing

Even through the results from the fine mesh show some oscillations near the shocks, the improvement in their sharpness is dramatic when compared to those from the coarse mesh. •

Version 4.02

Quit pro-STAR by selecting File > Quit > Quit, Nosave

6-15

Tutorial 6.1



6-16

Version 4.02

Introduction

Tutorial 7 MULTIPLE ROTATING REFERENCE FRAMES Introduction This tutorial outlines the steps needed to set up and run a rotating radial fan analysis. It uses the multiple rotating frame methodology (implicit formulation), a steady-state approach involving two or more frames of reference that can be stationary or spinning. In this case, two frames are used to perform the analysis — a spinning one representing the fan and blades and a stationary one representing the fan body and inlet. Physical Problem Description The radial fan geometry to be used is shown below:

Figure T7.0-1

Radial fan geometry

The fan consists of three parts: the inlet pipe leading into the main solution domain, the rotating fan body and blades, plus the stationary body section leading to the outlet. The model’s mesh is saved in three separate Nastran files corresponding to each of the above parts. The spinning effect of the fan axis will be ignored in the inlet section but will be accounted for in the rotating housing. Baffle cells are used to represent the 12 equally-spaced blades. The rotation speed is 2,000 RPM and the fluid within the fan is air at atmospheric conditions.

Version 4.02

7-1

Tutorial 7.1

ROTATING-FRAME FAN ANALYSIS


Tutorial 7.1


The tutorial aims to show the user how to: • • • • •

Import grids from CAD files Create and transform cell couples between mismatched grid regions Define multiple rotating reference frames Define rotating and non-rotating walls Change the coordinate reference frame for vector plots

Pre-Processing Preliminaries Create a sub-directory for the tutorial. The mesh for this case is supplied as three separate Nastran files, inlet.nas, fan.nas and body.nas, corresponding to the three fan regions mentioned earlier. Therefore, before starting the tutorial, make sure that the supplied files are copied into your current directory. • • • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, fan_mrf) in the Casename text box Click Continue In the main window, select File > Model Title In the Title text box type: RADIAL FAN SIMULATION USING MULTIPLE ROTATING FRAMES

• •

Click Apply If the STAR GUIde window does not appear on screen automatically, open it by clicking the STAR GUIde button on the main window

This completes the preliminary steps for this tutorial. Setting the Analysis Type

The first operation is to set the analysis type for rotating machinery, as follows: • • •

In the STAR GUIde window, open the Select Analysis Features panel Select option On from the Rotating Reference Frame Status menu Click Apply

Note that an additional folder called Rotating Reference Frames now appears in the NavCenter tree. The implicit solution option will be chosen later on using a panel within this folder. Mesh Import

You can now continue with importing the grid to be used in the analysis. It is assumed that its three parts have been created separately and that there is no continuity between them. In other words, the mesh blocks are not joined together with common vertex numbering at the block interfaces. To import the Nastran files: • • • •

7-2

In the STAR GUIde window, select the Create and Import Grids folder and then open the Import Grids panel Select the Nastran option for Format Select Type in the Option menu (for cell table types) Use the selector button to select file inlet.nas for the Bulk Data File Version 4.02

Tutorial 7.1


Pre-Processing Mesh Import

•

Click Import Grid

Following this last operation, the I/O window will indicate that the numbers of nodes (vertices) and elements (cells) that were read in were 7128 and 5760, respectively. The current maximum values of vertices and cells in pro-STAR after reading in the mesh are also shown — in this case they are the same as for the original mesh. These values must be used as offsets for the next Nastran file import, so that the second part of the mesh does not re-use the vertex and cell numbers assigned to the first part. Read in the next part of the mesh: •

• •

Turn on the Add to End option. Note that the Vertex Offset and Cell Offset values are automatically set to mxv and mxc, respectively. These parameters are internal functions that provide the current highest value + 1 for the entity of interest. In this case, mxv will be interpreted as being equal to 7129 and mxc equal to 5761. The user can supply alternative values if desired. Use the selector button to select file fan.nas for Bulk Data File Click Import Grid

Again, the I/O window provides the maximum vertex and cell numbers after import is complete. The final part of the mesh is then imported as follows: • •

Use the selector button to select file body.nas for Bulk Data File Click Import Grid

This completes the import process. You should check the cell table indices set up during the mesh import. •

Click the CTAB button on the main pro-STAR window to open the Cell Table Editor dialog and inspect its contents. Alternatively, issue the CTLIS,ALL command in the I/O window which results in the output shown below:

Figure T7.1-1

Cell table listing

As can be seen, there are four cell types defined: three for fluid cells and one for baffle cells. These cell types were defined within the Nastran files and represent the following mesh regions: 1. Fluid cells within the rotating fan body 2. Fluid cells within the stationary fan body 3. Baffle cells representing the fan blades Version 4.02

7-3

Tutorial 7.1


Pre-Processing Cell Type Properties

4. Fluid cells within the stationary fan inlet duct You may now inspect the mesh visually as follows: • • • • •

In the main pro-STAR window, select C > All Change the mesh orientation by selecting Plot > Up Axis > Z Change to an isometric viewing direction by selecting View > Isometric > 1,1,1 Click Cell Plot Select cell plot type Quick Hidden Line; this will allow you to see the fan blades inside the mesh, as shown in Figure T7.1-2

Figure T7.1-2

Cell Type Properties

Imported grid

The cells in each part of the mesh must now be correctly defined and named so that each fan component can be clearly distinguished from the others. To determine what kind of cells have been created by the import process: •

Select option Utility > Count > Cells

As mentioned in the “Mesh Import” section, cells in the rotating fan body have a cell table index of 1. Cells in the stationary body domain have cell table index 2 and those in the inlet pipe index 4. Cells with index 3 are interpreted as baffles representing the fan blades among the rotating cells. The desired modifications to the cell type parameters may be done via the cell table editor, as follows: • • • 7-4

In the main pro-STAR window, click CTAB to open the Cell Table Editor dialog Check that table entry #1 is selected in the scroll list Change the Spin Index value to 2 Version 4.02

Tutorial 7.1



• •

Enter ROTATING_FAN in the Name box Click Apply

The above actions assign a spin index of 2 to the rotating fan body cells. All other cells will have the default spin index of 1. These will be defined later as the spinning and stationary frames of reference, respectively. Next, change the settings for cell type no. 2, corresponding to the stationary body cells: • • • •

Select table entry #2 in the scroll list Change the Color Table Index to 3 (green) Enter BODY in the Name box Click Apply

Note that the spin index is left at a value of 1, so that the ‘BODY’ cells will remain stationary. Check the properties of cell type 3: • • • • •

Select table entry #3 in the scroll list Check that the Cell Type setting is Baffle Check that the Color Table Index setting is 4 (blue) Enter FAN_BLADES in the Name box Click Apply

Note that the baffle spin index may be left at 1; this is because they are already part of the spinning fan body and thus do not require a spin index setting. In fact, pro-STAR will not allow you to change the spin index for a baffle-type cell. Finally, the inlet pipe (type 4 cells) can be modified: • • • • •

Version 4.02

Select table entry #4 in the scroll list Change the Color Table Index to 5 (cyan) Enter INLET in the Name box Click Apply and then Close In the main pro-STAR window, click Replot and notice the change in cell colours in the model, shown in Figure T7.1-3

7-5

Tutorial 7.1


Pre-Processing Mesh Structure

Figure T7.1-3

Mesh Structure

7-6

Fan model grid showing cell colour changes

In their present form, the three mesh parts are not joined together. As mentioned earlier, the imported mesh is not continuous in the areas where the rotating fan body meets the stationary inlet and body mesh. This can be clearly seen in the zoomed-in view shown in Figure T7.1-4 below.

Version 4.02

Tutorial 7.1


Pre-Processing Mesh Structure

Mismatched Grid Areas

Figure T7.1-4

Mismatched grid areas in the model

The three meshes should therefore be joined together using pro-STAR’s cell-face matching and couple creation facilities, as described below: • •

In the STARGUIde window, locate the Create and Import Grids folder and open the Assemble Grids panel Go to the Create Couples tab

Begin by joining the rotating region (cell type 1) to the stationary body region (cell type 2). • • • • •

Check that the Choose Cells option is set to Cell Set Select Choose Cell Types from the Master/Slave Option menu Change the Master Cell Type to Specify and enter 1 in the adjacent box Change the Slave Cell Type to Specify and enter 2 in the adjacent box Click Apply. The I/O window feedback should indicate that 720 couples were created along the interface between the two regions.

Next, repeat the steps above in order to couple the rotating region to the stationary inlet region (cell type 4): • •

Version 4.02

Change the Slave Cell Type value to 4 Click Apply. The I/O window feedback should indicate that a further 648 couples were created along the second interface. 7-7

Tutorial 7.1


Pre-Processing Boundary Location

•

In the main pro-STAR window click Cell Plot to display the joined-up mesh, as shown in Figure T7.1-5 below.

Figure T7.1-5

Fan model grid display with coupled cells

Complete the mesh re-structuring process by using pro-STAR’s couple transformation facility. This creates additional cell faces at the junction between rotating and stationary regions, resulting in a mesh with one-to-one cell face connectivity and the elimination of all cell couples. • • •

Boundary Location

As well as the normal inlet and pressure outflow boundaries, a spinning wall condition needs to be applied to those areas of the stationary fan casing that form part of the rotating mesh. Such wall boundaries must be defined as spinning in the opposite direction to the fan rotation in order to produce a stationary wall relative to the flow. An effective way of locating the counter-spinning boundary regions is given below, where use is made of various cell and vertex set options that help identify their edges. First, create a new cell set containing just the rotating and inlet cells: • • •

7-8

In the main window, select Tools > Couple Tool Click Couple Transform Verify the result of this operation by selecting Cp > All from the main window. The I/O window feedback should verify that no couples were found in the model.

Select C > New > Type... and click on any of the rotating (red) cells Without plotting the new set, select C > Add > Type... and click on any of the inlet (cyan) cells Click Cell Plot Version 4.02

Tutorial 7.1



Now isolate the edge vertices of the above cell set and display them on screen: • •

Select V > New > Cell Set Edge Turn on the vertex display by clicking the Vertex Cell Plot Display button to display Figure T7.1-6

Figure T7.1-6

Inlet and rotating cell types showing edge vertices

Next, remove the inlet cells from the cell set; also remove vertices that are no longer part of this new cell set from the vertex set: • • •

Select C > Unselect > Type... and click on any one of the cyan inlet cells Select V > Subset > Cell Set Click Cell Plot to display the red rotating cells and the set of vertices that describe the edges of the counter-spinning wall boundaries

We are now in a position to define a separate region for these boundaries. • •

In the main window, change the viewpoint to be along the negative Z direction by choosing View > Axis > -Z In the STAR GUIde window, go to the Locate Boundaries folder and open the Create Boundaries panel

Follow the instructions below to specify the wall boundaries in four stages. The first stage defines boundaries on the bottom surface of the fan using the ZONE method. The last three stages use the FIND method to generate boundaries from a starting seed vertex on the surface. In the Create Boundaries panel: • • • Version 4.02

Select Reg#3 in the Boundary Regions scroll list Select Wall as the boundary Type from the pull-down menu below Click Define Region 7-9

Tutorial 7.1



• •

Click Select a Zone Draw a polygon around the entire visible mesh. This will define the fan base as part of boundary region 3.

1,152 new boundaries should be created by this method. Next: • • •

In the main window, change the view back to isometric using View > Isometric > 1,1,1 In the Create Boundaries panel, click the Surface Based on Vset button Use the cursor to pick a vertex anywhere between the two concentric rings of vertices at the top of the visible mesh

An additional 576 boundaries should be created by the above operation. Note that in this particular example, the core axle will be considered as spinning with the fan, so no additional boundaries need to be defined in that location. The inlet and pressure boundaries will be defined next. Start by restoring a view of the entire model: • • • •

In the main window, select C > All Change the plot type to Hidden Surface Turn off the Vertex display option button Click Cell Plot

To define the inlet boundary: • • • • •

Go to the Create Boundaries panel and select Reg#1 in the Boundary Regions scroll list Select Inlet as the boundary Type from the pull-down menu Click Define Region Click Surface Based on Edges Pick a vertex on the top surface of the inlet pipe

Define the pressure boundary in a similar way: • • • • •

7-10

Select Reg#2 in the Boundary Regions scroll list Select Pressure as the boundary Type from the pull-down menu Click Define Region Click Surface Based on Vset Pick a vertex on the surface of the outlet plane, as shown in Figure T7.1-7

Version 4.02

Tutorial 7.1



Select a Vertex Here

Figure T7.1-7

Pressure boundary definition

To view all the boundaries created: •

Turn on the boundary display option by clicking the Bound button. The result is shown in Figure T7.1-8

Figure T7.1-8

Version 4.02

Boundary regions displayed on top of the mesh

7-11

Tutorial 7.1


Pre-Processing Spin Parameters

•

Turn off the boundary display by clicking the Bound button again

This completes the boundary set-up stage. Spin Parameters

The rotating frame of reference in this case should be defined with respect to the Zaxis of the global cylindrical coordinate system. Check where the origin of this system is positioned within the model: • • • • •

Click the CSYS button in the main pro-STAR window to display the Coordinate Systems dialog Select coordinate system Number 2 in the scroll list Click Show Triad Click Close Position the viewpoint above the mesh by selecting View > Axis > +Z

The triad for the global cylindrical coordinate system shows that the origin is positioned on the fan axis and that its Z-axis runs parallel to it. Therefore, this system is correctly aligned and positioned for the model’s purposes. Had this not been the case, a new local cylindrical coordinate system would have had to be defined (via the Coordinate Systems dialog) whose Z-axis would be the axis of rotation. We can now specify the implicit solution option and spin parameters for the analysis as shown below. For this case, cells with a spin index of 1 are to be stationary (ω = 0) while those with a spin index of 2 are to have an angular velocity of 2000 r.p.m. • • • • • • • •

In the STAR GUIde window, go to the Rotating Reference Frames folder and open the Rotating Reference Frames panel Select option Multiple Frames - Implicit from the Reference Frame Treatment menu Select Spin Index 1 in the Spin Parameters scroll list In the boxes at the bottom of the panel, enter a value of 0 for Omega and 2 for Co-ord. Sys Click Apply Select Spin Index 2 Enter a value of 2000 for Omega and 2 for Co-ord. Sys Click Apply

The implicit solution method for this multiple rotating reference frame problem has now been set up. All cells with a spin index of 2 will be treated as rotating at 2000 r.p.m., while those with the default setting of 1 will remain stationary. Material Properties

Check the properties of the fluid present in the model. The default fluid for material no. 1 in pro-STAR is air at standard pressure and temperature. Therefore its molecular properties do not need to be altered and you can go directly to setting up the turbulence model. • • • •

7-12

Open the Turbulence Models panel in STAR GUIde by selecting the Thermophysical Models and Properties and Liquids and Gases folders Select the On switch for turbulence modelling Choose the K-Epsilon/High Reynolds Number option Click Apply Version 4.02

Tutorial 7.1



Set up some essential monitoring and reference parameters: • • • • Boundary Conditions

Open the Monitoring and Reference Data panel Enter 20938 for the Monitoring cell number Enter 5669 for the Reference Pressure Cell Number Click Apply

An inlet velocity of 5 m/s will be specified, with all flow leaving the fan through the pressure outlet. • • • • • •

Locate the Define Boundary Regions panel in the Define Boundary Conditions folder Select Reg# 1 Inlet in the Boundary Regions scroll list Enter a value of -5 for the W-velocity component Select option TI/Length from the Turb. Switch menu Enter a Turb. Intensity of 0.05 and a Length of 0.001 Click Apply

The pressure boundary is defined next: • • • • • •

Select Reg# 2 Pressure in the Boundary Regions scroll list Choose the Static pressure Option Retain the default relative pressure (0) at the boundary. This means that the absolute pressure at the boundary is equal to the reference pressure. Select option TI/Length from the Turb. Switch menu Enter a Turb. Intensity of 0.05 and a Length of 0.001. These values would be used if there is any inflow through the boundary faces. Click Apply

Finally, define conditions at the counter-rotating wall regions: • • • •

Select Reg# 3 Wall in the Boundary Regions scroll list Enter 2 for the Coord. System defining the axis of rotation Enter -2000 for Omega Click Apply

Turning on the boundary display by clicking Bound in the main window enables you to verify the boundary conditions entered above. Check that an inflow velocity component is displayed across the inlet plane, plus a rotational component on each of the boundaries on the counter-rotating part of the wall. This can be most easily done by selecting each region in turn and displaying it. Analysis Controls

Most of the default control parameters are adequate for the analysis to follow. The only items that need to be modified are concerned with solution output. • • • • •

Version 4.02

In the STAR GUIde window, select the Analysis Controls folder followed by the Output Controls sub-folder Open the Analysis Output panel Set the Solution Output Frequency to 10 Select Additional Output item Shear Force and then click the Post button Click Apply 7-13

Tutorial 7.1


CFD Analysis Running the Model

The actions above will tell STAR to update the solution data file every 10 iterations and write wall shear forces as well as the normal flow field variables into it. Running the Model

Set the run time controls, i.e. the maximum number of iterations to be performed, for this case: • • •

Go to the Analysis Preparation/Running folder and open the Set Run Time Controls panel Set the Number of Iterations to 200 Click Apply

The solution should satisfy the convergence criteria within 200 iterations. Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR as shown below. Alternatively, you may run STAR interactively as described in the next section. • • • • • •

In the main window, select File > Write Geometry File Check that the Scale Factor is set to 0.001, as the geometry was originally specified in millimetres Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit


Select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that the Scale Factor is 0.001 Click Start New Analysis

The analysis will then start automatically and will converge within the 200 iteration limit. Convergence information can be viewed while the analysis is still running by using the StarWatch utility. Results may also be viewed part-way through the analysis by using the Post-Processing facilities in the STAR GUIde window. Post-Processing First, display a plot of the velocity vectors on the mesh surface: • • • • • • • 7-14

Select folder Post-Processing Open the Load Data panel to display the File(s) tab Click Open Post File In the Data tab, select Velocity Components UVW from the Vector Data list Click Get Data Select Go To > Create Plots In the 3-D Surface tab, select options Vector and Edge Version 4.02

Tutorial 7.1



• •

Click Plot To Screen Select View > Isometric > 1,1,1 to display Figure T7.1-9

Figure T7.1-9

Velocity vectors displayed on the mesh surface

This plot is not an accurate depiction of the flow field because the reference frame in which the results are presented is, by default, the computational frame. This means that, within the rotating mesh region, the results are viewed from the perspective of someone spinning with the fan blades, i.e. a component equal to rω is automatically subtracted from the velocity magnitude. This is apparent upon close examination of this region. To obtain a velocity vector plot with all velocities measured relative to the same frame, a stationary reference frame needs to be selected prior to any results being loaded into pro-STAR. To do this: • • • • • •

Version 4.02

Select the Coordinate Systems tab in the Load Data panel. This controls the reference frame in which the solution is viewed. Select the Static option Click Apply Go to the Data tab and select Velocity Components UVW from the Vector Data list Click Get Data Click Replot in the main pro-STAR window to display Figure T7.1-10

7-15

Tutorial 7.1



Figure T7.1-10

Velocity vectors relative to a static reference frame

The difference between the plots is apparent in the displayed maximum velocity. Now display contour plots of some scalar flow parameters in a plane bisecting the main flow region (inlet region excluded). • • • • • • • • •

7-16

In the Data tab, select Smooth Option On Select Pressure from the Scalar Data list Click Get Data Select Go To > Create Plots In the Section Clipped tab, select Contour(filled) and None To define the plane, enter 0, 0, 34 as the Point and 0, 0, 1 as the Normal parameters Click Apply Click Plot To Screen Select View > SNORMAL to display Figure T7.1-11

Version 4.02

Tutorial 7.1



Figure T7.1-11

Pressure contours displayed in a plane parallel to the inlet plane

Note that the relative pressure at the pressure boundary is roughly zero. Now display the turbulence kinetic energy distribution: • • • •

Version 4.02

Click Go To Load Data Select Turb Kinetic Energy from the Scalar Data list Click Get Data Click Replot to display Figure T7.1-12

7-17

Tutorial 7.1



Figure T7.1-12

Final Operations

7-18

Contours of turbulence kinetic energy

End the pro-STAR session: •


Version 4.02

Tutorial 8 LAGRANGIAN TWO-PHASE FLOW The next two tutorials model steady and transient Lagrangian two-phase flow with fuel spray injection. The model geometry consists of an intake port and part of a cylinder for an idealised internal combustion engine, with an intake valve separating the two regions. The air inlet and pressure boundary are shown in Figure T8.0-1. Also shown is the fuel spray injector, located between the inlet and the valve.

Injector

Inlet

Pressure boundary

Figure T8.0-1

Version 4.02

Engine intake port geometry

8-1

Tutorial 8.1

STEADY FLOW WITH FUEL SPRAY INJECTION


Tutorial 8.1


This tutorial is intended to show the user how to: • • • • • • •

Set up a steady-state Lagrangian two-phase problem Choose droplet thermophysical models Model droplet evaporation Define a spray injector Display droplet plots Use the Overlay plotting option Display animated and still plots of particle tracks

Physical Problem Description In this tutorial, a constant stream of air flows into the chamber at 5 m/s. A nozzle, positioned 5 mm away from the inlet and near the centre of the channel, injects heptane droplets into the air stream at a mass flow rate of 0.001 kg/s. The nozzle has a diameter of 1 mm and emits the droplets in a spray cone with an angle of 10o. The droplets are grouped into 50 parcels; this number is chosen as a reasonable compromise between computational cost and solution accuracy. Outflow occurs through a notional pressure boundary shown in Figure T8.0-1, and gravity is assumed to be acting in a direction normal to it. All walls in the model are at a fixed temperature of 400K, while the incoming air and heptane fuel are at 350K. The fuel is assumed to evaporate instantly upon contact with the walls. Pre-Processing Preliminaries Create a sub-directory for this tutorial called tut8-1. The mesh filling the model geometry has already been created and the relevant data may be found in the cell, vertex, boundary and problem files supplied for the tutorial (files intake.cel, intake.vrt, intake.bnd and intake.inp). Copy these files into your working directory. Start pro-STAR and enter the case name: • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say intake_ss) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is intake.inp Click Apply Click Close

This will read in the mesh geometry and boundary locations, plus some basic problem settings. Now name the model: • 8-2

In the main pro-STAR window, select File > Model Title Version 4.02

Tutorial 8.1



• • Mesh Checking

Type STEADY FLOW WITH LIQUID SPRAY INJECTION in the Title box Click Apply

Check the imported polyhedral mesh visually: • • •

Select C > All Change the viewpoint by selecting View > Isometric > -1,-1,1 Click Cell Plot to display Figure T8.1-1

Figure T8.1-1

Mesh geometry

Analysis Features

Specify that the problem involves Lagrangian two-phase flow:

Material Properties

Turn on gravity and specify its magnitude and direction:

• • •

• • • •

In the STAR-GUIde window, open the Select Analysis Features panel Under Multi-Phase Treatment, select Lagrangian Multi-Phase Click Apply. You should notice that an extra folder will now appear in the STAR-GUide tree.

Select the Thermophysical Models and Properties folder and then open the Gravity panel Enter a value of 9.8 m/s2 in the Acceleration box Check that the Coordinate System is set to 1 and that the Direction of Gravity Force is 0, 0, -1 Click Apply

The default fluid for the continuous phase is air, so its molecular properties do not require alteration. However, turbulence and thermal models still need to be Version 4.02

8-3

Tutorial 8.1


Pre-Processing Scalar Definition

specified: • • • • • •

Select the Liquids and Gases folder Open the Turbulence Models panel and turn On turbulence modelling Select the k-Epsilon/High Reynolds Number model from the pull-down menu Click Apply Open the Thermal Models panel and select Temperature Calculation On Click Apply

Specify the monitoring and pressure reference cells: • • • • Scalar Definition

Assign scalar no. 1 to the product of droplet evaporation, i.e. heptane vapour, and import its physical properties from pro-STAR’s built-in database: • • •

• •

Dispersed Phase Models

Select the Additional Scalars folder Open panel Molecular Properties (Scalar) Check that the Scalar # slider at the bottom of the panel is set to 1 and then choose option Select scalar from database from the menu at the top of the panel Select the appropriate physical substance, HEPTANE(V) in this case, from the Scalar Database scroll list and then click Select Scalar The physical properties of heptane vapour are read in from pro-STAR’s property database and entered into the appropriate boxes of panel Molecular Properties (Scalar). Check that the displayed values are reasonable and then click Apply.

Now specify the properties of the dispersed phase using the Lagrangian Multi-Phase folder: • • • • • • • • • • • •

8-4

Open the Monitoring and Reference Data panel Enter 10054 for the Monitoring cell number. This cell is near the valve. Enter 4337 for the Reference Pressure Cell Number. This cell is adjacent to the pressure boundary. Click Apply

Open the Droplet Controls panel and check the default settings, all of which are appropriate for this problem Open the Droplet Physical Models & Properties panel Under the Global Physical Models tab, turn On Turbulent Dispersion Turn On Gravity Effects Click Apply Under the Droplet Physical Models tab, select Standard Momentum Transfer Change the Slip Factor to 0 For Mass Transfer, select option Standard For Heat Transfer, select option Standard Select the Reitz Droplet Breakup model In the Droplet-Wall Interaction section, set the droplets to Evaporate upon contact with the walls Click Apply Version 4.02

Tutorial 8.1


Pre-Processing Injector Properties

• • • • • • • Injector Properties

Under the Droplet Properties tab, click Select from Database Choose # HEPTANE(L) as the droplet material from the Choose Database Material list Click Select Material, then Close Change the Saturation Pressure to 1e5 Pa Specify the previously-defined scalar (HEPTANE(V)) as the product of evaporation by clicking the Select button next to Evaporates to Scalar Click on scalar 1 in the list and click Close Click Apply in the Droplet Properties tab

The droplet thermophysical models and properties are now fully defined, so move on to specifying the properties of the spray injector. First, though, a new coordinate system needs to be defined, centred at the injection point: • • • •

• • • •

In the main pro-STAR window, click the CSYS button Select number 4 from the Coordinate System List Select Cylindrical from the pull-down menu at the bottom left of the Coordinate Systems box Enter the following values in the seven boxes to the right of this menu: 100, 19, 35, 0, 0, -100, 0. These position the coordinate system’s origin at the injector location. Click New (Global) Click Show Triad Close the Coordinate Systems dialog Click Cell Plot

The triad for the newly-defined coordinate system should now be visible at the start of the refined mesh region. The spray cone will be centred around its Z-axis. Now enter the spray injector properties: • • • • • • • • • • Boundary Conditions

Specify the fixed wall temperature: • • • • •

Version 4.02

Open the Spray Injection with Atomisation panel The default Spray Options are satisfactory, so click Apply Spray Options Change the Injection Temperature to 350 K Change the Hole Diameter to 0.001 m Enter 4 for the injector Coordinate System Check that the Cone Angle is set to 10o Enter a Mass Flow Rate of 0.001 kg/s Change the Number of Parcels/Injector to 50 Check that the Droplet Type is number 1, Heptane (L) Click Update Injector

Go to the Define Boundary Conditions folder and open the Define Boundary Regions panel Select Region 0 from the boundary regions list Change the Wall Heat option to Fixed Enter 400 in the Temp. (K) box Click Apply

8-5

Tutorial 8.1



The inlet velocity and temperature also need to be specified: • • • •

Select Region 1 from the boundary regions list Enter a U velocity of -5 m/s Change the Temp. to 350 K Click Apply

The mean temperature and heptane mass fraction at the pressure boundary are estimated on the basis of temperatures and mass flow rates at the inlet and in the injector. To specify these values: • • • • • • • Run Time Controls

Select Region 2 from the boundary regions list Change the Temp. to 360 K Click Apply Open the Scalar Boundaries panel Select Boundary Region 2, Pressure, from the list Change the Mass Fraction value to 0.155 Click Apply

Increase the maximum number of iterations to allow the analysis to converge: • • • •

Final Operations

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Change the Number of Iterations to 200 Click Apply

The pre-processing task for this tutorial is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • • •

In the main pro-STAR window, select File > Write Geometry File Check that the Scale Factor is set to 0.001, as the geometry was created in millimetres Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit


Select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Choose Double Precision and check that the Scale Factor is 0.001 Click Start New Analysis

The analysis will then start automatically. The solution should satisfy the default convergence criteria within the specified maximum number of iterations. 8-6

Version 4.02

Tutorial 8.1



Post-Processing Preliminaries Read in the analysis results: • • • Continuous Phase

In the Post-Processing folder, open the Load Data panel Check that intake_ss.ccm is displayed in the Steady State Post File box Click Open Post File

Plot velocity vectors on a plane bisecting the valve: • • • • • • • • •

Go to the Data tab and select Velocity Components UVW from the Vector Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select Vector and Edge Define the cross-section plane by entering 0, 19, 0 for the Point and 0, 1, 0 for the Normal values Click Apply and then Plot to Screen Under the Vectors tab, change the Scale Factor to 0.5 Click Apply In the main pro-STAR window, select View > SNORMAL to display Figure T8.1-2

Figure T8.1-2

Velocity vectors on a plane bisecting the valve

Now create a temperature contour plot on the same plane: • • • • Version 4.02

Click Go To Load Data Select Data Type Cell Turn On the Smooth Option Select Temperature from the Scalar Data list 8-7

Tutorial 8.1


Post-Processing Continuous Phase

• • • •

Click Get Data Select Go To > Create Plots Under the Section Clipped tab, choose Contour (filled) and Edge Click Plot To Screen to display Figure T8.1-3

Figure T8.1-3

Temperature contours on a plane bisecting the valve

In addition, plot contours of the heptane vapour mass fraction: • • • •

8-8

Click Go To Load Data Select C7H16 from the Scalar Data list Click Get Data Click Replot to display Figure T8.1-4

Version 4.02

Tutorial 8.1


Post-Processing Dispersed Phase

Figure T8.1-4

Dispersed Phase

Contours of heptane vapour concentration on a plane bisecting the valve

The dispersed phase can be visualised by creating droplet plots. In this instance, the droplet tracks will be plotted on top of the previous contour plot of heptane vapour concentration using the Overlay option: • • • • • • • • •

In the Post-Processing folder, open the Particle Tracks sub-folder Open the Plot Droplets/Particle Tracks panel In the Load Droplet Data section, choose Load From Track File and accept the default intake_ss.trk file Click Load Data In the Droplet Plot Options section, select Off under Edge Plot Options Select a Diameter dependent Droplet Radius and enter 1.0 as the Size Select None from the Vectors pull-down menu Click Apply In the interests of display clarity, select a subset of the computed droplet tracks by typing the following command in the I/O window: DSET NEWS DRAN 2 50 3

• •

Select Plot > Display > Overlay from the main pro-STAR window’s menu bar to turn on the Overlay option Enter command PLFIX ON

•

Version 4.02

in the I/O window to prevent the display from automatically adjusting to the scale of the plot that follows Click Droplet Plot to display Figure T8.1-5

8-9

Tutorial 8.1



Figure T8.1-5

Heptane droplets overlaid onto a heptane vapour concentration plot

The droplets can also be displayed as particle tracks: •

Turn off the Overlay and Plot Fix options by entering the following commands in the I/O window: OVERLAY OFF PLFIX OFF

• • • • • • • •

8-10

Return to the Load Data panel and, under the File(s) tab, click Open Post File Select Geometry Plot and Quick Hidden Line as the plot attributes in the main pro-STAR window Click Cell Plot Go back to the Plot Droplets/Particle Tracks panel and select the Particle Tracks tab Select Display Option Segments Click Plot Tracks to produce an animated display of the droplet trajectories Select Display Option Continuous Click Plot Tracks to display Figure T8.1-6

Version 4.02

Tutorial 8.1



Figure T8.1-6

Particle tracks showing paths of heptane droplets

Figure T8.1-5 and Figure T8.1-6 show that all droplets evaporate before they reach the cylinder. This leads to the cool region of high heptane vapour concentration near the valve and low concentration in parts of the cylinder. The region of high concentration can be shown effectively in three dimensions by plotting an isosurface: • • • • • • • • •

Version 4.02

Go back to the Particle Tracks tab of the Plot Droplets/Particle Tracks panel Click Clear Tracks Open the Create Plots panel Under the IsoSurf tab, select Edge On Enter a Value of 0.3 Click Apply In the main pro-STAR window, select a Quick Hidden Line plot Click Cell Plot to display Figure T8.1-7 Rotate the view to examine the details of the isosurface shape

8-11

Tutorial 8.1



Figure T8.1-7

Final Operations

8-12

Isosurface of heptane vapour concentration with mass fraction = 0.3



Version 4.02

Tutorial 8.2

TRANSIENT FLOW WITH FUEL SPRAY INJECTION


Tutorial 8.2


This tutorial is intended to show the user how to: • • •

Set up a transient Lagrangian two-phase flow problem Produce on-screen animations using command loops Save screen shots for creating animations externally

Physical Problem Description The problem geometry and flow conditions in this tutorial are the same as in Tutorial 8.1. However, the injection is more complex, with the heptane fuel no longer injected in a constant stream but in two short bursts. For the first burst, the mass flow rate through the injector starts at 0.001 kg/s (the mass flow rate in the steady-state solution) and then falls linearly to 0.0001 kg/s. The same pattern is then repeated for the second burst. The total injection period is 0.05 s. Pre-Processing Preliminaries Create a sub-directory for this tutorial called tut8-2. Most of the case set-up has already been performed in Tutorial 8.1 so the model file, intake_ss.mdl, should be copied across to the new working directory and renamed intake_tr.mdl before continuing. Start up pro-STAR and open the model file: • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Check that the case name is intake_tr and that the Resume existing .mdl file option is selected Deselect the append to .echo file option Click Continue

Now change the model title: • •

Select File > Model Title... In the Title box, enter TRANSIENT FLOW WITH LIQUID SPRAY INJECTION and click Apply

Analysis Features

Change to a transient analysis setting:

Injector Properties

The injector position and droplet properties have already been defined in the previous tutorial. However, the flow rate profile during the injection period must be created from scratch:

• • •


In the STAR-GUIde window, open the Select Analysis Features panel Select Transient as the Time Domain Click Apply

Click on the Lagrangian Multi-Phase folder Open the Spray Injection with Atomisation panel 8-13

Tutorial 8.2


Pre-Processing Analysis Output

• •

• • • • • •

In the Define Injectors section, select Table from the Mass Flow Rate pull-down menu and click the New button displayed to its right The Table Editor should now appear. Enter the data shown below:

Click Write Table, then Graph to display Figure T8.2-1 Close the Table Editor Click the file browser button in the Spray Injection with Atomisation panel to display the available injection table files Choose intake_tr.tbl from the Files list and then click OK. The selected file will now appear in the file name box. Change the Number of Parcels/Injector to 1000 /s Click Update Injector

Figure T8.2-1

Analysis Output

Instruct STAR to write the analysis results in the transient post data file (intake_tr.pstt) at every single time step. In addition, specify what cell data (including scalar variable data) are to be written during the run. • • •

8-14

Graph showing the mass flow rate profile over the injection period

Go to the Analysis Controls folder and select sub-folder Output Controls Open the Analysis Output panel and then select the Transient tab Specify the frequency of writing data to the transient post file by typing 0.001 Version 4.02

Tutorial 8.2


CFD Analysis Set Run Time Controls

•

in the Write data every box. As discussed below, this is equivalent to outputting data at every time step. As can be seen in the scroll list, velocity and pressure are already selected by default. Change this selection by (a) removing Pressure (b) adding Temperature (c) adding the mass fraction of scalar C7H16

•

In each case, click the Post button to include or exclude the desired item Click Apply

Set Run Time The time interval of interest in this case is 0 ≤ t ≤ 0.05 seconds. Specify that it is to Controls be covered in steps of 0.001 seconds, i.e. 50 time steps in total. • • • • • Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Type 0.05 s in the Run for box Click Apply Type 0.001 s in the Time Step for Period box Click Set period

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the problem and geometry files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

Select File > Write Geometry File Accept the default value, 0.001, shown in the Scale Factor text box Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit


File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Select the Double Precision option for the STAR executable Click Start New Analysis

Inspect the information written in files intake_tr.run and intake_tr.info once the run has finished.

Version 4.02

8-15

Tutorial 8.2



Post-Processing Preliminaries Read in the results of the analysis: • • • • • •

Select folder Post-Processing Open the Load Data panel to display the File(s) tab Select the Transient Analysis option Choose position number 1 in the Transient Post File(s) list Click Add File to List Select the file intake_tr.pstt from the Transient Post File(s) list and click Open Transient Post File

Droplet Plots As in Tutorial 8.1, the droplet plots will be overlaid on contour plots of heptane vapour concentration. A combined plot of this type will be produced for each time step using a command loop. The resulting sequence of plots will then form an on-screen animation. First, set the droplet plot options: • • • • • • •

In the STAR-GUIde window, select the Particle Tracks folder Open the Plot Droplets/Particle Tracks panel Under the Droplets tab, turn Off Edge Plot Options Specify the displayed Droplet Radius to be proportional to the actual droplet Diameter and enter a Size of 1.2 Specify the Fill Color to be dependent upon the Mass Change the Vectors option to None Click Apply

Set the cell plot characteristics: • • •

In the main pro-STAR window, turn on the ‘Edge’ plot option Select Contour Plot and Section (Surface). Ignore the warning stating that no scalar data are stored Enter the commands: SNORMAL 0 1 0 SPOINT 0 19 0

The command loop used to produce the plots will now be entered into the I/O window. It utilises the OVERLAY and PLFIX commands demonstrated in Tutorial 8.1. Also, the CSCALE command is used to enable droplet and contour plots to have different colour scales. •

Enter the following commands: *SET IT 1 1 *DEFINE STORE ITER IT CSCALE 14 USER 0 0.8 GETV CONC CPLOT OVERLAY ON PLFIX ON SCDUMP GIF IT

8-16

Version 4.02

Tutorial 8.2



CSCALE 14 USER 0.4e-7 0.2e-5 GETD POST DSET ALL DPLOT OVERLAY OFF SCDUMP OFF *END *LOOP 1 49 PLFIX OFF The SCDUMP command in the above loop saves a screen shot of each combined plot in a file with extension .gif. It is turned on and off again at each time step because otherwise it would save screen shots of the contour plots as well as the combined plots. The .gif files produced may subsequently be combined into an animation sequence using an external package. For more details on pro-STAR’s animation capabilities, see “Animation Sequence Definition and Display” on page -2 of the Post-Processing User Guide. Final Operations

Version 4.02



8-17


Tutorial 9 COMBUSTION Physical Problem Description A model of an idealised CAN type gas turbine combustion chamber is chosen to familiarise users with STAR-CD’s combustion modelling capabilities and introduce various recommended practices for computing combusting flows. The mesh used in this case is shown in Figure T9.0-1 and was created in Tutorial 7.2 of the Meshing Tutorials volume. The problem geometry consists of three sets of air inlets placed circumferentially at the combustor head to promote maximum mixing and flame stabilisation. Swirling air enters the primary combustion zone through the two sets of inlets nearest to the axis of symmetry. Non-swirling air enters the upper inlet and thence the primary, secondary and dilution zones via five injection holes on the liner. This liner, separating the cooling passage from the main combustion area, is represented in the model by baffle cells. Air is assumed to be composed of 23.2% oxygen and 76.8% nitrogen, by mass, and to be at a pressure of 1 bar and temperature of 293 K throughout this tutorial. Unless stated otherwise, its physical properties are assumed to be as follows: Density Molecular viscosity Specific heat Thermal conductivity

Ideal gas with pressure dependence Pa s 1.81 × 10–5 1006 J/kg K –2 2.637 × 10 W/m K

Only a sixty-degree sector of the combustor is simulated (see Figure T9.0-1). This is achieved by using STAR-CD’s cyclic boundary option which allows the transmission of information across boundaries of this type. To demonstrate the full combustion capabilities of STAR-CD, both gaseous and liquid fuels are employed in the simulation. Gaseous fuels are supplied through an inlet at the combustor head whilst liquid fuels are injected as droplets from a single injector located on the axis. The physical properties of air and fuel and details of the individual simulations are presented in the corresponding sub-tutorials.

Version 4.02

9-1


Figure T9.0-1

9-2

Mesh structure for the combustion chamber model

Version 4.02

Tutorial 9.1

PROPANE COMBUSTION (ADIABATIC PPDF)


Tutorial 9.1


In this tutorial, a propane combustion case is set up using the Presumed Probability Density Function (PPDF) reaction model for unpremixed flames. The model assumes adiabatic conditions (no heat loss) and a local instantaneous chemical equilibrium. The main aim is to: • • • •

Familiarise users with the adiabatic PPDF model setup Demonstrate the use of the CEA package for calculating polynomial coefficients required by the model Evaluate the accuracy of the analysis results and suggest a way of improving them Illustrate the use of user-defined panels as a way of facilitating post-processing operations

For adiabatic PPDF, the physical properties of the fuel (pure propane in this case) are not utilised as no additional transport equations requiring these properties are solved. Temperature, density and species mass fractions are evaluated using the β function formulation outlined in the Methodology volume (see “Presumed-PDF (PPDF) Model for Unpremixed Turbulent Reaction” in Chapter 10). Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut9-1. The mesh for this problem has already been created in the Meshing Tutorials volume (Tutorial 7.2) and the relevant cell, vertex, boundary and problem setup files are already available (files combustor.cel, combustor.vrt, combustor.bnd and combustor.inp, respectively). Therefore, before starting the tutorial, make sure that the supplied files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, PPDF_ad) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is combustor.inp Click Apply Click Close

This will read default problem settings from file combustor.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: PROPANE COMBUSTION (ADIABATIC PPDF)

Version 4.02

9-3

Tutorial 9.1



•

Click Apply

Plot the mesh to confirm the data read in: • • • •

In the main pro-STAR window, select Plot > Up Axis followed by X Select C > All Select View > Isometric > 1, 1, -1 Click Cell Plot

Make sure that the STAR GUIde window is displayed on your screen, next to the main pro-STAR window. If not, activate it by clicking the special ‘Open STAR GUIde’ panel button shown below:

Specify the key feature of this case, i.e. chemically reacting flow: • • • •

Material Properties

In the STAR GUIde window, go to panel Select Analysis Features Select option Chemical Reaction from the Reacting Flow menu Click Apply Select folder Thermophysical Models and Properties and note that an extra sub-folder called Reacting Flow now appears in the STAR GUIde tree. This will be used in this and all subsequent sub-tutorials to supply chemical reaction definitions.

Set up material properties and thermofluid models using the appropriate STAR GUIde panels. The required actions are as follows: 1. 2. 3. 4. 5. 6. • • • • • • • • • • • •

9-4

Select the Ideal Gas Law density variation (with pressure dependence) Select the standard k-ε turbulence model Turn on the temperature solver Set the initial temperature distribution Choose the monitoring cell location Choose the reference pressure and its location Select sub-folder Liquids and Gases Open the Molecular Properties panel Select option Ideal-f(T,P) from the Density menu Click Apply Open the Turbulence Models panel Click On to switch on turbulence modelling Select option K-Epsilon/High Reynolds Number from the model menu Click Apply Open the Thermal Models panel Turn on the solution of the energy equation by clicking Temperature Calculation On Click Apply Open the Initialization panel Version 4.02

Tutorial 9.1


Pre-Processing Combustion Model

• • • • • •

•

• Combustion Model

In the Flow Conditions tab, confirm that a value of 293.0 is displayed in the Temperature box Go to the Turbulence tab and select option TI/Mixing Length from the Turbulence Parameters menu Enter 0.05 and 0.2 in the Intensity and Mixing Length boxes, respectively Click Apply Open the Monitoring and Reference Data panel Choose a monitoring cell location (say, half way between the axis and the outer casing and towards the outlet). This may be done by entering a cell number in the text box. Alternatively, click the ‘mouse’ icon and then use the screen cursor to select the required cell on the mesh plot. In this case, we assume that the chosen cell no. is 1760 Make the reference pressure location the same as the monitoring cell location by entering 1760 in the Reference Pressure Cell Number box. Confirm that 1.0e+5 appears in the Pressure box. Click Apply

Use STAR GUIde’s Reacting Flow folder to set up the combustion model as follows: • • • •

• •

Select sub-folder Reacting Flow followed by Chemical Reactions Open the Scheme Definition panel Select option Unpremixed/Diffusion from the Reaction Type menu Select option PPDF Single Fuel from the Reaction Model menu. Note that scheme no. 1 is selected by default in the Chemical Scheme # slider at the bottom of the panel Accept the Chemical Equilibrium setting in the Option menu and click Apply. A pop-up window will now appear warning you that the default chemical reaction settings will be changed. Click Continue. A message will appear at the bottom of the STAR GUIde panel confirming your combustion model selection.

Continue by using the CEA package to specify the fuel (C3H8) and its combustion products. In a non-adiabatic PPDF model, only chemical species polynomial coefficients are required. These are derived separately using an equilibrium calculation for a mixture of pure propane and air at a temperature of 293 K and pressure of 1 bar. To read these values into pro-STAR, proceed as follows: • • •

•

Version 4.02

Open the Reaction System panel In the Parameter Definition tab, check that option CEA is selected in the Input/Control menu Supply the names of all chemical substances involved plus relevant reaction parameters, as shown below: Pressure — 1.0e+5 Select Stream to Define -> Stream1 (Fuel) and then enter the following data in the boxes underneath: Species Name 1 — C3H8 Mass Fraction 1 — 1 Temperature — 293 9-5

Tutorial 9.1



• •

• •

•

Click Define Stream Select Stream to Define -> Stream2 (Oxidizer) and then enter the following data in the boxes underneath: Species Name 1 — O2 Mass Fraction 1 — 0.232 Species Name 2 — N2 Mass Fraction 2 — 0.768 Temperature — 293 Click Define Stream Go to the All Species scroll list and enter the following data by selecting each species line in turn: 1 — C3H8 2 — O2 3 — N2 4 — CO 5 — CO2 6 — H2O Click Apply

Note that all chemical names, such as C3H8, should be entered exactly as they appear in the material names file (material.list) supplied under the STAR-CD installation directory. Define the basic character of the reaction: • •

Go to the Heat Option tab Check that option Adiabatic is selected in the Heat Option menu

Start up the CEA application: • •

•

Go to the Integration Control tab Check that option Polynomial is selected in the Integration Method menu. Note that all items in the PPDF Dependent Variables list are initially flagged as ‘Undefined’ Click Apply

Updated items will now appear on the PPDF Dependent Variables scroll list. Selecting each item in turn will display the corresponding coefficients in the PPDF Polynomial Coefficients scroll list. Confirm that there are 20 coefficients each for density, temperature and all chemical species involved (CO, CO2, C3H8, H2O, N2, O2). To check these coefficients graphically: •

9-6

Click Graph Data to generate plots of the available data automatically, as shown in Figure T9.1-1

Version 4.02

Tutorial 9.1



Figure T9.1-1

PPDF polynomial coefficient plots

Reset the graph registers before proceeding further • •

In the main pro-STAR window, select Graph > Greset Click OK to confirm your action

The CEA output is passed to pro-STAR which in turn generates suitable scalar variables and maps them automatically to the constituents of the reaction scheme. The reaction scheme is also assigned automatically to the current fluid domain (material no. 1). To check the results of this operation: •

• •

Scalar Properties

Open the Scheme Association panel. Note that chemical scheme no. 1 (the non-adiabatic PPDF defined above) is assigned to material no. 1 (the background fluid in the current domain) Select sub-folder Liquids and Gases in the Thermophysical Models and Properties folder Open the Molecular Properties panel. Note that as a result of the chemical scheme definition, the setting of the Density menu has changed automatically to PPDF.

Check the properties of the scalar variables that were automatically set up by the combustion model’s mapping process, described above: • •

Select sub-folder Additional Scalars and then open the three panels under it in turn In the Molecular Properties (Scalar) panel, use the Scalar # scroll bar to inspect the available scalars.

It will be seen that a total of 8 scalars are present and that, in addition to the species Version 4.02

9-7

Tutorial 9.1



from the PPDF database (C3H8, O2, CO, CO2, H2O and N2), scalar nos. 1 and 2 (for mixture fraction and variance) have also been created automatically. This because transport equations for these variables need to be solved, as can be seen from the formulation of the PPDF model in Chapter 10 of the Methodology volume. Boundary Conditions

Check the current boundary definitions and specify boundary conditions where appropriate. • •

Select folder Define Boundary Conditions Open the Define Boundary Regions panel

Specify boundary conditions for the inlet boundaries, choosing the ‘Mixing Length’ option for turbulence parameter input. Note that all fluid streams except the one flowing through the cooling passage have swirl velocity components on entry into the combustor. Starting with the fuel inlet: • • •

Select region 3 In the boundary regions scroll list Select option TI/Length from the Turb. Switch menu Enter inlet boundary values for the fuel stream in the appropriate boxes as shown below:

•

Click Apply

Specify conditions at the remaining boundaries: • • •

9-8

Select region 4 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

Version 4.02

Tutorial 9.1



Version 4.02

• • • •

Click Apply Highlight region 5 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

• • • •

Click Apply Highlight region 6 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate text boxes, as shown below:

9-9

Tutorial 9.1


Pre-Processing Control Parameters

•

Click Apply

Check the wall boundary conditions for the first inlet-side wall (region 7) •

Select region 7 in the scroll list. The default settings are acceptable, so no further action is required

This is also true of the wall boundary conditions assigned to regions 8 to 13. Check region 14 (the outlet) and region 15 (the baffle boundaries): • •

Highlight region 14 in the scroll list. The default settings are acceptable, so no further action is required Highlight region 15 in the scroll list. The default settings for side no. 1 are acceptable, so no further action is required. The settings for side no. 2 are automatically made the same as side no. 1

Specify a boundary condition for the mixture fraction variable at the fuel inlet: • • •

Open the Scalar Boundaries panel Select region no. 3 in the boundary regions scroll list Select MIXTURE_FRACTION in the Scalar scroll list, type 1.0 in the Mass Fraction box and then click Apply

Modify the air inlet boundary values (regions 4, 5 and 6) for the O2 and N2 scalars as follows: • • •

Select region no. 4 in the boundary regions scroll list Select N2 in the Scalar scroll list, type 0.768 in the Mass Fraction box and click Apply Select O2 in the Scalar scroll list, type 0.232 in the Mass Fraction box and click Apply

Repeat the above sequence of steps for regions 5 and 6. Control Parameters

Check the solution control parameters and then change the under-relaxation factor and residual tolerance for the mixture fraction and variance: •

9-10

Select folder Analysis Controls Version 4.02

Tutorial 9.1



• • • • • • • • • • Run Time Controls

Select sub-folder Solution Controls and then Equation Behavior Open the Additional Scalars panel Select MIXTURE FRACTION in the Scalar scroll list Type 0.7 in the Under-Relaxation Factor box Type 0.001 in the Residual Tolerance box Click Apply Select VARIANCE in the Scalar scroll list Type 0.7 in the Under-Relaxation Factor text box Type 0.001 in the Residual Tolerance text box Click Apply

Check the status of the run time control parameters: • • •

Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 500 for the maximum number of iterations and then click Apply. Open the Analysis (Re)Start panel. The setting of the Restart File Option menu should be None, confirming that this is a run from initial conditions.

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • •

In the main pro-STAR panel, select File > Write Geometry File In the Geometry File Write dialog, click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis For flows involving chemical reactions, it is recommended that STAR is run in double precision mode, as follows: • • • •

In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Select the Double Precision option button. Leave all other settings at their default values Click Start New Analysis

The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Start the post-processing task by re-plotting the mesh: Version 4.02

9-11

Tutorial 9.1



• •

In the main window, select C > All Click Cell Plot

This tutorial employs two user-defined panels, Pgetc and Pgetv, that are specially designed to facilitate post-processing operations. These may already be available to you, ready-to-use, in a local or global panel sub-directory (see “Panels” in Chapter 16 of the CCM User Guide). If the panels are not available, or if you want to practice creating panels, see “Panel Definition” on page 9-17 for a general discussion of the subject and for specific instructions on how to create these particular panels. Use the panels to generate a 3-D display of the velocity magnitude distribution: •

• • • • •

Click Panels in pro-STAR’s menu bar to display the available panels and then select Pgetc. Note that the name of the menu item may be L Pgetc or G Pgetc, depending on whether a local or global panel sub-directory is being used. If no items appear in the menu, either the required panel does not exist or it is necessary to specify the name and location of the above sub-directories. In either case, you will need to refer to the section on “Panel Definition” in this tutorial for further instructions. Select option Case from the Pgetc panel’s Load menu to get the current case name Select option Load St. to read in the analysis results In the main window, select plot option Contour Plot and plot type Hidden Surface In the Pgetc panel, click VM In the main window, click the Edge plotting button to display Figure T9.1-2

Figure T9.1-2

Velocity magnitude plot

Define a section whose plane bisects the mesh and passes through the axis of 9-12

Version 4.02

Tutorial 9.1



symmetry: • • •

• •

In the main window, select View > Axis > +X Click Edge Plotting again to deselect it Click Section Slice and then use the screen cursor to draw a vertical line that bisects the visible mesh (mark the end points of the line using the screen cursor). This represents the trace of a longitudinal section plane through the middle of the mesh and passing through the axis. Select a viewpoint at right angles to the section by choosing View > SNORMAL Select cell plot type Section (Surface)

Use the Pgetc panel to create a cell-averaged temperature profile in the section: • • •

On the Pgetc panel, click button TA to display the absolute temperature distribution Average the cell values by selecting Post > Caverage > Cset from the main pro-STAR window Click Replot to display the temperature profile shown in Figure T9.1-3

Figure T9.1-3

Temperature distribution

Note that the cell-averaged temperature contours continue unbroken across the baffle. This implies a heat flow situation that is unrealistic (given that the baffle is adiabatic) and is solely due to the interpolation technique employed by pro-STAR to create a smooth-looking plot. You should be aware of this when creating smoothed contour plots in geometries containing baffles and solid-fluid interfaces. Close the Pgetc panel: • Version 4.02

Select File > Close 9-13

Tutorial 9.1



Open panel Pgetv and plot the vertex-based mass fraction profiles for the fuel and one of the combustion products (CO2) in the section: • • •

Select Panels > Pgetv Click button Conc5 to display the propane distribution, shown in Figure T9.1-4 Click button Conc4 to display the carbon dioxide distribution, shown in Figure T9.1-5

Figure T9.1-4

9-14

Propane distribution

Version 4.02

Tutorial 9.1



Figure T9.1-5

Carbon dioxide distribution

As for the cell-averaged temperature plot, the vertex-averaged CO2 plot shows unrealistic values in the vicinity of the baffle. This effect could be minimised by using a finer mesh. Analysis of Results

The predicted maximum temperature in the model is lower than would normally be expected from this type of combustor. It is therefore instructive to consider the likely accuracy of the temperature distribution obtained here. A good quality measure to use for this purpose is the ratio gf f ′-2 = ------------------f f where f is the mean mixture fraction (calculated as scalar no. 1) and gf its variance (scalar no. 2). To display the distribution of the above variable over the combustion region (encompassing approximately the first six cell layers in the radial direction) proceed as follows: • • •

Change the plot option setting to Geometry Plot Change the cell plot type to Section (All) Select C > New > Zone and then draw a closed rectangle encompassing the entire mesh in the z-direction and the first six cell layers in the x-direction, starting from the axis

Load the variance in post register no. 1 and take its square root: • • Version 4.02

In the main window, select Post > Operate In the Post Register Operations dialog, go to the Function pop-up menu and 9-15

Tutorial 9.1



• • • •

select option Load Cell Data > Scalar Concentration Accept the default Register 1 as the destination register for the data and type 2 in the Scalar # text box Click Apply In the Function pop-up menu, select option Single-Register > Sqrt( ) Click Apply

Load the mixture fraction in post register no. 2: • • •

In the Post Register Operations dialog, go to the Function pop-up menu and select option Load Cell Data > Scalar Concentration Select Register 2 as the destination register and type 1 in the Scalar # text box Click Apply

Calculate the required ratio by dividing the contents of register 1 by those of register 2 and putting the results in register 4 (reserved for scalar data). • • •

Go to the Function pop-up menu and select option Multi-Register > Divide Choose appropriate register numbers in the register pop-up menus so that the end result is Register 4 = Register 1/Register 2 Click Apply and then Close

Now plot the distribution: • • •

Change the plot option setting to Contour Plot Turn off mesh plotting Click Cell Plot to display Figure T9.1-6

Figure T9.1-6

Distribution of quality measure ratio

It will be seen that the value of the ratio is generally rather high, implying that the 9-16

Version 4.02

Tutorial 9.1


Panel Definition Analysis of Results

predicted maximum temperature is considerably lower than the adiabatic flame temperature. In a realistic modelling exercise, a considerably finer mesh would be needed to increase confidence in the calculated temperatures. Terminate the session: •


Panel Definition Panel Pgetc is designed as an aid to post-processing cell-centre based data. To set up the panel, shown below, proceed as follows:

• • •

•

Panels > Define Panel Click on the text box at the bottom of the dialog and type Pgetc, the panel’s name Click New. This adds a new panel with that name in the scroll list. Note that the full stop (‘.’) in front of the name signifies that the panel definition is placed by default in the present working directory, in a file called Pgetc.PNL With the panel name still highlighted, click Open to display the new (blank) panel

Specify the basic panel appearance via the panel menu options, as follows: • • • • • •

File > Layout In the Define Panel Layout dialog box, type 7 in the Number of Buttons Horizontally text box Type 4 in the Number of Buttons Vertically text box Type 260 in the Panel Height text box Type 550 in the Panel Width text box Click Apply and then move the panel to the screen location where you want it to appear every time you enter pro-STAR

Proceed with the definition of panel buttons. The latter are numbered in column order, so that buttons nos. 0-3 appear on the left-hand side of the panel and nos. 24-27 on the right-hand side. To create the first column: • • • •

Version 4.02

Click on button no. 0 Type SU in the Button Name text box Click on the Definition sub-window and type: getc u v w su$repl Click File > Save

9-17

Tutorial 9.1



• • • • • • • • • • • •

Click on button no. 1 Type SV in the Button Name text box Click on the Definition sub-window and type: getc u v w sv$repl Click File > Save Click on button no. 2 Type SW in the Button Name text box Click on the Definition sub-window and type: getc u v w sw$repl Click File > Save Click on button no. 3 Type VM in the Button Name text box Click on the Definition sub-window and type: getc u v w vmag$repl Click File > Save

The remaining columns are created in a similar manner, according to the definitions given below: ID= 4 Label= P Command= getc u v w p$repl ID= 5 Label= PA Command= getc u v w p abso$repl ID= 6 Label= Pstat Command= getc u v w pstat$repl ID= 7 Label= PstatA Command= getc u v w pstat abso$repl ID= 8 Label= Ptot Command= getc u v w ptot$repl ID= 9 Label= PtotA Command= getc u v w ptot abso$repl ID= 10 9-18

Version 4.02

Tutorial 9.1



Label= T Command= getc u v w t rela$repl ID= 11 Label= TA Command= getc u v w t abso$repl ID= 12 Label= Ttot Command= getc u v w ttot rela$repl ID= 13 Label= TtotA Command= getc u v w ttot abso$repl ID= 14 Label= K Command= getc u v w te$repl ID= 15 Label= E Command= getc u v w ed$repl ID= 16 Label= Visc Command= getc u v w vis$repl ID= 17 Label= Dens Command= getc u v w dens$repl ID= 18 Label= Conc1 Command= getc u v w conc 1$repl ID= 19 Label= Conc2 Command= getc u v w conc 2$repl ID= 20 Label= Conc3 Version 4.02

9-19

Tutorial 9.1



Command= getc u v w conc 3$repl ID= 21 Label= Conc4 Command= getc u v w conc 4$repl ID= 22 Label= Conc5 Command= getc u v w conc 5$repl ID= 23 Label= Conc6 Command= getc u v w conc 6$repl ID= 24 Label= Conc7 Command= getc u v w conc 7$repl ID= 25 Label= Conc8 Command= getc u v w conc 8$repl ID= 26 Label= Conc9 Command= getc u v w conc 9$repl ID= 27 Label= Conc10 Command= getc u v w conc 10$repl The panel also provides additional facilities for executing common data loading operations, in the form of a local, user-defined menu (ee “Panels” in Chapter 16 of the CCM User Guide). The definition of this special menu is as follows: Menu Load MENU_ITEM 0 Case *get name,case MENU_ITEM 1 Event evfi conn MENU_ITEM 2 Load St. load {name}.ccm MENU_ITEM 3 Load Tr. 9-20

Version 4.02

Tutorial 9.1



trload {name}.pstt Complete the panel definition as follows: • • •

File > Layout Type 160 in the Panel Height text box and then click Apply Close the Define Panel dialog

Note that, in going through this process, you have the choice of leaving the panel in your present working directory, where it will be available only to the case you are working on at the moment, or copying/moving it to a local or global panel directory. You might do the latter if you want the panel to be available for use by other members of your team (global) or by yourself in all your case directories (local). If the panel is moved or copied to a local or global directory, you need to make sure that pro-STAR knows the latter’s name and location. This information may be available already in the form of environment variable definitions in your operating system set-up. In such a case, next time you enter pro-STAR you will see the panel name displayed (preceded by ‘L’ or ‘G’, as appropriate) when you click Panels in the main menu bar. If environment variables are not set, it is still possible to supply the required information as part of the current session, as follows: • • •

Panels > Environment Type the full filename path in the PANEL_GLOBAL or PANEL_LOCAL text box, depending on the location of the panel definition file Click Apply

SETENV PANEL LOCAL • • • •

Panels > Define Panel > Re-Scan The above operation causes the View panel name to be displayed in the list, preceded by ‘L’ or ‘G’, as appropriate Click Close Choose Panels from the main menu bar to confirm that Pgetc is included as a menu option

Note that, if you are working with a local or global directory, any new panels you create can be placed directly in that directory simply by prefixing the new panel name with an ‘L’ or ‘G’, as appropriate.

Panel Pgetv is essentially identical to Pgetc apart from the fact that it performs vertex based post-processing operations. The appearance and button definitions for this panel is given below:

Version 4.02

9-21

Tutorial 9.1



ID= 0 Label= SU Command= getv u v w su$repl ID= 1 Label= SV Command= getv u v w sv$repl ID= 2 Label= SW Command= getv u v w sw$repl ID= 3 Label= VM Command= getv u v w vmag$repl ID= 4 Label= P Command= getv u v w p$repl ID= 5 Label= PA Command= getv u v w p abso$repl ID= 6 Label= Pstat Command= getv u v w pstat$repl ID= 7 Label= PstatA Command= getv u v w pstat abso$repl ID= 8 Label= Ptot Command= 9-22

Version 4.02

Tutorial 9.1



getv u v w ptot$repl ID= 9 Label= PtotA Command= getv u v w ptot abso$repl ID= 10 Label= T Command= getv u v w t rela$repl ID= 11 Label= TA Command= getv u v w t abso$repl ID= 12 Label= Ttot Command= getv u v w ttot rela$repl ID= 13 Label= TtotA Command= getv u v w ttot abso$repl ID= 14 Label= K Command= getv u v w te$repl ID= 15 Label= E Command= getv u v w ed$repl ID= 16 Label= Visc Command= getv u v w vis$repl ID= 17 Label= Dens Command= getv u v w dens$repl ID= 18 Label= Conc1 Command= getv u v w conc 1$repl Version 4.02

9-23

Tutorial 9.1



ID= 19 Label= Conc2 Command= getv u v w conc 2$repl ID= 20 Label= Conc3 Command= getv u v w conc 3$repl ID= 21 Label= Conc4 Command= getv u v w conc 4$repl ID= 22 Label= Conc5 Command= getv u v w conc 5$repl ID= 23 Label= Conc6 Command= getv u v w conc 6$repl ID= 24 Label= Conc7 Command= getv u v w conc 7$repl ID= 25 Label= Conc8 Command= getv u v w conc 8$repl ID= 26 Label= Conc9 Command= getv u v w conc 9$repl ID= 27 Label= Conc10 Command= getv u v w conc 10$repl

9-24

Version 4.02

Tutorial 9.2

PROPANE COMBUSTION (THREE-STEP EDBR)

Tutorial 9.2

Additional Modelling Notes


The main aim of the tutorial is to: • •

•

Familiarise users with the eddy break-up model setup Demonstrate a simulation in which the overall combustion reaction is represented by several steps, describing fuel pyrolysis and the subsequent oxidation into combustion products Illustrate the use of the ‘numerical’ scheme for modelling the ignition process

Thus, the simulation performed in Tutorial 9.1 is repeated using a three-step reaction of the following form: C 3 H 8 + 1.5O 2 → 3CO + 4H 2 CO + 0.5O 2 → CO 2 H 2 + 0.5O 2 → H 2 O The mesh set up in Tutorial 7.2 of the Meshing Tutorials volume is utilised and boundary conditions that are appropriate for this type of model are applied. The physical properties of air (23.2% oxygen and 76.8% nitrogen, by mass), leading reactants (C3H8, CO, H2) and products (CO2, H2O) are assumed to be as follows: Air

C3H8

CO

H2

CO2

H2O

28.96

44.0

28.0

2.0

44.0

18.0

Molecular weights Density Molecular viscosity

Ideal gas 1.81 × 10–5

Specific heat

8.27 × 10–6

1.79 × 10–5

8.88 × 10–6

1.49 × 10–5

1.27 × 10–5

Polynomial function of temperature

Thermal conductivity 2.637 × 1.769 × 2.497 × 18.62 × 1.696 × 2.533 × 10–2 10–2 10–2 10–2 10–2 10–2 It is assumed that both air and fuel enter the combustion chamber at a pressure of 1 bar and temperature of 293 K. Additional Modelling Notes •

•

Version 4.02

Transport equations are solved for the leading reactants and their mixture fractions (Mixture fraction = Unburnt fuel mass fraction + Burnt fuel mass fraction) The oxygen mass fraction may be obtained from its fixed fraction in the inlet air stream and the amount of fuel burnt. Thus, an internal linear equation is employed to compute this quantity. The nitrogen mass fraction is obtained from its fixed fraction in the inlet air stream. 9-25

Tutorial 9.2


Numerical Considerations Preliminaries

•

• • •

The mass fraction of products (carbon dioxide and water vapour) is obtained from the amount of burnt fuel and is therefore also computed from a linear equation Using linear equations for oxygen and product mass fractions implies that the molecular diffusivities of all species are assumed to be identical It is assumed that the combustion rate is controlled by turbulent mixing of fuel and air and is calculated via the eddy break-up model The mixture’s specific heat is assumed to be dependent on component specific heats, i.e. Cp =

∑ C pi Y i i

where Yi is the species mass fraction and i

i

C p ≡ C p( T ) •

for all i

In this model, it is necessary to initiate combustion by an ignition mechanism. A flow domain region lying downstream of the inlets is chosen for this purpose. Ignition comprises an artificial reduction of the fuel mass fraction used to determine the combustion rate and is performed over a pre-defined number of iterations. It is expected that the final solution will be independent of the choice of ignition cells, the fuel mass fraction reduction mentioned above and the duration of the ignition process.

Numerical Considerations • •

•

The combustion source term in the leading reactant transport equations is large; therefore, the fuel mass fraction requires under-relaxation. Using the chemico-thermal option for enthalpy, the enthalpy and mixture fraction variables must develop numerically at the same rate as the fuel fraction. Therefore, the under-relaxation factors for enthalpy and transported species must be identical. Small errors in calculating the fuel mass fraction can strongly influence the computed temperature. Therefore, it is necessary to solve the transport equations for species and enthalpy to a tight solver tolerance.

Pre-processing Preliminaries Create a sub-directory for the tutorial called tut9-2. The mesh for this problem has already been created in the Meshing Tutorials volume (Tutorial 7.2) and the relevant cell, vertex, boundary and problem setup files are already available (files combustor.cel, combustor.vrt, combustor.bnd and combustor.inp, respectively). Therefore, before starting the tutorial, make sure that the above files are copied into your current directory. Also copy the user-defined panels Pgetc and Pgetc defined in Tutorial 9.1. These are stored in files Pgetc.PNL and Pgetv.PNL. • 9-26

Start up pro-STAR by typing prostar at the command line Version 4.02

Tutorial 9.2


Pre-processing Ignition Region

• • •

Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, EDBR_va) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is combustor.inp Click Apply Click Close


In the main window, select File > Model Title In the Title text box type: PROPANE COMBUSTION (3-STEP EDBR)

•

Click Apply


In the main pro-STAR window, select Plot > Up Axis > X Select C > All Select View > Isometric > 1, 1, -1 Click Cell Plot


Ignition Region

In the STAR GUIde window, go to panel Select Analysis Features Select option Chemical Reaction from the Reacting Flow menu Click Apply Select folder Thermophysical Models and Properties and note that an extra sub-folder called Reacting Flow now appears in the STAR GUIde tree. This will be used in this tutorial to supply chemical reaction definitions.

As explained in the “Additional Modelling Notes” section, an ignition region needs to be defined for this type of model. To do this, collect the cells to be designated as ignition cells as follows: •

In the I/O window, type command CSET NEWS GRAN 0.049 0.0751,,,-0.1 0.51 2

•

Click Cell Plot

A total of 90 cells will be selected. Now assign a separate cell type with a different colour to them so that they can be distinguished easily from the rest of this model’s cells: • • Version 4.02

In the main window, select Tools > Cell Tool Select Table # 4 in the Cell Table scroll list 9-27

Tutorial 9.2


Pre-processing Material Properties

• • • • • • • • Material Properties

Click Edit Types to display the Cell Table Editor Enter 5 in the Color Table Index box Enter Ignition_cells in the Name box Click Apply and then Close In the Cell Tool, select Modify Type > Cell Set Click Replot and notice the change of cell colour in the ignition region Close the Cell Tool In the main window, select C > All and then Cell Plot to see all cells in the model

Set up material properties and thermofluid models using the appropriate STAR GUIde panels. The required actions are as follows: 1. Select the Ideal Gas Law density variation (with pressure dependence) 2. Since this is a high-temperature combustion case, assign a polynomial variation to the specific heat of the background fluid (air) as a function of temperature. In this tutorial, we assume that the specific heat polynomial for air is virtually identical to that for N2 3. Select the standard k-ε turbulence model 4. Turn on the chemico-thermal enthalpy equation solver 5. Set the initial temperature and turbulence distribution 6. Choose the monitoring cell location 7. Choose the reference pressure and its location • • • •

•

• •

• • • • • • • • • 9-28

In the STAR GUIde window, select sub-folder Liquids and Gases Open the Molecular Properties panel Select option Ideal-f(T,P) from the Density menu Select option Polynomial in the Specific Heat menu. Note that pro-STAR displays an additional Molecular Weight box whose default value, 28.96, is appropriate for air. Click Apply. A pop-up panel will appear, warning you that pro-STAR was not able to find the background material name (AIR) in its built-in database and suggesting an alternative action. Click OK to close the panel and then click Define/Edit Polynomial to open the Polynomial Function Definition dialog Find a substance called N2 in the scroll list on the left-hand side of this dialog, select it, and then click Apply Database Substance. pro-STAR will retrieve the corresponding polynomial coefficients and assign them to material no. 1, i.e. the background material. Click Graph Data to display a graph of specific heat versus temperature, together with corresponding graphs for normalised enthalpy and entropy Click Close to exit from the dialog Open the Turbulence Models panel Click On to switch on turbulence modelling Select option K-Epsilon/High Reynolds Number from the model menu Click Apply Open the Thermal Models panel Turn on the solution of the energy equation by clicking Temperature Calculation On and then click Show Options Select option Chemico-Thermal from the Enthalpy menu Version 4.02

Tutorial 9.2


Pre-processing Combustion Model

• • • • • •

Click Apply Open the Initialization panel In the Flow Conditions tab, confirm that a value of 293.0 is displayed in the Temperature box Go to the Turbulence tab and select option TI/Mixing Length from the Turbulence Parameters menu Enter 0.05 and 0.2 in the Intensity and Mixing Length boxes, respectively Click Apply

It is good practice to define one of the ignition cells as the monitoring point. This makes checking for the onset of ignition easier, as temperature and product mass fractions build-up rapidly at that point once ignition begins. • • •


Open the Monitoring and Reference Data panel Type 114 in the Monitoring cell number box Choose the same reference pressure location as Tutorial 9.1, i.e. half way between the axis and the outer casing and towards the outlet, by entering 1760 in the Reference Pressure Cell Number box. Confirm that 1.0e+5 appears in the Pressure box. Click Apply


• •

Select sub-folder Reacting Flow followed by Chemical Reactions Open the Scheme Definition panel Select option Unpremixed/Diffusion from the Reaction Type menu Accept the default EBU Standard option from the Reaction Model menu. Note that scheme no. 1 is selected by default in the Chemical Scheme # slider at the bottom of the panel Click Apply A pop-up window will now appear warning you that the default chemical reaction settings will be changed. Click Continue. A message will appear at the bottom of the STAR GUIde panel confirming your combustion model selection.

Specify the chemical reaction equations and other basic model parameters: • • •

• •

Version 4.02

Open the Reaction System panel. Note that reaction no. 1 is selected by default in the Reaction scroll box. Type the first reaction definition, C3H8 + 1.5O2 -> 3CO + 4H2, in the adjacent box Accept the default settings on the Status, Tscale and Rate Equation menus and then click Update Reaction 1. pro-STAR will fill in default values for parameters Amix, Bmix, confirm the chemical names entered above and enter them in the appropriate list (Leading Reactants, Products and Reactant parameters) at the bottom of the panel Increment the scroll box setting to 2 and type the second reaction definition, CO + 0.5O2 -> CO2, in the box Click Update Reaction 2. pro-STAR will update the various lists as necessary 9-29

Tutorial 9.2


Pre-processing Scalar Properties

• •

Increment the scroll box setting to 3 and type the third reaction definition, H2 + 0.5O2 -> H2O in the box Click Update Reaction 3. pro-STAR will update the various lists as necessary

Check the treatment to be applied to the ordinary reactant (oxygen): • • •

In the Reactant Parameters list, select reactant no. 1 Check that option Fixed-Fraction is shown in the drop-down menu underneath Check that the (fixed) oxygen mass fraction in the incoming air stream is 0.233

This completes the specification of leading reactants and combustion products. pro-STAR will automatically map scalar variables to the constituents of the reaction scheme, define their initial conditions and assign physical properties using its built-in database (props.dbs). If a chemical species cannot be mapped to a scalar variable, a warning will be displayed in the I/O window and a new scalar of that name (but with default, i.e. air, properties) will be created and added to the scalars list. A stoichiometric check under this condition will fail, indicating that the assigned properties (molecular weights, in particular) are not appropriate. It is therefore advisable to check the I/O window to confirm that the model and chemical species have been correctly set up. Finally, specify the ignition parameters as follows: • • • • • • •

Open the Ignition panel Accept the default setting (Numerical) in the Model/Treatment panel Type 4 in the Cell Type box Type 0.05 in the Fraction Burnt box Accept the default option, Time Step/Iteration, in the When? menu Type 50 and 150 in the Start and End boxes, respectively Click Apply

Assign the chemical reaction scheme just defined to the model’s fluid domain: • • • Scalar Properties

Open the Scheme Association panel Select option Chemical Scheme Number and then type 1 in the adjacent box Click Apply

Check the properties of the scalar variables set up as a result of the scalar mapping described earlier: •

Select the Additional Scalars folder and then open the Molecular Properties (Scalar) panel

Use the Scalar # scroll bar to scroll through the available scalars. It will be seen that a total of 10 scalars have been created, including three ‘passive’ scalars representing the mixture fractions of the leading reactants. Note that a solution for this group of scalars is required by the EDBR formulation (see Chapter 10 of the Methodology volume). Inspect each of the remaining scalars in turn to verify that they have been set up as ‘active’, i.e. their influence on the flow field will be taken into account through the density calculation. 9-30

Version 4.02

Tutorial 9.2


Pre-processing Boundary Conditions

As a result of the ‘Polynomial’ setting for the background fluid, you need to assign a polynomial specific heat function to the scalar variables representing the chemical reaction species and display this graphically for verification purposes. • •

•

• • •

Boundary Conditions

Select scalar no. 1 (C3H8) with the Scalar # slider Clicking Apply causes pro-STAR to search for the coefficients of this substance in its internal database. In this case, they are found and a message to that effect appears in the I/O window. Click the Define/Edit Polynomials button for specific heat to open the Polynomial Function Definition dialog. This will display the coefficients just retrieved. Click Graph Data to display a graph of specific heat .vs. temperature, together with corresponding graphs for normalised enthalpy and entropy Click Close to exit from the dialog In the Molecular Properties (Scalar) panel, retrieve polynomial coefficients for the remaining species (i.e. scalar nos. 3, 4, 5, 6, 8 and 10) by selecting them in turn with the Scalar # slider and then following the same procedure as for scalar no. 1



Specify boundary conditions for the inlet boundaries, choosing the ‘Mixing Length’ option for turbulence parameter input. Note that all fluid streams except the one flowing through the cooling passage have swirl velocity components on entry into the combustor. Starting with the fuel inlet:

Version 4.02

• • •

Select region 3 In the boundary regions scroll list Select option TI/Length from the Turb. Switch menu Enter inlet boundary values for the fuel stream in the appropriate boxes as shown below:

•

Click Apply

9-31

Tutorial 9.2



Specify conditions at the remaining boundaries:

9-32

• • •

Select region 4 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

• • • •

Click Apply Select region 5 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

• • • •

Click Apply Select region 6 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate text boxes, as shown below:

Version 4.02

Tutorial 9.2


Pre-processing Control Parameters

•

Click Apply

Check the wall boundary conditions for the first inlet-side wall (region 7) •

Select region 7 in the scroll list. The default settings are acceptable, so no further action is required

This is also true of the wall boundary conditions assigned to regions 8 to 13. Check region 14 (the outlet) and region 15 (the baffle boundaries): • •

Highlight region 14 in the scroll list. The default settings are acceptable, so no further action is required Highlight region 15 in the scroll list. The default settings for side no. 1 are acceptable, so no further action is required. The settings for side no. 2 are automatically made the same as side no. 1

Specify scalar boundary conditions at the fuel inlet: • • • • Control Parameters

Check the solution control parameter settings and specify new values for under-relaxation factors and tolerances where appropriate: • • • • • • • • •

Version 4.02

Open the Scalar Boundaries panel Select region no. 3 in the boundary regions scroll list Select MIX_FRAC-FUEL_1 in the Scalar scroll list, type 1.0 in the Mass Fraction box and then click Apply Select C3H8 in the Scalar scroll list, type 1.0 in the Mass Fraction box and then click Apply

Select folder Analysis Controls Select sub-folder Solution Controls and then Equation Behavior Open the Primary Variables panel and then select the Solver Parameters tab Type 0.7 in the Relaxation Factor box for Temperature Type 0.001 in the Residual Tolerance box for Temperature Type 0.8 in the Relaxation Factor box for Density Click Apply Open the Additional Scalars panel Select all scalars in the scroll list one-by-one and check the under-relaxation 9-33

Tutorial 9.2



factor and the residual tolerance settings. It will be seen that they are the same as those for temperature. This is because, when option Chemico-Thermal is selected for enthalpy, pro-STAR changes these values automatically to match those for temperature. This ensures that enthalpy and all transported scalars are developed numerically at the same rate. Run Time Controls

Check the status of the run time control parameters: • • • •

Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 500 for the maximum number of iterations and 0.0001 for the maximum residual tolerance Click Apply Open the Analysis (Re)Start panel. The setting of the Restart File Option menu should be None, confirming that this is a run from initial conditions.

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • •


CFD Analysis As in Tutorial 9.1, a double precision STAR executable needs to be employed, as follows: • • • •


The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file EDBR_va.ccm: • • •

9-34


Version 4.02

Tutorial 9.2



Basic Plots

Start by re-plotting the mesh:. • •

In the main pro-STAR window, select C > All Click Cell Plot

The user-defined panels, Pgetc and Pgetv, described in Tutorial 9.1 are to be used to generate a 3-D display of the velocity magnitude distribution: • • • •

Select Panels > Pgetc In the Pgetc panel, click VM Select Contour Plot as the cell plot type In the main window, click the Edge plotting button to display Figure T9.2-1

Figure T9.2-1

Contours of velocity magnitude

Close the Pgetc panel • •

File > Close In the main window, click the Edge Plotting button again to deactivate it

Define a section whose plane bisects the mesh and passes through the axis of symmetry: • •


In the main window, select View > Axis > +X Click Section Slice and then use the screen cursor to draw a vertical line that bisects the visible mesh (click the end points of the line). This represents the trace of a longitudinal section plane through the middle of the mesh and passing through the axis. Select a viewpoint at right angles to the section by choosing View > SNORMAL Select cell plot type Section (Surface) 9-35

Tutorial 9.2



Open panel Pgetv and plot the vertex-based temperature profile in the section: • •

Select Panels > Pgetv On the Pgetv panel, click button TA to display the absolute temperature distribution shown in Figure T9.2-2

Figure T9.2-2

Temperature distribution

Note that the temperature contours continue unbroken across the baffle. This implies a heat flow situation that is unrealistic (given that the baffle is adiabatic) and is solely due to the interpolation technique employed by pro-STAR to create a smooth-looking plot. You should be aware of this when creating smoothed contour plots in geometries containing baffles and solid-fluid interfaces. Repeat for the mass fraction profiles of the fuel and one of the combustion products (CO2). This time use panel Pgetc to read in the cell-based values and then obtain the vertex-based values by averaging: • • • • • • •

9-36

Select Panels > Pgetc Click Conc1 Select Post > Caverage > Cset In the main window, click Replot to display the propane distribution shown in Figure T9.2-3 Click Conc8 Select Post > Caverage > Cset In the main window, click Replot to display the carbon dioxide distribution shown in Figure T9.2-4

Version 4.02

Tutorial 9.2



Figure T9.2-3

Contour plot of C3H8 concentration

Figure T9.2-4

Contour plot of CO2 concentration

As with the temperature plot, the CO2 contour plot incorrectly suggests that the scalar concentration is continuous across the baffle. To terminate the session:

Version 4.02

9-37

Tutorial 9.2



•

9-38


Version 4.02

Tutorial 9.3

C7H8 DROPLET COMBUSTION (EDBR, RADIATION)

Pre-processing Preliminaries

Tutorial 9.3


In Tutorial 9.2, a three-step eddy break-up model was used to simulate propane combustion. This sub-tutorial employs the same reaction model but under a significantly different set of conditions, as follows: 1. The fuel is toluene (C7H8) and is injected into the combustor in the form of droplets that subsequently evaporate into the combustible vapour. 2. An externally supplied subroutine is used to model the physical process involved in fuel droplet evaporation 3. A single-step chemical reaction of the following form is used: C 7 H 8 + 9O 2 → 7CO 2 + 4H 2 O 4. Radiation effects are introduced. Some preparatory work for this feature, in the form of extra boundary region definitions, was done in Tutorial 7.2 of the Meshing Tutorials volume where the basic mesh setup is described. This sub-tutorial makes use of those definitions. It also introduces participating media radiation (due to the gases within the combustor) in addition to radiative heat transfer between the various boundary surfaces. 5. Some boundary condition modifications are made to represent the combustion conditions, droplet injection and surface radiation properties. The aim of this tutorial is therefore to demonstrate: •

•

The combination of several advanced STAR-CD features (chemical reaction, Lagrangian two-phase and radiation simulation) in building a physically realistic model of a typical combustion problem The importance of user subroutines in enhancing the accuracy of droplet material property models

Pre-processing Preliminaries Create a sub-directory for the tutorial called tut9-3. The mesh for this problem has already been created in the Meshing Tutorials volume (Tutorial 7.2) and the relevant cell, vertex, boundary and problem setup files are already available (files combustor.cel, combustor.vrt, combustor.bnd and combustor.inp, respectively). Therefore, before starting the tutorial, make sure that the above files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, EDBR_dr) in the Casename text box Click Continue

Read in the available problem data: • • • • Version 4.02

Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is combustor.inp Click Apply Click Close 9-39

Tutorial 9.3


Pre-processing Ignition Region


In the main window, select File > Model Title In the Title text box type: TOLUENE COMBUSTION (1-STEP EDBR,DROPLETS,RADIATION)

•

Click Apply


In the main pro-STAR window, select Plot > Up Axis followed by X Select C > All Select View > Isometric > 1, 1, -1 Click Cell Plot

Specify the key features of this case, i.e. chemically reacting flow in the presence of droplets: • • • • •

Ignition Region

In the STAR GUIde window, go to panel Select Analysis Features Select option Lagrangian Multi-Phase from the Multi-Phase Treatment menu Select option Chemical Reaction from the Reacting Flow menu Click Apply. An additional folder called Lagrangian Multi-phase will appear in the NavCenter tree. Select folder Thermophysical Models and Properties and note that an extra sub-folder called Reacting Flow now appears in the STAR GUIde tree. This will be used in this tutorial to supply chemical reaction definitions.

Given that an eddy break-up model is to be used here, an ignition region needs to be specified for this model, similar to the one described in Tutorial 9.2. To do this, collect together the cells to be designated as ignition cells as follows: •

In the I/O window, type command CSET NEWS GRAN 0.074 0.101,,,-0.1 0.51 2

•

Click Cell Plot

A total of 90 cells will be selected. Now assign a separate cell type with a different colour to them so that they can be distinguished easily from the rest of this model’s cells: • • • • • • • 9-40

In the main window, select Tools > Cell Tool Select Table # 4 in the Cell Table scroll list Click Edit Types to open the Cell Table Editor Enter 5 in the Color Table Index box Select On from the Radiation menu. This is a necessary setting for performing radiation calculations, as explained below Type Ignition_cells in the Name box Click Apply Version 4.02

Tutorial 9.3


Pre-processing Thermal Options

• • • • Thermal Options

In the Cell Tool, select Modify Type > Cell Set Click Replot and notice the change of cell colour in the ignition region Close the Cell Tool In the main window, select C > All and then Cell Plot to see all cells in the model

The radiation model in this tutorial includes the effects of the intervening gas, using default gaseous radiation properties, as well as surface-to-surface radiation. This requires the use of beams that can be tracked only through cell types that are explicitly defined as participating in radiative heat transfer. Since ignition cells have already been prepared for this type of analysis, all cells in the rest of the fluid domain need to be re-set for this purpose: • • • •

Go to the Cell Table Editor and select Table# 1 in its scroll list Select On from the Radiation menu Click Apply Close the Cell Table Editor

Turn radiation on, choosing the Discrete Transfer analysis method in conjunction with the participating media calculation option: • • • • • Radiation Patches

Select the Thermophysical Models and Properties folder and open the Thermal Options panel In the Radiation section of the panel, select option Discrete Transfer Enter 100 in the Beams per patch box Select option Participating to include gaseous radiation effects in the calculations Accept the remaining default settings and then click Apply

To use the discrete beam radiation model, it is necessary to subdivide all boundary regions present in the problem (except for cyclic boundaries) into so-called ‘patches’. These are used both during view factor calculations and for evaluating the radiative heat transfer. Assign a unique patch to every boundary in every relevant region. This can be done most conveniently by means of a pro-STAR command loop, shown below: typed into the I/O window: •

In the I/O window, type the following commands: BSET NONE *SET NREG 3 1 *DEFINE BPATCH NREG,,BYFA BSET ADD REGI NREG *END *LOOP 1 12

The above loop will create 535 patches. Display the patches to confirm that the operation has been carried out correctly: • • Version 4.02

In the main window, select the Patch plot display option Verify that patches appear in the right places and then deselect the Patch plot 9-41

Tutorial 9.3


Pre-processing Material Properties

display option Material Properties

Set up material properties and thermofluid models using the appropriate STAR GUIde panels. The required actions are as follows: 1. Select the Ideal Gas Law density variation (with pressure dependence) 2. Since this is a high-temperature combustion case, assign a polynomial variation to the specific heat of the background fluid (air) as a function of temperature. In this tutorial, we assume that the specific heat polynomial for air is virtually identical to that for N2 3. Select the standard k-ε turbulence model 4. Turn on the chemico-thermal enthalpy equation solver 5. Set the initial temperature and turbulence distribution 6. Choose the monitoring cell location 7. Choose the reference pressure and its location • • •

•

• •

• • • • • • • • • •

• • • • 9-42

Go to the STAR GUIde window and open the Molecular Properties panel in sub-folder Liquids and Gases Select option Ideal-f(T,P) from the Density menu Select option Polynomial in the Specific Heat menu. Note that pro-STAR displays an additional Molecular Weight box whose default value, 28.96, is appropriate for air. Click Apply. A pop-up panel will appear, warning you that pro-STAR was not able to find the background material name (AIR) in its built-in database and suggesting an alternative action. Click OK to close the panel and then click Define/Edit Polynomial to open the Polynomial Function Definition dialog Find a substance called N2 in the scroll list on the left-hand side of this dialog, select it, and then click Apply Database Substance. pro-STAR will retrieve the corresponding polynomial coefficients and assign them to material no. 1, i.e. the background material. Click Graph Data to display a graph of specific heat .vs. temperature, together with corresponding graphs for normalised enthalpy and entropy Click Close to exit from the dialog Open the Turbulence Models panel Click On to switch on turbulence modelling Select option K-Epsilon/High Reynolds Number from the model menu Click Apply Open the Thermal Models panel Turn on the solution of the energy equation by clicking Temperature Calculation On and then click Show Options Select option Chemico-Thermal from the Enthalpy menu Note that the panel includes a section labelled Participating Media. Check the radiative properties assigned to the gas. In this case the Radiative Properties setting should be Constant, the Absoption coefficient 0.1 and the Scattering coefficient 0.0 Click Apply Open the Initialization panel In the Flow Conditions tab, type a value of 500.0 in the Temperature box Click Apply Version 4.02

Tutorial 9.3


Pre-processing Combustion Model

• • •

Go to the Turbulence tab and select option TI/Mixing Length from the Turbulence Parameters menu Enter 0.05 and 0.2 in the Intensity and Mixing Length boxes, respectively Click Apply

It is good practice to define one of the ignition cells as the monitoring point. This makes checking for the onset of ignition easier, as temperature and product mass fractions build-up rapidly at that point once ignition begins. Begin by inspecting the cell numbers in the region of interest: • • • • • • •


In the main window, select Plot > Numbers and then click option Cell on the dialog displayed Zoom in on the mesh shown on-screen to have a closer look at the displayed numbers and then choose cell no. 482 as the monitoring cell Click Zoom Off Deselect option Cell on the Plot Numbers dialog and then click Close Go back to the STAR GUIde window and open the Monitoring and Reference Data panel Type 482 in the Monitoring cell number box Choose the same reference pressure location as Tutorial 9.1, i.e. half way between the axis and the outer casing and towards the outlet, by entering 1760 in the Reference Pressure Cell Number box. Confirm that 1.0e+5 appears in the Pressure box. Click Apply


• •

Select sub-folder Reacting Flow followed by Chemical Reactions Open the Scheme Definition panel Select option Unpremixed/Diffusion from the Reaction Type menu Accept the default EBU Standard option from the Reaction Model menu. Note that scheme no. 1 is selected by default in the Chemical Scheme # slider at the bottom of the panel Click Apply A pop-up window will now appear warning you that the default chemical reaction settings will be changed. Click Continue. A message will appear at the bottom of the STAR GUIde panel confirming your combustion model selection.

Specify the reaction equation for this scheme and other basic model parameters: • • •

Version 4.02

Open the Reaction System panel. Note that reaction no. 1 is selected by default in the Reaction scroll box. Type the required reaction definition, C7H8 + 9O2 -> 7CO2 + 4H2O, in the Reaction 1 box Accept the default settings on the Status, Tscale and Rate Equation menus and then click Update Reaction 1. pro-STAR will fill in default values for parameters Amix, Bmix, confirm the chemical names entered above and enter them in the appropriate list (Leading Reactants, Products and Reactant parameters) at the bottom of the panel 9-43

Tutorial 9.3


Pre-processing Droplet Properties

Check the treatment to be applied to the ordinary reactant (oxygen): • • •

In the Reactant Parameters list, select reactant no. 1 Check that option Fixed-Fraction is shown in the drop-down menu underneath Check that the (fixed) oxygen mass fraction in the incoming air stream is 0.233

This completes the specification of leading reactants and combustion products. pro-STAR will automatically map any required scalar variables to the constituents of the reaction scheme. Note that appropriate scalar variables already exist for all the chemical species constituents, so no additional scalar definitions for them are necessary. Specify the ignition parameters as follows: • • • • • • •

Open the Ignition panel Accept the default setting (Numerical) in the Model/Treatment panel Type 4 in the Cell Type box Type 0.05 in the Fraction Burnt box Select option Time Step/Iteration in the When? menu Type 20 and 120 in the Start and End boxes, respectively Click Apply

Assign the chemical reaction scheme defined earlier (no. 1) to the model’s fluid domain:. • • •

Open the Scheme Association panel Select option Chemical Scheme Number and then type 1 in the adjacent box Click Apply

Check the properties of the scalar variables set up as a result of the scalar mapping described earlier: • •

Select sub-folder Additional Scalars Open the Molecular Properties (Scalar) panel and scroll through the available scalars using the Scalar # scroll bar at the bottom of the panel

It will be seen that a total of 6 scalars have been defined, including an additional ‘passive’ scalar (no. 2) representing the mixture fraction of the fuel. Note that a solution for this scalar is required by the EDBR formulation (see Chapter 10 of the Methodology volume). Droplet Properties

Check the basic control settings for droplets and then re-define the maximum size of the droplet track file (in Mb), taking into account droplet trajectories and the maximum tracking times: • • • • •

9-44

Select folder Lagrangian Multi-Phase and open the Droplet Controls panel Check that option Coupled is set in the Two-Phase Lagrangian Calculations menu Type 100 in the Droplet Trajectory Max File Size box Accept the default value (100) for Maximum Tracking Time Select option Explicitly defined parcel injection Version 4.02

Tutorial 9.3


Pre-processing Droplet Properties

• •

Accept all other default settings on the panel and click Apply A panel will appear warning you that “the current injection definitions will be overwritten”. Since no definitions have been supplied yet, you may continue by clicking Yes.

Activate the turbulent dispersion model and define transport mechanisms and physical properties for the droplets on the basis of: 1. STAR’s standard methodology for momentum, heat and mass transfer between the dispersed and continuous phases 2. STAR’s default model for droplet break-up 3. Droplets bouncing off solid obstacles in the event of a collision The above parameters are set as follows: • • • • • • • • • •

Open the Droplet Physical Models and Properties panel Select the Global Physical Models tab Turn On the Turbulent Dispersion option and then click Apply Select the Droplet Physical Models tab and check that the Droplet Type # slider is set to 1 For Momentum Transfer, select option Standard and accept the default Mass Coef. and Slip Factor values For Mass Transfer select option Standard For Heat Transfer select option Standard For Droplet Breakup select option Reitz and accept the default values for We(Bag), We(Strip), Te(Bag), Te(Strip) For Droplet-Wall Interaction select option Rebound Click Apply

Specify droplet physical properties corresponding to liquid toluene. The heat of vaporisation and saturation pressure is to be defined by user coding in subroutine DROPRO, as discussed in section “User Subroutines” of this tutorial: • • • • •

• • • • • • •

Version 4.02

Select the Droplet Properties tab Click Select from Database to open the Droplet Properties Database dialog Scroll down the database material list to locate item TOLUENE(L), highlight it and then click Select Material Close the Droplet Properties Database dialog Check the contents of the Droplet Properties tab. All property values retrieved from the database are now displayed in the appropriate boxes. Since these are valid for a lower (room) temperature, adjust the values for the actual droplet injection temperature (350 K) as follows: Density — 725 Surface Tension Coef. — 0.0262 Viscosity — 0.00035 Specific Heat — 2107.86 Select option Subroutine Usage for both the Heat of Vaporisation and Saturation Pressure properties Click the Evaporates to Scalar Select button Define scalar no. 1 (i.e. the toluene fuel vapour) as representing the product of evaporation by selecting it in the Scalars list. 9-45

Tutorial 9.3


Pre-processing Droplet Creation

• •

Click Close. The chosen scalar number (1) will now appear in the Evaporates to Scalar box Click Apply

Note that the effect of toluene vapour on the mixture density will be taken into account by virtue of the fact that the scalar variable representing toluene (no. 1) is designated as an active scalar. Make a local copy of user subroutine DROPRO and put it in a sub-directory called ufile under your current working directory, as described in Chapter 14 of the CCM User Guide. • • •

In the main window, select File > System Command Type ufiles in the text box, click Apply and then Close Go back to the Droplet Properties tab and click Define User Coding

Once you have exited from pro-STAR at the end of this session, this subroutine should be edited as shown in section “User Subroutines” of this tutorial. Note that DROPRO in turn calls two auxiliary subroutines, CALHVP and CALSVP, that supply values for the heat of evaporation and saturation pressure, respectively. These should also be included in the ufile directory. All subroutines will be included automatically as part of the STAR executable before the model is run. Droplet Creation

Create the required number of parcels (each parcel is represented by a typical droplet) and specify their initial conditions. The parcels are to be injected into the combustor via an annular slit of radius 5 mm, centred around the axis of symmetry and projecting 2 cm into the combustion chamber. It is therefore convenient to use a cylindrical coordinate system (no. 2) when specifying initial parcel positions and velocities. All parcels in this model are to be included in a single injection group. Define the group’s injection characteristics, including the initial diameter, velocity magnitude and temperature of a typical droplet: • •

•

Open the Injection Definition panel Specify injection data as indicated below: Diameter — 250.0e-6 Velocity Magnitude — 4.4721 (based on initial velocity components Unit, Vinit, Winit of 2, 0, 4 in coordinate system no. 2) Temperature — 350 Mass Flowrate applies to — Each Injection Point Mass Flowrate — 4.152e-4 (based on an injection rate of 7.0e+4 droplets per parcel per second) No. of Parcels/injection point — 1 Click Apply

Specify the injection location for 21 parcels, uniformly distributed over an arc of 50˚ around the injector ring so that the interval between them is 2.5˚. All parcels are to have identical injection directions given by (0.4472, 0, 0.8944) in coordinate system no. 2: • • 9-46

Open the Injection Points panel Select option Line from the Set Type menu Version 4.02

Tutorial 9.3



• • • • • •

Enter 2 in the Coordinate System box Enter 21 in the Number of Points box Select option Specify for Point 1 (the first end-point of the circular arc) and enter its coordinates (0.005, -25.0, 0.02) in the X, Y, Z boxes Enter coordinates (0.005, 25.0, 0.02) for Point 2 (the second end-point of the arc) in the other set of X, Y, Z boxes Specify the entrance velocity direction in terms of unit vector components by entering (0.4472, 0, 0.8944) in the DX, DY, DZ boxes Click Add New Set. The injection points list at the top of the panel will confirm that a group of 21 injection points has been created.

For a visual check of particle initial conditions: • •

Select the parcel group (set no. 1) in the Injection Points list Click Plot points in set

Make the droplet size and colour dependent on particle diameter. • • • • • • Boundary Conditions

Select folder Post-Processing followed by sub-folder Particle Tracks Open panel Plot Droplets/Particle Tracks and then select the Droplets tab Select option Diameter in the Droplet Radius menu and type in 1. and 0.025 in the Size and Ref. Value boxes, respectively Select option Diameter in the Fill Color menu Click Apply Click Droplet Plot



In view of the fact that fuel is injected a short distance into the combustion chamber, it is necessary to close off the fuel stream inlet previously defined in Tutorial 7.2. This is done by re-defining region 3 from type ‘Inlet’ to type ‘Wall’. Surface temperature and radiation property data should also be supplied: • • • •

•

In the boundary regions scroll list, select region 3 Select option Wall from the Region Type menu Choose option Fixed in the Wall Heat pop-up menu Enter surface temperature and radiation property data in the appropriate boxes as shown below: Temp. — 600.0 Resis. — 0.8 Emissivity — 0.8 Ther. Reflect. — 0.2 Ther. Transmis. — 0.0 Click Apply

Specify conditions at the air inlet boundaries, including surface radiative data such as emissivity and reflectivity: • Version 4.02

Select region 4 in the scroll list 9-47

Tutorial 9.3



9-48

• •

Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

• • • •

Click Apply Select region 5 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate boxes, as shown below:

• • • •

Click Apply Highlight region 6 in the scroll list Select option TI/Length from the Turb. Switch menu Enter inlet conditions in the appropriate text boxes, as shown below:

Version 4.02

Tutorial 9.3



•

Click Apply

Supply surface radiative data for the outlet (region 14): • •

Select region 14 in the scroll list Type 900.0 in the T Radiation box, 1.0 in the Emissivity box and click Apply

Specify radiation conditions for the walls (regions 7 to 13) via a pro-STAR command loop. Walls are defined as thermally conducting with emissivity and reflectivity of 0.8 and 0.2, respectively. •

In the I/O window, type the following commands: *SET NREG 7 1 *DEFINE RMOD NREG U U U U U U U U FIXE 600.0 0.8 0.8 0.2 0.0 *END *LOOP 1 6

Finally, define the baffles as thermally conducting boundaries having the same radiation properties as the walls. • • • •


Select region no. 15 in the Boundary Regions scroll list Choose option Conduction in the Wall Heat pop-up menu Type 0.8 in the Resistance box Enter radiation property data in the appropriate boxes as shown below: Emissivity box — 0.8 Ther. Reflect. box — 0.2 Ther. Transmis. box — 0.0 Click Apply Enter radiation property data for the reverse side of the baffle in the 9-49

Tutorial 9.3


User Subroutines Control Parameters

• Control Parameters

Check the solution control parameters and then change the under-relaxation factor for temperature and density and the residual tolerance for temperature: • • • • • • • • •

Run Time Controls

appropriate dialog text boxes, as shown below: Emissivity box — 0.8 Ther. Reflect. box — 0.2 Click Apply again to apply the boundary conditions to this side of the baffle

Select folder Analysis Controls Select sub-folder Solution Controls and then Equation Behavior Open the Primary Variables panel and then select the Solver Parameters tab Type 0.7 in the Relaxation Factor box for Temperature Type 0.001 in the Residual Tolerance box for Temperature Type 0.8 in the Relaxation Factor box for Density Click Apply Open the Additional Scalars panel Select each scalar in turn and check that the Under-Relaxation Factor and Residual Tolerance values are set to 0.7 and 0.001, respectively

Check the status of the run time control parameters: • • • •

Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 800 for the maximum number of iterations and 0.0001 for the maximum residual tolerance Click Apply Open the Analysis (Re)Start panel. The setting of the Restart File Option menu should be None, confirming that this is a run from initial conditions.

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • •


User Subroutines As explained previously, sub-directory ufile should contain a file called dropro.f, corresponding to subroutine DROPRO. Use pro-STAR’s built-in editor to edit this subroutine and introduce the required code, as follows: • • • • • 9-50

In the main pro-STAR panel, select File > Edit File In the pro-STAR Editor dialog, click File > Open When the File Selection dialog appears, choose sub-directory ufile and then file dropro.f Click OK Edit the contents of the subroutine so that it looks exactly as shown below Version 4.02

Tutorial 9.3


User Subroutines Final Operations

•

Click File > Save to save the new version of the subroutine

C*********************************************************************** SUBROUTINE DROPRO(DENDR,CPDR,HV,PS,SFTC,DRVIS,DRCOND) C Droplet properties C*********************************************************************** C--------------------------------------------------------------------------* C STAR-CD VERSION 4.02 C--------------------------------------------------------------------------* INCLUDE ’comdb.inc’ COMMON/USR001/INTFLG(100) INCLUDE ’usrdat.inc’ INTEGER IFTYPE,RON COMMON /FULTYP/ IFTYPE,RON DIMENSION DRMAFR(50) EQUIVALENCE( UDAT08(001), DRMAFR(01) ) EQUIVALENCE( UDAT07(001), DRM ) EQUIVALENCE( UDAT04(005), PR ) EQUIVALENCE( UDAT05(001), IDR ) EQUIVALENCE( UDAT05(002), IDRT ) EQUIVALENCE( UDAT06(004), TD ) EQUIVALENCE( UDAT06(009), XD ) EQUIVALENCE( UDAT06(010), YD ) EQUIVALENCE( UDAT06(011), ZD ) EQUIVALENCE( UDAT05(004), ICO ) EQUIVALENCE( UDAT05(005), NDRCO ) C----------------------------------------------------------------------C C This subroutine enables the user to calculate the droplet C physical properties. C C ** Parameters to be returned to STAR: DENDR, CPDR, HV, PS, SFTC, C DRVIS and DRCOND C C----------------------------------------------------------------------C C..... Droplet heat of evaporation CALL CALHVP(NDRCO,ICO,TD,HV) C..... Droplet saturation pressure CALL CALSVP(NDRCO,ICO,TD,PS) C c WRITE(76,’(A19,2I6,1P3E16.5)’) ’ IP,ICO,TD,HV,PS : ’, c + IP,ICO,TD,HV,PS C C----------------------------------------------------------------------RETURN END C***********************************************************************

Note that this subroutine calls two auxiliary routines, CALHVP and CALSVP. These routines are fuel-specific and should therefore not be used for other chemical species. Two additional files called calhvp.f and calsvp.f containing the necessary code should now be created, as shown below: • • Version 4.02

In the pro-STAR Editor dialog, click File > Open When the File Selection dialog appears, and under sub-directory ufile, 9-51

Tutorial 9.3



• • • • •

enter a new file name called calhvp.f Click OK Input the contents of the new subroutine exactly as shown below Click File > Save to save the subroutine contents Repeat the above steps for the second subroutine, calsvp.f Click File > Quit to exit from the editor

C*********************************************************************** SUBROUTINE CALHVP(NDRCO,ICO,TDRP,HV) C Droplet heat of evaporation C See Reid pg 228 eqt 7-12.1 C*********************************************************************** INCLUDE ’comdb.inc’ C PARAMETER (NDRCL=1) DIMENSION WTMOL(NDRCL),TBOIL(NDRCL),TCRIT(NDRCL),PCRIT(NDRCL), + OMEGA(NDRCL) C.... Properties of C7H8 droplet vapour components DATA WTMOL/ 92.1410 / DATA TBOIL/ 383.8000 / DATA TCRIT/ 591.8000 / DATA PCRIT/ 41.0000 / DATA OMEGA/ 0.2630 / C C.... Other required data PARAMETER (RCONS=8.3143) DIMENSION TREFL(NDRCL) DATA TREFL/ 450.0 / C C------------------------------------------------------------------------C IF(NDRCO.GT.NDRCL) THEN WRITE(6,*)’ SUBROUTINE CALHVP: NDRCO.GT.NDRCL ’ WRITE(6,*)’ NDRCO=’, NDRCO WRITE(6,*)’ NDRCL=’, NDRCL STOP ENDIF C IF(TDRP.LT.TCRIT(ICO)) THEN TRED1=TREFL(ICO)/TCRIT(ICO) THAW1=1.0-TRED1 TERM1=7.08*(THAW1)**0.354 TERM2=10.95*OMEGA(ICO)*(THAW1)**0.456 HV1=(RCONS*TCRIT(ICO)*(TERM1+TERM2))*(1.0E+3/WTMOL(ICO)) C TRATIO=TBOIL(ICO)/TCRIT(ICO) TTE=(LOG(PCRIT(ICO))-1.013)/(0.93-TRATIO) DELHVB=1.093*RCONS*TCRIT(ICO)*TRATIO*TTE C TERM=0.00264*(DELHVB/(RCONS*TBOIL(ICO))) PN=(TERM+0.8794)**10 TRED2=TDRP/TCRIT(ICO) THAW2=1.0-TRED2 HV=HV1*(THAW2/THAW1)**PN ELSE HV=0.0 9-52

Version 4.02

Tutorial 9.3



ENDIF C C------------------------------------------------------------------------RETURN END

C*********************************************************************** SUBROUTINE CALSVP(NDRCO,ICO,TDRP,PS) C Droplet saturation pressure C See Reid pg 212 eqt 7-5.2 C*********************************************************************** INCLUDE ’comdb.inc’ C C------------------------------------------------------------------------C C.... Constants for the reference fluids C 1=PROPANE ; 2=OCTANE ; 3=Benzene ; 4=Pentafluorotolnene PARAMETER (NRFL=4) DIMENSION ARFL(NRFL),BRFL(NRFL),CRFL(NRFL),DRFL(NRFL),ORFL(NRFL) DATA ARFL/ -6.72219,-7.91211,-6.98273,-8.05688 / DATA BRFL/ 1.33236, 1.38007, 1.33213, 1.46673 / DATA CRFL/ -2.13868,-3.80435,-2.62863,-3.82439 / DATA DRFL/ -1.38551,-4.50132,-3.33399,-2.78727 / DATA ORFL/ 0.15300, 0.39800, 0.21200, 0.41500 / C PARAMETER (NDRCL=1) DIMENSION TBOIL(NDRCL),TCRIT(NDRCL),PCRIT(NDRCL), OMEGA(NDRCL) C.... Properties of C7H8 droplet vapour components DATA TBOIL/ 383.8000 / DATA TCRIT/ 591.8000 / DATA PCRIT/ 41.0000 / DATA OMEGA/ 0.2630 / C C.... Calculated data DIMENSION PVPR(NRFL) C C------------------------------------------------------------------------C IF(NDRCO.GT.NDRCL) THEN WRITE(6,*)’ SUBROUTINE CALSVP: NDRCO.GT.NDRCL ’ WRITE(6,*)’ NDRCO=’, NDRCO WRITE(6,*)’ NDRCL=’, NDRCL STOP ENDIF C IF(TDRP.LT.TCRIT(ICO)) THEN TRED=TDRP/TCRIT(ICO) THAW=1.0-TRED DO 200 JR=3,NRFL T1NU=ARFL(JR)*THAW T2NU=BRFL(JR)*THAW**1.5 T3NU=CRFL(JR)*THAW**3.0 T4NU=DRFL(JR)*THAW**6.0 PVPR(JR)=(T1NU+T2NU+T3NU+T4NU)/TRED 200 CONTINUE OTERM=(OMEGA(ICO)-ORFL(3))/(ORFL(4)-ORFL(3)) Version 4.02

9-53

Tutorial 9.3



PVPRC=PVPR(3)+(PVPR(4)-PVPR(3))*OTERM PS=EXP(PVPRC)*PCRIT(ICO)*1.0E+05 ELSE PS=PCRIT(ICO)*1.0E+05 ENDIF C C------------------------------------------------------------------------RETURN END

CFD Analysis As in Tutorial 9.1, a double precision STAR executable needs to be employed, as follows: • • • •


The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Start the post-processing task by loading the post file (EDBR_dr.ccm) and re-plotting the mesh:. • • • •

In STAR-GUIde, open the Post Processing folder and click on the Load Data panel Click Open Post File In the main window, select C > All Click Cell Plot

Activate the user-defined panels Pgetc and Pgetv as described in Tutorial 9.2 and use them to generate a 3-D display of the velocity magnitude distribution: • • • •

9-54

Select Panels > Pgetc In the main window, select plot option Contour Plot In the Pgetc panel, click VM In the main window, click the ‘edge’ plotting button to display Figure T9.3-1

Version 4.02

Tutorial 9.3



Figure T9.3-1

Cell-centred plot of velocity magnitude

Close the Pgetc panel: • •

File > Close In the main window, click the Edge Plotting button again to deactivate it

Plot the steady-state droplet distribution by choosing plot options such that droplet colour and radius depend on temperature and calculated diameter, respectively. The droplet velocity is not displayed. • • • • • • • • • • • • Version 4.02

In the STAR GUIde window, select folder Post-Processing followed by sub-folder Particle Tracks Open panel Plot Droplets/Particle Tracks and then select the Droplets tab In the Load Droplet Data section, select option Track File from the Load From menu and then click the file browser button underneath Select file EDBR_dr.trk from the Files list and then click OK. The contents of the File Name box will be updated to confirm your choice. Accept the default option (Particles) in the Plot Option menu and then click Load Data In the Droplet Options section, select After, Unhidden and Cplot from the Edge Plot Options menus Select Diameter in the Droplet Radius menu and enter 1. and 0.025 in the Size and Ref. Value boxes, respectively Select Temperature in the Fill Color menu Select None in the Vectors menu Click Apply In the Collect/Plot section, select Dp > All In the Plot Droplets panel, click Droplet Plot to display Figure T9.3-2 9-55

Tutorial 9.3



Figure T9.3-2

Plot of toluene droplets with the droplets coloured by their temperature

Now make the droplet colour dependent on droplet mass and replot: • •

In the Droplet Plot Options section, select Mass in the Fill Color menu Click Apply and then Droplet Plot to display Figure T9.3-3

Figure T9.3-3 9-56

Plot of toluene droplets with the droplets coloured by their mass Version 4.02

Tutorial 9.3



The above plot shows that the vast majority of the droplets have evaporated before they reach the combustor outlet. To view the fuel and combustion product distribution, first define a section whose plane bisects the mesh and passes through the axis of symmetry: • • • •

• •

In the main window, select D > None Select plot option Geometry Plot and then click Cell Plot View > Axis > +X Click Section Slice and then use the screen cursor to draw a vertical line that bisects the visible mesh (click the end points of the line). This represents the trace of a longitudinal section plane through the middle of the mesh and passing through the axis. Select a viewpoint at right angles to the section by choosing View > SNORMAL Select cell plot type Section (Surface)

Open panel Pgetv and use it to plot the vertex-based temperature profile in the section: • • •

In the main window, select plot option Contour Plot Select Panels > Pgetv On the Pgetv panel, click button TA to display the absolute temperature distribution shown in Figure T9.3-4

Figure T9.3-4

Absolute temperature distribution

For the reason described in Tutorial 9.2, the temperature plot is somewhat misleading as it implies that heat is flowing through the adiabatic baffle. The same is also true for the CO2 distribution shown in Figure T9.3-6 below. Version 4.02

9-57

Tutorial 9.3



Produce contour plots for the concentration profiles of fuel and carbon dioxide. This time use panel Pgetc to read in the cell-based values and then obtain the vertex-based values by averaging: • • • • • • •

Select Panels > Pgetc Click Conc1 Post > Caverage > Cset In the main window, click Replot to display the toluene distribution shown in Figure T9.3-5 Click Conc4 Post > Caverage > Cset In the main window, click Replot to display the carbon dioxide distribution shown in Figure T9.3-6

Figure T9.3-5

9-58

Toluene distribution

Version 4.02

Tutorial 9.3



Figure T9.3-6

CO2 distribution

To terminate the run: •

Version 4.02


9-59

Tutorial 9.4

HYDROGEN COMBUSTION (LAMINAR FLAMELETS)


Tutorial 9.4


In this tutorial, a hydrogen combustion case is modelled using a Laminar Flamelets model for unpremixed flames. Unlike PPDF models that assume chemical equilibrium, this model allows for non-equilibrium effects such as flame stretch and detailed chemical kinetics. The model also assumes adiabatic conditions (no heat loss). The main aims of the tutorial are to: • • •

Familiarise users with the Laminar Flamelets model setup Demonstrate the process of specifying chemical species that are not included in pro-STAR’s species database (props.dbs) Demonstrate how to set up boundary conditions and analysis controls for scalars used in the simulation

Pre-Processing Preliminaries Create a new directory for the tutorial called tut9-4. The mesh for this problem has already been created in the Meshing Tutorials volume (Tutorial 7.2) and the relevant cell, vertex, boundary and problem setup files are already available (files combustor.cel, combustor.vrt, combustor.bnd and combustor.inp, respectively). Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, flamelet) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog, check that the File Name is combustor.inp Click Apply Click Close

This will read default problem settings from file combustor.inp, plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: HYDROGEN COMBUSTION (LAMINAR FLAMELETS)

•

Click Apply

Plot the mesh to confirm that the data have been read in correctly: • • • • Version 4.02

In the main pro-STAR window, select Plot > Up Axis followed by X Select C > All Select View > Isometric > 1, 1, -1 Click Cell Plot 9-61

Tutorial 9.4




Material Properties

In the STAR GUIde window, go to panel Select Analysis Features Select option Chemical Reaction from the Reacting Flow menu Click Apply Select folder Thermophysical Models and Properties and note that an extra sub-folder called Reacting Flow now appears in the STAR GUIde tree.

Set up material properties and thermofluid models using the appropriate STAR GUIde panels. The necessary actions are as follows: 1. 2. 3. 4. 5. • • • • • • • • • • • • • • • • • •

Combustion Model

Select sub-folder Liquids and Gases Open the Turbulence Models panel Click On to switch on turbulence modelling Select option K-Epsilon/High Reynolds Number from the model menu Click Apply Open the Thermal Models panel Turn on the solution of the energy equation by clicking Temperature Calculation On Click Apply Open the Initialization panel In the Flow Conditions tab, confirm that a value of 293.0 is displayed in the Temperature box Go to the Turbulence tab and select option TI/Mixing Length from the Turbulence Parameters menu Enter 0.05 and 0.2 in the Intensity and Mixing Length boxes, respectively Click Apply Open the Monitoring and Reference Data panel Specify the Monitoring cell number as 1760. This is roughly in the centre of the outlet boundary region. Make the reference pressure location the same as the monitoring cell location by entering 1760 in the Reference Pressure Cell Number box Check that 1.0e+5 appears in the Pressure box Click Apply

Use STAR GUIde’s Reacting Flow folder to set up the combustion model, as follows: • • • •

9-62

Select the standard k-ε turbulence model Turn on the temperature solver Set the initial temperature distribution Choose the monitoring cell location Choose the reference pressure and its location

Select sub-folder Reacting Flow followed by Chemical Reactions Open the Scheme Definition panel Select option Unpremixed/Diffusion from the Reaction Type menu Select option PPDF Single Fuel from the Reaction Model menu. Note that scheme no. 1 is selected by default on the Chemical Scheme # slider at the Version 4.02

Tutorial 9.4



• •

bottom of the panel. Select the Laminar Flamelet Model Option and click Apply A pop-up window will now appear warning you that the default chemical reaction settings will be changed. Click Continue. A message will appear at the bottom of the STAR GUIde panel confirming your combustion model selection.

The next step is to specify an appropriate reaction mechanism for the Laminar Flamelet model. This must be written in CHEMKIN format, which requires a listing of all participating elements, species and reactions. For a detailed description of how to specify reaction mechanisms in this format, see , “Laminar flamelet model” in the CCM User Guide. Supply the basic data required as follows: • •

Open the Reaction System panel In the Reaction Mechanism tab, copy the description given below into the displayed box:

ELEMENTS H O N END SPECIES H HO2 H2 H2O H2O2 N2 O OH O2 END REACTIONS H+O2+M=HO2+M 3.61E+17 -0.720 H2O/18.6/ H2/2.86/ H+H+M=H2+M 1.00E+18 -1.000 H+H+H2=H2+H2 9.20E+16 -0.600 H+H+H2O=H2+H2O 6.00E+19 -1.250 H+OH+M=H2O+M 1.60E+22 -2.000 H2O/5/ H+O+M=OH+M 6.20E+16 -0.600 H2O/5/ O+O+M=O2+M 1.89E+13 0.000 H2O2+M=OH+OH+M 1.30E+17 0.000 H2+O2=2OH 1.70E+13 0.000 OH+H2=H2O+H 1.17E+9 1.300 O+OH=O2+H 3.61E+14 -0.500 O+H2=OH+H 5.06E+04 2.670 OH+HO2=H2O+O2 7.50E+12 0.000 H+HO2=2OH 1.40E+14 0.000 O+HO2=O2+OH 1.40E+13 0.000 2OH=O+H2O 6.00E+08 1.300 H+HO2=H2+O2 1.25E+13 0.000 HO2+HO2=H2O2+O2 2.00E+12 0.000 H2O2+H=HO2+H2 1.60E+12 0.000 H2O2+OH=H2O+HO2 1.00E+13 0.000 END •

Version 4.02

0.000 0.000 0.000 0.000 0.000 0.000 -1788.000 45500.000 47780.000 3626.000 0.000 6290.000 0.000 1073.000 1073.000 0.000 0.000 0.000 3800.000 1800.000

Click Save Mechanism. Confirm that you wish to proceed with this operation in the displayed pop-up warning panel. pro-STAR will then store the supplied data in file chemf.inp01 in a sub-directory called PPDF. 9-63

Tutorial 9.4



•

Click Apply to validate the file contents and create the chemistry libraries needed subsequently by the flamelet calculations. Again, confirm that you wish to proceed with this operation in the displayed pop-up warning panel.

Now that the reaction mechanism has been specified, the flamelets description needs to be created: • • •

In the Flamelet Setup tab, select the Composition sub-tab Click Generate Flamelet file to generate and store the first flamelet description in file flame01.inp01 within the PPDF sub-directory Examine the Mole Fractions and Valences for the Fuel, Oxidizer and Product streams by selecting each of them in turn from the Select Stream to Define pop-up menu. The default values displayed are suitable for this case.

Four flamelets are to be generated for this problem, as follows: •

• • • • • • • •

Move the Flamelet No. slider to 2 and click Generate Flamelet file again. This will generate a new flamelet description and store it in file flame02.inp01within the PPDF sub-directory Repeat this procedure for Flamelet Nos. 3 and 4, thus generating files flame03.inp01 and flame04.inp01 Select the Flow Conditions sub-tab For Flamelet No. 2, change the Strain Rate of Oxidizer to 200 Click Apply to store the updated flamelet description in file flame02.inp01 For Flamelet No. 3, change the Strain Rate of Oxidizer to 300 Click Apply to store the updated flamelet description in file flame03.inp01 For Flamelet No. 4, change the Strain Rate of Oxidizer to 0, which corresponds to the equilibrium condition Click Apply to store the updated flamelet description in file flame04.inp01

Flamelet libraries must now be calculated from the above flamelet descriptions and stored in a set of files called flame$$.lib01. Output information for this calculation is written to a set of corresponding files called flame$$.out01. • • • • • • • • • • • 9-64

Select the Flamelet Generation tab Select Flamelet No. 1 from the list. Note that option New is selected by default. Click Apply to calculate the corresponding flamelet library. This process may take a few seconds. Select Flamelet No. 2 from the list Choose option Restart From Flamelet No. 1. This should reduce the computation time because the two flamelets have similar properties. Click Apply Select Flamelet No. 3 from the list Choose option Restart From Flamelet No. 2 Click Apply Select Flamelet No. 4 from the list Click Apply Version 4.02

Tutorial 9.4



The STAR-CD solver requires that flamelet library data should be provided in tabular form. The relevant table is created as follows: • • •

Select the Look-up Table tab Check that the Plot Flamelet Data for Flamelet Number option is set to 1 Click Plot to display graphs of flamelet data for flamelet number 1, as shown in Figure T9.4-1.

Figure T9.4-1

• • • • •

Scalar Properties

Plot similar graphs for flamelets 2, 3 and 4. There should be a few slight differences between the four graphs. Change the Mixture Fraction Dimension to 40. This is the number of points used to define the mixture fraction profile in the table. Change the Mixture Fraction Variance Dimension to 30 Select flamelets 1, 2, 3 and 4 from the Flamelet No list and use the arrow button, , to add them to the Selected flamelet No list Click Apply to create the required look-up table and store it in file flamelet.tbl01 in your working directory. An error message will appear stating that some of the species included in the mechanism have not been found in pro-STAR’s built-in property database file props.dbs. Data for these species must be specified next.

The I/O window lists the problem species as OH, O, H, HO2 and H2O2. As props.dbs does not contain property data for such species, and since their molecular weights are needed to calculate polynomial distributions of their mole fractions, the required properties must be specified explicitly: •

Version 4.02

Graphs of flamelet data for flamelet number 1

Select the Additional Scalars sub-folder from within the Thermophysical 9-65

Tutorial 9.4



• • • • • • • • • • • •

Models and Properties folder Open the Molecular Properties (Scalar) panel Select Scalar # 7 using the slider at the bottom of the panel Change the Molecular Weight of Scalar # 7 to 17 Click Apply Change the Molecular Weight of Scalar # 8 to 16 Click Apply Change the Molecular Weight of Scalar # 9 to 1 Click Apply Change the Molecular Weight of Scalar # 10 to 33 Click Apply Change the Molecular Weight of Scalar # 11 to 34 Click Apply

All the properties and parameters of the chosen chemical reaction scheme have now been specified, so it can now be assigned to the fluid material in the model: • • • Boundary Conditions

The next step is to specify boundary conditions, starting with the fluid inlet conditions: • • • • • • • • • • • • • • • • • • • • • • •

9-66

Open the Scheme Association panel in the Reacting Flow folder Select Chemical Scheme Number and enter 1 in the box Click Apply

Select the Define Boundary Conditions folder Open the Define Boundary Regions panel Select Reg# 3, Fuel_inlet from the boundary regions list Specify the U, V and W velocity components as -28, -60 and 100 m/s, respectively Change the Coord. System to 2 Select TI/Length from the Turb. Switch pull-down menu Change the Turb. Intensity to 0.1 and the Length to 0.01 m Change the Density to 1.8 kg/m3 Click Apply Select Reg# 4, Air_inlet1 from the boundary regions list Specify the U, V and W velocity components as -11, -24 and 42 m/s, respectively Change the Coord. System to 2 Select TI/Length from the Turb. Switch pull-down menu Change the Turb. Intensity to 0.1 and the Length to 0.01 m Change the Density to 1.19 kg/m3 Click Apply Select Reg# 5, Air_inlet2 from the boundary regions list Specify the U, V and W velocity components as -11, -24 and 42 m/s, respectively Change the Coord. System to 2 Select TI/Length from the Turb. Switch pull-down menu Change the Turb. Intensity to 0.1 and the Length to 0.01 m Change the Density to 1.19 kg/m3 Click Apply Version 4.02

Tutorial 9.4



• • • • • • •

Select Reg# 6, Air_inlet3 from the boundary regions list Specify the W velocity component as 15 m/s Change the Coord. System to 2 Select TI/Length from the Turb. Switch pull-down menu Change the Turb. Intensity to 0.1 and the Length to 0.01 m Change the Density to 1.19 kg/m3 Click Apply

The scalar concentrations at the inlet boundaries must also be specified: • • • • • • • • • • • • •

Analysis Controls

Some of the analysis controls need to be changed to ensure a reasonably rapid convergence rate: • • • • • • • • • • •

Run Time Controls

Select the Analysis Controls folder followed by the Solution Controls sub-folder Select the Equation Behavior sub-folder Open the Additional Scalars panel Select MIXTURE_FRACTION from the Scalar list Change the Under-Relaxation Factor to 0.7 Change the Residual Tolerance to 0.001 Click Apply Select VARIANCE from the Scalar list Change the Under-Relaxation Factor value to 0.7 Change the Residual Tolerance to 0.001 Click Apply

The run time controls must also be adjusted: • • • •

Version 4.02

Open the Scalar Boundaries panel Select region number 3 from the Boundary Region list Select MIXTURE_FRACTION from the Scalar list Change the Mass Fraction to 1 Click Apply Select region number 4 from the Boundary Region list Select N2 from the Scalar list Change the Mass Fraction to 0.79 Click Apply Select O2 from the Scalar list Change the Mass Fraction to 0.21 Click Apply For regions 5 and 6, set the N2 and O2 Mixture Fractions to 0.79 and 0.21, respectively, as for region number 4

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Enter 400 for the maximum Number of Iterations Change the Max. Residual Tolerance to 0.0001 Click Apply

9-67

Tutorial 9.4



Final Operations

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • •


CFD Analysis For problems involving chemical reactions, it is recommended that STAR is run in double precision mode as follows: • • • •


The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Start the post-processing task by re-plotting the mesh: • •

In the main window, select C > New > Fluid Click Cell Plot

Now load the solution results and plot velocity vectors on an x-z plane bisecting the model geometry: • • • • • • • • • •

9-68

Go to the STAR GUIde window and select the Post-Processing folder Open the Load Data panel Under the File(s) tab, click Open Post File Under the Data tab, select Velocity Components UVW from the Vector Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, change the Normal values to 0, 1, 0 Click Apply Click Plot To Screen In the main pro-STAR window, select View > SNORMAL to display Figure T9.4-2

Version 4.02

Tutorial 9.4



Figure T9.4-2

Section Clipped plot of velocity vectors

Contour plots of temperature and mixture fraction can now be plotted as follows: • • • • • • • • •

Under the Data tab of the Load Data panel, select Smooth Options On and All Select Temperature from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select the Option Contour(filled) Click Plot To Screen to display Figure T9.4-3 Under the Data tab of the Load Data panel, select MIXTURE_FRACTION from the Scalar Data list Click Get Data Click Replot to display Figure T9.4-4

As explained in Tutorial 9.1, the contour plot smoothing effect leads to a physically unrealistic temperature profile in the vicinity of the baffle.

Version 4.02

9-69

Tutorial 9.4



Figure T9.4-3

Section Clipped plot of temperature contours

Figure T9.4-4

Section Clipped plot of contours of mixture fraction

Terminate the session: •

9-70

In the main pro-STAR window, select File > Quit, Nosave

Version 4.02

Introduction

Tutorial 10 BUOYANCY AND RADIATION EFFECTS Introduction This tutorial illustrates various STAR-CD facilities for simulating a heat transfer problem involving natural convection, conduction, solid-fluid heat transfer and radiation. The example used in the tutorial consists of a heated aluminium alloy fin placed within a rectangular box filled with air (see Figure T10.0-1).

T = 293 K

T = 293 K

1 10

4

2

1

1

2

4 T = 343 K

Figure T10.0-1

Heated fin geometry (all dimensions in cm)

The problem is simulated in two dimensions for ease of mesh generation and speed of numerical calculation. The mesh employed is shown in Figure T10.0-2.

Version 4.02

10-1

Material Properties

Figure T10.0-2

Mesh structure for the heated fin model

Material Properties Three variants of this problem are considered, with different modes of heat transfer applying in each. Material properties for the solid fin and the surrounding air are as follows: Aluminium alloy fin: Density (ρ) = 2800 kg/m3 Specific heat (Cp) = 880 J/kg K Thermal conductivity (λ) = 180 W/m K Surrounding air (incompressible, turbulent): Density (ρ) = variable, based on Ideal Gas Law for molecular weight 28.96 Specific heat (Cp) = 1006 J/kg K Thermal conductivity (λ) = 0.0264 W/m K Molecular viscosity (µ) = 1.81E–5 Pa s

10-2

Version 4.02

Tutorial 10.1

BUOYANCY DRIVEN FLOW AROUND A HEATED FIN


Tutorial 10.1


This sub-tutorial employs a simple, uniform two-dimensional mesh to model the shape and size of the solid fin, followed by cell indexing and specification of material properties for the fin and surrounding fluid. Heating of the fin is achieved by fixing the temperature at the base to 343 K. The sides of the surrounding box are set to a fixed temperature of 293 K and the remaining wall boundaries are assumed to be either conducting (at solid/fluid interfaces) or adiabatic (at the top and bottom walls of the box), as shown in Figure T10.0-1. This tutorial aims to show the user how to: • • •

Model solid-fluid heat transfer Model buoyancy-driven flows Create streamline plots

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut10-1. The mesh for this problem is supplied in advance, i.e. cell, vertex, boundary and problem setup files (fin.cel, fin.vrt, fin.bnd and fin.inp, respectively) are available in the STAR-CD installation directories. Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, fin_bu) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is fin.inp Click Apply Click Close

This will read default problem settings from file fin.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: BUOYANCY DRIVEN FLOW ROUND A HEATED FIN

• Mesh Checking

Verify that the correct mesh has been imported by selecting all cells and plotting the mesh in ‘Hidden Surface’ mode: • •

Version 4.02

Click Apply

In the main window, select C > All. The I/O window output shows that 2,500 cells were read in Check that Hidden Surface is the default cell plot type 10-3

Tutorial 10.1



• •

Click Cell Plot Change the viewpoint to approximately (0.4, 0.5, 1) by dragging with the left mouse button to display Figure T10.1-1

It will be seen that the mesh matches that shown in Figure T10.0-2 and that it contains two cell types, corresponding to fluid and solid cells. Note that because of the difference in cell type, fluid and solid cells are displayed in different colours.

Figure T10.1-1

Cell Type Properties

Check and, if necessary, specify appropriate material property indices, colours and names for cell types 2 and 1, representing the solid fin and its surrounding fluid, respectively: • • • • •

• • Thermal and Gravity Options

In the main window, click the CTAB button to open the Cell Table Editor In the Cell Table Editor, select Table# 1 in the scroll list Type AIR in the Name box Accept the current settings for all other parameters and click Apply Select Table# 2 and change the following parameters: Material Number — 2 (the solid properties index) Color Table Index — 4 Name — AL Click Apply and then Close Click Replot to confirm the change (the solid cell colour will change)

Turn on the solid-fluid heat transfer option. This also has the effect of switching on the temperature solver inside the solid fin: • •

10-4

Mesh geometry

In the STAR GUIde window, select the Thermophysical Models and Properties folder and then open the Thermal Options panel Choose Heat Transfer On in the Solid-Fluid Heat Transfer section Version 4.02

Tutorial 10.1


Pre-Processing Fluid Properties

•

Click Apply

In order to take buoyancy effects into account, you need to specify the gravitational force in the global Cartesian y-direction. Check the current setting: • • • • Fluid Properties

Open the Gravity panel Type 9.81 in the Acceleration box to specify the gravitational acceleration value to be used for this problem Specify the correct direction of gravity in the model by typing -1 in the Y box and 0 in the Z box Click Apply

Check the material properties of the model’s fluid substance: • • •

In the Thermophysical Models and Properties folder, select the Liquids and Gases folder Open the Molecular Properties panel and check that the material number shown on the Material # scroll bar is 1. It can be seen that material no. 1 is, by default, a fluid whose properties are those of air. This is what is required in this case.

The density variation is assumed to follow the Ideal Gas Law. However, the fluid itself is incompressible since the pressure effect on density variations is deemed to be negligible. •

Select option Ideal-f(T) in the Density pop-up menu and click Apply.

Default values are accepted for the remaining properties. Assuming the flow is turbulent, select the k-ε model: • • •

Open the Turbulence Models panel Click the On button and then choose K-Epsilon/High Reynolds Number in the Turbulence menu Click Apply

Check the temperature equation setting: •

Open the Thermal Models panel. Note that the temperature calculation has been turned on as a result of selecting the solid-fluid heat transfer option.

Choose cell number 927 as the monitoring location for the fluid cells: • • •

Open the Monitoring and Reference Data panel Type 927 in the Monitoring cell number box Click Apply

Specify a datum location and density for the purpose of calculating buoyancy effects: • • • • • Version 4.02

Open the Buoyancy panel Click On to turn on the buoyancy calculation Select option Enter Coordinates from the Define Datum Location menu Enter coordinates 0, 0, 0 in the X, Y, Z boxes Select option Specify from the Define Datum Density menu 10-5

Tutorial 10.1


Pre-Processing Solid Properties

•

• Solid Properties

Define properties for the solid cells making up the fin (i.e. for material property reference no. 2): • •

•

• • • Checks

Select the Solids sub-folder within the Thermophysical Models and Properties folder Open the Material Properties panel and select material no. 2 using the Material # scroll bar. This will display properties for the default solid material (Carbon Steel). Change the property values to those for aluminium as follows: Name — AL Density — 2800 Conductivity — 180 Specific Heat — 880 Click Apply Select the Monitoring and Reference Data panel and choose a monitoring location within the solid by typing 924 in the Monitoring cell number box Click Apply

Check the boundaries by listing their properties and then displaying them graphically: •

• • •

10-6

Type 1.27588 in the Density box for the required datum density. As noted in the STAR GUIde on-line Help (“Useful Points”), it is important to calculate body forces as accurately as possible; hence the high degree of precision for the density value. Click Apply

In the main window, choose Utility > Count > Boundaries and then check the information displayed in the I/O window, i.e. number and type of regions and number of boundaries in each region Select Cell Plot Display Option Bound Select B > All and then B > Unselect > Symplane to exclude the symmetry planes from the boundary plot that is about to be produced Click Replot to display Figure T10.1-2. Only regions 1 and 2 are shown; all other boundary surfaces are allocated to region 0 by default.

Version 4.02

Tutorial 10.1



Figure T10.1-2

Boundary Conditions

Boundary region display

You can now impose the required thermal boundary conditions. Define fixed temperature boundaries at 293 K for the container’s side walls, as follows: • • • • •

Select the Define Boundary Conditions folder and open the Define Boundary Regions panel Select region no. 1 in the scroll list Select option Fixed in the Wall Heat pop-up menu Type the required fixed wall temperature, 293, in the Temperature box Accept the default values for the remaining parameters and click Apply

Define a fixed temperature boundary at 343 K for the base of the fin: • • • •

Select region no. 2 in the scroll list Select option Fixed in the Wall Heat pop-up menu Type the required fixed wall temperature, 343, in the Temperature box Accept the default values for the remaining parameters and click Apply

The remaining boundary surfaces, i.e. those allocated to region 0, default to adiabatic walls (at external surfaces) or conducting walls (at solid/fluid interfaces). Control Parameters

In buoyancy-driven flow calculations there is very strong coupling between the temperature and flow fields. It is therefore advisable to use the PISO algorithm (see the STAR GUIde on-line Help, “Useful Points”) which is more suitable for this type of problem: • •

Version 4.02

Select the Analysis Controls folder, followed by the Solution Controls sub-folder Open the Solution Method panel and choose option PISO from the Solution 10-7

Tutorial 10.1



•

Algorithm menu Click Apply

As the model is two-dimensional, we need not solve the W-momentum equation: • • •

Select the Equation Behavior folder and open the Primary Variables panel On the Equation Status tab, deselect the Solve button for W-Mom Click Apply

Given the strong effect of temperature and density variations on flow development, it is important to apply some under-relaxation to these variables. This helps in avoiding potential numerical stability problems. • •

•

Go to the Solver Parameters tab Type a new under-relaxation factor, 0.95, in the Density box under the Relaxation Factor column (note that this value must equal that for temperature, to ensure that the calculated magnitudes for the two variables are in step) Click Apply

Choose the MARS differencing scheme for some of the variables to be solved. This gives an optimum combination of stability and accuracy. • •

•

Go to the Differencing Schemes tab Choose option MARS in all active menus under the Differencing Scheme column, with the exception of Turb. KE and Turb. Diss which should be left to the default setting (UD). Accept the default value of 0.5 for the blending factor. Click Apply

Choose the type of data output and dumping frequency. For post-processing purposes, it is generally useful to save additional flow and thermal wall data (in this case, heat transfer coefficients at the walls): • • • • • • Run Time Controls

Set the number of iterations to 300: • • •

Final Operations

10-8

Select the Output Controls sub-folder and open the Analysis Output panel Accept the default option (On) for Write solution (restart) file and type 20 in the Output frequency box Go to the Additional Output Data section and then select item Heat Transfer Coef. from the Wall Data scroll list Click option button Post Repeat the above for item Heat Flux Click Apply

Select the Analysis Preparation/Running folder and then open the Set Run Time Controls panel Type 300 in the Number of Iterations box Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, write the geometry file, making sure that the scaling factor for the problem units (centimetres) is specified. Then write the problem file and exit from Version 4.02

Tutorial 10.1



pro-STAR, saving all model data as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •



In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Check that option other has been selected for the model units; 0.01 should appear inside the Scale Factor box

For simulations involving buoyancy, it is usually advisable to run STAR in Double Precision mode. This prevents relatively small buoyancy source terms which dominate the flow from being discarded as round-off error. • •

Select option Double Precision Leave all other settings at their default values and then click Start New Analysis

The analysis will then start automatically. This run should produce a converged solution within the specified maximum number of iterations. Post-Processing Preliminaries Launch pro-STAR (if the analysis was run outside pro-STAR). Read in the results of the analysis from file fin_bu.ccm: • • • Postprocessing

Version 4.02

In the STAR GUIde window select the Post-Processing folder Open the Load Data panel Click Open Post File

First look at the velocity field in the fluid surrounding the fin: • • • • • •

In the main window, select C > New > Fluid Click Cell Plot Deselect the Bound Cell Plot Display Option button Change the viewpoint to (0, 0, 1) by selecting View > Axis > +Z In the Load Data panel, go to the Data tab Select item Velocity Components UV option for Vector Data list and then click Get Data to load the velocity field 10-9

Tutorial 10.1



• • •

Select Go To > Create Plots, where the plot style will be defined In the 3-D Surface tab, check that Option Vector is selected and then choose Edge from the Edge/Mesh menu Click Plot to Screen to display Figure T10.1-3

Figure T10.1-3


Now view the streamlines: • • • • • • •

10-10

Click Go To Load Data Select Cell & Wall/Bound (Smooth) from the Data Type menu Select option Stream Function from the Calculated Scalar Data list Click Get Data Select Go To > Create Plots In the 3-D Surface tab, select Option Contour (line) Click Plot to Screen to display Figure T10.1-4

Version 4.02

Tutorial 10.1



Figure T10.1-4

Streamline plot

Examine the temperature profiles, first in the surrounding fluid and then in the solid fin: • • • • • • • • • • •

Version 4.02

Click Go To Load Data Select item Temperature from the Scalar Data list Click Get Data and then select Go to > Create Plots In the Create Plots panel, choose Option Contour (filled) Click Plot to Screen to display Figure T10.1-5 In the main window, select C > New > Solid In the Create Plots panel, click Go To Load Data In the Data tab, select Data Type Cell Select item Temperature in the Scalar Data list and then click Get Data To plot a smooth distribution ignoring boundary values, the cell data are averaged by selecting Post > Caverage > Cset in the main window Click Cell Plot to display Figure T10.1-6

10-11

Tutorial 10.1



Figure T10.1-5

Temperature plot in the fluid region

Figure T10.1-6

Temperature plot in the solid region

Heat flux data at the walls can be plotted as follows: • • 10-12

In the Data tab, select Data Type Wall Select item Heat Flux from the Scalar Data list Version 4.02

Tutorial 10.1



•

Click Get Data

Collect the shells created by pro-STAR at the walls (i.e. cells of type 5) and plot: • • • • • • •

Tools > Cell Tool Select cell type 5 in the Cell Table scroll list In the main window, select C > New > Type (Current) Select Post > Caverage > Cset Set the viewpoint to (1, 1, 1) by selecting View > Isometric > 1, 1, 1 Switch off the edge and mesh plotting facilities by clicking the ‘edge’ and ‘mesh’ buttons Select Plot > Wall Plot to display Figure T10.1-7

Figure T10.1-7

Final Operations

Version 4.02

Wall plot of heat flux

Terminate the session •


10-13

Tutorial 10.2

SURFACE-TO-SURFACE RADIATION


Tutorial 10.2


This sub-tutorial examines the effect of surface-to-surface radiation on heat transfer and temperature distribution. The boundary conditions remain the same as in Tutorial 10.1, except that radiative surface properties such as emissivity and reflectivity are now added. A surface-to-surface mode of radiative heat transfer is assumed. The aim of this tutorial is to show the user how to: • • • •

Model radiative heat transfer between walls through non-participating media Use the Initial Field Restart option when resuming from a previous analysis Compare results of different runs Use pro-STAR’s OPERATE utility


Create a sub-directory for the tutorial called tut10-2 and copy the model file generated in Tutorial 10.1 (fin_bu.mdl) into it Rename this file as fin_ra.mdl You will use this as a starting point for a revised model that introduces radiation to the heat transfer calculations. Since the solution obtained in Tutorial 10.1 will act as the starting point of the present analysis, it is also necessary to copy the solution file for the non-radiating case (fin_bu.ccm) to the current directory

Start up the pro-STAR GUI interface: • • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Accept the default case name (fin_ra) displayed in the Casename text box Select the Resume existing .mdl file? option Deselect the Append to .echo file? option Click Continue

This will read all data contained in file fin_ra.mdl and will set up the model as it was at the end of Tutorial 10.1. • •

In the main window, select File > Model Title In the Title text box, change the title to: BUOYANCY DRIVEN FLOW ROUND A HEATED FIN WITH RADIATION

• New Boundary Definitions

Click Apply

In problems where surface-to-surface radiation is being modelled, it is necessary to provide radiative boundary information such as emissivity and reflectivity, for all wall surfaces including solid-fluid interfaces. Solid-fluid interface This region is currently assigned to the default wall region (no. 0). You therefore

Version 4.02

10-15

Tutorial 10.2


Pre-Processing Thermal Options

need to define a new boundary region for it, extending round the entire fin perimeter. • • • • • • • • • • • • • •

In the main window, turn off the Bound option in the Cell Plot Display Options section Select C > New > Solid Click Cell Plot to display just the solid cells In the STAR GUIde window, select folder Locate Boundaries and then open the Create Boundaries panel In the Regions tab, select region no. 4 in the scroll list Select option Wall from the Type menu Enter a region name (S-F_interface) in the Name box Click Define region In the main window, change the viewpoint to (1, 0, 0) by selecting View > Axis > +X Click Select a Zone and draw a closed polygon around the visible mesh In the main window, change the viewpoint to (-1, 0, 0) by selecting View > Axis > -X Click Select a Zone and draw a closed polygon around the visible mesh In the main window, change the viewpoint to (0, 1, 0) by selecting View > Axis > +Y Again, click Select a Zone and draw a closed polygon around the visible mesh

The top and bottom adiabatic walls also need to be assigned explicitly to a separate region, no. 5. This is because radiation patches (to be defined later) cannot be applied to boundaries assigned to the default wall region 0. Top wall • • • • • • •

In the main window, select C > All Click Cell Plot In the Create Boundaries panel, select region no. 5 in the scroll list Select option Wall from the Type menu Enter a region name (T-B_wall) in the Name box Click Define region Click Select a Zone and draw a closed polygon around the visible mesh

Bottom wall • • • • Thermal Options

Switch radiation on, choosing the Discrete Transfer analysis method (DTRM). For this case, use the default number of beams per patch (100) and neglect radiative effects from the intervening gas: •

10-16

Change the viewpoint to (0, -1, 0) by selecting View > Axis > -Y Select C > Unselect > Zone and then draw a closed polygon around the (blue) cells belonging to the fin Click Cell Plot to display only cell faces belonging to the bottom wall In the Regions tab, click Select a Zone and then draw a closed polygon around the visible mesh

Select folder Thermophysical Models and Properties and then open the Version 4.02

Tutorial 10.2



• • •

Thermal Options panel In the Radiation section of the panel, select option Discrete Transfer Internal VF Calc. Enter 100 in the Beams per patch box Accept the displayed default settings in the rest of the panel and click Apply

For the chosen calculation method, surface-to-surface radiation can be tracked only through cell types that are explicitly defined as participating in radiative heat transfer. In this case, we assume that the fin is opaque and hence we only track radiation through the fluid: • • • • • Boundary Conditions

Open the Cell Table Editor using the CTAB button on the main window Select Table# 1 in the scroll list Select On from the Radiation pop-up menu Click Apply Close the Cell Table Editor

We must revisit the boundary conditions for all wall regions participating in radiative heat transfer in order to define their emissivity and reflectivity. In this case, we have not chosen to track radiation through the solid so we can ignore region 2 (the fin base). However, boundary conditions for the side walls need to be updated. • • • • • •

Select folder Define Boundary Conditions and open the Define Boundary Regions panel Select region no. 1 in the scroll list Specify the required radiation properties by entering the following data: Emissivity box — 0.5 Ther. Reflect. box — 0.5 Accept the current values for the remaining parameters and click Apply

The boundary conditions for the solid-fluid interface should correspond to a conducting wall with emissivity and reflectivity of 0.2 and 0.8, respectively. • • • • • •

Select region no. 4 in the scroll list Select option Conduct. in the Wall Heat pop-up menu. This is essential for solid-fluid interfaces that are not part of region 0. Specify the required radiation properties: Emissivity box — 0.2 Ther. Reflect. box — 0.8 Accept the current values for the remaining parameters and click Apply

Similarly, the top and bottom walls will be adiabatic radiative walls with emissivity and reflectivity of 0.5: • • • • •

Version 4.02

Select region no. 5 in the scroll list Specify the required radiation properties: Emissivity box — 0.5 Ther. Reflect. box — 0.5 Accept the current values for the remaining parameters and click Apply

10-17

Tutorial 10.2


Pre-Processing Patch Specification

Patch All non-symmetry boundary regions need to be divided into radiation patches; these Specification are used both during view factor calculations and for simulating radiative heat transfer. The number of patches per region can be anything between a minimum of one patch covering the entire region to a maximum of one patch per boundary face. The accuracy of radiation calculations is directly proportional to the number of patches per region. Given the two-dimensional character of the problem, it is computationally reasonable to use the maximum number of patches. Patches will be defined for all wall boundaries, with the exception of the fin base; no patches are needed there as this surface does not participate in radiative heat transfer. •

• •

• • • • • Checks

Check the boundaries by listing their properties and then displaying them graphically: •

• • • •

10-18

In the main window, select the Bound Cell Plot Display Option. The fin base boundaries should now be visible, lying in between the two sections of the bottom wall boundaries. Select B > New > Wall Select B > Unselect > Region (Cursor Select) and then click on any boundary belonging to the fin base. This removes all base boundaries from the current set. Select folder Locate Boundaries and open the Create Boundaries panel Go to the Patches tab to create patches using one of the Automatic options Check that option Current Boundary Set is selected in the Boundaries to Patch menu Select By Individual Boundary from the Patch Option menu Click Apply

In the main window, choose Utility > Count > Boundaries and then check the information displayed in the I/O window, i.e. number and type of regions and number of boundaries in each region. You will need to type c in the I/O window to scroll to the end of the list of boundary patches. Select B > New > Wall Select C > All Change the viewpoint to (1, 1, 1) by selecting View > Isometric > 1, 1, 1 Switch on the edge plotting facility by clicking the ‘edge’ button and then click Cell Plot to display Figure T10.2-1

Version 4.02

Tutorial 10.2


Pre-Processing Checks

Figure T10.2-1

Wall boundary plot

Check the patch distribution: •

Select Cell Plot Display Option Patch to display Figure T10.2-2

Figure T10.2-2

Version 4.02

Radiation patch plot

10-19

Tutorial 10.2



Final Operations

It is possible to restart the analysis from the previous non-radiating solution, but since new boundaries have been added we need to use the ‘initial field’ restart option. • • • • •

In the STAR GUIde window, select the Analysis Preparation/Running folder and open the Analysis (Re)Start panel Choose Restart File Option Initial Field Restart. Click the browser button next to the Restart File box, select file fin_bu.ccm from the browser dialog and then click OK Check that the Initial Field Restart menu is set to Restart (New Boundary Types) Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •


CFD Analysis To perform the analysis interactively, proceed as follows: • • • • • •

In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Accept the default Scale Factor of 0.01 Select the Double Precision option Click Write New Geometry File Click the Restart Analysis button

Note that the starting iteration number is shown as no. 1 despite the fact that this is a restart run. This is because we have chosen the initial field restart option. The analysis will start with the calculation of view factors which are then stored in file fin_ra.vfs. These can be used again in future runs as long as the boundaries and patch definitions have not changed. If, however, such changes have been made, you can instruct STAR to re-calculate the view factors through the -noskip option. Post-Processing Preliminaries Check that both the solution file from this tutorial (fin_ra.ccm) and the one from the previous tutorial (fin_bu.ccm) are present in your working directory. 10-20

Version 4.02

Tutorial 10.2



Comparisons will be drawn between the two. Postprocessing

First look at the temperature distribution in the fluid: • • • • • • • • • • • •

In the STAR GUIde window, select the Post-Processing folder and open the Load Data panel In the File(s) tab, click Open Post File Deselect the Patch Cell Plot Display Option in the main window Click Cell Plot Change the viewpoint to (0, 0, 1) by selecting View > Axis > +Z Select C > New > Fluid In the Load Data panel, go to the Data tab Choose Cell & Wall/Bound (Smooth) as the Data Type Select item Temperature from the Scalar Data list Click Get Data and then select Go To > Create Plots In the 3-D Surface tab, choose plot options Contour (filled) and Edge Click Plot to Screen to display Figure T10.2-3

Figure T10.2-3

Temperature contours in the fluid region

To compare the temperatures of the radiation and no-radiation cases, first load the no-radiation solution file: • • • •

Click Go To Load Data In the Load Data panel, select the File(s) tab Use the built-in browser to select file fin_bu.ccm, whose name should then appear inside the Steady State Post File box Click Open Post File

To examine the temperature differences, you will need to use pro-STAR’s OPERATE utility as follows: Version 4.02

10-21

Tutorial 10.2



• • • •

In the main window, select Post > Operate In the Post Register Operations dialog, select Function > Load Cell Data > Temperature Select Load Cell Temperature into Register 2 using Absolute Values Click Apply

Re-load the results of the radiation case by reading the calculated cell temperatures stored in file fin_ra.ccm and then store them in post register 1: • • • •

In the File(s) tab, use the built-in browser to select file fin_ra.ccm, whose name should appear inside the Steady State Post File box Click Open Post File In the Post Register Operations dialog, select Register 1 from the registers pop-up menu Click Apply

Calculate the required differences by subtracting the no-radiation from the radiation temperatures and putting the results in register 4 (the one normally used for scalar data contour plots). • • • •

In the Post Register Operations dialog, select Function > Multi-Register > Subtract In the Post Register Operations dialog, select Register 4 = Register 1 Register 2 Click Apply Close the Post Register Operations dialog

Now plot the differences: • •

10-22

Select Post > Caverage > Cset In the main window, click Replot to display Figure T10.2-4

Version 4.02

Tutorial 10.2



Figure T10.2-4

Contour plot of temperature difference caused by use of radiation model

It can be seen that the introduction of the radiation model has a significant effect on the fluid temperature distribution across the domain. The temperature differences in the solid region can be examined in a similar way. However, they are much less significant, with the variation less than 0.1% of the no-radiation temperature value. Final Operations

Version 4.02

Terminate the session. •


10-23

Tutorial 10.3

RADIATION THROUGH A TRANSPARENT SOLID


Tutorial 10.3


This sub-tutorial examines the effect of replacing the aluminium fin present in the previous two tutorials of this set by an identically-shaped fin made of transparent material (Pyrex glass). As in Tutorial 10.2, the analysis includes the effects of surface-to-surface radiation on heat transfer and temperature distribution. This time, however, the effect of the intervening media (air and transparent solid) on the thermal radiation passing through and being absorbed by them is also investigated. This tutorial aims to show the user how to: • • •

Model radiative heat transfer in the presence of participating media Specify material properties (including radiative properties) for transparent solid domains Use the Discrete Ordinates method (DORM) to solve the problem. Unlike the Discrete Transfer method (DTRM) employed in Tutorial 10.2, DORM does not require radiation patches on the boundaries.


Create a sub-directory for this tutorial called tut10-3 and copy the model file generated in Tutorial 10.1 (fin_bu.mdl) into it Rename this file as fin_dorm.mdl You will use this as a starting point for a revised model that includes the transparent solid. Since the solution obtained in Tutorial 10.1 will act as the starting point of the present analysis, it is also necessary to copy the solution file for the non-radiating case (fin_bu.ccm) to the current directory

Start up the pro-STAR GUI interface: • • • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Accept the default case name (fin_dorm) displayed in the Casename text box Select the Resume existing .mdl file? option Deselect the Append to .echo file? option Click Continue

This will read all data contained in file fin_dorm.mdl and will set up the model as it was at the end of Tutorial 10.1. • •

In the main window, select File > Model Title In the Title text box, change the title to: BUOYANCY DRIVEN FLOW ROUND A HEATED TRANSPARENT FIN

•

Click Apply

Radiative and As mentioned in Tutorial 10.2, radiation can be tracked only through cell types that Thermal are explicitly defined as participating in radiative heat transfer. Since in this case the Properties solid cells are transparent, both fluid and solid cells need to be given this property: Version 4.02

10-25

Tutorial 10.3


Pre-Processing New Boundary Definitions

• • • • • • • • •

Open the Cell Table Editor using the CTAB button on the main window Select Table# 1 (the Fluid cell type) in the scroll list Select On from the Radiation menu Click Apply Select Table# 2 (the Solid cell type) in the scroll list Select On from the Radiation menu Type Pyrex in the Name box Click Apply Close the Cell Table Editor

Specify that both fluid and solid regions will participate in the radiative heat exchange: • • • •

• •

Go to the STAR GUIde window and select the Thermophysical Models and Properties folder Open the Thermal Options panel Select Discrete Ordinates for the Radiation option In the Radiation section, change the Discrete Ordinate Set option to S2. This is the lowest accuracy setting but will ensure that a solution can be reached relatively quickly (see “Capabilities and Limitations of the DORM Method” on page 7-7 of the CCM User Guide). In this panel, note that option (Solid-Fluid) Heat Transfer On is already selected Click Apply

Define relevant material properties: • • • • • • • •

• • • • New Boundary Definitions

The top and bottom adiabatic walls as well as the solid-fluid interface are currently assigned to the default wall region (no. 0). You therefore need to define a separate boundary region for the interface, extending round the entire fin perimeter, in order to assign the appropriate radiative surface properties to it. •

10-26

Select the Liquids and Gases folder Open the Thermal Models panel and then click Show Options Check the default values for the absorption and scattering coefficients (0.1 and 0, respectively). These are reasonable for air. Click Apply Select the Solids folder Open the Material Properties panel and select Material # 2 using the slider at the bottom of the panel Type the transparent solid name (Pyrex) in the Name box Specify appropriate thermal properties for the solid material as follows: Density — 2230 Conductivity — 1.35 Specific Heat — 837.4 Click Apply Open the Radiative Properties panel Enter 0 for both the absorption and scattering coefficients of the solid material Click Apply

In the main window, turn off the Bound option in the Cell Plot Display Version 4.02

Tutorial 10.3



• • • • • • • • • • • • •

Boundary Conditions

Options section Select C > New > Solid Click Cell Plot to display just the solid cells In the STAR GUIde window, select folder Locate Boundaries and then open the Create Boundaries panel In the Regions tab, select region no. 4 in the scroll list Select option Wall from the Type menu Enter a region name (S-F_interface) in the Name box Click Define region In the main window, change the viewpoint to (1, 0, 0) by selecting View > Axis > +X Click Select a Zone and draw a closed polygon around the visible mesh In the main window, change the viewpoint to (-1, 0, 0) by selecting View > Axis > -X Click Select a Zone and draw a closed polygon around the visible mesh In the main window, change the viewpoint to (0, 1, 0) by selecting View > Axis > +Y Again, click Select a Zone and draw a closed polygon around the visible mesh

You must now revisit the boundary conditions of all wall regions in order to define their emissivity, reflectivity and transmissivity. Region 1 (side walls) Specify surface properties for the side walls: • • • • • •

Select folder Define Boundary Conditions and open the Define Boundary Regions panel Select region no. 1 in the scroll list Specify the required radiation properties by entering the following data: Emissivity box — 0.5 Ther. Reflect. box — 0.5 Accept the current values for the remaining parameters and click Apply

Region 2 (the fin base) Define surface properties for the fin base. In addition, change its temperature to 593 K to compensate for the lower thermal conductivity of the glass: • •

•

Select region no. 2 in the scroll list Specify the required temperature and radiation properties: Temperature box — 593 Emissivity box — 0.5 Ther. Reflect. box — 0.5 Accept the current values for the remaining parameters and click Apply

Region 4 (the fluid-solid interface) The solid-fluid interface’s properties have to be set so as to reflect the fact that the solid is transparent: • • Version 4.02

Select region no. 4 in the scroll list Change the Wall Heat option to Conduct. This is essential for solid-fluid 10-27

Tutorial 10.3


Pre-Processing Final Operations

•

•

interfaces that are not part of region 0. Specify appropriate radiation properties: Emissivity box — 0.0 Ther. Reflect. box — 0.0 Ther. Transmis. box — 1.0, i.e. the interface is totally transparent Accept the current values for the remaining parameters and click Apply

Note that the above values imply that the absorptivity of the interface (1 transmissivity - reflectivity = 0) is consistent with the absorptivity defined earlier for the new solid material. Region 0 (top amd bottom walls) As for the side walls, the top and bottom walls will be assigned an emissivity and reflectivity of 0.5: • • • • • Final Operations

Select region no. 0 in the scroll list Specify the required radiation properties: Emissivity box — 0.5 Ther. Reflect. box — 0.5 Accept the current values for the remaining parameters and click Apply

It is possible to restart the analysis from the previous non-radiating solution, but since new boundaries have been added we need to use the ‘initial field’ restart option. • • • • • •

In the STAR GUIde window, select the Analysis Preparation/Running folder and open the Analysis (Re)Start panel Choose Restart File Option Initial Field Restart. Click the browser button next to the Restart File box, select file fin_bu.ccm from the browser dialog and then click OK Check that the Initial Field Restart menu is set to Restart (New Boundary Types) Check that the Iteration Counter option is set to Reset Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively. This process is described in the next section. • • • • • •

10-28

In the main pro-STAR panel, select File > Write Geometry File In the Geometry File Write dialog, check that 0.01 appears in the Scale Factor box Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

Version 4.02

Tutorial 10.3



CFD Analysis To perform the analysis interactively, proceed as follows: • • • • • •

In the main pro-STAR panel, select File > Save Model In the Analysis Preparation/Running folder, open the Run Analysis Interactively panel Accept the default Scale Factor of 0.01 Select the Double Precision option Click Write New Geometry File Click the Restart Analysis button

Note that the starting iteration number is shown as no. 1 despite the fact that this is a restart run. This is due to the initial field restart options specified. Post-Processing Preliminaries Read in the results of the analysis from file fin_dorm.ccm: • • • Postprocessing

First look at the velocity field in the fluid surrounding the fin: • • • • • • • •

Version 4.02

In the STAR GUIde window select the Post-Processing folder Open the Load Data panel Click Open Post File

In the main window, select C > New > Fluid Click Cell Plot Change the viewpoint to (0, 0, 1) by selecting View > Axis > +Z In the Load Data panel, go to the Data tab Select item Velocity Components UV option for Vector Data list and then click Get Data to load the velocity field Select Go To > Create Plots, where the plot style will be defined In the 3-D Surface tab, check that Option Vector is selected and then choose Edge from the Edge/Mesh menu Click Plot to Screen to display Figure T10.3-1

10-29

Tutorial 10.3



Figure T10.3-1

Velocity vectors

Examine the temperature profiles, both in the surrounding fluid and in the solid fin: • • • • • • • • • • • • •

10-30

Click Go To Load Data Select Cell & Wall/Bound (Smooth) from the Data Type menu Select item Temperature from the Scalar Data list Click Get Data and then select Go to > Create Plots In the 3-D Surface panel, choose Option Contour (filled) Click Plot to Screen to display Figure T10.3-2 In the main window, select C > New > Solid In the Create Plots panel, click Go To Load Data In the Data tab, select Data Type Cell Select On and Cset for the Smooth Option Select item Temperature from the Scalar Data list Click Get Data Click Cell Plot to display Figure T10.3-3

Version 4.02

Tutorial 10.3



Final Operations

Version 4.02

Figure T10.3-2

Temperature contours in the fluid region

Figure T10.3-3

Temperature contours in the solid region

Terminate the session. •


10-31

Tutorial 11 MOVING GRIDS To be included in the next STAR-CD 4 release.

Version 4.02

11-1

11-2

Version 4.02

Tutorial 12 EULERIAN TWO-PHASE FLOW The following tutorials are intended to familiarise users with the process of setting up Eulerian two-phase simulations. The four cases presented are: 1. Bubble terminal velocity simulation 2. Bubbly flow in which bubbles are allowed to escape through the free surface of the liquid 3. Fluidised bed simulation 4. Boiling simulation

Version 4.02

12-1

Tutorial 12.1

TERMINAL VELOCITY OF BUBBLES

Tutorial 12.1


In this case, air bubbles and water are injected at the bottom of a vertical channel at 1 m/s. The main forces acting on the bubbles are buoyancy and drag. Starting at the inlet, the bubbles are accelerated due to buoyancy but pulled back due to drag from the surrounding water and reach their terminal rise velocity when the drag force is balanced by the buoyancy force. Mathematically, we can express this force balance as: 3 2 CD πd 2πd ---------- ∆ρ g = ------- ρ c u r ---------6 2 4

where d is the bubble diameter, ρ the density, ∆ρ = ρ c – ρ d the density difference between the two phases, g the acceleration of gravity, C D the drag coefficient and u r = u c – u d the relative velocity between the two phases. Subscripts c and d denote the continuous and dispersed phase, respectively. The above equation can be re-arranged to give an expression for the relative velocity between the phases, which in this case is also the bubble terminal rise velocity: ur =

4 ∆ρ gd -- ------ ------3 ρc C D

In this tutorial we will use the following data for the two phases: • •

Phase 1 is water with density of 1000 kg/m3 and viscosity of 0.001 kg/m/s Phase 2 is air bubbles of 2 mm diameter with density of 1 kg/m3 and viscosity of 1 × 10–5 kg/m/s

Assuming C D = 0.44 and substituting the physical properties of the two phases into the above equation, we obtain: ur =

29.7d

For 2mm bubbles, the relative velocity is 0.24 m/s. Since the water phase is moving up the channel at 1 m/s, the terminal rise velocity of the bubbles is 1.24 m/s. We will now set up this case, carry out an Eulerian two-phase flow calculation and check whether the computed bubble rise velocity agrees with the value given by the equations above.

12-2

Version 4.02

Tutorial 12.1



0.1 m Outlet gy

1.0 m Slip wall on all side walls

y

x Inlet Figure T12.1-1

Schematic of vertical flow channel

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut12-1. The mesh for this problem is supplied in advance, i.e. cell, vertex, boundary and problem setup files (channel.cel, channel.vrt, channel.bnd and channel.inp, respectively) are available in the STAR-CD installation directories. Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, ter_vel) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is channel.inp Click Apply Click Close

This will read default problem settings from file channel.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: TERMINAL VELOCITY OF BUBBLES

Version 4.02

12-3

Tutorial 12.1


Pre-Processing Material Properties and Thermofluid Models

•

Click Apply

Verify that the correct mesh has been imported by selecting all cells and plotting the mesh in ‘Hidden Surface’ mode: • • • • •

In the main window, select C > All Check that Hidden Surface is the default cell plot type Select View > Isometric > 1, 1, 1. A 2D mesh corresponding to Figure T12.1-1 should appear on your screen. Click Cell Plot Select View > Axis > +Z

Make sure that the STAR-GUIde window is displayed on your screen, next to the main pro-STAR window. •


This enables you to set the basic features of your model and ensures that only those panels that are essential for your analysis are activated. For this tutorial, the following special settings are required: • • Material Properties and Thermofluid Models

Select option Eulerian Multi-Phase from the Multi-Phase Treatment menu Click Apply

We now assign physical properties to the two phases: • • • • • • •

• • •

•

Select the Thermophysical Models and Properties folder Open the Gravity panel and change the Direction of Gravity Force to (0, -1, 0) Click Apply Select the Liquid and Gases folder Open the Molecular Properties panel Make sure the Phase# slider at the bottom of the panel is in the Phase#1 position Assign appropriate property values for phase 1. Thermal properties are not relevant in this case so they may be left at their default values: Name — Water Density – 1000 Molecular Viscosity – 0.001 Click Apply Move the Phase# slider to the Phase#2 position Assign appropriate property values for phase 2 as follows: Name — Air Density – 1 Molecular Viscosity – 1.0e-5 Click Apply

Initialize phase 1 field values as follows: • • • 12-4

Open the Initialization panel Make sure the Phase# slider at the bottom of the panel is in the Phase#1 position Set the V velocity to 1 m/s Version 4.02

Tutorial 12.1



•

Click Apply

Initialize phase 2 field values as follows: • • • •

Move the Phase# slider to the Phase#2 position Set the V velocity to 1 m/s Set the Volume fraction to 0.001 Click Apply

Select locations for the pressure reference and monitoring cells as follows: • • •

•

Open the Monitoring and Reference Data panel Click the mouse icon button next to the Monitoring cell number box and then pick the top middle cell in the main window (or enter 150 in the box). Click the mouse button next to the Reference Pressure Cell Number box and then pick the top right hand corner cell in the main window (or enter 250 in the box). Click Apply

Turn on the buoyancy force as follows: • • • • •

Open the Buoyancy panel Click On Select option Centroid of pressure reference cell for the datum location Select option Use reference and/or initial values, together with Reference pressure and Reference temperature for the datum density value Click Apply

We now define the interaction between the two phases: • • • •

Select the Eulerian Multi-Phase folder followed by the Interphase Momentum Transfer sub-folder Open the Drag Forces panel Select Constant in the menu at the top of the panel and accept the default Drag Coefficient value of 0.44 shown in the Constant box Click Apply

Set the bubble diameter to 2 mm: • • • Boundary Conditions

First we re-define all walls as ‘slip’ walls: • • • • • • • •

Version 4.02

Open the Particle Size panel Enter 0.002 in the Mean Diameter box. Click Apply

Select the Define Boundary Conditions folder and then open the Define Boundary Regions panel Select Reg#0 for Wall in the scroll list Move the Phase# slider at the bottom of the panel to the Phase#1 position Select Slip from the Slip Option menu Click Apply Move the Phase# slider to the Phase#2 position Select Slip from the Slip Option menu Click Apply 12-5

Tutorial 12.1



We now define the inlet conditions: • • • • • • •

Select Reg#1 in the scroll list Move the Phase# slider at the bottom of the panel to the Phase#1 position Enter 1 m/s for the V velocity and 1000 kg/m3 for the Density Click Apply Move the Phase# slider to the Phase#2 position Enter 1 m/s for the V velocity, 1 kg/m3 for the Density and 0.001 for the Vol. Fraction Click Apply

No extra input is needed for the Outlet boundary. Analysis Controls

We will now specify various solver parameters required for this case: • • • • • • • • • • • • • • •

Run Time Controls

Set the number of iterations to 1000 for this case: • • • •

Final Operations

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Change the Number of Iterations to 1000 and the Max. Residual Tolerance to 1.0e-5 Click Apply

If you wish to terminate the session at this stage, write the geometry and problem files and exit from pro-STAR, saving the model data as shown below: • • • • •

12-6

Select folder Analysis Controls followed by Solution Controls followed by Equation Behavior Open the Primary Variables panel and go to the Equation Status tab Move the Phase# slider at the bottom of the panel to the Phase#1 position Deselect item W-mom since we are solving a 2D flow in the x-y plane only Click Apply Move the Phase# slider to the Phase#2 position Deselect item W-mom Click Apply Go to the Solver Parameters tab Move the Phase# slider to the Phase#1 position Change the Relaxation Factor to 0.3 for Momentum and 0.1 for Pressure Click Apply Move the Phase# slider to the Phase#2 position Change the Relaxation Factor to 0.3 for Momentum and 0.1 for Volume Fraction Click Apply


Version 4.02

Tutorial 12.1



CFD Analysis You can now continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively without quitting pro-STAR. Alternatively, you may run the CFD analysis (in double precision) by typing star -dp in your session window. Post-Processing Examine the velocities of the two phases at the channel exit: the water velocity (phase 1) should remain close to 1 m/s and the bubble velocity (phase 2) should be around 1.24 m/s, as calculated by equation above. This can be done very effectively by plotting the monitored value for the V velocity as follows: • • • •

Select folder Analysis Preparation/Running Open the Run History of Previous Analysis panel Select item V-Component and then move the Phase# slider to the Phase#1 position Click Plot Monitor History to display monitored values for the V-velocity component of phase 1, as shown in Figure T12.1-2

Figure T12.1-2

• • • Version 4.02

V-velocity history plot for phase 1

Move the Phase# slider to the Phase#2 position Click Plot Monitor History to display monitored values for the V-velocity component of phase 2, as shown in Figure T12.1-3 In the main window, select File > Quit > Quit,Nosave 12-7

Tutorial 12.1


Suggestions for Further Exercises Final Operations

Figure T12.1-3

V-velocity history plot for phase 2

Suggestions for Further Exercises Other bubble rise cases You may wish to repeat this tutorial with different input parameters; for example, change the density of the fluid or use a different bubble diameter. Recalculate the terminal velocity using equation and compare the answer with the simulation results. Terminal velocity of solid particles Another exercise you may want to perform is to simulate the terminal velocity of a falling solid sphere. In this case, both phases are moving in the same direction as gravity (downwards). To re-use the setup described above, you can simply change the gravity vector direction to (0, 1, 0). Try this exercise with the following parameters: • •

Phase 1 is water, density = 1000, viscosity = 0.001 Phase 2 is steel spheres, density = 8000, viscosity = 1.0e-5, diameter = 1.0e-4

Substituting these parameters into equation , we get: ur =

208.1d

For steel spheres of 1.0e-4m diameter, the terminal velocity is 1.144 m/s with the background fluid moving at 1 m/s. The terminal velocity relative to the background fluid is 0.144 m/s.

12-8

Version 4.02

Tutorial 12.2

AERATION TANK


Tutorial 12.2

AERATION TANK

Aeration is used in many process industries. Air or gas bubbles are injected into a liquid to promote mixing and mass transfer of chemical species between the phases. An example of this is the transfer of oxygen from air bubbles to a liquid for oxidation reactions. In this tutorial, we consider an aeration tank commonly used in the treatment of waste water. 2m Degassing outlet gy 1m

y

x Air inlet Figure T12.2-1

Outline of an aeration tank

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut12-2. The mesh for this problem is supplied in advance, i.e. cell, vertex, boundary and problem setup files (tank.cel, tank.vrt, tank.bnd and tank.inp, respectively) are available in the STAR-CD installation directories. Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, aer_tank) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is tank.inp Click Apply Click Close

This will read default problem settings from file tank.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. Version 4.02

12-9

Tutorial 12.2

AERATION TANK


• •

In the main window, select File > Model Title In the Title text box type: AERATION TANK

•

Click Apply



Make sure that the STAR-GUIde window is displayed on your screen, next to the main pro-STAR window. This enables you to set the basic features of your model and ensures that only those panels that are essential for your analysis are activated. •

Material Properties and Thermofluid Models

Open the Select Analysis Features panel and check the current settings. It will be seen that option Eulerian Multi-Phase is already selected from the Multi-Phase Treatment menu so no further adjustment is necessary.

We now assign physical properties to the two phases. • • • • • • •

• • •

•

Select the Thermophysical Models and Properties folder Open the Gravity panel and change the Direction of Gravity Force to (0, -1, 0) Click Apply Select the Liquid and Gases folder Open the Molecular Properties panel Make sure the Phase# slider at the bottom of the panel is in the Phase #1 position Assign appropriate property values for phase 1. Thermal properties are not relevant in this case so they may be left at their default values: Name — Water Density – 1000 Molecular Viscosity – 0.001 Click Apply Move the Phase# slider to the Phase#2 position Assign appropriate property values for phase 2 as follows: Name — Air Density – 1 Molecular Viscosity – 1.0e-5 Click Apply

Specify that the flow is turbulent and set up the turbulence drag force: • • • 12-10

Open the Turbulence Models panel In the Turbulence tab, click On and then Apply Go to the Multiphase Options tab Version 4.02

Tutorial 12.2

AERATION TANK


• •

Select option Bubble-Eddy Interaction from the Ct Model menu Select On for Turbulence Drag and then click Apply

Initialise phase 1 field values as follows: • • •

Open the Initialization panel Move the Phase# slider at the bottom of the panel to the Phase#1 position Click Apply, since the default values are all acceptable.

Initialise phase 2 values as follows: • • •

Move the Phase# slider to the Phase#2 position Set the Volume fraction to 0.001 Click Apply

Select locations for the pressure reference and monitoring cells as follows: • •

•

•

Go to the Monitoring and Reference Data panel Click the mouse icon button next to the Monitoring cell number box and then pick a cell above the air injector in the top row of cells (or enter 650 in the box). Click the mouse button next to the Reference Pressure Cell Number box and then pick the top right hand corner cell in the main window (or enter 5000 in the box). Click Apply



We now define the interactions between the two phases: • • • •

Select the Eulerian Multi-Phase folder followed by the Interphase Momentum Transfer sub-folder Open the Drag Forces panel Select Bubbles in the menu at the top of the panel Click Apply

Set the bubble diameter to 3 mm: • • • Boundary Conditions

We now define boundary conditions at the inlet: • •

Version 4.02

Open the Particle Size panel Enter 0.003 in the Mean Diameter box Click Apply

Select the Define Boundary Conditions folder and then open the Define Boundary Region panel Select Reg#1 in the scroll list 12-11

Tutorial 12.2

AERATION TANK


• • •

Move the Phase# slider at the bottom of the panel to the Phase#1 position Enter 1000 kg/m3 for Density Click Apply

Define the injection of air bubbles (phase 2) at the inlet: • • •

Move the Phase# slider to the Phase#2 position Enter 0.25 m/s for the V velocity, 1 kg/m3 for Density and 0.5 for the Vol. Fraction Click Apply

No user input is needed for Reg#2 in the scroll list which is already defined as the Degassing outlet. Analysis Controls

We will now specify appropriate solver parameters for this case: • • • • • • • • • • • • • • •

Run Time Controls

Set the number of iterations to 6,000 for this case: • • • •

Final Operations



12-12

Select folder Analysis Controls followed by Solution Controls followed by Equation Behavior Open the Primary Variables panel and go to the Equation Status tab Move the Phase# slider at the bottom of the panel to the Phase#1 position Deselect item W-mom since we are solving a 2D flow in the x-y plane only. Click Apply Move the Phase# slider to the Phase#2 position Deselect item W-mom Click Apply Go to the Solver Parameter tab Move the Phase# slider to the Phase#1 position Change the Relaxation Factor to 0.3 for Momentum and 0.1 for Pressure. Click Apply Move the Phase# slider to the Phase#2 position Change the Relaxation Factor to 0.3 for Momentum and 0.1 for Volume Fraction. Click Apply


Version 4.02

Tutorial 12.2

AERATION TANK


CFD Analysis You may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively without quitting pro-STAR. Alternatively, you may run the CFD analysis (in double precision) by typing star -dp in your session window. Post-Processing Preliminaries Use pro-STAR to check the analysis results by first reading in the data stored in file aer_tank.ccm: • • • Postprocessing

First, examine the velocity of phase 1: • • • • • • •

Version 4.02


Go to the Data tab and check that Data Type Cell is selected Check that the Phase# slider is in the Phase #1 position In the Vector Data list, select item Velocity Components UV to load the two velocity components in the plane of analysis for phase 1 Click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select Vector from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen to display Figure T12.2-2

12-13

Tutorial 12.2

AERATION TANK


Figure T12.2-2

Velocity vector plot for phase 1

Next, plot velocity vectors of phase 2: • • • • •

12-14

Go back to the Load Data panel by clicking Go To Load Data Move the Phase# slider to the Phase #2 position In the Vector Data list, select item Velocity Components UV to load the two velocity components in the plane of analysis for phase 2 Click Get Data In the main window click Replot to display Figure T12.2-3

Version 4.02

Tutorial 12.2

AERATION TANK


Figure T12.2-3

Velocity vector plot for phase 2

Finally, display a contour plot of the phase 2 volume fraction: • • • • • •

Version 4.02

In the Data tab, select option Cell & Wall/Bound (Smooth) from the Data Type menu In the Vector Data list, select None In the Scalar Data list, select item Volume Fraction and then click Get Data Select Go To > Create Plots to display the Create Plots panel In the 3-D Surface tab, select plot options Contour (filled) and Edge Click Plot to Screen to display Figure T12.2-4

12-15

Tutorial 12.2

AERATION TANK

Suggestions for Further Exercises Post- processing

Figure T12.2-4

Phase 2 volume fraction contour plot

It will be seen that bubbles rise from the injection point to the top surface. The rising bubbles also lift the water around them and create an up-flow of liquid above the injector. Under the top surface, the flow turns horizontally to the right and then downwards on the right-hand-side of the tank. The bubbles are carried by the flow and spread across the top surface, some being carried downwards again by the down-flow on the right-hand-side. Suggestions for Further Exercises Bubble columns Changing the geometry of this tutorial to a cylindrical tank results in a model for a bubble column. Gas-liquid mixing vessels Adding a rotating impeller to the tank results in a model for a gas-liquid mixing vessel (see Tutorial 11.2 describing the setup of a moving-mesh case involving a rotating impeller).

12-16

Version 4.02

Tutorial 12.3

FLUIDISED BED RISER


Tutorial 12.3

FLUIDISED BED RISER

This tutorial is intended to familiarise users with the process of setting up an Eulerian two-phase calculation for fluidised beds. Fluidised beds are used in many process industries for drying, gasification and burning of coal particles and in fluidised catalytic crackers (FCC’s). Usually the lower portion of the equipment is loaded with solid particles. The particle concentration is close to the maximum packing limit, around 63% in volume fraction. A gas is blown through the bottom inlet boundary and through the particles, lifting and moving them by virtue of drag forces. The particle motions are random and constantly changing with time, hence it is necessary to model fluidised beds in transient mode. Often, the gas moves through the particles in the form of large gas pockets called ‘bubbles’. In this tutorial, we consider a simple fluidised bed similar to the riser of a fluidised catalytic cracker unit. 0.15m × 0.15m Pressure outlet Free board

gy 1m

Fluidised bed y x Air inlet Figure T12.3-1

Outline of a FCC riser

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut12-3. The mesh for this problem is supplied in advance, i.e. cell, vertex, boundary and problem setup files (riser.cel, riser.vrt, riser.bnd and riser.inp, respectively) are available in the STAR-CD installation directories. Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, fcc_riser) in the Casename text box Click Continue

Read in the available problem data: • Version 4.02

Select File > Read File... in the main pro-STAR window 12-17

Tutorial 12.3

FLUIDISED BED RISER


• • •

In the Input Coded Command File dialog check that the File Name is riser.inp Click Apply Click Close

This will read default problem settings from file riser.inp plus the problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: FLUIDISED BED RISER

•

Click Apply





This enables you to set the basic features of your model and ensures that only those panels that are essential for your analysis are activated. For this tutorial, the following special settings are required: • • • Material Properties

Select option Transient from the Time Domain menu Select option Eulerian Multi-Phase from the Multi-Phase Treatment menu Click Apply

We now assign physical properties to the two phases: • • • • •

Select the Thermophysical Models and Properties folder Open the Gravity panel and change the Direction of Gravity Force to (0, -1, 0) Click Apply Select the Liquid and Gases folder Open the Molecular Properties panel

Assign appropriate property values to phase 1. Thermal properties are not relevant in this case so they may be left at their default values. • •

12-18

Make sure the Phase# slider at the bottom of the panel is in the Phase#1 position Enter the following values: Name — Air Density — 1.205 Version 4.02

Tutorial 12.3

FLUIDISED BED RISER

Pre-Processing Initialisation

•

Molecular Viscosity — 1.81e-5 Click Apply

Assign appropriate property values to phase 2. In this case, the only relevant property is the particle density. However, in the “Other Model Settings” section, the kinetic theory model will be used to calculate solid-phase forces and this employs an internally calculated solid-phase viscosity. Since the value supplied in the current panel is added to the calculated one and in order not to affect the latter, the panel’s phase viscosity should to be set to a very small value. • •

• Initialisation

Move the Phase# slider to the Phase#2 position Enter the following values: Name — Solid Density — 2600 Viscosity — 1.0e-6 Click Apply

As can be seen in Figure T12.3-1, the particles are initally situated in the lower half of the riser. Therefore, all cells in the model below 0.5m in the vertical (y-direction) need to be assigned a value for the initial particle volume fraction, 0.58 in this case. Above the 0.5m level, the volume fraction has to be set to a small value, say 0.001, in order to ensure the stability of the numerical solution algorithm. The above initialisation is performed using subroutine INITFI, as shown below: • • • • • •

Signal to pro-STAR that this case requires a user subroutine by choosing File > System Command from the main window Type ufiles in the text box, click Apply and then Close Open the Initialization panel Move the Phase# slider at the bottom of this panel to Phase#1 position Select option User from the Values menu and then click Define user coding Accept the default values in the rest of the panel by clicking Apply

The complete contents of INITFI for this case are shown in the “User Subroutine” section below. Other Model Settings

Select locations for the pressure reference and monitoring cells as follows: • • • •

Go to the Monitoring and Reference Data panel Click the mouse icon button next to the Monitoring cell number box and then pick a cell in the lower half of the model geometry (or enter 1121 in the box). Click the mouse button next to the Reference Pressure Cell Number box and then pick the top right hand corner cell (or enter 2000 in the box). Click Apply

Turn on the buoyancy force as follows: • • •

Open the Buoyancy panel Click On Accept the default setting by clicking Apply

We now define the interaction between the two phases: • Version 4.02

Select the Eulerian Multi-Phase folder followed by the Interphase Momentum 12-19

Tutorial 12.3

FLUIDISED BED RISER


• • • • • • •

Transfer sub-folder Open the Drag Forces panel Select option High Particle Loading, leaving the default values unchanged Click Apply Open the Other Forces panel Select option Kinetic Theory Model from the Solid Particle Stress menu Accept the defaults shown for Maximum Volume Fraction and Restitution Coefficient Click Apply

Finally, set the particle diameter to 0.3 mm: • • • Boundary Conditions

Open the Particle Size panel Enter 0.0003 in the Mean Diameter text box. Click Apply

Define boundary conditions at the inlet: • • • • •

Select the Define Boundary Conditions folder, then open the Define Boundary Regions panel Select Reg#1 in the scroll list Move the Phase# slider at the bottom of the panel to Phase#1 position Enter 0.35 m/s for the V velocity Click Apply

Now define particle (phase 2) conditions at the inlet: • • •

Move the Phase# slider l to the Phase#2 position Enter 2600 kg/m3 for Density and 0 for Vol. Fraction Click Apply

Finally, define boundary conditions at the pressure outlet: • • • • Analysis Controls

Output Controls 12-20

Select Reg#2 in the scroll list Move the Phase# slider at the bottom of the panel to the Phase#2 position Select option Vol. Frac. from the VF Switch menu and enter 0 in the Vol. Fraction box Click Apply

Specify various solver parameters relevant to this case: • • • • • • • • •

Select folder Analysis Controls followed by Solution Controls Select sub-folder Equation Behavior Open the Primary Variables panel and go to the Equation Status tab Move the Phase# slider at the bottom of the panel to the Phase#1 position Deselect option W-Mom since we are only solving a 2D flow in the x-y plane Click Apply Move the Phase# slider to the Phase#2 position Deselect option W-mom Click Apply

Set the frequency of outputting calculated transient data during the analysis: •

Select the Output Controls folder and then open the Analysis Output panel Version 4.02

Tutorial 12.3

FLUIDISED BED RISER

User Subroutine Run Time Controls

• • •

• • •

In the Post tab, enter 1000 for both the Output frequency and Backup frequency Click Apply In the Transient tab, enter 0.025 (seconds) in the Write data every box. As can be seen on the panel, velocity and pressure data will be written by default at the above frequency. Move the Phase# slider to the Phase#2 position and select item Volume Fraction from the list of data items shown Click the Post button, which selects this item (along with the phase velocity) for output to the transient post file Click Apply

Set the run duration to 2 seconds and the time step to 1 x 10-4 seconds:

Run Time Controls

• • • • • •

Final Operations

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Enter 2 in the Run for box Click Apply Enter 1e-4 in the Time Step for Period box Click Set Period at the bottom of the panel

If you wish to terminate the session at this stage, write the geometry and problem files and exit from pro-STAR, saving the model data as shown below. • • • • •


User Subroutine Introduce the user code needed to initialise particle volume fractions and gas velocities via pro-STAR’s built-in editor. For this purpose, edit subroutine INITFI (in file initfi.f, sub-directory ufile) as follows: • • • • • • • •

In the main pro-STAR panel, select File > Edit File In the pro-STAR Editor dialog, click File > Open In the File Selection dialog, enter sub-directory ufile and select file initfi.f Click OK Edit the contents of the subroutine by adding extra lines of code after the explanatory section, as shown below Click File > Save In the File Selection dialog, re-specify ufile / initfi.f as the save location of the modified subroutine Click File > Quit to exit from the editor

C************************************************************************* SUBROUTINE INITFI(U,V,W,PR,TE,ED,T,SCALAR,XVF2) C Initialise fields C************************************************************************* C--------------------------------------------------------------------------* Version 4.02

12-21

Tutorial 12.3

FLUIDISED BED RISER


C STAR-CD VERSION 4.00 C--------------------------------------------------------------------------* INCLUDE 'comdb.inc' COMMON/USR001/INTFLG(100) DIMENSION SCALAR(50) INCLUDE 'usrdat.inc' EQUIVALENCE( UDAT12(001), ICTID ) EQUIVALENCE( UDAT03(001), CON ) EQUIVALENCE( UDAT04(001), CP ) EQUIVALENCE( UDAT04(002), DEN ) EQUIVALENCE( UDAT04(062), VISM ) EQUIVALENCE( UDAT04(063), VIST ) EQUIVALENCE( UDAT04(067), X ) EQUIVALENCE( UDAT04(068), Y ) EQUIVALENCE( UDAT04(069), Z ) C------------------------------------------------------------------------C C This subroutine enables the user to initialise the following C dependent variables: U,V,W,PR,TE,ED,T,SCALAR,XVF2 to arbitrary C values. C C ** Parameters to be returned to STAR: U,V,W,PR,TE,ED,T, C SCALAR,XVF2 C C The returned velocity components (U, V and W) are in the C coordinate system requested for initialisation. C C-------------------------------------------------------------------------C C.....HEIGHT OF FLUIDISED BED HBED=0.5 C.....SOLID VOLUME FRACTION IN BED VFSOL=0.58 C.....MINIMUM VOLUME FRACTION VFMIN=0.001 C U=0.0 V=0.0 W=0.0 IF (IPHA.EQ.2) THEN IF (Y.LE.HBED) THEN XVF2=VFSOL ELSE XVF2=VFMIN END IF ENDIF C RETURN END

CFD Analysis You may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively without quitting pro-STAR. Alternatively, you may run the CFD analysis (in double precision) by typing 12-22

Version 4.02

Tutorial 12.3

FLUIDISED BED RISER


star -dp in your session window. Post-Processing Use pro-STAR to display the results stored in the .pstt file and check the volume fraction of the second phase: • • • • • •

• • • • • • • •

Version 4.02

In the STAR GUIde window, select folder Post-Processing Open the Load Data panel to display the File(s) tab Select option Transient from the Analysis menu Check that file fcc_riser.pstt appears in the File Name box and then select the first position in the Transient Post File(s) list Click Add File to List Select the first position in the list again and then click Open Transient Post File; the time steps at which analysis results were stored during the run should appear in the Select Time Step scroll list In the Select Time Step list, select the fourth step at which data are available (i.e. at time 0.1 s) Click Store Iter/Time Go to the Data tab and select Cell & Wall/Bound (Smooth) in the Data Type menu Move the Phase# slider to the Phase#2 position and select item Volume Fraction from the Scalar Data list Click Get Data at the bottom of the panel Select Go To > Create Plots In the 3-D Surface tab select Contour (filled) for Option and Edge for Edge/Mesh Click Plot to Screen to display the particle volume fraction at the chosen time step, as shown in Figure T12.3-2

12-23

Tutorial 12.3

FLUIDISED BED RISER


Figure T12.3-2

Phase 2 volume fraction at time 0.1s

Now fix the colour scale to a range between 0 and 1: • • • •

Go to the Options tab In the Color Scale section, select User from the Range menu and enter 0 in the first box and 1 in the second Click Apply In the main graphics window, click Replot

The above process may be repeated for each of the results calculated every 0.025 seconds in the analysis. However, the best way of displaying these is by instructing pro-STAR to loop over the entire post file. To do this, type the following commands in the I/O window: *set itno 250 250 *define stor iter itno egev 2 none vf cset news fluid cplot *end *loop 1 79 1 Examine the volume fraction plots in the time sequence of your outputs. You should see ‘gas bubbles’ rise through the particle bed. The flow is rather random and chaotic, with particles pushed around by the gas flow. The maximum particle volume fraction should be around the maximum packing value set in the model (typically 0.63). From time to time a higher maximum volume fraction can occur in one or two spots. 12-24

Version 4.02

Tutorial 12.4

BOILING SIMULATION


Tutorial 12.4

BOILING SIMULATION

This tutorial is intended to familiarise users with the process of setting up an Eulerian two-phase model for boiling problems. The solution domain is a vertical channel whose geometry is shown below. The flow regime consists of superheated water entering the channel at the bottom, some of the water evaporating into steam bubbles, and a water/steam mixture emerging from the pressure boundary outlet at the top. 0.1m × 0.1m Steam/water outlet Steam bubbles

gy 2m

y x Superheated water Figure T12.4-1

Outline of flow channel with boiling

Pre-Processing Preliminaries Create a sub-directory for the tutorial called tut12-4. The mesh for this problem is supplied in advance, i.e. cell, vertex, boundary and problem setup files (channel2.cel, channel2.vrt, channel2.bnd and channel2.inp, respectively) are available in the STAR-CD installation directories. Therefore, before starting the tutorial, make sure that these files are copied into your current directory. • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name (say, boil) in the Casename text box Click Continue


Select File > Read File... in the main pro-STAR window In the Input Coded Command File dialog check that the File Name is channel2.inp Click Apply Click Close

This will read default problem settings from file channel2.inp plus the Version 4.02

12-25

Tutorial 12.4

BOILING SIMULATION


problem’s cell, vertex and boundary location definitions from the remaining three files. • •

In the main window, select File > Model Title In the Title text box type: CHANNEL FLOW WITH BOILING

•

Click Apply





This enables you to set the basic features of your model and ensures that only those panels that are essential for your analysis are activated. For this tutorial, the following special settings are required: • • Material Properties and Thermofluid Models

Assign physical properties to the two phases. • • • • • • •

• • •

12-26

Select option Eulerian Multi-Phase from the Multi-Phase Treatment menu Click Apply

Select the Thermophysical Models and Properties folder Open the Gravity panel and change the Direction of Gravity Force to (0, -1, 0) Click Apply Select the Liquid and Gases folder Open the Molecular Properties panel Make sure the Phase# slider at the bottom of the panel is in the Phase#1 position Assign appropriate property values for phase 1 as follows: Name – Water Density – 958 Molecular Viscosity – 0.000283 Specific Heat – 4218 Conductivity – 0.681 Molecular Weight – 18 Click Apply Move the Phase# slider to the Phase#2 position Assign appropriate property values for phase 2 as follows: Name – Steam Density – 0.6 Version 4.02

Tutorial 12.4

BOILING SIMULATION


•

Molecular Viscosity – 1.2e-5 Specific Heat – 2034 Conductivity – 0.0248 Molecular Weight – 18 Click Apply

Turn on the solution of the energy equation: • •

Open the Thermal Models panel For each of the two phases: Click Temperature Calculation On Click Apply

Initialise field values as follows: • • •

• • •

•

Open the Initialization panel Move the Phase# slider at the bottom of the panel to the Phase#1 position Check that Values option is Constant and then enter the following values: V velocity – 0.5 m/s Temperature – 375 Accept the default values for the remaining parameters and then click Apply Move the Phase# slider to the Phase#2 position Enter the following values: V velocity – 0.5 m/s Volume Fraction – 0.01 Temperature – 373 Accept the default values for the remaining parameters and then click Apply

Select locations for the pressure reference and monitoring cells as follows: • • •

• •

Go to the Monitoring and Reference Data panel Click the mouse icon button next to the Monitoring cell number box and then pick a cell in the lower half of the geometry (or enter 44 in the box). Click the mouse button next to the Reference Pressure Cell Number box and then pick the top right hand corner cell in the main window (or enter 100 in the box). Enter 273 for Temperature Click Apply



Define the interactions between the two phases: • • Version 4.02

Select the Eulerian Multi-Phase folder followed by the Interphase Momentum Transfer sub-folder Open the Drag Forces panel 12-27

Tutorial 12.4

BOILING SIMULATION


• •

Select Bubbles in the menu at the top of the panel Click Apply

Interphase heat transfer will be defined later via a user subroutine, so the Nusselt Number shown in STAR GUIde may be set to zero: • • •

Open the Interphase Heat Transfer panel Select Constant and enter 0 in Nusselt number box Click Apply

Set the bubble diameter to 1 mm: • • •

Open the Particle Size panel Enter 0.001 in the Mean Diameter box Click Apply

The boiling heat and mass transfers are to be defined as source terms via user subroutines. First, you need to create a ufile sub-directory in your working directory to store the subroutines: • •

Signal to pro-STAR that this case requires user subroutines by choosing File > System Command from the main window Type ufiles in the text box, click Apply and then Close

Prepare the user subroutines for mass and energy sources as follows: • • • Boundary Conditions

Select the Sources folder and then open the Source Terms panel In the Mass tab, click On, select User Coding and then click Apply and Define User Coding In the Enthalpy tab, click On, select User Coding and then click Apply and Define User Coding

Define boundary conditions at the inlet: • • • •

• • •

•

Select the Define Boundary Conditions folder and then open the Define Boundary Region panel Select Reg#1 in the scroll list Move the Phase# slider at the bottom of the panel to the Phase#1 position Enter the following values: V velocity – 0.5 Dens. – 958 Temp. – 375 Click Apply Move the Phase# slider to the Phase#2 position Enter the following values: V velocity – 0.5 Dens. – 0.6 Temp. – 373 Vol. Fraction – 0.01 Click Apply

Define boundary conditions at the pressure outlet: • 12-28

Select Reg#2 in the scroll list Version 4.02

Tutorial 12.4

BOILING SIMULATION

User Subroutines Analysis Controls

• • • • • • • Analysis Controls

Move the Phase# slider at the bottom of the panel to Phase#1 position Select Zero Grad for the Temp. Switch Click Apply Move the Phase# slider to the Phase#2 position Select Zero Grad for the Temp. Switch Select Zero Grad for the VF Switch Click Apply

Specify various solver parameters required for this case: • • • • • • • • • • • • • • •

Run Time Controls

Select folder Analysis Controls followed by Solution Controls followed by Equation Behavior Open the Primary Variables panel and go to the Equation Status tab Move the Phase# slider at the bottom of the panel to the Phase#1 position Deselect item W-mom since we are solving a 2D flow in the x-y plane. Click Apply Move the Phase# slider to the Phase#2 position Deselect item W-mom Click Apply Go to the Solver Parameter tab Move the Phase# slider to the Phase#1 position Change the Relaxation Factor to 0.3 for Momentum, 0.1 for Pressure, 0.3 for Temp. Click Apply Move the Phase# slider to the Phase#2position Change the Relaxation Factor to 0.3 for Momentum, 0.1 for Volume Fraction, 0.3 for Temp. Click Apply

Set the number of iterations to 1000 for this case: • • • •

Final Operations




User Subroutines The boiling model is implemented in user subroutines FLUINJ for interphase mass transfer and SORENT for interphase heat transfer. These are located in files fluinj.f and sorent.f, respectively, of sub-directory ufile. The mass Version 4.02

12-29

Tutorial 12.4

BOILING SIMULATION


transfer rate due to evaporation is defined in subroutine UBOIL, called from FLUINJ, so this subroutine should also be resident in file fluinj.f. For further details of the boiling model, see the Eulerian Multiphase Flows Training Notes. •

Replace the default contents of both files with the code shown below, using pro-STAR’s built-in editor or any other editor. For file fluinj.f the appropriate code is as follows:

C******************************************************************* SUBROUTINE FLUINJ(FLUXI,UI,VI,WI,TEI,EDI,TI,SCINJ,IPMASS) C Fluid injection C******************************************************************* C--------------------------------------------------------------------------* C STAR-CD VERSION 4.00 C--------------------------------------------------------------------------* INCLUDE 'comdb.inc' DIMENSION SCINJ(50) COMMON/USR001/INTFLG(100) C C.....USER'S ADDITIONAL DEFINITIONS REAL DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG REAL TSAT,H1SAT,H2SAT,QLATEN REAL SMASS,UR,VR,WR COMMON/UBOIL1/ DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG COMMON/UBOIL2/ TSAT,H1SAT,H2SAT,QLATEN C INCLUDE 'usrdat.inc' DIMENSION SCALAR(50) EQUIVALENCE( UDAT12(001), ICTID ) EQUIVALENCE( UDAT03(001), CON ) EQUIVALENCE( UDAT03(019), VOLP ) EQUIVALENCE( UDAT04(001), CP ) EQUIVALENCE( UDAT04(002), DEN ) EQUIVALENCE( UDAT04(003), ED ) EQUIVALENCE( UDAT04(005), PR ) EQUIVALENCE( UDAT04(008), TE ) EQUIVALENCE( UDAT04(009), SCALAR(01) ) EQUIVALENCE( UDAT04(059), U ) EQUIVALENCE( UDAT04(060), V ) EQUIVALENCE( UDAT04(061), W ) EQUIVALENCE( UDAT04(062), VISM ) EQUIVALENCE( UDAT04(063), VIST ) EQUIVALENCE( UDAT04(007), T ) EQUIVALENCE( UDAT04(067), X ) EQUIVALENCE( UDAT04(068), Y ) EQUIVALENCE( UDAT04(069), Z ) C------------------------------------------------------------------------C C This subroutine enables the user to specify fluid injection C (addition or removal) into live cells. In the case of mass C removal (sink), only the mass flux (FLUXI) can be specified. In C the case of mass addition (source), the fluid will bring all its C user-specified properties (momentum, turbulence, temperature and C concentrations). Zero will be assumed for omitted properties. C C ** Parameters to be returned to STAR: 12-30

Version 4.02

Tutorial 12.4

BOILING SIMULATION


C (Sink) FLUXI (<0) C (Source) FLUXI (>0),UI,VI,WI,TEI,EDI,TI, C SCINJ,IPMASS C C IPMASS is an interphase mass transfer indicator used in C Eulerian two-phase (E2P) simulations only. C The default value, passed from STAR to FLUINJ, is always zero. C IPMASS=0: no interphase heat transfer - the mass sources specified C in FLUINJ are independent for each phase. C IPMASS=1: the phases are exchanging mass - the mass source specified C is directed from one phase into the other phase. C For more information, please refer to the E2P sections of the C manuals. C C------------------------------------------------------------------------C C Sample coding: Fluid injection and removal C C IF(ICTID.EQ.3) THEN CC Injection C FLUXI=0.1 C WI=0.05 C TI=373.0 C SCINJ(1)=1.0 C ELSE IF(ICTID.EQ.4) THEN CC Removal C FLUXI=-0.05 C ENDIF C-------------------------------------------------------------------------C C DENL=DEN VISL=VISM CPL=CP TKL=CON UR=U-UCEL2 VR=V-VCEL2 WR=W-WCEL2 SLIP=SQRT(UR*UR+VR*VR+WR*WR) DIAP=DIAM TL=T TG=TCEL2 VFG=VFCEL2 C CALL UBOIL(SMASS) C C.....SET INTERPHASE MASS FLUX IF(IPHA.EQ.1) THEN FLUXI=-SMASS UI=UCEL2 VI=VCEL2 WI=WCEL2 TI=TSAT ELSE IF(IPHA.EQ.2) THEN FLUXI=SMASS UI=U VI=V WI=W Version 4.02

12-31

Tutorial 12.4

BOILING SIMULATION


TI=TSAT ENDIF IPMASS=0 C RETURN END SUBROUTINE UBOIL(SMASS) C============================================================ C C CALCULATE EVAPORATION/CONDENSATION RATE C C CREATED BY SIMON LO 27/04/04 C C============================================================ C C IMPLICIT DOUBLE PRECISION (A-H,O-Z) C REAL DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG REAL TSAT,H1SAT,H2SAT,QLATEN REAL AI,HTCOEF,HTCGAS,QLIQ,QGAS REAL REY,PRT,RNU,SMASS C COMMON/UBOIL1/ DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG COMMON/UBOIL2/ TSAT,H1SAT,H2SAT,QLATEN COMMON/UBOIL3/ AI,HTCOEF,HTCGAS,QLIQ,QGAS C C****************************************************************** CHAPTER 1 MODEL DATA C C.....SET ADDITIONAL MODEL DATA HERE C TSAT = SATURATION TEMPERATURE (K) C H1SAT = SATURATION ENTHALPY OF PHASE 1 (J/KG) C H2SAT = SATURATION ENTHALPY OF PHASE 2 (J/KG) C TSAT=100.0+273.0 H1SAT=419.2E3 H2SAT=2676.0E3 QLATEN=H2SAT-H1SAT C C****************************************************************** CHAPTER 2 MASS TRANSFER RATE C C.....SIMPLE BULK BOILING/CONDENSATION MODEL C (ASSUME GAS PHASE AT SATURATION TEMPERATURE, C IF T(LIQ) < TSAT, I.E. SUB-COOLED LIQUID, WE HAVE CONDENSATION C IF T(LIQ) > TSAT, I.E. SUPER-HEATED LIQUID, WE HAVE EVAPORATION C C COMPUTE MASS TRANSFER RATE SMASS C PHASE 1 IS LIQUID AND PHASE 2 IS VAPOUR C IF SMASS < 0, CONDENSATION, MASS GOES FROM PHASE 2 TO PHASE 1 C IF SMASS > 0, EVAPORATION, MASS GOES FROM PHASE 1 TO PHASE 2 C C C.........REYNOLDS NUMBER REY=DENL*SLIP*DIAP/VISL C C.........PRANDTL NUMBER 12-32

Version 4.02

Tutorial 12.4

BOILING SIMULATION


PRT=CPL*VISL/TKL C C.........NUSSELT NUMBER C RNU=2.0+0.6*REY**0.5*PRT**0.3 C.........USE CONSTANT RNU=2.0 FOR SIMPLICITY RNU=2.0 C C.........LIQUID-SIDE HEAT TRANSFER COEFFICIENT HTCOEF=RNU*TKL/DIAP C C.........INTERFACIAL AREAM IN CELL AI=6.0*VFG/DIAP C C.........HEAT TRANSFER ACROSS INTERPHASE QLIQ=HTCOEF*AI*(TL-TSAT) C C.........GAS-SIDE HEAT TRANSFER COEFFICIENT HTCGAS=10.0 C C.........HEAT TRANSFER FROM GAS TO INTERPHASE QGAS=HTCGAS*AI*(TG-TSAT) C C.........MASS TRANSFER RATE SMASS=(QLIQ+QGAS)/QLATEN C RETURN END

•

For file sorent.f the appropriate code is as follows:

C******************************************************************* SUBROUTINE SORENT(S1P,S2P) C Source-term for enthalpy C******************************************************************* C--------------------------------------------------------------------------* C STAR-CD VERSION 4.00 C--------------------------------------------------------------------------* INCLUDE 'comdb.inc' COMMON/USR001/INTFLG(100) C.....USER'S ADDITIONAL DEFINITIONS REAL DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG REAL TSAT,H1SAT,H2SAT,QLATEN REAL AI,HTCOEF,HTCGAS,QLIQ,QGAS REAL SMASS,UR,VR,WR COMMON/UBOIL1/ DENL,VISL,CPL,TKL,SLIP,DIAP,TL,VFG,TG COMMON/UBOIL2/ TSAT,H1SAT,H2SAT,QLATEN COMMON/UBOIL3/ AI,HTCOEF,HTCGAS,QLIQ,QGAS INCLUDE 'usrdat.inc' DIMENSION SCALAR(50) EQUIVALENCE( UDAT12(001), EQUIVALENCE( UDAT03(001), EQUIVALENCE( UDAT03(019), EQUIVALENCE( UDAT04(001), Version 4.02

ICTID ) CON ) VOLP ) CP ) 12-33

Tutorial 12.4

BOILING SIMULATION


EQUIVALENCE( UDAT04(002), DEN ) EQUIVALENCE( UDAT04(003), ED ) EQUIVALENCE( UDAT04(004), HP ) EQUIVALENCE( UDAT04(006), P ) EQUIVALENCE( UDAT04(008), TE ) EQUIVALENCE( UDAT04(009), SCALAR(01) ) EQUIVALENCE( UDAT04(059), U ) EQUIVALENCE( UDAT04(060), V ) EQUIVALENCE( UDAT04(061), W ) EQUIVALENCE( UDAT04(062), VISM ) EQUIVALENCE( UDAT04(063), VIST ) EQUIVALENCE( UDAT04(007), T ) EQUIVALENCE( UDAT04(067), X ) EQUIVALENCE( UDAT04(068), Y ) EQUIVALENCE( UDAT04(069), Z ) C----------------------------------------------------------------------C C This subroutine enables the user to specify a source term (per unit C volume) for enthalpy in linearized form: C C Source = S1P-S2P*T, (W/m3) C C in an arbitrary manner. C C If temperature is to be fixed to a given value T, then the C following may be used: C C S1P=GREAT*T C S2P=GREAT, C C where T can be a constant or an arbitrary function of the C parameters in the parameter list. C C ** Parameters to be returned to STAR: S1P,S2P C C------------------------------------------------------------------------C C Sample coding: Fix temperature to the value of 300 K in solid C No 3 (IMAT=-3) C C IF(IMAT.EQ.-3) THEN C S1P=GREAT*300. C S2P=GREAT C ENDIF C------------------------------------------------------------------------C DENL=DEN VISL=VISM CPL=CP TKL=CON UR=U-UCEL2 VR=V-VCEL2 WR=W-WCEL2 SLIP=SQRT(UR*UR+VR*VR+WR*WR) DIAP=DIAM TL=T TG=TCEL2 12-34

Version 4.02

Tutorial 12.4

BOILING SIMULATION


VFG=VFCEL2 C CALL UBOIL(SMASS) C C.....SET HEAT TRANSFER BETWEEN PHASE AND INTERFACE IF(IPHA.EQ.1) THEN S1P=HTCOEF*AI*TSAT S2P=HTCOEF*AI ELSE IF(IPHA.EQ.2) THEN S1P=HTCGAS*AI*TSAT S2P=HTCGAS*AI ENDIF C RETURN END

CFD Analysis You may continue with the CFD analysis, using the STAR GUIde facilities for running STAR interactively without quitting pro-STAR. Alternatively, you may run the CFD analysis (in double precision) by typing star -dp in your session window. Post-Processing Use pro-STAR to check and examine the results. • • •

Select folder Post-Processing Open the Load Data panel to display the Files(s) tab Click Open Post File

Plot the volume fraction for phase 2 as follows: • • • • • • •

Version 4.02

Go to the Data tab and check that Data Type Cell is selected Set the Smooth Option to On Move the Phase# slider to the Phase#2 position and select item Volume Fraction from the Scalar Data list Click Get Data Select Go To > Create Plots to open the Create Plots panel In the 3-D Surface tab, select Contour (filled) from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen to display Figure T12.4-2

12-35

Tutorial 12.4

BOILING SIMULATION


Figure T12.4-2

Contours of phase 2 volume fraction

The steam volume fraction at the exit should be about 0.85. Now plot the temperature as follows: • • • •

12-36

Go back to the Load Data panel by clicking Go To Load Data Select item Temperature from the Scalar Data list Click Get Data In the main pro-STAR window click Cell Plot to display Figure T12.4-3

Version 4.02

Tutorial 12.4

BOILING SIMULATION


Figure T12.4-3

Phase 2 temperature contour plot

Note that the steam temperature remains within its saturation value of 373 K throughout the solution domain. Repeat the above steps to obtain a phase 1 temperature plot: • • •

Version 4.02

Move the Phase# slider to the Phase#1 position and select item Temperature from the Scalar Data list Click Get Data In the main pro-STAR window click Cell Plot to display Figure T12.4-4

12-37

Tutorial 12.4

BOILING SIMULATION


Figure T12.4-4

Phase 1 temperature contour plot

Note that the water temperature drops to the saturatiuon value (373 K) in the upper part of the solution domain. Finally, obtain a V-velocity component plot for the second phase: • • •

12-38

Move the Phase# slider to the Phase#2 position and select item Velocity Component V from the Scalar Data list Click Get Data In the main pro-STAR window click Cell Plot to display Figure T12.4-5

Version 4.02

Tutorial 12.4

BOILING SIMULATION

Discussion of Results Final Operations

Figure T12.4-5

Contour plot of velocity component V

Discussion of Results In • we can see that water enters at 375 K. As energy is lost due to steam generation, the water temperature drops gradually to the saturation value of 373K. In •, the volume fraction of steam shows an immediate increase from its inlet value of 0.01 to 0.425 and peaks at 0.852. When the water temperature reaches saturation no further steam is generated. • shows that the steam temperature remains at the saturation value of 373 K. Validation Check According to the inlet boundary conditions, water enters the channel with a two degrees superheat (i.e. two degrees above saturation). The volume fraction for water is 0.99 and inlet velocity is 0.5 m/s. The amount of thermal energy above saturation can be calculated as: q˙liq = m˙ liq c p, liq ( T liq – T sat ) The water flow rate is: m˙ liq = α liq ρ liq A v liq Substituting appropriate values into the above formulae, we obtain q˙liq = 40 kJ/s

Version 4.02

12-39

Tutorial 12.4

BOILING SIMULATION


Assuming that all this excess energy is used in generating steam, the latter’s generation rate is: q˙liq m˙ g = ------h fg where h fg is the latent heat, in this case 2256.7 kJ/kg. The steam generation rate is therefore 0.0177 kg/s. We can check this result against the exit conditions of steam shown in the plots above. From these plots, the volume fraction equals 0.8522 and the V-velocity equals 3.445 m/s. Using the specified density value of 0.6 kg/m3 and the channel cross-sectional area of 0.01 m2., the mass flow rate of steam calculated from these results is 0.0176 kg/s. Suggestions for Further Exercises Condensation The same model can be used to study condensation. 0.1m × 0.1m Water outlet gy 2m Steam bubbles y x Sub-cooled water + steam Figure T12.4-6

Outline of flow channel

Start by copying the entire working directory for boiling tutorial tut12-4 to another directory, say tut12-4b, as follows: cp -r tut12-4 tut12-4b Enter the tut12-4b directory and start a pro-STAR session as normal, re-using the model settings of tut12-4. Now make the following changes: •

12-40

Initial and inlet conditions: Water temperature = 372 K (i.e. one degree subcool) Steam volume fraction = 0.1 Version 4.02

Tutorial 12.4

BOILING SIMULATION


• •

Version 4.02

Save the problem and model files Run STAR and post-process the results as described above.

12-41

Introduction

Tutorial 13 AEROACOUSTIC ANALYSIS Introduction The tutorials in this group illustrate STAR-CD’s facilities for performing an aeroacoustic analysis. The problem analysed is air flow around a cylinder which, for simplicity, is modelled as a two-dimensional problem. The air density and laminar viscosity are 1.205 kg/m3 and 1.81 x 10-5 Pa s, respectively. The circle representing the cylinder has a diameter of 0.15 m and the inlet velocity is 5 m/s. These values are chosen to produce a flow with a Reynolds number of 50,000, based on the cylinder diameter. The mesh employed is refined in the vicinity of the cylinder and also in the region where the wake is expected to appear.

inflow

Figure T13.0-1

Flow around a cylinder

The features demonstrated in these tutorials provide only basic data on the aeroacoustic properties of a flow system. More detailed aeroacoustic analyses may be performed using STAR-CD in conjunction with CD-adapco’s es-acoustics tool.

Version 4.02

13-1

Tutorial 13.1

STEADY FLOW AROUND A CYLINDER


Tutorial 13.1


This tutorial aims to demonstrate: • •

The application of an aeroacoustic model in a steady-state problem Methods for determining whether an analysis has converged to a steady-state solution

The aeroacoustic properties of the flow will be analysed by calculating a Lilley source term representing broadband shear noise (see “Aeroacoustic Analysis” on page -7 of the Methodology volume). This scalar is useful in identifying those areas of the problem geometry where shear noise dominates and hence can assist in design modification to minimise noise. However, being a steady-state method, it cannot be expected to capture the acoustic effects of large-scale transient features such as vortex shedding. Thus, the method can only assist in a qualitative examination of the acoustic features of the flow system. Turbulence is modelled using the low-Reynolds number k-ε model (see “Standard low Reynolds number two-equation k-ε models” on page -13 of the Methodology volume). Pre-Processing Preliminaries Create a directory for the tutorial named tut13-1. The mesh to be used has already been created and the relevant cell, vertex, boundary and problem setup files are supplied with STAR-CD (files cyl.cel, cyl.vrt, cyl.bnd and cyl.inp, respectively). Therefore, before starting the tutorial, make sure these files are copied into your current directory. Start up pro-STAR and enter the case name and title: • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Type aac in the Casename text box Click Continue

Read in the available problem data: • • •

In the main pro-STAR window, select File > Read File... Check that the name displayed in the File Name box is cyl.inp Click Apply and then Close

This will read default problem settings from file cyl.inp as well as the problem geometry and boundary location definitions from the remaining three files. • • • • • • • • 13-2

In the main window, select File > Model Title Type AEROACOUSTIC ANALYSIS OF FLOW AROUND A CYLINDER in the Title text box Click Apply Select C > All Select B > All Select B > Unselect > Symplane Choose Bound as the Cell Plot Display Options setting Click Cell Plot to display the mesh and the inlet and pressure boundaries, as Version 4.02

Tutorial 13.1



shown in Figure T13.1-1. The symmetry boundaries omitted from the plot are placed on the two surfaces lying in the plane of view.

Figure T13.1-1

Mesh geometry

Turn on the aeroacoustic analysis option: • • •

Open the Select Analysis Features STAR GUIde panel Turn On Aeroacoustic Analysis Click Apply

Note that an additional folder called Aeroacoustic Analysis now appears in the NavCenter tree. •

Material Properties

The aeroacoustic source term calculation depends upon a fluctuating velocity, obtained from calculated or derived values of k and ε using the “Synthetic turbulence” method described in Chapter 16 of the Methodology volume. In this case, the low-Reynolds number k-ε turbulence model, which calculates both these quantities directly, will be used. If a model that does not calculate k and ε directly is chosen, these quantities would be derived indirectly by STAR prior to performing the aeroacoustic analysis. • • • •

Version 4.02

Go to this folder and open the Aeroacoustic Analysis panel. All default settings and parameter values shown are appropriate for this case, so no changes are needed here.

Go to the Thermophysical Models and Properties folder and select sub-folder Liquids and Gases Open the Turbulence Models panel Turn On turbulence modelling Select the k-Epsilon/Low Reynolds Number model from the Turbulence 13-3

Tutorial 13.1



• • •

menu Click Apply Under the Near-Wall Treatment tab, select option Hybrid Wall Click Apply

Initialize the flow field (the initial velocity is chosen to match that at the inlet boundary, as set below) and specify the monitoring and pressure reference cells: • • • • • • • • • • Boundary Conditions

Specify the velocity and turbulence parameters at the inlet. The former is set such that, based on the diameter of the cylinder, the Reynolds number is 50,000: • • • • • • • •

Analysis Controls

• • • • • •

13-4

Select the Define Boundary Conditions folder Open the Define Boundary Regions panel Select the inlet, Reg# 1, from the list Enter 5 m/s as the U velocity Change the Turb. Switch to TI/Length Enter a Turb. Intensity of 0.001 Enter a Length of 0.05 m Click Apply

Since the flow is two-dimensional, solving the momentum equation in the z-direction is unnecessary. To turn this off and activate a second-order differencing scheme for the other two momentum equations: •

Run Time Controls

Open the Initialization panel Specify the U velocity as 5 m/s Click Apply Under the Turbulence tab, select option TI/Mixing Length from the Turbulence Parameters menu Set the Intensity and Mixing Length values to 0.01 and 0.005, respectively Click Apply Open the Monitoring and Reference Data panel Enter 6275 as the Monitoring cell number Enter 7213 as the Reference Pressure Cell Number Click Apply

Select the Analysis Controls folder followed by the Solution Controls sub-folder Select the Equation Behaviour folder Open the Primary Variables panel Under the Equation Status tab, deselect the W-Mom option to make the analysis two-dimensional Click Apply Under the Differencing Schemes tab, change the momentum Differencing Scheme to MARS Click Apply

The run time controls must also be adjusted as follows: •

Select folder Analysis Preparation/Running and open the Set Run Time Version 4.02

Tutorial 13.1



• • Final Operations

Controls panel Enter 600 for the maximum Number of Iterations Click Apply

Write the geometry and problem files: • • • •

Select File > Write Geometry File... In the Geometry File Write dialog, click Apply and then Close Select File > Write Problem File... In the Problem File Write dialog, click Apply and then Close



The analysis will then start automatically. At the end of the run, note that the normalised residual sums will not have satisfied the convergence criterion within the specified maximum number of iterations. The reason for this will be discussed in the post-processing section. Post-Processing Preliminaries Begin by reading in the results of the analysis: • • • Flow Field

Given that the analysis has so far failed to satisfy the convergence criterion, the results may not represent a true steady-state. To evaluate this possibility, examine the flow field by displaying the velocity vectors: • • • • • • • •

Version 4.02


Under the Data tab of the Load Data panel, select Data Type Cell Select Velocity Components UV from the Vector Data list Click Get Data Choose Go To > Create Plots Under the 3-D Surface tab, select options Vector and Edge Click Plot To Screen Turn off the Bound Cell Plot Display Option In order to be able to see the flow field details, zoom in using the middle mouse button until the values at the bottom of the display window show the plot Center to be approximately 0.1, 0, 0 and the viewing Distance approximately 0.25. The resulting plot should resemble Figure T13.1-2

13-5

Tutorial 13.1


Post-Processing Monitor History Plots

Figure T13.1-2

Plot of velocity vectors near to the cylinder

The flow field is clearly not symmetrical despite the geometry being so. This suggests that a converged steady-state solution has not been reached. Monitor Examining history plots of the monitored flow variables is a good way to reveal History Plots whether a steady-state solution has been reached and, if not, why not. To create a suitable history plot: • • • •

Select the Analysis Preparation/Running folder Open the Run History of Previous Analysis panel Check the U-Component box Click Plot Monitor History

By default, the graph frame fills only half the screen. To make it larger: • • • • •

13-6

Select the Graphs sub-folder in the Post-Processing folder Open the Customize Graphs panel Under the Display tab, change the frame Location to Default Click Apply Click Redraw to display Figure T13.1-3

Version 4.02

Tutorial 13.1


Post-Processing Turbulence Energy

Figure T13.1-3

History plot for the U velocity component

The oscillating graph shows that a steady-state solution was not reached and suggests that the real solution to this problem is periodic. In order to obtain a full solution, a transient analysis would need to be run. Such an analysis is the basis of Tutorial 13.2. Despite the absence of a steady-state solution, the results obtained from this run (which effectively show the instantaneous solution at a point within the periodic cycle) can be used to discuss some aspects of an aeroacoustic analysis. Turbulence Energy

A plot of the turbulence kinetic energy will show the shape and position of the wake downstream of the cylinder: • • • • • • • •

Version 4.02

Open the Load Data panel Under the Data tab, select Data Type Cell and Smooth Option On Select Turb. Kinetic Energy from the Scalar Data list Click Get Data Choose Go To > Create Plots Under the 3-D Surface tab, select options Contour (filled) and None Click Plot To Screen Click Zoom Off to display Figure T13.1-4

13-7

Tutorial 13.1


Post-Processing Aeroacoustic Source Term

Figure T13.1-4

Contour plot of the turbulence kinetic energy

Aeroacoustic The aeroacoustic Lilley source term is loaded from the results file in the same way Source Term as any other scalar. Therefore, a contour plot of it can be produced as follows: • • • • •

13-8

Open the Load Data panel Under the Data tab, select Data Type Cell and Smooth Option On Select Aeroacoustic Source from the Scalar Data list Click Get Data Click Replot to display Figure T13.1-5

Version 4.02

Tutorial 13.1


Post-Processing Aeroacoustic Source Term

Figure T13.1-5

Contour plot of the aeroacoustic Lilley source term

Figure T13.1-5 shows that the shear noise produced by the flow is primarily in the wake of the cylinder. The shape of the noise wake is similar to that of the turbulence wake shown in Figure T13.1-4. This is due to the Lilley source dependence on the turbulence parameters k and ε. A separate analysis using the es-acoustics tool shows that the mesh provided for this case is only capable of resolving noise resulting from turbulent eddies for frequencies of up to about 500 Hz. Therefore, the next tutorial (Tutorial 13.2) will analyse the same case as a transient problem and with a finer mesh, enabling frequencies of up to about 1,000 Hz to be captured. Quit pro-STAR by selecting: •

Version 4.02


13-9

Tutorial 13.2

TRANSIENT FLOW AROUND A CYLINDER

Tutorial 13.2


This tutorial aims to demonstrate: • • • • • •

The application of a Detached Eddy Simulation (DES) turbulence model How to monitor cell behaviour using an .ecd file The solution mapping (SMAP) process The specification of boundary conditions based on mapped solution data How to check a transient analysis for stability How to create animations using the Animation module and a neutral plot file

Such techniques are typically used in external aerodynamics problems where analyses involving refined meshes around individual components (for example, wing mirrors, spoilers, wiper blades, high-lift devices and landing gear) are performed with boundary conditions mapped from a coarser global simulation. As a demonstration of these techniques, this tutorial models the same two-dimensional flow around a cylinder as Tutorial 13.1, but this time as a transient simulation. Examination of the time-dependent pressure profile at specified locations will allow for assessment of the acoustic and structural excitation via the frequency and amplitude of the unsteady pressure fluctuations. To reduce the computational cost, the solution domain extent is reduced to cover only the important flow regions in the vicinity of the cylinder and wake, and the mesh within is refined. The analysis restarts from the steady state solution of the previous tutorial which is mapped onto the new mesh. The conditions on the inlet and pressure boundaries are also mapped from the steady state result using user subroutines. Besides the above changes to domain, mesh and boundary conditions, the only other change in the problem specification is the use of the Detached Eddy Simulation (DES) option based on the low-Reynolds number k-ε model employed in Tutorial 13.1. This means that the results can include large eddy structures that would not appear if a RANS model was used. Due to the hybrid nature of DES, using such a model rather than full LES also benefits from not having to resolve the boundary layer fully. Given a cylinder radius of 0.15 m, a bulk flow velocity of ~5 m/s and the knowledge that, for flow around a cylinder, vortex shedding at Reynolds number 50,000 occurs at a Strouhal number fd St = ----u of ~0.2, it is possible to estimate the vortex shedding frequency as f = 6.67Hz To produce a well-resolved waveform for these oscillations, the time step should be at least one tenth of the inverse of the frequency, i.e. 1.5 x 10-2 seconds. Stability considerations based on the Courant number require the time step to be much smaller than this, so a value of 5 x 10-5 seconds is chosen. This should enable oscillations with frequencies of up to 2,000 Hz to be resolved faithfully.

Version 4.02

13-11

Tutorial 13.2



Pre-Processing Preliminaries Create a directory for the tutorial named tut13-2 and copy the model and results files created in Tutorial 13.1 (aac.mdl and aac.ccm, respectively) into it. In addition, make a copy of aac.mdl named aac_tr.mdl, ensuring that you do not delete the original aac.mdl model file as this will be required for the solution mapping operation. You should also copy a command macro called REFINE.MAC into the working directory, which will be used to create the new mesh. Start up pro-STAR using the aac_tr.mdl file created above: • • • •

Type prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Check that the Case Name is aac_tr Click Continue

To give the case a new title: • • • Mesh Refinement

A command macro, which deletes those cells lying outside the desired solution domain, refines the remaining cells and creates new boundaries, is provided as part of the installation. To execute the macro: • • •

Analysis Features

Select Panels > Define Macro Select REFINE in the Define Macro panel Click Execute

The next step is to change the analysis type to transient: • • •

• Material Properties

In the main pro-STAR window, select File > Model Title... Type ANALYSIS OF AEROACOUSTIC EFFECTS IN TRANSIENT FLOW in the Title box Click Apply

Open the Select Analysis Features panel Change the Time Domain option to Transient Click Yes in the dialog that appears, warning that aeroacoustic modelling cannot be performed in a transient analysis. This refers to the calculation of the Lilley source term, which is a steady state feature. Click Apply

Switch on the DES variant of the current turbulence model: • • • •

Select the Thermophysical Models and Properties folder Select the Liquids and Gases sub-folder and open the Turbulence Models panel Check the DES box Click Apply

The monitoring and pressure reference cells must be redefined, as those used in the steady-state analysis no longer exist: • • •

13-12

Open the Monitoring and Reference Data panel Change the Monitoring cell number to 9419 Change the Reference Pressure Cell Number to 6232. This cell is at one end of the pressure boundary. Version 4.02

Tutorial 13.2



• Boundary Conditions

The mapping of the inlet and pressure boundary conditions is performed via user subroutines. These must be activated as follows: • • • • • • • • • • • •

Analysis Controls

Click Apply

In the main window, choose File > System Command Type ufiles in the text box, click Apply and then Close In STAR GUIde, select the Define Boundary Conditions folder Open the Define Boundary Regions panel Select Reg# 1, the inlet, from the boundary regions list Select User from the Options menu Click Define User Coding to write the default version of subroutine BCDEFI in sub-directory ufile, ready for editing later Click Apply Select Reg# 2, the pressure boundary, from the boundary regions list Select User from the Options menu Click Define User Coding to write the default version of subroutine BCDEFP in sub-directory ufile, ready for editing later Click Apply

Specify what transient data will be written to the .pstt file and how often: • • •

• • • • • •

Select the Analysis Controls folder followed by the Solution Controls folder Select the Equation Behavior sub-folder and then open the Primary Variables panel Change the momentum Differencing Scheme to CD. This should provide greater accuracy as, despite being second-order, the MARS gradient limiter has been shown to be diffusive when used with LES sub-grid scale turbulence models. Click Apply Select the Output Controls folder and open the Analysis Output panel Under the Transient tab, choose to Write data every 0.015 s Select Turb Kinetic Energy from the Choose data to write list. The data will be used to create an animation in the “Post-Processing” part of this tutorial. Check the Post box Click Apply

Pressure data will be monitored at a location about 1.5 cylinder radii downstream of the cylinder and the monitor data stored in an .ecd file. Define the location by creating a cell set containing a single cell: •

Enter the following command in the I/O window: CSET NEWSET CLIST 9419

Store the location in a .set file: • • •

In the main pro-STAR window, select INFO > Store Set/Surface/View Enter pmon as the Set Name Click Write and then Close

Specify which data are to be stored in the .ecd file: Version 4.02

13-13

Tutorial 13.2



•

In the Output Controls folder, select the Monitor Engineering Behavior sub-folder Open the Monitor Cell Behavior panel Select On Using the file browser to the right of the Set File box, choose the file aac_tr.set Select pmon from the Select Entry list Select Pressure in the Select Monitoring Information section Click Apply

• • • • • • Run Time Controls

Specify the time step size and the length of the run: •

Select the Analysis Preparation/Running folder and open the Set Run Time Controls panel Change the Time Step for Period to 5e-5 s Click Set Period Change the Run Time to 1.5 s. This is equivalent to 30,000 time steps. Click Apply

• • • • Solution Mapping

The solution mapping process involves the following stages: 1. 2. 3. 4. 5. 6. 7.

Save the new mesh geometry created above in its corresponding .ccm file Save the new model file Resume the original model file and load the corresponding solution file Perform the solution mapping (SMAP) operation Resume the new model file View and check the restart solution data Set up the run to start from the mapped solution

Write the new geometry and model files and load the model and results files from Tutorial 13.1: • • • • • • • • • •

In the main pro-STAR window, select File > Write Geometry File... In the Geometry File Write dialog, click Apply then Close Select File > Save Model Select File > Resume From... In the Resume From dialog, enter aac.mdl Click Apply and then Close Select the Post-Processing folder in STAR GUIde Open the Load Data panel to display the File(s) tab Change the Steady State Post File name to aac.ccm Click Open Post File to load the results from Tutorial 13.1

To perform the solution mapping: • •

13-14

In the main pro-STAR window, select Utility > Solution Mapping... In the Smap/Tsmap dialog, specify the options shown below:

Version 4.02

Tutorial 13.2


Pre-Processing Solution Mapping

•

Click Apply. The solution mapping operation may take a few minutes, depending upon the speed of your computer. Once it is complete, click Close.

The new model file can now be resumed and the mapped results displayed: • • • • • • • • • • • • • •

Version 4.02

Select File > Resume From... In the Resume From dialog, enter aac_tr.mdl Click Apply then Close Select C > All Select the Post-Processing folder in STAR GUIde Open the Load Data panel to display the File(s) tab Change the Steady State Post File name to aac_tr.ccm Change the State Name to smap Click Open Post File to load the mapped results Under the Data tab, select Velocity Magnitude from the Calculated Scalar Data list Click Get Data Select Go To > Create Plots Under the 3-D Surface tab, select options Contour (filled) and None Click Plot to Screen to display Figure T13.2-1

13-15

Tutorial 13.2



Figure T13.2-1

Velocity magnitude profile resulting from the solution mapping

You must now specify that the transient run should restart from the above mapped solution: • • • • • •

Select the Analysis Preparation/Running folder in STAR GUIde Open the Analysis (Re)Start panel Select Initial Field Restart as the Restart File Option Enter aac_tr.ccm as the Restart File In the Initial Field Restart section, select Restart (Smapped) from the drop-down menu Check that the State Name is smap and then click Apply

This completes the solution mapping process. Final Operations

The geometry file has already been written but it is also necessary to write the problem file: • •

Select File > Write Problem File... In the Problem File Write dialog click Apply then Close

User Subroutines The boundary mapping process requires two user subroutines, one for the inlet boundary and one for the pressure boundary. These are supplied in files bcdefi.f and bcdefp.f which should be copied into the ufile directory, replacing the default subroutines. Alternatively, you may edit the default subroutines so that they match those shown below.

13-16

Version 4.02

Tutorial 13.2


User Subroutines Inlet Boundary

Inlet Boundary

The user subroutine mapping the inlet boundary data is BCDEFI, given below:

C************************************************************************* SUBROUTINE BCDEFI(SCALAR,U,V,W,TE,ED,T,DEN,TURINT) C Maps inlet boundary conditions from cell data C************************************************************************* C C STAR VERSION 4.02.000 C C************************************************************************* INCLUDE ‘comdb.inc’ COMMON/USR001/INTFLG(100) DIMENSION SCALAR(50) LOGICAL TURINT INCLUDE ‘usrdat.inc’ DIMENSION SCALC(50) EQUIVALENCE( UDAT12(001), ICTID ) EQUIVALENCE( UDAT04(002), DENC ) EQUIVALENCE( UDAT04(003), EDC ) EQUIVALENCE( UDAT02(005), PR ) EQUIVALENCE( UDAT04(005), PRC ) EQUIVALENCE( UDAT04(009), SCALC(01) ) EQUIVALENCE( UDAT04(007), TC ) EQUIVALENCE( UDAT04(008), TEC ) EQUIVALENCE( UDAT04(059), UC ) EQUIVALENCE( UDAT04(060), VC ) EQUIVALENCE( UDAT04(061), WC ) EQUIVALENCE( UDAT04(064), UCL ) EQUIVALENCE( UDAT04(065), VCL ) EQUIVALENCE( UDAT04(066), WCL ) EQUIVALENCE( UDAT02(070), X ) EQUIVALENCE( UDAT02(071), Y ) EQUIVALENCE( UDAT02(072), Z ) c-inclusion_1 start ---------------------------------------------------PARAMETER(MAXPB=209528) DIMENSION USTORE(MAXPB),VSTORE(MAXPB),WSTORE(MAXPB), * TESTORE(MAXPB),EDSTORE(MAXPB) SAVE USTORE,VSTORE,WSTORE,TESTORE,EDSTORE,ITFLAG,IFILEFLAG LOGICAL FILEEXIST c-inclusion_1 end -----------------------------------------------------C----------------------------------------------------------------------c-inclusion_2 start ---------------------------------------------------IF (INTFLG(1).EQ.0) THEN INTFLG(1) = 1 ITFLAG = ITER END IF IF(IREG.EQ.1) THEN IF (ITER.EQ.ITFLAG) THEN IF (IBP.GT.MAXPB)STOP’BCDEFI:MAXPB too small’ IF (INTFLG(2).EQ.0) THEN INTFLG(2) = 1 INQUIRE(FILE=’inlet.inp’, EXIST=FILEEXIST) IF (FILEEXIST) THEN Version 4.02

13-17

Tutorial 13.2


User Subroutines Inlet Boundary

IFILEFLAG = 1 ELSE IFILEFLAG = 0 END IF END IF IF (IFILEFLAG.EQ.0) THEN IF (INTFLG(3).EQ.0) THEN WRITE(*,*) ‘ *** WARNING: Setting inlet boundary ‘ * // ‘to near cell value and writing inlet.inp file’ INTFLG(3) = 1 END IF USTORE(IBP)=UC VSTORE(IBP)=VC WSTORE(IBP)=WC TESTORE(IBP)=TEC EDSTORE(IBP)=EDC call freeunit(iunit) OPEN (iunit,FILE=’inlet.inp’,FORM=’formatted’, * STATUS=’unknown’) 10 CONTINUE READ(iunit,*,END=11) TMP GO TO 10 11 CONTINUE WRITE(iunit,*) IBP,UC,VC,WC,TEC,EDC CLOSE (iunit) ELSE IF (INTFLG(4).EQ.0) THEN WRITE(*,*) ‘ *** WARNING: Reading inlet profile’ * // ‘ from inlet.inp’ INTFLG(4) = 1 END IF OPEN (iunit,FILE=’inlet.inp’,FORM=’formatted’, * STATUS=’unknown’) 12 CONTINUE READ(iunit,*,END=13) IBPR,UR,VR,WR,TER,EDR IF (IBP.NE.IBPR) THEN GO TO 12 ELSE USTORE(IBP)=UR VSTORE(IBP)=VR WSTORE(IBP)=WR TESTORE(IBP)=TER EDSTORE(IBP)=EDR END IF CLOSE (iunit) END IF C-SPOT CHECK IF(IBP.EQ.690) PRINT *,’STARTU,V,W,IBP=’,U,V,W,IBP END IF U=USTORE(IBP) V=VSTORE(IBP) W=WSTORE(IBP) TE=TESTORE(IBP) ED=EDSTORE(IBP) T=293.0 DEN=1.205 C-SPOT CHECK IF(IBP.EQ.690) PRINT *,’U,V,W,IBP=’,U,V,W,IBP END IF 13-18

Version 4.02

Tutorial 13.2


User Subroutines Pressure boundary

c-inclusion_2 end -----------------------------------------------------RETURN 13 CONTINUE WRITE(*,*) ‘ ***ERROR: Could not find pro-STAR boundary ‘, * IBP, ‘ in file inlet.inp’ WRITE(60,*) ‘ ***ERROR: Could not find pro-STAR boundary ‘, * IBP, ‘ in file inlet.inp’ CALL STQUIT(1) END

Pressure boundary

The user subroutine mapping the pressure boundary data is BCDEFP, given below:

C************************************************************************* SUBROUTINE BCDEFP(UB,VB,WB,PR,TE,ED,T,SCALAR,TURINT) C Maps pressure boundary conditions from cell data C************************************************************************* C C STAR VERSION 4.02.000 C C************************************************************************* INCLUDE ‘comdb.inc’ COMMON/USR001/INTFLG(100) DIMENSION SCALAR(50) LOGICAL TURINT INCLUDE ‘usrdat.inc’ DIMENSION SCALC(50) EQUIVALENCE( UDAT12(001), EQUIVALENCE( UDAT02(002), EQUIVALENCE( UDAT04(002), EQUIVALENCE( UDAT04(003), EQUIVALENCE( UDAT04(005), EQUIVALENCE( UDAT04(009), EQUIVALENCE( UDAT04(007), EQUIVALENCE( UDAT04(008), EQUIVALENCE( UDAT04(059), EQUIVALENCE( UDAT04(060), EQUIVALENCE( UDAT04(061), EQUIVALENCE( UDAT04(064), EQUIVALENCE( UDAT04(065), EQUIVALENCE( UDAT04(066), EQUIVALENCE( UDAT02(070), EQUIVALENCE( UDAT02(071), EQUIVALENCE( UDAT02(072),

ICTID ) DEN ) DENC ) EDC ) PRC ) SCALC(01) ) TC ) TEC ) UC ) VC ) WC ) UCL ) VCL ) WCL ) X ) Y ) Z )

SAVE PSTOR, ITFLG, IFILEFLAG LOGICAL FILEEXIST PARAMETER (MAXPB = 209528) DIMENSION PSTOR(MAXPB), TESTOR(MAXPB), EDSTOR(MAXPB) IF (INTFLG(41).EQ.0) THEN INTFLG(41) = 1 C C set the starting iteration Version 4.02

13-19

Tutorial 13.2


User Subroutines Pressure boundary

C ITFLG = ITER END IF IF (IREG.EQ.2) THEN C C Check is array pstor has been sized correctly C IF (IBP.GT.MAXPB) STOP ‘BCDEFP: MAXPB TOO SMALL’ C C If in the first iteration of run C IF (ITER.EQ.ITFLG) THEN IF (INTFLG(42).EQ.0) THEN INTFLG(42) = 1 C C check if file containing pressure data exists C INQUIRE(FILE=’pressure.inp’, EXIST=FILEEXIST) IF (FILEEXIST) THEN IFILEFLAG = 1 ELSE IFILEFLAG = 0 END IF END IF C C If file pressure.inp does not exist write warning message to screen. C IF (IFILEFLAG.EQ.0) THEN IF (INTFLG(43).EQ.0) THEN INTFLG(43) = 1 WRITE(*,*) ‘ ***WARNING: Setting pressure boundary ‘ * // ‘to near cell value and writing pressure.inp file’ END IF C C Get pressure from cell value and store C PSTOR(IBP) = PRC TESTOR(IBP) = TEC EDSTOR(IBP) = EDC call freeunit(iunit) OPEN(iunit,FILE=’pressure.inp’,FORM=’formatted’, * STATUS=’unknown’) 10 CONTINUE READ(iunit,*,END=11) TMP GO TO 10 11 CONTINUE WRITE(iunit,*) IBP, PRC, TEC, EDC CLOSE (iunit) ELSE IF (INTFLG(44).EQ.0) THEN INTFLG(44) = 1 WRITE (*,*) ‘ *** WARNING: Reading pressure boundary’ * // ‘ profile from file pressure.inp’ END IF OPEN (iunit,FILE=’pressure.inp’,FORM=’formatted’, * STATUS=’unknown’) 12 CONTINUE 13-20

Version 4.02

Tutorial 13.2



13

READ(iunit,*,END=13) IBPR,PRCR, TECR, EDCR IF (IBPR.NE.IBP) THEN GOTO 12 ELSE PSTOR(IBP) = PRCR TESTOR(IBP) = TECR EDSTOR(IBP) = EDCR END IF CLOSE (iunit) END IF END IF END IF PR = PSTOR(IBP) TE = TESTOR(IBP) ED = EDSTOR(IBP) T = 293.0 RETURN CONTINUE WRITE (*,*) ‘ ***ERROR: Cannot find pressure boundary in file’ CALL STQUIT() END

CFD Analysis The description in the next two sections assumes that STAR will be run from the command line whilst leaving pro-STAR running in the background. If possible, you should also run the analysis on multiple CPUs to minimise the elapsed run time. To run the analysis in parallel, on two local CPUs and in double precision, type: star -dp 2 To run the analysis sequentially, in double precision mode, type: star -dp However you choose to run the analysis, it will take at least a few hours to complete. In our experience, the run takes 9 hours on a dual-processor Pentium 4 Xeon 2.8Ghz running under Linux. Long run times are typical for DES cases as they require very fine meshes and a large number of time steps (in this case 30,000). Post-Processing Preliminaries Before post-processing the results, it is advisable to check the performance of the run by examining the information in the .info file: • • • •

Version 4.02

In STAR GUIde, select the Analysis Preparation/Running folder Open the Run History of Previous Analysis panel Click Browse Additional Output File to display the .info file contents Examine the Maximum Courant number and the Mean Courant number at a selection of time steps through the run. You should see that these two quantities stay within the ranges 1.0 to 9.0 and 0.15 to 0.5, respectively. Ideally, the Courant number should not exceed 1.0 but, in this case, it is reasonable to assume that large Courant numbers are found only in a few very 13-21

Tutorial 13.2


Post-Processing Animated Plots

•

small cells near the cylinder surface. Examine the NUMBER OF PISO CORRECTORS at a selection of time steps through the run. This should be either 2 or 3. A stable transient calculation will not regularly exceed 4 PISO correctors.

Begin the post-processing session by opening the transient post data file: • • • • • • Animated Plots

In STAR GUIde, select the Post-Processing folder and open the Load Data panel Under the File(s) tab, select Transient as the Analysis option Select the first empty position, 1, in the Transient Post File(s) list Click Add File to List Select file aac_tr.pstt from the Transient Post File(s) list Click Open Transient Post File

An animation of turbulence kinetic energy contours will now be created to help visualize the unsteady character of the flow. The animation may be defined by writing a sequence of plots to a neutral plot file, which are then played back. These operations are performed using the Animation module as follows: • • • • • • • • • • • • •

• • • • • • • •

Under the File(s) tab of the Load Data panel, select the first time step from the Select Time Step list Click Store Iter/Time Under the Data tab, select Data Type Cell & Wall/Bound (Smooth) Select Turb Kinetic Energy from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Options tab of the Create Plots panel, change the Range option to User and specify a range of 0 to 4 Click Apply. This will fix the legend scale for all animation frames. Click Replot to display a contour plot of turbulence kinetic energy at time = 0.015 seconds In the main pro-STAR window, select Modules > Animation In the Animation module, change the Number of Frames in Sequence to 100 Select Edit Frame Definitions.. > First Frame... In the Animation Graphics Parameter Block dialog window, select Copy > Current Plot. This will set the plotting options for the first animation frame to be the same as those of the current plot Change the Time to 0.015 Click Apply Select the End of Animation Sequence radio button Select Copy > First Frame Change the Time to 1.5 Click Apply and then Close In the Animation module, click Edit Sequence Parameters Enter the following commands in the first two lines of the Post-Animation Sequence Commands box: STORE NEXT GETV TE

13-22

Version 4.02

Tutorial 13.2


Post-Processing Pressure Trace

• • • •

Change the Command For Initial Plot to Replot Click Close Click Record to write the animation data to the neutral plot file Once the data have been written, click Play to view the animation

You should notice that the vortex shedding in the wake of the cylinder is quite irregular. This is due to the random fluctuations introduced by the DES turbulence model. Pressure Trace

The vortex shedding irregularity can also be seen in a plot of pressure at the monitoring point: •

Increase the maximum number of available graph register locations by typing MEMORY MXSTOR 1000000

• • • • • • • • • • •

at the command line Select the Post-Processing folder in STAR GUIde Select the Graphs folder followed by the Extract/Graph Data folder Open the Engineering Data panel Change the Read ... file option to Cell Click the read file button, , to display the contents of the .ecd file Select PMON from the Select Entry list Select PMAX in the Select data to graph section. As there is only one cell in the set, PMAX = PMIN = PVAV = PMAV. Click Add data to list Click Create Graph Click Yes when asked if you wish to continue Select Draw Frame > Current

The default graph setting does not show the profile clearly enough. To obtain a better view of this profile, resize the graph and adjust the axes: • • • • • • • • • • •

Version 4.02

Select the Graphs sub-folder in the Post-Processing folder Open the Customize Graphs panel Under the Axis tab, select the Y-Axis Parameters sub-tab Change Ymin to -80 and Ymax to 20 Change the Title to Pressure - Pa Click Apply Under the Axis tab, change Xmin to 0, Xmax to 1.5, Xmajor to 0.15 and #ticks to 2 Change the Numbers option to Real Change the Title to Time (s) Click Apply Click Redraw to display Figure T13.2-2

13-23

Tutorial 13.2


Post-Processing Pressure Trace

Figure T13.2-2

Pressure profile at the monitoring point

Figure T13.2-2 shows that the frequency of pressure fluctuations due to vortex shedding is regular even though the amplitude is not. By measuring the time between pressure peaks on the graph, the frequency of these oscillations is found to be around 6.2 Hz. This is fairly close to the value predicted in the introduction to this tutorial. It is also possible to calculate the sound pressure level (volume) of these fluctuations using the following equation: ∆p 2 SPL = 10 log ⎛ ---------⎞ ⎝ p ref ⎠ Using ∆p = 45Pa (the approximate average amplitude of the pressure –5 oscillations) and P ref = 2 × 10 Pa (the lower limit of human perception), this gives a sound pressure level of 127 dB. The tutorial is now complete. Further analysis of the results may be performed using a specialised acoustics package. For example, es-acoustics may be used to perform a Fourier Transform on the pressure profile to derive a frequency profile for the aeroacoustic noise. To exit from pro-STAR: •

13-24


Version 4.02

Tutorial 14 LIQUID FILM SIMULATION The following tutorials are intended to familiarise users with the process of setting up liquid film simulations. The two cases presented are: 1. Evolution of a rectangular, two-dimensional, and initially stationary liquid blob flowing under gravity down a vertical wall, and comparison with the analytical solution 2. 3D film formation and transport due to spray impingement

Version 4.02

14-1

Tutorial 14.1

2D FILM FLOW DOWN A VERTICAL WALL

Tutorial 14.1



Physical Problem Description In this tutorial, we consider the evolution of a rectangular, two-dimensional and initially stationary blob of liquid flowing down a vertical wall under the action of gravity and forming a liquid film in the process, as shown in Figure T14.1-1. The calculation is compared with an analytical solution for film thickness δ as a function of position x and time t given in [1]: 1⁄2

µ 1⁄2 x --------δ = ⎛ --------- ⎞ 1⁄2 ⎝ gρf ⎠ t where µ is the film viscosity, ρ f the film density and g the value of gravity. The solution is independent of initial values, i.e. it is valid regardless of initial film profile, film thickness and wall area covered at the start of the calculation. y Initial blob

Air

2m

x

Wall

Gravity

Film Figure T14.1-1

Schematic of vertical film flow and CFD mesh

In the problem we assume that the initial 2D blob has a film thickness of 1 mm and covers a wall length of 250 mm. The case is run for a simulated time of 10 seconds, which is long enough for the similarity condition given by the above equation to be satisfied. Heat and mass transfer simulations are deactivated. The solution domain is 2 m long in the vertical direction and 50 cm wide in the wall-normal direction. A uniform mesh is used, as shown in Figure T14.1-1. [1] D.A. Acheson, “Elementary Fluid Dynamics”. Oxford University Press, 1992

14-2

Version 4.02

Tutorial 14.1



Pre-Processing Preliminaries Create a sub-directory for this tutorial called tut14-1 and copy file liquid_film.ccm supplied with the STAR-CD installation into it. In this directory: • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name, blob, in the Casename text box Click Continue

Make sure that the STAR GUIde window is displayed on your screen, next to the main pro-STAR window: • • • • • •

Open the Select Analysis Features panel in STAR GUIde Select Transient from the Time Domain menu Select On from the Liquid Films menu Click Apply In the main window, select File > Model Title In the Title text box type: TRANSIENT 2D FLOW DOWN A VERTICAL WALL


The mesh used in this case is two-dimensional, extending 2 m in the x-direction of the global Cartesian coordinate system and 50 cm in the y-direction and has 120 and 20 cells in each direction, respectively. The thickness of the mesh is set to 5 cm but will have no effect on the result, given the two-dimensional nature of the simulation. To import and display the mesh: • • • • • • • • •

Version 4.02

Click Apply

Select the Create and Import Grids folder in STAR GUIde Open the Import Grids panel Select the CCM button from the Format list. liquid_film.ccm will be selected as the CCM File name Check that the State Name entry is set to default Click Import Grid In the main window, select C > All to put all cells into the current cell set Check that the Geometry Plot mode and Hidden Surface plot type are selected Click Cell Plot Click View > Isometric and select 1, 1, 1 to display the grid shown in Figure T14.1-2

14-3

Tutorial 14.1



Figure T14.1-2

Boundary Locations

2D hexahedral mesh

In addition to mesh data, file liquid_film.ccm also contains information on boundary region locations. The latter can be displayed on the grid plot as follows: • • •

Select the Locate Boundaries folder in STAR GUIde Open the Create Boundaries panel Select each entry on the Boundary Regions list in turn (except no. 0) and then click Plot Region to display its location

Note that the wall boundary is split into two regions, of which no. 1 is that part of the wall where film is initially present, and no. 2 the part where film appears at a later time once the analysis begins. This subdivision is necessary purely for the purposes of specifying film initial conditions (see “Initial and Boundary Conditions”) Display the location of all the key boundaries in the problem: • •

14-4

In the main window, select B > New > Wall and B > Add > Pressure to display the boundaries shown in Figure T14.1-3 Turn off the Bound Cell Plot Display Option

Version 4.02

Tutorial 14.1


Pre-Processing Material Properties and Physical Models

Figure T14.1-3

Wall and pressure boundaries

Material The following properties are used for the two phases: Properties 1. The gas phase is ambient air with a density of 1.205 kg/m3 and viscosity of and Physical 1.81 × 10-5 Pas Models 2. The liquid phase is pure water with a density of 1000 kg/m3 and viscosity of 0.00089 Pas Define the direction of gravity and assign physical properties to the two phases: • • • • • • • •

Select the Thermophysical Models and Properties folder Open the Gravity panel Change the Acceleration due to gravity to 9.81 m/s2 Change the gravity Direction to (1, 0, 0) in coordinate system 1 Click Apply Select the Liquid and Gases folder Open the Molecular Properties panel. The displayed default properties of air are acceptable so no input is needed for this panel. Open the Initialization panel. Again, the displayed defaults are appropriate for this case so no input is needed.

Select locations for the pressure reference and monitoring cells as follows: • • • •

Open the Monitoring and Reference Data panel Enter 501 in the Monitoring cell number box Enter 501 in the Reference Pressure Cell Number box Click Apply

Define liquid film physical properties and model controls: Version 4.02

14-5

Tutorial 14.1


Pre-Processing Initial and Boundary Conditions

• • • • • • • •

• • • Initial and Boundary Conditions

Select the Liquid Film folder and then open the Film Controls panel Select the Gravity Force option Click Apply Check that both wall regions (nos. 1 and 2) are set up for liquid film support by scrolling the Region # slider at the bottom of the panel Open the Film Physical Models and Properties panel On the Film Models tab, turn On the Liquid Film (Type) Activation option and then click Select from Database In the Droplet Properties Database list, select H2O_l [Water (L)] and click Select Material Click Close to exit from the Droplet Properties Database panel and return to the Film Models tab. Note that your selection is now displayed in the First component name box and thus defines the film material to be used in this problem. Check that the Evaporation and Condensation option is deselected and then click Apply On the Film Properties tab enter 1000 for Density and 0.00089 for Viscosity. The rest of the property values displayed are not used in this case. Click Apply

Define the film’s initial conditions: • • • • •

Open the Film Initialization panel Check that the Region # scroll bar is set to 1 (the region initially occupied by the film) and click Initialize Enter 0.001 in the Thickness box (leaving all other initial conditions at their defaults) and click Apply Set the Region # scroll bar to 2 (the rest of the wall region) and click Initialize Enter 0 in the Thickness box (leaving all other initial conditions at their defaults) and click Apply. This signifies that initially there is no film on this part of the wall.

Define film boundary conditions for all wall regions. Before doing this, you may want to review all boundaries again, as done in section “Boundary Locations”, to remind yourself of the relevant region numbers and locations: • •


Specify various solver parameters and output controls required for this case: • • • •

14-6

Open the Film Boundaries panel and check that the Condition # scroll bar at the bottom of the panel is set to 1 Enter 2 (the wall region where a film will form at a later stage) in the Film Region # box and 6 (the pressure region next to it) in the Adjacent Region # box and select Outlet for the film boundary condition. Click Apply

Select folder Analysis Controls followed by Solution Controls followed by Equation Behavior Open the Primary Variables panel On the Equation Status tab, deselect option W-Mom since we are solving a 2D flow in the x-y plane only Click Apply Version 4.02

Tutorial 14.1



• • • •

• • • • • Run Time Controls

Select folder Output Controls and open the Analysis Output panel Under the Post tab, check that option Write final solution (restart) file is selected with an Output Frequency of 100 time steps Click Apply Select the Transient tab. Enter 0 in the Starting at time box and 0.1 in the Write data every box. In view of the time step size chosen below, this will result in transient post data being saved every 10 time steps. Select the Wall data button Scroll down to find Film Thickness in the variable list Select this item and also the Post option (if not selected) Repeat this process for Film Velocity Click Apply

Run the analysis for a total of 10 seconds using two time periods. The first period covers 1 s and uses a time step of 0.001 s in order to ensure computational stability. The second period covers the remaining 9 s and uses a time step of 0.01 s. • • • • • •

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Select the Run for button, enter 10 in the adjacent box and click Apply In the Time Step Option section, enter 0 for the Period Start Time and 0.001 for the Time Step for period entry Click Set Period Now enter 1.0 for the Period Start Time and 0.01 for the Time Step for Period entry and click Set Period again

These settings will be listed in the Time Periods window. Final Operations

You can run this simulation from STAR GUIde. However, it is more common to run (lengthy) transient cases from the command line. Write the geometry and problem files and save the model file: • • • • • •

In the main pro-STAR window, select File > Write Geometry File In the Geometry File Write dialog, check that 1.0 is entered as the Geometry Scale Factor Click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis Check that you are in the current working sub-directory (tut14-1) and run the CFD analysis in double precision by typing star -dp at the command line.

Version 4.02

14-7

Tutorial 14.1



Post-Processing Preliminaries When the simulation is complete and whilst in the tut14-1 sub-directory: • • • • • •

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name, blob, in the Casename text box Select the Resume existing .mdl file? option Select the Append to .echo file? option Click Continue

Open the file containing the transient post data (blob.pstt): • • • •

Basic Plots

Read in the last set of results and make a contour plot of film thickness: • • • • • • • •

14-8

In the STAR GUIde window, select the Post-Processing folder and then open the Load Data panel Under the File(s) tab, select Transient as the Analysis option Select entry no. 1 in the Transient Post File(s) list and click Add File to List Select file blob.pstt from the list and then click Open Transient Post File. All the stored transient time step data will now be displayed in the Select Time Step window

In the Select Time Step list, scroll to the end of the list, select step number 1900 and click Store Iter/Time Go to the Data tab and select Wall for the Data Type In the Scalar Data list, select item Film Thickness Click Get Data In the main window, select plot option Contour Plot Click Plot > Wall Plot Turn mesh plotting Off by clicking the mesh on/off button Rotate the plot using the mouse controls so that it is displayed approximately as shown in Figure T14.1-4 (View 0, -1, 0.5, Angle -90)

Version 4.02

Tutorial 14.1



Figure T14.1-4

Animations

Film thickness contour at t=10 seconds

pro-STAR loops can be used to produce on-screen animations, as described in Tutorial 8.2 and Tutorial 12.3. However, in this tutorial we will use pro-STAR’s macro facility (see Chapter 16 of the CCM User Guide) to produce an animation of the film thickness development. Before proceeding further, ensure that film thickness contours are displayed as shown above. • • •

Select Panels > Define Macro ... from the menu bar on the main pro-STAR window Enter anim as the macro name and click New Click Open and then type in the following commands: store first *define noex store next getw lfthk bset news regi 1 bset add regi 2 vset news bset cset news name wall cset subs vset any wplot *end *loop 1 99


On the [MACRO] anim.MAC panel, click File > Save followed by File > Quit. File anim.MAC file will be saved to your local directory. Click Execute on the Define Macro ... panel 14-9

Tutorial 14.1


Post-Processing Graphs

The resulting animation shows the movement of the film from rest over a 10 second period. Graphs

The spatial distribution of film thickness at a particular time (e.g. at 10 seconds) can be plotted using pro-STAR’s graph facilities. Again, it is more convenient to save the relevant commands in a pro-STAR macro file: • • •

Select Panels > Define Macro ... Enter graph as the macro name and click New Click Open and then type in the following commands: ! *** select the wall film cells bset news region 1 bset add region 2 vset news bset cset news name wall cset subs vset all ! *** reset the graph properties greset y ! *** load x value gload,1,wall,cset,0,0,1 gvalue,2,1,wall,x,2 ! *** load film thickness gvalue,4,1,wall,pst4,0 ! *** draw the graph frame,1,locate,1.70,2.10,9.65,9.45 frame,1,legend,none frame,1,xrange,0,2 frame,1,xtick,0,0,real,noindent,bottom frame,1,xtitle,5.25,1.3 Distance (m) frame,1,yrange,0,0 frame,1,ytick,2.5e-05,0,real,left frame,1,ytitle,0.28,7.58 Film thickness (m) frame,1,legend,none frame,1,xreg,init, 2, frame,1,yreg,init, 4, gdraw,1 ! *** save the data in a ASCII file named fthick.grf sdata,fthick.grf,2,2,2,coded close fthick.grf

• •

14-10

On the [MACRO] graph.MAC panel, click File > Save followed by File > Quit. File graph.MAC file will be saved to your local directory. On the Define Macro ... panel click Execute to display the graph shown in Figure T14.1-5

Version 4.02

Tutorial 14.1


Suggestions for Further Exercises Graphs

Figure T14.1-5

Spatial distribution of film thickness

The data saved in file fthick.grf may then be used for comparison against analytical solutions. •


Suggestions for Further Exercises The agreement between model predictions and the analytical solution can be improved further if a smaller time step is used. The user may also wish to test the theory that the similarity solution for film thickness is independent of the initial film profile by setting up a film covering the full length of the wall at the start of the simulation.

Version 4.02

14-11

Tutorial 14.2

SPRAY IMPINGEMENT ON A WALL

Problem Description Preliminaries

Tutorial 14.2


Problem Description In this tutorial, a diesel fuel spray (n-Dodecane, C12H26) is injected into the closed box shown in Figure T14.2-1 (dimensions 16 × 16 × 44 mm). The injection point is a nozzle with its axis perpendicular to the bottom of the box and located 24 mm above it. The nozzle diameter is 0.3 mm. The injection lasts for 1.2 ms, the total fuel injected is approximately 8 mg and the fuel temperature is 293 K. The fluid in the box is quiescent air at room temperature (293 K) and at an elevated pressure of 15 bar. The Huh atomisation and Reitz-Diwakar break-up models are used for the spray simulation. Furthermore, inter-droplet collisions and spray-wall interactions are taken into account. Liquid film is formed on the bottom wall due to spray impingement. The case will be set up as a transient liquid film simulation and run for 100 time steps with a time step size of 2.0 × 10–5 s.

20 mm

24 mm

16 mm Figure T14.2-1

16 mm

Problem geometry

Pre-Processing Preliminaries Create a sub-directory for this tutorial, say tut14-2. The mesh data for the problem, in the form of cell and vertex definitions, are supplied ready-to-use in files impinge.cel and impinge.vrt. Therefore, before starting the tutorial, make sure that the supplied files are copied into your current directory. • • • Version 4.02

Start up pro-STAR by typing prostar at the command line Specify your preferred graphics driver (xm, mesa or glm) Enter the case name, impinge, in the Casename text box 14-13

Tutorial 14.2


Pre-Processing Mesh Creation

• • •

Click Continue In the main window, select File > Model Title In the Title box type SPRAY WALL IMPINGEMENT AND LIQUID FILM

•

In the Subtitle Line 1 box type Impingement distance: 24 mm

•

Click Apply

Make sure that the STAR GUIde window is displayed on your screen, next to the main pro-STAR window and then: • • • • • Mesh Creation

Open the Select Analysis Features panel in STAR GUIde Select option Transient from the Time Domain menu Select option Lagrangian Multi-Phase from the Multi-Phase Treatment menu Select On from the Liquid Films menu Click Apply

The computational mesh data are stored in files impinge.cel and impinge.vrt. These can be imported using pro-STAR’s GUI panels as follows: • • • • • • • • • • • •

In the main window, select Tools > Cell Tool to open the Cell Tool Click Cell Read to open the Cell Read panel Accept the default values and click Apply (pro-STAR will read in cell data from file impinge.cel) Close the Cell Read panel Close the Cell Tool In the main window, select Tools > Vertex Tool to open the Vertex Tool Click on Vertex Read to open the Vertex Read panel Accept the default values and click Apply (pro-STAR will read in vertex data from file impinge.vrt) Close the Vertex Read panel Close the Vertex Tool In the main window, collect all cells into a set by selecting C > All Collect all vertices into a set by selecting V > All

Define the z-axis as the vertical axis and then display the imported mesh: • • • •

In the main window, select Plot > Up Axis > Z Check that the Geometry Plot mode and Hidden Surface plot type are selected Click Cell Plot Select View > Isometric > 1 1 1

Check the coordinate system used to create the mesh: • • • 14-14

In the main window, click the CSYS button Select coordinate system no. 1 (Cartesian) and then click Show Triad Change the plot type to Quick Hidden Line to display the mesh, as shown in Version 4.02

Tutorial 14.2


Pre-Processing Mesh Creation

Figure T14.2-2

Figure T14.2-2

3D Cartesian mesh

It can be seen that the origin is already at the desired location (the injector nozzle tip). What is now needed is to define a local cylindrical coordinate system with the same origin and with its z-axis along the injection direction: • • •

In the Coordinate Systems dialog, click Hide Triad Select system no. 10 Select Cylindrical from the pop-up menu and enter the following values in the adjacent boxes: xc = 0 yc = 0 zc = 0 Rxy = 0 Ryz = 0 Rzx = –180

• • • • • •

Version 4.02

Click New (Local) Click Show Triad In the main window, click Replot to display the location of this system, shown in Figure T14.2-3, and confirm that it has been defined correctly Click Hide Triad Select system no. 1 and then click Set Active Close the Coordinate Systems dialog

14-15

Tutorial 14.2


Pre-Processing Boundary Specification

Figure T14.2-3

3D Cartesian mesh with the injector location at 0, 0, 0, in local coordinate system number 10

Boundary We next define the bottom and side walls as distinct boundary regions. The bottom Specification wall is the only region that can support a liquid film. The side walls are defined as separate regions only in order to facilitate the film boundary specification. • • • • • • • • • • • • • • • • 14-16

Select the Locate Boundaries folder in the STAR GUIde window Open the Create Boundaries panel Select Reg#1 in the Boundary Regions scroll list Select Wall for Type, enter Film_Wall-Z in the Name box and then click Define region In the main window, select View > Axis > -Z In the Create Boundaries panel, select Surface Based on Edges and then click on any bottom-wall vertex displayed in the main window Select Reg#2 in the Boundary Regions scroll list Select Wall for Type, enter Side_Wall+X in the Name box and then click Define region In the main window, select View > Axis > +X In the Create Boundaries panel, select Surface Based on Edges and then click on any side-wall vertex displayed in the main window Select Reg#3 in the Boundary Regions scroll list Select Wall for Type, enter Side_Wall-X in the Name box and then click Define region In the main window, select View > Axis > -X In the Create Boundaries panel, select Surface Based on Edges and then click on any side-wall vertex displayed in the main window Select Reg#4 in the Boundary Regions scroll list Select Wall for Type, enter Side_Wall+Y in the Name box and then click Version 4.02

Tutorial 14.2


Pre-Processing Material Properties and Physical Models

• • • • • • • • • •

Define region In the main window, select View > Axis > +Y In the Create Boundaries panel, select Surface Based on Edges and then click on any side-wall vertex displayed in the main window Select Reg#5 in the Boundary Regions scroll list Select Wall for Type, enter Side_Wall-Y in the Name box and then click Define region In the main window, select View > Axis > -Y In the Create Boundaries panel, select Surface Based on Edges and then click on any side-wall vertex displayed in the main window Select View > Isometric > 1,1,1 In the main window, select B > All Click Bound in the Cell Plot Display Options area to check the boundaries just defined Click Bound to turn off boundary plotting

The mesh set-up is now complete. Material Properties and Physical Models

Although the problem in this case is essentially isothermal, the model set-up described below is for a non-isothermal case. This is done purely in order to prepare the model in advance for a more general simulation in which heat and mass transfer occur between the spray droplets, the liquid film, and their surrounding gas. Assign physical properties to the two gaseous components (air and fuel vapour) in the solution domain: • • • • • • • • • • • • • •

Select the Thermophysical Models and Properties folder Open the Gravity panel Check that the Direction of Gravity Force is set to (0, 0, -1) in coordinate system number 1 and then click Apply Select the Liquid and Gases folder Open the Molecular Properties panel and check that the Material # slider at the bottom of the panel is set to 1 Select Ideal-f(T,P) as the Density option and then click Apply Activate the turbulence calculations by opening the Turbulence Models panel and selecting On Choose k-Epsilon/High Reynolds Number from the Turbulence menu and then click Apply Open the Thermal Models panel and select Temperature Calculation On Click Show Options and check that option Thermal is selected in the Enthalpy menu Click Apply Open the Initialization panel and check the values in the Flow Condition tab. All defaults are acceptable Open the Monitoring and Reference Data panel Enter 1.5e6 in the Pressure box and then click Apply

Define scalar no. 1 to be the product of droplet evaporation and import its physical properties from pro-STAR’s built-in database: • Version 4.02

In the Thermophysical Models and Properties folder, select the Additional Scalars sub-folder 14-17

Tutorial 14.2


Pre-Processing Droplet Properties

• • • •

Droplet Properties

Open the Molecular Properties (Scalar) panel and check that the Scalar # slider at the bottom of the panel is set to 1 Choose option Select scalar from database from the menu at the top of the panel Select Dodecane (V) from the Scalar Database scroll list and then click Select Scalar The physical properties of dodecane vapour are read in from pro-STAR’s property database into the appropriate panel boxes. Check that the displayed values are reasonable and then click Apply.

The maximum number of droplet parcels required for this case (10,000) is above the default maximum allowed by the code, so it is necessary at this point to resize pro-STAR by issuing the following commands from the I/O window: MEMORY MAXDRP 10000 MEMORY WRITE Check the basic control settings for droplets: • • • • • • •

Select folder Lagrangian Multi-Phase and open the Droplet Controls panel Check that option Coupled is selected in the Two-Phase Lagrangian Calculations menu and keep the default Courant number Check that option Use Gradient is selected in the Interpolation Method menu Accept the default value of 0.35 for the Under-Relaxation of Lagrangian Sources term Type 10000 in the Maximum Number of Parcels box Select option Spray injection with atomisation Click Apply

Activate the turbulent dispersion model and define transport mechanisms and physical properties for the droplets: • • • • • • • • • • •

Open the Droplet Physical Models & Properties panel and select the Global Physical Models tab Activate the Turbulent Dispersion and Gravity Effects options Select option Standard for the Collision Model Click Apply Select the Droplet Physical Models tab For Momentum Transfer, select option Standard and accept the default Mass Coef. and Slip Factor values Select option Standard for the Mass Transfer Select option Standard for the Heat Transfer Select option Reitz for the Droplet Breakup and accept the default values of the model constants Select option Bai for the Droplet-Wall Interaction and accept the default values of the model constants Click Apply

Specify droplet physical properties for n-Dodecane, which in this case are to be calculated by STAR using its internal fuel property functions: • 14-18

Select the Droplet Properties tab Version 4.02

Tutorial 14.2



• •

• • • • •

Click Select from Database to open the Droplet Properties Database dialog Scroll down the database material list to locate item # DODECANE(L), select it, check the Use Internal Property Calculation box and then click Select Material Close the Droplet Properties Database dialog Click the Evaporates to Scalar Select button Define scalar no. 1 as the product of evaporation by selecting it in the Scalars list Click Close In the Droplet Properties tab, click Apply

The injector location was specified earlier using local coordinate system 10. Its geometric and physical properties can now be specified: • • • • •

• • • • • • Boundary Conditions

Specify thermal boundary conditions for the spray impingement plane at the bottom of the box: • • • •

Film Model Controls

Open the Spray Injection with Atomisation panel Select 3 Dimensional for the Domain and Huh for the Atomization Model Accept the default settings in the Nozzle specification section Click Apply Spray Options In the Define Injectors section, enter the following parameters: Injection Temperature — 293 Hole Diameter — 0.0003 Coordinate System — 10 Select option Fixed for the fuel Mass Flow Rate, and then enter a value of 0.007 (kg/s) in the box next to the drop-down menu Enter 0 in the Start of Injection box Enter 0.0008 in the End of Injection box Enter 1.0e+06 in the Number of Parcels/Injector box Check that the value in the Droplet Type list box is 1 and the name DODECANE(L) appears next to it Click Update Injector

Select the Define Boundary Conditions folder and then open the Define Boundary Regions panel Select Reg#1 (named Film-Wall-Z) in the scroll list Select option Fixed from the Wall Heat menu and enter 293 for the boundary Temperature and 0 for its thermal Resistance Click Apply

Now define the liquid film model controls. Note that since the film is formed entirely from wall-impinging droplets, its physical properties will be inherited from those droplets and therefore do not need to be specified explicitly. • • •

Select the Liquid Film folder followed by the Film Controls panel Turn On the Gravity Force Click Apply

Define the film’s initial conditions: • Version 4.02

Open the Film Initialization panel 14-19

Tutorial 14.2



• •

Check that the Region # scroll bar is set to 1 and click Initialize Enter 0 in the Thickness box (leaving all other initial conditions at their defaults) and click Apply. This signifies that initially there is no film on this wall.

Define film boundary conditions for all wall regions. Before doing this, you may want to review all boundaries again, as done in the “Boundary Specification” section, to remind yourself of the relevant region numbers and locations: • •

• • • •

Open the Film Boundaries panel and check that the Condition # scroll bar at the bottom of the panel is set to 1 Enter 1 (the wall region where a film will form at a later stage) in the Film Region # box and 2 (Side_Wall+X) in the Adjacent Region # box and select Outlet for the boundary condition to be applied to the film. Click Apply Set the Condition # scroll bar to 2 Enter 1 in the Film Region # box and 3 (Side_Wall-X) in the Adjacent Region # box and select Outlet for the film boundary condition. Click Apply

Repeat the above process for the adjacent regions 1 and 4 (Side_Wall+Y) and 1 and 5 (Side_Wall-Y) to complete the liquid film boundary condition set-up. Analysis Controls

Specify various solver parameters and output controls required for this case: • • • • • • •

• • •

• • • • • •

14-20

Select folder Analysis Controls followed by Solution Controls Open the Solution Method panel and change the Under-Relax. for Press. Correction value to 0.5 Click Apply Select the Equation Behavior folder and then open the Primary Variables panel Go to the Differencing Schemes tab and select MARS for all Flow Variables, accepting the default value of the compression level for all equations Click Apply Open the Additional Scalars panel and select C12H26 from the Scalar list. Change the Residual Tolerance to 0.01 and set the Differencing Scheme to MARS, accepting the default value of the compression level. Click Apply Select the Output Controls folder and then open the Analysis Output panel Select the Transient tab. First enter 0 in the Starting at time and 4.0e-5 in the Write data every box. The last setting will ensure that post data will be saved every 2 time steps. Scroll to locate item C12H26 in the data scroll list. Select it and then click the Post button Deselect the Cell Data option and then select Wall data Locate and select item Film Thickness in the data scroll list Click Post Repeat for items Film Velocity and Film Temperature Click Apply

Version 4.02

Tutorial 14.2



Run Time Controls

Set the run time control parameters: • • • • • •

Final Operations

Select the Analysis Preparation/Running folder Open the Set Run Time Controls panel Select the Run for button and then enter 0.002 in the adjacent box Click Apply In the Time Step Option section, enter 0 in the Period Start Time and 2.0e-5 in the Time Step for Period boxes Click Set Period

If you wish to terminate the session at this stage, write the geometry and problem files and exit from pro-STAR, saving the model data as shown below: • • • • • •

Select File > Write Geometry File Enter 1 in the Geometry Scale Factor box Click Apply and then Close Select File > Write Problem File Click Apply and then Close Select File > Quit > Save & Quit

CFD Analysis For flows involving sprays, it is recommended that STAR is run in double precision mode, by typing star -dp in your session window. The analysis will then start automatically. The simulation should run for 100 time steps and save flow field data to file tut.pstt every 2 time steps. Post-Processing Open the file containing the transient post data (impinge.pstt): • • • • •

In the STAR GUIde window, select folder Post-Processing Open the Load data panel Toggle the Analysis option to Transient Select entry no. 1 in the Transient Post File(s) list and click Add File to List Select file impinge.pstt from the list and then click Open Transient Post File. All stored transient time step data will now be displayed in the Select Time Step window.

Plot the film thickness formed at the 20th time step: • • • • • Version 4.02

In the Select Time Step list, scroll down to the 10th entry, select it and click Store Iter/Time button Go to the Data tab. Select Wall for the Data Type and On for the Smooth Option In the Scalar Data list, select item Film Thickness Click Get Data In the main window, select plot options Contour Plot and Hidden Surface 14-21

Tutorial 14.2



• • •

Select View > Isometric > 1,1,-1 Deselect mesh plotting by clicking off the mesh plotting button Select edge plotting by clicking on the edge plotting button

Add droplets to this plot: • • • • • • • • • • •

In the main window, select the droplet display option by choosing Plot > Cell Display >Droplets In the STAR GUIde window, select the Particle Tracks folder Open the Plot Droplets/Particle Tracks panel and go to the Droplets tab In the Load Droplet Data section, select Current Post Data File from the Load from menu Click Load Data In the Droplet Plot Options section, select Off for the Edge Plot Options Select Diameter for the Droplet Radius and enter 0.0005 in the Size box Select None for the Vectors option Click Apply In the main window, select D > All to collect all droplets in the domain into a set Click Plot > Wall Plot

Figure T14.2-4

Droplet and liquid film thickness contour plot

The above steps may be repeated for other times and variables of interest. Animations

14-22

As pointed out in Tutorial 14.1, transient results for spray and liquid film problems are best viewed by means of an on-screen animation. Again, use pro-STAR’s macro facility (see Chapter 16 of the CCM User Guide) to produce an animation of the film and droplet development.

Version 4.02

Tutorial 14.2



• • •

Select Panels > Define Macro ... from the menu bar on the main window Enter anim as the macro name and click New Click Open and then type in the following commands: store first *define noex store next getd post dset all getw lfthk cave all bset news regi 1 vset news bset cset news name wall cset subs vset all wplot *end *loop 1 49

• •

On the [MACRO] anim.MAC panel, click File > Save followed by File > Quit. File anim.MAC file will be saved in your local directory. Click Execute on the Define Macro ... panel

The above executes all commands within the loop 50 times to produce successive snapshots of the spray and liquid film state at every saved time step. Final Operations

Version 4.02

•

Select File

> Quit > Quit,Nosave

14-23


Tutorial 15 COAL COMBUSTION Physical Problem Description The following tutorials describe in detail how to set up, run and post-process a simple CFD problem involving coal combustion. The problem geometry represents a furnace with three concentric air inlets, a primary (inner), a secondary (middle) and a tertiary (outer) one, located at one end. The primary inlet also acts as a pulverised coal carrier. Air enters the solution domain through the tertiary inlet and has a swirling velocity component. Flow exits the domain through an outlet situated at the opposite end of the furnace. A hexahedral mesh is used to model the problem, as shown in Figure T15.0-1. The mesh was previously generated and stored as a .ccm format file, and this is provided with the STAR-CD installation.

Primary Inlet

Outlet

Furnace Wall Secondary Inlet Tertiary Inlet Figure T15.0-1

Coal combustion furnace mesh geometry

Modelling Strategy The following modelling strategy was adopted: • • •

Perform an initial run in non-reacting and isothermal mode (Tutorial 15.1) Run the model using the Constant Rate Devolatilisation and Eddy Break-Up gaseous combustion models (Tutorial 15.2) Run the model using the Two-Competing-Steps Devolatilisation and Eddy Break-Up gaseous combustion models (Tutorial 15.3)

Using this type of modelling strategy to achieve a solution in three stages is the Version 4.02

15-1

Modelling Strategy

recommended method for all coal combustion cases. However, for some problems, it may be possible to reach a good solution by missing out the first or second stages, or even, for very simple problems, both.

15-2

Version 4.02

Tutorial 15.1

ISOTHERMAL, NON-REACTING FLOW


Tutorial 15.1


For most coal combustion simulations it is advisable to run the case initially as an isothermal problem. This will allows a stable flow field to be obtained before the coal combustion models are introduced. This tutorial gives a detailed account of how to set up the isothermal, non-reacting coal case for the furnace shown in Figure T15.0-1. Pre-Processing Preliminaries Create a working directory for the tutorial named tut15-1. For this problem, the mesh geometry data are supplied in file furnace.ccm. Therefore, before starting the tutorial, make sure that this file is copied into your working directory. Start up pro-STAR in this directory and begin the modelling task by specifying the case name and problem title: • • • • • •

Type prostar at the command line Specify the graphics driver (xm, mesa or glm) Type coal_iso in the Enter Case Name text box Click Continue In the main pro-STAR window, select File > Model Title In the Title text box type COAL COMBUSTION - ISOTHERMAL ANALYSIS

•

Click Apply

Importing the Make sure that the STAR GUIde window is displayed on your screen, next to the Mesh main pro-STAR window. If not, activate it by clicking the special ‘Show STAR GUIde’ button shown below:

• • • •

Select folder Create and Import Grids and then open the Import Grids panel Select CCM as the file Format Change the CCM File name to furnace.ccm Click Import Grid

The following information should appear in the I/O window:

Verify that the mesh has been imported correctly by selecting all cells and boundaries and plotting the mesh in ‘Hidden Surface’ mode: • Version 4.02

In the main window, select C > All to select all cells 15-3

Tutorial 15.1


Pre-Processing Model Specification

• • • • • • •

Select B > All to select all boundaries Check that Hidden Surface is the default cell plot type Select Bound for the Cell Plot Display Option Click Cell Plot Change the viewpoint to approximately (-1.0, 0.5, -1.0) using the orientation cube’s slider controls Remove the wall boundaries from the display by selecting B > Unselect > Wall and clicking Replot Zoom in on the red inlet boundaries to create a plot resembling Figure T15.1-1

Note the positions of the three concentric inlet boundaries.

Figure T15.1-1

Furnace inlet boundaries

Model Set up the basic models used in the isothermal case: Specification • Open the Select Analysis Features panel in STAR GUIde • Under Time Domain, check that Steady State is selected. This is essential because coal combustion simulations are not feasible in transient mode • Click Apply Material Assignment and Thermal Options

15-4

All fluid cells should already be assigned to material number 1 by default. Check this via the Cell Table Editor: • • • •

In the main pro-STAR window, click CTAB to display the Cell Table Editor Select cell type no. 1 and verify that the Material Number value is 1 Click Close to exit the Cell Table Editor Go to the STAR GUIde window and select the Thermophysical Models and Properties folder followed by sub folder Liquids and Gases Version 4.02

Tutorial 15.1



• •

• • • • • • • • • • • • Boundary Conditions

The model consists of inlet, outlet and wall boundary regions. The velocity, thermal and turbulence boundary conditions need to be specified for these: • • • • • • • • • • • • • • • • •

• • • • Version 4.02

Open the Molecular Properties panel The default material is air, which is suitable for this case. The flow is compressible and without pressure dependency so select Ideal-f(T) for the Density option Select Polynomial for the Specific Heat option and click on Define/Edit Polynomial In the Polynomial Function Definition dialog, select N2 from the CHEMKIN Database scroll list Click Apply Database Substance Close the dialog and then click Apply at the bottom of the Molecular Properties panel Open the Turbulence Models panel and turn On turbulent flow Choose the k-Epsilon/High Reynolds Number model Leave all settings as their default values and click Apply Open the Thermal Models panel and select Temperature Calculation On Click Apply Open Monitoring and Reference Data panel The default monitoring location (cell number 1) is suitable. Change the Reference Pressure Cell number to 8279 and the Pressure to 1.0325E+05 Pa Click Apply

Select the Define Boundary Conditions folder, then open the Define Boundary Regions panel In this panel, select Reg# 1- Inlet. This is the primary air inlet. Enter an axial velocity value of 10 in the W (m/s) box Select TI/Length for the Turb. Switch option Enter a Turb. Intensity of 0.1 and a Length of 0.06 m Enter a value of 1 in the Dens. (kg/m3) box Enter a value of 353 in the Temp. (K) box Click Apply Select Reg# 2 - Inlet. This is the secondary air inlet. Enter an axial velocity value of 10 in the W (m/s) box Select TI/Length for the Turb. Switch option Enter a Turb. Intensity of 0.1 and a Length of 0.01 m Enter a value of 1 in the Dens. (kg/m3) box Enter a value of 353 in the Temp. (K) box Click Apply Select Reg# 3 - Inlet. This is the tertiary air inlet. To specify a swirling flow at this inlet, the velocity components need to be entered in the global cylindrical coordinate system. Enter 2 in the Coord. System box Enter an axial velocity component of 20 in the W (m/s) box and a tangential velocity component of 10 in the V (m/s) box Select TI/Length for the Turb. Switch option Enter a Turb. Intensity of 0.1 and a Length of 0.01 m Enter a value of 0.616 in the Dens. (kg/m3) box 15-5

Tutorial 15.1



• • • •

Enter a value of 573 in the Temp. (K) box Click Apply Select Reg# 4 - Outlet and enter a value of 1 in the Flow Split box Click Apply

The default conditions for wall boundaries are adiabatic, no-slip and stationary, which is suitable for this case so no changes are necessary for boundary regions 5 and 6. Analysis Controls

The solution and output controls need to specified next: • • • • • •

Run Time Controls

The aim of this tutorial is to establish a stable, non-reacting flow field which will help to achieve a stable flame and flow field once coal combustion is turned on. Therefore, the solver must perform a sufficiently large number of iterations to reach a converged isothermal flow field. This can be achieved by setting the maximum iteration number to 1000 and the residual error tolerance to 0.001: • • • • • • •

Final Operations

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Type 1000 in the Number of Iterations box Check that the Max. Residual Tolerance is 0.001 Click Apply Open the Analysis (Re)Start panel The setting of the Restart File Option menu should be None as this run starts from the default initial conditions Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, save all model data, write the geometry and problem files and exit from pro-STAR, as shown below. Alternatively, you may continue with the CFD analysis using the STAR GUIde facilities for running STAR interactively. • • • • •

15-6

Open the Analysis Controls > Solution Controls > Equation Behavior > Primary Variables panel In the Solver Parameters tab, check that the Relaxation Factor is 0.3 for Pressure and 0.7 for Momentum and Turbulence Click Apply Select the Output Controls folder and open the Monitor Numerical Behavior panel Turn on Print Iteration Residuals and Conservation Checks Leave all other options at their default values and click Apply


Version 4.02

Tutorial 15.1



CFD Analysis To perform the analysis interactively, proceed as follows: • • • • •

Select File > Save Model In the Analysis Preparation/Running folder open the Run Analysis Interactively panel Check that the units in which the model was built are correctly selected (option button meters) Select Double Precision. Leave all other settings at their default values. Click Start New Analysis

The analysis will then start automatically. Convergence should be achieved within the specified maximum number of iterations. Post-Processing Preliminaries Read in the results of the analysis from file coal_iso.ccm: • • • PostProcessing

Begin by displaying a temperature contour plot to show the mixing of the two inlet streams: • • • • • • • • • • • •

Version 4.02


Go to the Data tab of the Load Data panel Select Cell from the Data Type menu Select On and All for the Smooth Option Select Temperature from the Scalar Data list Click Get Data In the main pro-STAR window, select plot type Contour Plot Select View > Axis > -Z Turn off Bound for the Cell Plot Display Option Click Zoom Off Click Section Slice and draw a horizontal cross-section trace through the centre of the furnace Select View > SNORMAL Select plot type Section (Surface) to display Figure T15.1-2

15-7

Tutorial 15.1


Post-Processing Post- Processing

Figure T15.1-2

Temperature contours through the centre of the furnace

Next, plot velocity vectors on the surface of the furnace to show the swirling nature of the flow: • • • • • • • • • •

Return to the Data tab of the Load Data panel Select Cell from the Data Type menu Turn Off the Smooth Option Select item Velocity Components UVW from the Vector Data list Click Get Data Select Go To > Create Plots In the 3-D Surface tab select Option Vector Select Edge from the Edge/Mesh menu Click Plot to Screen Type VIEW -1.0 0.5 -1.0

•

15-8

in the pro-STAR output window Click Replot to display Figure T15.1-3

Version 4.02

Tutorial 15.1



Figure T15.1-3

Final Operations

Version 4.02

•

Velocity vectors shown on the furnace surface

Exit from pro-STAR by choosing File > Quit > Quit, Nosave from the main window menu.

15-9

Tutorial 15.2

CONSTANT RATE DEVOLATILISATION


Tutorial 15.2


This tutorial gives a detailed account of how to set up and run a coal combustion model. The problem geometry and flow conditions are as described at the beginning of Tutorial 15 and the analysis is run from the non-reacting solution produced in Tutorial 15.1. When running a large-scale simulation, it is generally necessary to employ the Constant Rate devolatilisation model to establish the combustion conditions and a stable flame and flow field. Therefore, the strategy in this case is to use the following sub-models: • • •

Constant rate devolatilisation First-order char oxidisation Eddy break-up two-step gas combustion

The model can then be changed to the Single-Step or 2-Competing-Steps devolatilisation model (as described in Tutorial 15.3) and the analysis continued from the Constant Rate solution. Pre-Processing Preliminaries Before running pro-STAR, create a directory for the tutorial named tut15-2 and copy the model and solution files obtained in Tutorial 15.1 (coal_iso.mdl and coal_iso.ccm) into it. Rename the model file coal_const.mdl. Start up pro-STAR and begin the modelling task by specifying the problem title: • • • • • •

Check that coal_const is shown in the Enter Case Name box Select the Resume From Existing .mdl File? option Deselect the Append to Previous .echo File? option Click Continue Select File > Model Title In the Title text box type COAL COMBUSTION WITH CONSTANT RATE DEVOLATILISATION

•

Click Apply

As part of setting up a coal combustion case, it is necessary to activate the Lagrangian Two-Phase and Coal Combustion models. To do this: • • • •

• • Thermal Options Version 4.02

Open the Select Analysis Features panel in STAR GUIde Select Lagrangian Multi-Phase for the Multi-Phase Treatment option Select Coal Combustion for the Reacting Flow option Click Apply and then click Yes to proceed. Additional folders named Lagrangian Multi-Phase and Thermophysical Models and Properties > Reacting Flow will be created in the STAR GUIde NavCenter tree. Select C > All and then click Cell Plot Click Zoom off to display the mesh

An important element in an accurate coal combustion simulation is radiation modelling. The radiation model in this tutorial includes the effects of the 15-11

Tutorial 15.2


Pre-Processing Radiation Patches

intervening gas, using default gaseous radiation properties, of particle radiation, and of surface-to-surface radiation. In STAR-CD, radiation beams are only tracked through those cells that are explicitly defined as participating in radiative heat transfer. To specify that radiation should be tracked through all cells in the furnace interior: • • • • •

Click CTAB in the main pro-STAR window to open the Cell Table Editor Select Table# 1 in the scroll list Select On from the Radiation menu Click Apply Close the Cell Table Editor

Turn radiation on, choosing the Discrete Transfer solution method in conjunction with the Internal view factor and Participating Media calculation options: • • • • • Radiation Patches

Select the Thermophysical Models and Properties folder and open the Thermal Options panel In the Radiation section of the panel, select option Discrete Transfer Internal VF Calc Select option Participating to include gaseous radiation effects in the calculation Change the Under-Relaxation for Wall Temperature to 1 Accept the remaining default settings and click Apply

To use the Discrete Transfer model, it is necessary to subdivide all boundary regions into radiation patches. These are used both during view factor calculations and for evaluating the radiative heat transfer. Assign a unique patch to every boundary in every relevant region. This can be done most conveniently by means of a pro-STAR command loop, shown below, typed into pro-STAR’s I/O window: BSET NONE *SET NREG 2 1 *DEFINE BPATCH NREG,,BYFA BSET ADD REGI NREG *END *LOOP 1 4 The above loop will create 1,984 patches. Display the patches to confirm that the operation has been carried out properly: •

15-12

In the main pro-STAR window select Patch in Cell Plot Display Options. The radiation patches should appear as shown in Figure T15.2-1.

Version 4.02

Tutorial 15.2


Pre-Processing Other Settings

Figure T15.2-1

Radiation patches on mesh surface

The entire surface of the mesh is coloured, indicating that radiation patches are present everywhere. There is also one radiation patch on each boundary face. • Other Settings

Deselect Patch from the Cell Plot Display Options

It is good practice to define one of the cells near the expected centre of the flame as the monitoring point. This eases the task of checking for the onset of combustion as temperature and product concentrations build up rapidly at that point once combustion begins. Start by inspecting the cell numbers in the region of interest: • • • • • • • • • •

In the main window, select Plot > Numbers... In the Plot Numbers dialog, select Cell and then click Close Click Replot Zoom in on the mesh shown on-screen to have a closer look at the displayed numbers. We will define cell number 5918 as the monitoring cell. Open the Thermophysical Models and Properties > Liquids and Gases > Monitoring and Reference Data panel Type 5918 in the Monitoring cell number box Click Apply Return to the Plot Numbers dialog and deselect Cell Close the Plot Numbers dialog Click Zoom off

Coal The next stage is to define the coal composition: Combustion • Open the Thermophysical Models and Properties > Reacting Flow > Coal Model Set-up Combustion > Coal Composition panel Version 4.02

15-13

Tutorial 15.2


Pre-Processing Coal Combustion Model Set-up

• • • • • • • • • • •

Select the Proximate tab to enter data for the coal’s proximate analysis Enter 34.5% Volatile Matter, 1.4% Moisture, 52.8% Fixed Carbon and 11.3% Ash Click Apply Select the Ultimate tab to enter data for the coal’s ultimate analysis Enter 84.6% C, 5.06% H, 7.6% O and 1.67% N Click Apply Select the Misc. tab Check that a value of 1.5 is displayed in the Q-factor box (see equation (8-3) in Chapter 8 of the CCM User Guide for the Q-factor definition) Enter a Net Calorific Value of 3.444 E+7 J/kg Check that the Fraction of Total N in Volatiles value is set to 1 Click Apply

The combustion models are specified next: • • •

• • • • •

Open the Sub Models panel Check that the Constant Rate Scheme is selected under the Volatiles tab Enter a Devolatilisation Time of 0.01 s and a Devolatilisation Temperature of 353 K. A low temperature is specified to ensure that combustion is initiated successfully. For most cases, the temperature should be increased to a more realistic value once a stable flow field is reached. This is not done in this run but is done for the Two-Competing-Steps case presented in Tutorial 15.3. Click Apply Check that the 1st Order Effect Scheme is selected under the Char tab Leave all options at their default settings and click Apply Select the Eddy-Break Up Scheme and the 2-step Combustion Mechanism under the Gas Comb. tab Click Apply. A warning message will appear telling you that pro-STAR will delete any existing scalars and reaction mechanisms and will create new ones. Click Yes.

The NOx and particle radiation model options and coal particle solution controls are specified next: • •

• • • • • •

15-14

Open the NOx/Radiation panel Check that option NOx Model Off is selected under the NOx tab. If required, the NOx solver can be turned on once the analysis is near convergence and the analysis restarted. This is not done in this run but is done for the Two-Competing-Steps case presented in Tutorial 15.3. Click Apply Select Particle Radiation On under the Radiation tab and enter a Particle Emissivity of 0.8 Click Apply Open the Control/Printout panel Enter a value of 0.1 in the Under-Relaxation Factor for Particle box Enter a very large value, e.g. 10000, in the Iteration Number to Begin Averaging box. This ensures that particle averaging does not occur in the calculation. Particle averaging is no longer recommended for use with Lagrangian multi-phase calculations in STAR-CD. Version 4.02

Tutorial 15.2


Pre-Processing Particle Properties and Injection Location

•

Click Apply

When a coal combustion model is selected, all scalars associated with that model are automatically set up by pro-STAR, the number of scalars depending on the reaction scheme chosen. For the Eddy Break-Up gas combustion scheme with the 2-Step combustion mechanism selected in this tutorial, 11 scalars are created. • • •

Open the Thermophysical Models and Properties > Additional Scalars > Molecular Properties panel Use the Scalar # slider to check that 11 scalars have been defined. There is no need to change any of the molecular properties for these scalars. Click Apply when you are done

Specify that the initial flow field consists entirely of air: • • • • •

Open the Additional Scalars > Initialisation panel Select scalar O2 and enter 0.233 in the Initial Mass Fraction box Click Apply Select scalar N2 and enter 0.767 in the Initial Mass Fraction box Click Apply

Particle The following steps define the particle properties and the injection rate and location: Properties • Select folder Lagrangian Multi-Phase and Injection • Open panel Droplet Controls Location • Check that Use Gradient is selected for the Interpolation Method and that Explicitly defined parcel injection is selected at the bottom of the panel • To increase the maximum allowable number of droplets, type the following commands in the I/O window: MEMO,MAXDRP,2400 MEMO,WRITE • • • • •

Return to the Droplet Controls panel and enter a value of 2400 in the Maximum Number of Parcels box Click Apply Open the Droplet Physical Models and Properties panel Turn On Turbulent Dispersion under the Global Physical Models tab Click Apply

The component properties shown in the Droplet Properties tab are set internally in STAR and should not normally be altered. However, the Heat of Vaporization (Hfg) for each of the seven components should be zero. If any of them do not have this value: • • •

Go back to the Coal Combustion folder and select the NOx/Radiation panel Under the NOx tab, select NOx Model On and click Apply Go back to the Lagrangian Multi-Phase > Droplet Physical Models and Properties > Droplet Properties tab then, in turn (a) Select each of the components listed under Component Properties (b) Enter a value of 0 in the Heat of Vaporisation box

Version 4.02

15-15

Tutorial 15.2


Pre-Processing Particle Properties and Injection Location

(c) Click Edit Component (d) After you have done this for every component, click Apply at the bottom of the panel • • •

Change the Density to 1200 kg/m3 under the Droplet Properties tab Click Apply Go back to the NOx tab, select NOx Model Off and click Apply

Next, specify the coal particle injector locations and injection rate: • • • • • • • • • • • • • •

• •

Select the Injection Definition panel Check that the Injection Group # slider at the bottom of the panel is set to 1 Enter a value of 1e-4 m in the Diameter box and a value of 10 m/s in the Velocity Magnitude box Enter a value of 353 K in the Temperature box Check that the Mass Flowrate applies to the Injection Group Enter a value of 0.1 kg/s in the Mass Flowrate box Enter a value of 300 in the No. of Parcels/injection point box Click Apply Open the Injection Points panel Select Set Type Circle Select Specify for the Circle option Check that the Cylindrical Coordinate System value is 2 Define a Circle of Radius 0.02 at Z = -0.19 For the Number of Points, type 1 for R (number of rows) and 8 for Theta. This will produce a circle of 8 injection points with a radius of 0.02 near to the primary inlet. Check that Constant is selected for the Entrance Dir. Vector and type 1 in the DZ box (DX=0, DY=0, DZ=1) Click Add New Set at the bottom of the panel

To display the particle injection locations: • • • • • • • •

15-16

Select the Post-Processing > Particle Tracks > Plot Droplets/Particle Tracks panel Under the Droplets tab and in the Load Droplet Data section, select Droplet Initial Conditions for the Load From option Click Load Data Change the Droplet Radius Size to 0.01 in the Droplet Plot Options section Click Apply In the Collect/Plot section, choose Dp > All Click Droplet Plot Zoom in on the injection points to display Figure T15.2-2

Version 4.02

Tutorial 15.2



Figure T15.2-2

Boundary Conditions

Many of the boundary conditions for inlet, outlet and wall boundaries have already been set in Tutorial 15.1. However, thermal and radiation boundary conditions still need to be specified: • • • • • • • • • • • • • • • • • • • • •

Version 4.02

Particle injection positions

In the STAR GUIde window, select folder Define Boundary Conditions and open the Define Boundary Regions panel Select Reg# 1- Inlet from the list Enter 353 in the T Radiation (K) box Enter a value of 1 in the Emissivity box Click Apply Select Reg# 2 - Inlet from the list Enter 353 in the T Radiation (K) box Enter a value of 1 in the Emissivity box Click Apply Select Reg# 3 - Inlet from the list Enter 573 in the T Radiation (K) box Enter a value of 1 in the Emissivity box Click Apply Select Reg# 4 - Outlet Enter 1000 in the T Radiation (K) box Enter a value of 1 in the Emissivity box Click Apply Select Reg# 5 - Wall Change the Wall Heat option to Fixed and enter a value of 400 in the Temp. (K) box Enter a value of 0.3663 for Resistivity Set the Emissivity to 0.72 and the Ther. Reflectivity to 0.28 15-17

Tutorial 15.2


Pre-Processing Scalar Boundaries

• • • • • • Scalar Boundaries

Specify that only air enters through the inlet boundaries: • • • • • • • •

Control Parameters

• •

• • • • • •

Open the panel Analysis Controls > Other Controls > Switches and Real Constants Select the Real Constants tab Check that a large value, e.g. 10000 appears in the C24 box. This high value prevents particle averaging taking place, as discussed in the “Coal Combustion Model Set-up” section Enter 2 in the C64 box. This constrains the scalar concentrations to values between 0 and 1. Check that a value of 0.8 is shown in the C82 box. This is the particle emissivity value. Enter 3000 in the C88 box. This is the maximum allowable particle temperature. Enter 283 in the C89 box. This is the minimum allowable gas temperature. Enter 3000 in the C90 box. This is the maximum allowable gas temperature. Click Apply at the bottom of the panel

Check the status of the run time control parameters and specify that the analysis should restart from the solution obtained in Tutorial 15.1: •

15-18

Open the Scalar Boundaries panel Select Reg# 1- Inlet from the Boundary Regions list Select O2 from the Scalar list Enter a value of 0.233 in the Mass Fraction box Click Apply Select N2 from the Scalar list and enter a value of 0.767 in the Mass Fraction box Click Apply Specify exactly the same scalar boundary conditions for Reg# 2 - Inlet and Reg# 3 - Inlet

Default values for analysis controls such as under-relaxation factors and differencing schemes are set when the models are selected. Although these defaults are suitable for this tutorial, the under-relaxation factors for other cases may need changing or a second-order differencing scheme may be required. To run a case involving coal combustion, it is also necessary to set some pro-STAR Constants that help control the analysis: •

Run Time Controls

Click Apply Select Reg# 6 - Wall Change the Wall Heat option to Fixed and enter a value of 400 in the Temp. (K) box Enter a value of 0.02 for Resistivity Set the Emissivity to 0.72 and the Ther. Reflectivity to 0.28 Click Apply

Select folder Analysis Preparation/Running and open the Set Run Time Controls panel Version 4.02

Tutorial 15.2



• • • • • • Final Operations

Change the Number of Iterations to 500 and check that the Max. Residual Tolerance is set to 0.001 Click Apply Open the Analysis (Re) Start panel Select Initial Field Restart for the Restart File Option Enter coal_iso.ccm as the Restart File Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, write the geometry and problem files and exit, saving all model data in file coal_const.mdl, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • • • •

In the main window, choose File > Write Geometry File In the Geometry File Write dialog, click Apply and then Close File > Write Problem File In the Problem File Write dialog, click Apply Ignore the warning shown in the I/O window. No ignition model is required. Close the Problem File Write dialog File > Quit > Save & Quit

CFD Analysis To perform the analysis interactively proceed as follows: • • • • •

Select File > Save Model Select the Analysis Preparation/Running folder and open the Run Analysis Interactively panel Select option Double Precision in the Star Executable Precision section Select the Write New Geometry File option Click Restart Analysis

As well as the usual residual and monitoring data, the screen output will show information about the coal combustion reaction at every iteration. Note that the analysis will take some time to run (over 1 hour on a 2.8 GHz Linux machine with 2 GB of RAM) and that the run time cannot be decreased by running in parallel since cases involving the discrete transfer radiation method with participating media cannot be run in this mode. The run should converge within the specified maximum number of iterations. Post-Processing Preliminaries Enter pro-STAR and start the post-processing task by re-plotting the mesh:. • • • • • Version 4.02

In the main window, select C > New > Fluid Click Cell Plot In STAR GUIde, select folder Post-Processing Open the Load Data panel and display the File(s) tab Click Open Post File 15-19

Tutorial 15.2



First, check the solution obtained by inspecting the velocity plot: • • • • • • • •

Go to the Data tab and check that Data Type Cell is selected In the Vector Data list, select item Velocity Component UVW In the Scalar Data list, check that the setting is None Click Get Data Select Go To > Create Plots to open the Create Plots panel Go to the 3-D Surface tab and choose Vector from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen Type: VIEW -1.0 0.5 -1.0

•

in the pro-STAR I/O window Click Zoom Off to display Figure T15.2-3

Figure T15.2-3

Velocity vectors inside the furnace

Next, plot the absolute temperatures on a section through the centre of the furnace and normal to the Y axis: • • • • • • 15-20

Go to the Data tab of the Load Data panel and check that Data Type Cell is selected Choose On and All for the Smooth Option In the Scalar Data list, select item Temperature Click Get Data Select Go To > Create Plots and choose Contour (filled) from the Option menu in the 3-D Surface tab Click Plot to Screen Version 4.02

Tutorial 15.2



• • • • •

Select View > Axis > -Z in the main pro-STAR window Select Section Slice, then use the cursor to draw a section trace through the centre of the furnace and parallel to the X axis Select plot type Section (Surface) Select View > SNORMAL Click Zoom off to display Figure T15.2-4

Figure T15.2-4

Temperature contours on a section bisecting the grid

Next, plot the CO2 mass fraction contours on the same section through the centre of the furnace: • • •

Version 4.02

Go to the Data tab and select item CO2 from the Scalar Data list Click Get Data Click Replot to display Figure T15.2-5

15-21

Tutorial 15.2



Figure T15.2-5

CO2 contours on a section bisecting the grid

Plot the steady-state coal particle distribution, specifying that the displayed particle colour and radius is to depend on temperature and calculated diameter, respectively. Also choose not to display particle velocity vectors: •

Type VIEW -1.0 0.5 -1.0

• • • • • • • • • • • •

15-22

in the pro-STAR I/O window In STAR GUIde, select folder Post-Processing followed by sub-folder Particle Tracks Open panel Plot Droplets/Particle Tracks and then select the Droplets tab In the Load Droplet Data section, select option Track File from the Load From menu Check that file coal_const.trk is shown in the File Name box Accept the default option (Particles) for the Plot Option menu and then click Load Data In the Droplet Plot Options section, select After, Unhidden and Cplot from the Edge Plot Options menus Select Diameter in the Droplet Radius menu and enter 1 and 0.001 in the Size and Ref. Value boxes, respectively Select Temperature in the Fill Colour menu Select None in the Vectors menu Click Apply In the main pro-STAR window, select D > All Click Droplet Plot at the bottom of the Droplets tab to display Figure T15.2-6

Version 4.02

Tutorial 15.2



Figure T15.2-6

Coal particles coloured by temperature

Now make the droplet colour dependent on droplet mass and replot: • • •

In the Droplet Plot Options section, select Mass from the Fill Color menu Click Apply Click Replot to display Figure T15.2-7

Figure T15.2-7 Version 4.02

Coal particles coloured by mass 15-23

Tutorial 15.2



Figure T15.2-6 and Figure T15.2-7 show that the coal particles have essentially burnt out well before reaching the furnace outlet. This burn-out accounts for all the char and volatiles in the fuel. By default, STAR stops coal particle tracking once more than 99.9% of char has been burnt out. By setting Constant 116 to 1 you can continue tracking the remaining (ash) particles through the rest of the solution domain but at the expense of additional computation time. Remember that all results presented in this tutorial were generated with the devolatilisation temperature set at the unrealistically low value of 353 K. In Tutorial 15.3, the devolatilisation temperature is raised to 550 K and the Two-Competing-Steps devolatilisation model is used instead of the Constant Rate model. NOx modelling is also turned on and the analysis is restarted from the solution obtained in this tutorial. Final Operations

15-24

•

Exit from pro-STAR by choosing File > Quit > Quit, Nosave from the main window menu

Version 4.02

Tutorial 15.3

TWO-COMPETING-STEPS DEVOLATILISATION


Tutorial 15.3


This tutorial gives a detailed account on how to set up and run a coal combustion model using the Two-Competing-Steps devolatilisation model. It should also be instructive to users wishing to employ the Single-Step devolatilisation model as the required set-up is very similar. The Two-Competing-Steps model is based on a pair of competing first-order reactions occurring uniformly throughout the particle. The rates of these reactions are calculated as described in Chapter 10, “Two-competing-steps model” of the Methodology volume. The modelling strategy in this tutorial is to use the following sub-models: • • •

Two-competing-steps devolatilisation First-order char oxidisation Eddy break-up two-step gas combustion

NOx modelling is also activated. The analysis restarts from the Constant Rate devolatilisation case set up in Tutorial 15.2, the problem geometry for which is shown in Tutorial 15. As a result, this tutorial only requires a brief specification of the options for the Two-Competing-Steps devolatilisation and NOx generation models. Pre-Processing Preliminaries Before running pro-STAR, create a directory for the tutorial named tut15-3 and copy the model and solution file obtained in Tutorial 15.2 (coal_const.mdl and coal_const.ccm) into it. Rename the model file coal_2step.mdl. Start up pro-STAR and begin the modelling task by specifying the problem title: • • • • • •

Check that coal_2step is shown in the Enter Case Name box Select the Resume From Existing .mdl File? option Deselect the Append to Previous .echo File? option Click Continue Select File > Model Title In the Title text box type COAL COMBUSTION WITH TWO-COMPETING-STEPS DEVOLATILISATION

• Coal Combustion Model Setup

Click Apply

The next stage is to change the devolatilisation model to the Two-Competing-Steps model: • • •

Open the Thermophysical Models and Properties > Reacting Flow > Coal Combustion > Sub Models sub-folder Select the Volatiles tab Select the 2 Competing Scheme

In the 1-Step section: • Version 4.02

Enter a value of 2.0e+05 in the Pre-exponential Factor box 15-25

Tutorial 15.3



• •

Enter a value of 1.047e+08 in the Activation Energy box Change the Mass Stoichiometric Coefficient to 0.3

In the 2-Step section: • • •

Enter a value of 1.3e+07 in the Pre-exponential Factor box Enter a value of 1.67e+08 in the Activation Energy box Check that the Mass Stoichiometric Coefficient is set to 0.7

To complete the model specification: • •

Enter a value of 550 K in the Devolatilisation Temperature box Click Apply

Now activate NOx modelling: • • • •


Open the Thermophysical Models and Properties > Reacting Flow > Chemical Reactions > Emission panel Turn On the NOx Model. Note that this has the same effect as turning on NOx modelling in the Coal Combustion > NOx/Radiation panel Turn On the Fuel NOx and Prompt NOx options Change the Tuchin setting to 10. This is the number of integration steps used to generate the beta function PDF and so increasing it will lead to a more accurate solution. Click Apply

To aid convergence, the under-relaxation factor for the energy equation will be reduced: • • • •

Open the Analysis Controls > Solution Controls > Equation Behavior > Primary Variables panel Select the Solver Parameters tab Change the Relaxation Factor for Temp. to 0.5 Click Apply

The under-relaxation factors for all active scalars should have changed automatically when the temperature factor was changed, ensuring that the scalar and energy equation solutions remain in synchronisation. To check that this has happened: • • • Run-time Controls

Check the status of the run-time control parameters and specify that the analysis should restart from the solution obtained in Tutorial 15.2: • •

15-26

Open the Additional Scalars panel Select scalars 1 - 8 from the list and check that their Under Relaxation Factors are 0.5 Click Apply

Select folder Analysis Preparation/Running and open the Analysis (Re) Start panel Change the Restart File Option to Standard Restart. This can be used because this analysis solves the same variables as the one for Tutorial 15.2. Version 4.02

Tutorial 15.3



• • Final Operations

Enter coal_const.ccm as the Restart File Click Apply

The pre-processing task is now complete. If you wish to terminate the session at this stage, write the geometry and problem files and exit, saving all model data in file coal_2step.mdl, as shown below. Alternatively, you may run STAR interactively, as described in the next section. • • • • • • •

In the main window, choose File > Write Geometry File In the Geometry File Write dialog, click Apply and then Close File > Write Problem File In the Problem File Write dialog, click Apply Ignore the warning shown in the I/O window. No ignition model is required. Close the Problem File Write dialog File > Quit > Save & Quit

CFD Analysis To perform the analysis interactively proceed as follows: • • • • •

Select File > Save Model Select the Analysis Preparation/Running folder and open the Run Analysis Interactively panel Select option Double Precision in the Star Executable Precision section Select the Write New Geometry File option Click Restart Analysis

As well as the usual residual and monitoring data, the screen output will show information about the coal combustion reaction at every iteration. Note that the analysis will take some time to run (over 1 hour on a 2.8 GHz Linux machine with 2 GB of RAM) and that the run time cannot be decreased by running in parallel since cases involving the discrete transfer radiation method with participating media cannot be run in this mode. The run will not converge within the specified maximum number of iterations. However, the only residual that fails to fall below the convergence criterion is that for HCN (scalar number 10). The very low values of the HCN scalar (less than 0.01 throughout the domain) mean that lack of convergence is not a concern for this tutorial. Post-Processing Preliminaries Enter pro-STAR and start the post-processing task by re-plotting the mesh: • • • • •

In the main window, select C > New > Fluid Click Cell Plot In STAR GUIde, select folder Post-Processing Open the Load Data panel and display the File(s) tab Click Open Post File

First, plot the absolute temperatures on a section through the centre of the furnace Version 4.02

15-27

Tutorial 15.3



and normal to the Y axis: • • • • • • • • • • •

Go to the Data tab of the Load Data panel and check that Data Type Cell is selected Choose On and All for the Smooth Option In the Scalar Data list, select item Temperature Click Get Data Select Go To > Create Plots and choose Contour (filled) from the Option menu in the 3-D Surface tab Click Plot to Screen Select View > Axis > -Z in the main pro-STAR window Click Zoom Off to display the whole mesh Select Section Slice, then use the cursor to draw a section trace through the centre of the furnace and parallel to the X axis Select plot type Section (Surface) Select View > SNORMAL to display Figure T15.3-1

Figure T15.3-1

Temperature contours on a section bisecting the grid

Next, plot the O2 mass fraction contours on the same section through the centre of the furnace: • • •

15-28

Go to the Data tab and select item O2 from the Scalar Data list Click Get Data Click Replot to display Figure T15.3-2

Version 4.02

Tutorial 15.3



Figure T15.3-2

O2 contours on a section bisecting the grid

Next, plot the NO mass fraction contours on the same section through the centre of the furnace: • • •

Version 4.02

Go to the Data tab and select item NO from the Scalar Data list Click Get Data Click Replot to display Figure T15.3-3

15-29

Tutorial 15.3



Figure T15.3-3

NO contours on a section bisecting the grid

Plot the steady-state coal particle distribution, specifying that the displayed particle colour and radius is to depend on temperature and calculated diameter, respectively. Also choose not to display particle velocity vectors: •

Type VIEW -1.0 0.5 -1.0

• • • • • • • • • • • •

15-30

in the pro-STAR I/O window In STAR GUIde, select folder Post-Processing followed by sub-folder Particle Tracks Open panel Plot Droplets/Particle Tracks and then select the Droplets tab In the Load Droplet Data section, select option Track File from the Load From menu Check that file coal_2step.trk is shown in the File Name box Accept the default option (Particles) for the Plot Option menu and then click Load Data In the Droplet Plot Options section, select After, Unhidden and Cplot from the Edge Plot Options menus Select Diameter in the Droplet Radius menu and enter 1 and 0.001 in the Size and Ref. Value boxes, respectively Select Temperature in the Fill Colour menu Select None in the Vectors menu Click Apply In the main pro-STAR window, select D > All Click Droplet Plot at the bottom of the Droplets tab to display Figure T15.3-4

Version 4.02

Tutorial 15.3



Figure T15.3-4

Coal particles coloured by temperature

Note that there are significant differences between the results shown above and those in Tutorial 15.2. These changes are partly due to the change in devolatilisation model and the introduction of NOx modelling. However, the greatest change is due to increasing the devolatilisation temperature to a more realistic value. The last plot created in this tutorial combines a contour plot of CO2 concentration with a plot showing the coal particles using the OVERLAY utility. • • • • • • • •

Return to the Data tab of the Load Data panel and select item CO2 from the Scalar Data list Click Get Data Select Go To > Create Plots Under the Section Clipped tab, select Contour (filled) and Edge Change the Normal vector to (1, 0, 0) Click Apply Click Cell Plot to display the CO2 contours Type VIEW -1.0 0.3 -0.7

• • • • • • • Version 4.02

in the pro-STAR I/O window Turn on edge plotting by selecting the Edge button Click Replot Use the mouse to zoom out slightly so that the edges of the problem geometry fit in the display window Return to the Droplets tab of the Plot Droplets/Particle Tracks panel Turn Off the Edge Plot Options In the Droplet Plot Options section, change the Droplet Radius Size to 0.005 Change the Fill Color option to Color and choose Color 1 15-31

Tutorial 15.3



• • •

Click Apply In the main pro-STAR window, select Plot > Display > Overlay Click Droplet Plot in the Droplets tab of the Plot Droplets/Particle Tracks panel to display Figure T15.3-5

Figure T15.3-5

Final Operations

15-32

•

Coal particles displayed over CO2 contours

Finally, exit from pro-STAR by choosing File > Quit > Quit, Nosave from the main window.

Version 4.02


Tutorial 16 LARGE EDDY SIMULATION OF FULLY-DEVELOPED CHANNEL FLOW Physical Problem Description This tutorial presents an example of applying the Large Eddy Simulation turbulence model to a fully-developed, isothermal, incompressible channel flow. A 2-D cross section through the problem geometry is shown in Figure T16.0-1, illustrating the primary direction of flow. The dimensions for the channel are taken from the work of Moser et al. [1] and correspond to a length, width and height of 2π m, π m and 2 m, respectively.

Channel Walls

2

y 2π x Figure T16.0-1

2-D cross section through the channel

The problem geometry represents a section of the channel and therefore cyclic boundary conditions are applied in both the streamwise (x-) and spanwise (z-) directions. Calculations are carried out at standard pressure and temperature (1 bar, 293K) for a Reynolds number (Reτ) of 395. The latter is based on the friction velocity, uτ , and half-channel height and is given by ρu Re τ = ---------τ µ where uτ =

τw ----ρ

and τ w is the wall shear stress. The fluid is assumed to have constant physical properties, as shown below: Density Molecular viscosity

1.0 kgm-3 1.0/Reτ Pa-s

These numbers have been chosen so as to give a value of uτ = 1.0 ms-1. The flow in the channel is driven by an imposed pressure gradient whose value Version 4.02

16-1

Modelling Strategy

is determined by balancing the pressure force in the streamwise direction with the shear force at the top and bottom walls of the channel, yielding ∆ pH = 2τ w L The wall shear stress is obtained from the friction velocity definition and has a value of 1.0 Nm-1. This is then combined with the channel height and length to give a pressure drop along the channel of 2π Pa. Modelling Strategy The major elements of the modelling strategy are: •

• •

Computational grid — non-uniform hexahedral mesh comprising 90,000 cells (see Figure T16.0-2). Cells in the y-direction are refined so as to yield a higher resolution near the channel walls. This is achieved using an expansion ratio of 1.1096 Wall and cyclic boundary conditions Isothermal, incompressible, steady and transient flow options

The tutorial is divided into two parts. The first, a steady-state Reynolds Averaged Navier-Stokes (RANS) simulation, is used to verify the mesh suitability for capturing the large-eddy turbulence structures as measured by the integral length scale, l = f(k/ε). The second part illustrates the recommended numerical settings for LES, including pre- and post-processing, and includes comparison of results with those obtained from a direct numerical simulation (DNS) [2].

Figure T16.0-2

16-2

The computational mesh.

Version 4.02

Tutorial 16.1

STEADY-STATE ANALYSIS

Pre-processing Preliminaries

Tutorial 16.1


To obtain accurate results using LES it is essential that: • •

The computational mesh is sufficiently refined in key areas to resolve the mean flow and large-eddy turbulence structures present The time step for the analysis is small enough to capture the cascade of energy over a wide spectrum, down towards the dissipative scales

These assessments can be made by examining the integral length and time scales for the problem. This tutorial shows how to obtain these quantities from a steady-state analysis using a Low Reynolds number k-ε turbulence model. The mesh provided in this case is much coarser in the streamwise direction than the full 90,000 cell mesh used in Tutorial 16.2, having only 9,000 cells. This is a reasonable simplification as the steady-state result should have no streamwise velocity gradient. The LES case will, of course, exhibit such a gradient and hence mesh refinement in the streamwise direction is also necessary. Pre-processing Preliminaries For convenience, the problem set-up for this tutorial is performed by executing a command macro, given in full in a separate section (“Macro”). The macro is supplied in a file called RANS.MAC which contains instructions for mesh set-up, boundary conditions, fluid properties and solution control settings. Create a directory for this tutorial named tut16-1 and ensure that the above macro file has been copied into it. Start pro-STAR, enter the tutorial name and make the appropriate choices for an initial run: • • • • • • Problem set-up

Type prostar at the command line Specify the graphics driver (xm, mesa or glm) Type channel_ss in the Enter Case Name text box Check that the Resume from Existing .mdl File? option is deselected Check that the Append to Previous .echo File? option is deselected Click Continue

Execute the command macro and save the model file: • • •

Open the macro panel by selecting Panels > Define Macro in the main pro-STAR window Highlight RANS in the macro panel and click Execute Save the model and exit from pro-STAR by selecting File > Quit > Save & Quit from the pro-STAR menu

CFD Analysis If your machine has more than one processor, performing this analysis in parallel can be very beneficial. Running on two CPUs instead of one, for example, should roughly halve the run time. To run the analysis in parallel, on two local CPUs and in double precision, type: star -dp 2 Version 4.02

16-3

Tutorial 16.1


Post-Processing Problem set-up

For a description of how to run problems in parallel across a network, see “Running a STAR-CD Analysis” on page 2-2 of the CCM User Guide. If your machine has only one processor, you will need to run sequentially. To perform this type of run in double-precision mode, type: star -dp The convergence criteria for this case are very strict and so the run will not converge within the specified 3,000 iterations. The reason for running the analysis for this number of iterations will be explained in the “Post-Processing” section. Post-Processing The nature of this problem makes the normalised residual sums a poor method for judging convergence. Instead, the justification for stopping the run after 3,000 iterations can be provided by examining the monitor history data: • • • •

Start up pro-STAR and resume from the channel_ss.mdl model file Select the Analysis Preparation/Running folder in STAR GUIde Open the Run History of Previous Analysis panel Check the U-Component box and click Plot Monitor History to display Figure T16.1-1

Figure T16.1-1

Monitor history plot of the U-component of velocity

Figure T16.1-1 shows that the U-velocity at the monitoring point has converged to a steady value. The results will now be analysed to yield information about the integral length (l) and time (t) scales, defined as:

16-4

Version 4.02

Tutorial 16.1



0.75 1.5

Cµ k k l = -----------------------, t = -ε ε Read in the analysis results file by typing the following command in the pro-STAR I/O window: LOAD channel_ss.ccm The next step is to load the relevant data into the post registers and perform the appropriate calculations. For the integral length scale l , this is achieved by typing the following commands: oper oper oper oper oper

getc getc v**s smul divi

te 5 ed 6 1.5 5 5 0.1643 5 5 5 6 4

Since we are trying to establish whether or not the mesh resolution in the wall-normal direction (y-axis) is adequate for LES, it is useful to display the ratio l/∆y (∆y being the cell height) for which a value greater than 1 should be observed. Since all cells in the grid have the same ∆x and ∆z, we can calculate ∆y from the cell volume by V ∆y = -----------------∆x ⋅ ∆z which, for this mesh, means ∆y = 7.6V Therefore, the ratio l/∆y is found by entering the following commands: oper getc volu 5 oper smul 7.6 5 5 oper divi 4 5 4 Now display the data as a contour plot: • • • •

In STAR GUIde, select the Post-Processing folder and open the Create Plots panel Under the 3-D Surface tab, select Contour (filled) from the Option dropdown menu and Edge from the Edge/Mesh drop-down menu Click Plot To Screen Select View > Axis > +Z in the main pro-STAR window to display Figure T16.1-2

The resulting plot shows that, except in the cells immediately adjacent to the wall, the ratio l/∆y is greater than 1.0. This confirms that the resolution of the mesh is sufficient for use in LES, although there may be some inaccuracy close to the wall.

Version 4.02

16-5

Tutorial 16.1



Figure T16.1-2

Contour plot showing the ratio l/∆y

It is also useful to check whether the cells adjacent to the wall are fine enough to satisfy the criterion that y+ should be ~1. To find out the ∆y for the near-wall cells, enter the following command: summ cset The information given in the output window includes the minimum value in post register 5, which contains the ∆y values. The minimum value is 5.0639x10-3 m, which corresponds to a y+ of ~2 according to the following equation: ρu τ ∆ y y + = --------------µ The integral time scale is calculated and displayed by entering the following commands: oper getc te 5 oper getc ed 6 oper divi 5 6 4 repl The resulting plot is shown in Figure T16.1-3.

16-6

Version 4.02

Tutorial 16.1



Figure T16.1-3

Contour plot of the integral time scale t

Figure T16.1-3 shows that the integral time scale, t, decreases from 1.21 s in the centre of the channel to 1.28x10-3 s near the wall. It is also possible to determine time scales associated with the turbulent eddies. Based on the cell sizes in the y- and z-directions, and fluctuating velocities determined from the turbulent kinetic energy predicted by the RANS analysis, time scales of 6.36x10-3 s (y-direction) and 0.0438 s (z-direction) are obtained. The chosen time step for an LES run should thus be sufficiently small to capture the turbulence structures in the vicinity of the wall i.e. < 1.28x10-3 s, whilst satisfying the numerical scheme’s stability criterion. To obtain a time step that satisfies the latter, the Courant number (Co) definition is rearranged to yield: Co ∆x ∆t = ------------U The quantities U and ∆x denote characteristic velocity and length scale, respectively. For LES it is recommended that the value of Co should not exceed 0.3. Using the channel dimensions and streamwise velocity shown in Table 1, a time step value of 3.2x10-3 s is obtained.

Version 4.02

16-7

Tutorial 16.1


Macro Problem set-up

Table 1: Parameters used to obtain time step for numerical stability Parameter Value Channel length (m) 2π Number of cells in streamwise direction 30a ∆x (m) 0.20944 -1 U (ms ) 19.61 a.This number relates to the refined mesh used for the LES case

A time step of 1x10-3 s is used in the LES tutorial (Tutorial 16.2), satisfying both criteria mentioned above. Having completed the calculations for mesh suitability and choice of time step, exit pro-STAR as follows: •


Macro !=============================================== ! Macro 16.1-1: Setting up the RANS analysis !=============================================== ! User-defined parameters: ! H - half-height of channel ! RETAU - Friction Reynolds number (Utau*H/nu) ! YPLS - Target y+ in near-wall cell ! COUR - Target Courant number ! NCX - Number of cells in streamwise direction ! NCY - Number of cells in normal direction ! NCZ - Number of cells in spanwise direction !=============================================== *set H 1.0 *set RETAU 395.0 *set YPLS 1.0 *set COUR 1.0 *set NCX 3.0 *set NCY 60.0 *set NCZ 50.0 !=============================================== ! Generate Mesh *set PI 3.141592654 *set LX 2.0 * H * PI *set LY 2.0 * H *set LZ H * PI ! Generate a uniform mesh vc3d 0.0 LX NCX -0.5 * LY 0.5 * LY NCY -0.5 * LZ 0.5 * LZ NCZ ! Define the ! directions *set NVX NCX *set NVY NCY *set NVZ NCZ

number of vertices in each of the coordinate + 1 + 1 + 1

! Iterate for the expansion factor. Based on a geometric ! progression with the initial cell height estimated from a balance 16-8

Version 4.02

Tutorial 16.1



! between the definition of y+ and the Reynolds number based on the ! wall shear velocity. Perform an iterative calculation to ! determine the expansion factor. *set Q RETAU / 2.0 / YPLS *set G 2.0 / NCY *set R 1.01 *def noex *set F R - 1.0 * Q + 1 *set R F ** G *end *loo 1 100 !============================================================ ! Locate boundaries. cset news flui plty ehid cplo view -1 0 0 bzon 1 all rdef 1 cycl$ $ $ $ $ view 1 0 0 bzon 2 all rdef 2 cycl$ $ $ $ $ view 0 0 -1 bzon 3 all rdef 3 cycl$ $ $ $ $ view 0 0 1 bzon 4 all rdef 4 cycl$ $ $ $ $ cyma 1 2 LX 0.0 0.0 cyma 3 4 0.0 0.0 LZ ! Make mesh non-uniform to achieve desired y+. vfil 1 NVY NVY - 2 2 1 NVX * NVZ NVY -1.0 * R !============================================================ ! Define common control parameters time steady nodefa iter 3000,1e-10 moni 8911 algo simple nodefa,,, solu scalar CG !============================================================ ! Define properties and models pmat 1 flui dens cons 1.0 lvis cons 1.0 / RETAU turb ke 1 stan lowre on coke,0.09,1.44,1.92,1.44,-0.33,0.419,1,1.219,0.9 nwall hybrid twol off init stan 21 0.0 0.0 1 0.0 0.0,keps,0.4,0.01 !============================================================ Version 4.02

16-9

Tutorial 16.1



! Define boundaries at either end in the streamwise direction as ! cyclic with a prescribed pressure drop across them. ! Define boundaries at either end in the spanwise direction as ! regular cyclic. rdef 0 wall stan nosl stan 9.0 0.0 0.0 0.0 1 0.0 rdef 1 cycl stan 1 part regu inte pdro LX / H / H / H rdef 2 cycl stan 1 part regu inte pdro -1.0 * LX / H / H / H rdef 3 cycl stan 1 all regu inte rdef 4 cycl stan 1 all regu inte !============================================================ ! Additional control parameters solve,y,y,y,y,y,y,n,y,n,n,n,n, relax,0.7,0.3,0.7, ,1, , , , , , , , , sweep,100,100,100,1000,100,100, , , , , , , , , , , , resid,0.1,0.1,0.1,0.05,0.1,0.1, , , , , , , , , , , , dsch,ud,uvw,,stan prch ,,, conv ! Write geometry file, problem file and save geom,, prob,, save,,

16-10

Version 4.02

Tutorial 16.2

LARGE EDDY SIMULATION


Tutorial 16.2


This tutorial illustrates the steps required to set up and perform a Large Eddy Simulation for channel flow. The focus will be on the specifics related to LES and thus the model set-up of Tutorial 16.1 will be used as the starting point. Pre-Processing Preliminaries The following files are required for this tutorial: • • • • • • •

REFINE.MAC DATA_AVERAGING.MAC MEAN_U.MAC REY_STRESS.MAC chan395.means chan395.reystress channel_demo.ccm

Create a directory called tut16-2 and ensure that the above files are copied into it. In addition, copy the model file channel_ss.mdl from Tutorial 16.1 to the new directory and rename it channel_les.mdl. Once all the files are in place, you may start a pro-STAR session: • • • • • • Mesh refinement

To refine the mesh in the streamwise direction to make it suitable for the LES calculation: • • • •

LES settings

Type prostar at the command line Specify the graphics driver (xm, mesa or glm) Check that channel_les appears in the Enter Case Name text box Check that the Resume from Existing .mdl File? option is selected Deselect the Append to Previous .echo File? option Click Continue

Select Panels > Define Macro from the main menu in pro-STAR Highlight REFINE in the Define Macro panel Click Execute Select View > Isometric > -1,1,1 to display the mesh shown in Figure T16.0-2

The calculation is no longer steady-state and so it is necessary change the analysis type: • •

Click Select Analysis Features and select Transient from the Time Domain menu Click Apply

Next, change the turbulence model and set the appropriate parameters, including the point at which statistical averaging will begin. The current simulation will be run for a total of 50 s, equivalent to approximately 160 passes through the domain. The flow is allowed to develop in the initial 25 s (25,000 time steps), after which the statistical averaging of flow variables will begin. Version 4.02

16-11

Tutorial 16.2


Pre-Processing Flow initialisation

• • • • • • •

Flow initialisation

Select folder Thermophysical Models and Properties Select sub-folder Liquids and Gases Open panel Turbulence Models Select the LES/Smagorinsky model from the pull-down menu Check that option Provide statistically av. values is selected and then type 25000 in the Time Step box Set the model constants to match those shown below Click Apply

In order to reduce the run time, the simulation can start from a flow field that will encourage the development of turbulence. The appropriate initial conditions may be specified through user subroutine INITFI as follows: • • •

Open the Initialization panel Select User from the Options menu Enter the following commands: SYSTEM UFILES

• • •

Click Define user coding in the Initialization panel Click Apply Use pro-STAR’s built-in text editor or an external editor to change the contents of the default initfi.f file (written by pro-STAR into the ufile sub-directory) to match the subroutine listing given in section “User Subroutine”

The effect of the user-defined initial flow field is to introduce vorticity into the domain. This is achieved by defining a region in the centre of the channel in which all three velocity components are set explicitly. In particular, the wall-normal component is set to a value greater than the streamwise component to encourage the development of turbulence. Solution controls

To obtain the best results from an LES model, the use of second-order schemes is recommended for both the temporal and spatial discretization. When using the SIMPLE solution algorithm, the residual tolerance for the outer iterations and the maximum number of outer iterations for each time step need to be set so that convergence is achieved at every time step. This can be judged by examining the residual and monitor information output during the run. • • •

16-12

Select the Analysis Controls folder Select the Solution Controls sub-folder Open the Solution Method panel Version 4.02

Tutorial 16.2


Pre-Processing Final operations

• •

• •

Change the Solution Algorithm to SIMPLE Change the Max. No. of Outer Iterations to 3. This may not be large enough for the algorithm to achieve convergence at every time step but should be sufficient for obtaining a good-quality overall solution. Select the Three Time Level Implicit scheme from the Temporal Discretization drop-down menu Click Apply

Next, change the solver parameters and change the spatial discretization scheme for the momentum equations to CD, ensuring that the blending factor is set to 1.0: • • • • • • • • • •

Select the Equation Behavior sub-folder Open the Primary Variables panel Select the Solver Parameters tab Change the Relaxation Factor for the U-Mom, V-Mom, W-Mom equations to 0.9 and the Number of Sweeps to 200 Change the Residual Tolerance to 0.001 for the three momentum equations For Pressure, change the Relaxation Factor to 0.5 and the Residual Tolerance to 0.0001 Click Apply Select the Differencing Schemes tab Select the CD scheme from the drop-down menu for the Differencing Scheme of the momentum equations and check that the blending factor is set to 1.0 Click Apply

Velocity data for a cell near the wall will be monitored throughout the run. The data will then be used to check whether the statistical averaging specified in the “LES settings” section starts after allowing a reasonable time for the flow to develop. •

Select the desired cell by typing the following command in pro-STAR’s I/O window: CSET NEWSET CLIST 89105

• • • • • • • • • • Final operations

Version 4.02

Select INFO > Store Set/Surface/View from pro-STAR’s main window In the Store Information dialog, enter monitor for the Set Name Click Write and then Close Go to the STAR GUIde window and select the Output Controls sub-folder followed by the Monitor Engineering Behavior sub-folder Open the Monitor Cell Behavior panel Select On Change the Set File name to channel_les.set Select monitor from the Select Entry list Select Velocity Data Click Apply

At this point, the basic problem definition is complete. The next step is to set the transient controls for the run. Set the calculation run time to 50 seconds with a time step of 0.001 seconds, as determined in Tutorial 16.1 on the basis of the integral time scale and Courant number. 16-13

Tutorial 16.2


User Subroutine Final operations

• • • • • •

Select folder Analysis Preparation/Running Open the Set Run Time Controls panel Enter 50 in the Run for box under Run Time Click Apply In the Time Step Option section, check that the Time Step Method is set to Constant and enter 0.001 in the Time Step for Period box Click Set Period

Write and save the geometry and problem files: • • • •

Select File > Write Geometry File In the Geometry File Write dialog, click Apply and then Close Select File > Write Problem File In the Problem File Write dialog, click Apply and then Close

Finally, before exiting from pro-STAR, make sure that the model file (channel_les.mdl) is saved for possible future modification. •

Select File > Quit > Save & Quit.

User Subroutine User subroutine INITFI is used for setting the initial flow field, as shown below: C**************************************************************** SUBROUTINE INITFI(U,V,W,PR,TE,ED,T,SCALAR,XVF2) C Initialise fields C**************************************************************** C----------------------------------------* C STAR VERSION 4.02.000 * C----------------------------------------* INCLUDE ’comdb.inc’ COMMON/USR001/INTFLG(100) DIMENSION SCALAR(50) INCLUDE ’usrdat.inc’ EQUIVALENCE( UDAT12(001), ICTID ) EQUIVALENCE( UDAT03(001), CON ) EQUIVALENCE( UDAT03(020), F2 ) EQUIVALENCE( UDAT03(021), F4 ) EQUIVALENCE( UDAT03(022), F6 ) EQUIVALENCE( UDAT04(001), CP ) EQUIVALENCE( UDAT04(002), DEN ) EQUIVALENCE( UDAT04(062), VISM ) EQUIVALENCE( UDAT04(063), VIST ) EQUIVALENCE( UDAT04(067), X ) EQUIVALENCE( UDAT04(068), Y ) EQUIVALENCE( UDAT04(069), Z ) C------------------------------------------------------------------------real*8 Ubulk,Uprime,Vprime,Wprime real*8 Myone,Mypfive,Mypone,Myppfive,myzero,mythree,myfour Ubulk=20.0 Myone=-1.0 Mypone=1.0 16-14

Version 4.02

Tutorial 16.2


CFD Analysis Convergence and averaging

Mypfive=-0.5 Myppfive=0.5 Myzero=0.0 Uprime=32.45 Vprime=-52.36 Wprime=5.532 mythree=3.0 myfour=4.0 c.... Initialise channel flow u=Ubulk v=0.0 w=0.0 if (x.ge.Mythree.and.x.le.Myfour.and. * y.ge.Myzero.and.y.le.Myppfive.and. * z.ge.Mypfive.and.z.le.Myppfive) then u=Uprime v=Vprime w=Wprime endif RETURN END

CFD Analysis To run the analysis in parallel, on two local CPUs and in double precision, type: star -dp 2 To run the analysis sequentially in double precision, type: star -dp No matter how you choose to run the analysis, it will take at least a few days to complete. Such long run times are typical for LES cases as they require refined meshes and a large number of time steps (in this case 50,000). If you choose not to run the analysis, the results are supplied in file channel_demo.ccm which was copied into your working directory at the start of this tutorial. Post-Processing Convergence The transient nature of LES makes it necessary to average the data over some period and of time. The choice of this period will affect the quality of the results and should averaging therefore be sufficiently large to be statistically meaningful. Moreover, averaging should begin only when the flow is fully developed. The point at which averaging should begin can be judged by examining the velocity components at a suitable monitoring location. In the present example, this point is located near the wall where turbulence generation is greatest and was set up as described in the “Solution controls” section. Figure T16.2-1 shows a plot of the cross-stream velocity components at the prescribed monitoring point. It can be clearly seen that after 25s, or 25,000 time steps, component values are oscillating Version 4.02

16-15

Tutorial 16.2



about a mean value (in this case zero) and thus it is appropriate to begin averaging data. In fact, with the benefit hindsight, it would have been reasonable for such averaging to begin after only 10,000 time steps, which is roughly equivalent to 33 passes. This is much greater than the recommended number of passes before averaging, given in the “LES models” section of the On-line Help. This is because the use of periodic boundary conditions delays the establishment of a fully developed flow.

Figure T16.2-1

Monitoring-point velocity components throughout the simulation

Preliminaries The first post-processing task is to load file channel_les.ccm, containing the analysis results: • • • • Inst. results

Before analysing the averaged data, an example is shown of the instantaneous results representing a snapshot of the flow in time. Begin by displaying contours of the streamwise velocity component: • • • • • • •

16-16

Start up pro-STAR and resume from the channel_les.mdl model file In STAR GUIde, select the Post-Processing folder Open the Load Data panel Click Open Post File

Click on the Data tab Select On and All from the pull-down menus next to Smooth Option Select Velocity Component U from the Scalar Data list Click Get Data Click on Go To and select Create Plots Select Contour(filled) from the Option menu and Edge from the Edge/Mesh menu Select C > All in the main window Version 4.02

Tutorial 16.2


Post-Processing Inst. results

• •

Click Plot to Screen in the Create Plots panel In the main window, select View > Isometric > 1,1,1 to display Figure T16.2-2

Figure T16.2-2

Contour plot of the instantaneous streamwise velocity

The snapshot shows the flow field non-uniformity generated by the presence of eddies, with a predicted peak velocity of 24 m/s. The eddy structure can be viewed in more detail by creating a plot of the secondary flow field. To do this, create a vector plot of the V and W velocity components: • • • • • • • •

Version 4.02

Click Go To Load Data Select Off from the Smooth Option menu Select Velocity Component VW from the Vector Data list Click Get Data Select Go To > Create Plots Select Vector from the Option menu and Edge from the Edge/Mesh menu Click Plot to Screen In the main window, select View > Axis > +X to display Figure T16.2-3

16-17

Tutorial 16.2


Post-Processing Averaged results

Figure T16.2-3

Averaged results

Having looked at the structure of the instantaneous flow field, attention is turned to the time averaged data. Figure T16.2-4 shows a contour plot of the mean streamwise velocity component. The plot is similar to that obtained from a simulation using a RANS turbulence model, indicating that the averaging window is sufficiently large for the data to be statistically meaningful.

Figure T16.2-4 16-18

Vector plot of the instantaneous secondary flow field

Contour plot of the average streamwise velocity Version 4.02

Tutorial 16.2



Profiles of the mean and fluctuating components are now generated and compared to the DNS data of Moser et al. [2]. The plots are produced using the ready-made macros supplied with the tutorial files of your STAR-CD installation and listed in the “Macros” section. It should be noted here that LES post-processing is casedependent and that the macros provided are specifically for channel flow. Prior to generating any graphs, the time-averaged LES data must also be spatially-averaged. To do this: • • •

Select Panels > Define Macro from the main menu in pro-STAR Highlight DATA_AVERAGING in the Define Macro panel Click Execute

Next, create a plot of the normalised time-averaged mean velocity: •

Highlight MEAN_U and clicking Execute. Figure T16.2-5 shows the resulting plot of U+ against ln(y+).

Due to the problem symmetry about y = H, only half of the profile is shown. It can be observed that whilst the qualitative behaviour is reproduced by the LES model, the velocity at the centre of the channel is over-predicted by about 10% when compared to the DNS data.

Figure T16.2-5

•

Graph of mean streamwise velocity component

Reynolds stress profiles are produced by selecting REY_STRESS in the macro panel and clicking Execute

To view these plots: •

Version 4.02

Select Graph > Gdraw and then the appropriate frame number from the main pro-STAR window. For instance, selecting Graph > Gdraw > Frame1 will 16-19

Tutorial 16.2



produce a plot of u’u’, non-dimensionalised with the friction velocity, against ln(y+), as shown in Figure T16.2-6. Figures T16.2-6, T16.2-7 and T16.2-8 show profiles of u’u’, v’v’ and w’w’, respectively, non-dimensionalised by the friction velocity uτ = 1. These profiles represent the turbulence intensity and show good qualitative agreement with the DNS data. In addition, they highlight the anisotropic nature of the flow. It can be observed that the LES model over-predicts the streamwise fluctuations (Figure T16.2-6) whilst under-predicting the cross-stream fluctuations (Figures T16.2-7 and T16.2-8). Under-prediction of v’v’ and w’w’ is common in LES calculations where a large part of the turbulence spectrum lies in the subgrid scales. Closer agreement with the DNS results can only be obtained through further mesh refinement.

Figure T16.2-6

16-20

Graph of streamwise fluctuating component u’u’

Version 4.02

Tutorial 16.2



Figure T16.2-7

Graph of cross-stream fluctuating component v’v’

Figure T16.2-8

Graph of cross-stream fluctuating component w’w’

The u’v’ Reynolds stress profile is shown in Figure T16.2-9. It can be observed that the u’v’ component is well predicted by the LES model, both qualitatively and quantitatively.

Version 4.02

16-21

Tutorial 16.2


Bibliography Final operations

Figure T16.2-9

Graph of Reynolds stress u’v’

Components u’w’ and v’w’ are up to two or three orders of magnitude smaller and are therefore less important. These are not shown here but may be viewed by displaying the contents of graph frames 5 and 6. Final operations

As there were no changes to the model geometry or solution parameters, there is no need to save file tut.mdl •


Bibliography [1] Kim, Moin and Moser, 1987. ‘Turbulence Statistics in Fully Developed Channel Flow at Low Reynolds Number’. J Fluid Mechanics, 177, 133-166. [2] Moser, Kim and Mansour, 1999. ‘DNS of Turbulent Channel Flow up to Ret=590’. Physics of Fluids, 11, 943-945. Macros Mesh refinement in the Xdirection

16-22

! ============================================== ! Macro 16.2-1 Refining mesh in X direction ! ============================================== curs file CREF,10,1,1,ALL *set NCX NCX * 10 BSET ALL BDEL BSET cyde all cset all Version 4.02

Tutorial 16.2


Macros Spatial averaging of LES data

view,-1,1,1 cplot surf,on $vset,news,edge $bfin,1,vx, !SCRN, 0 1.8543 3.6749 !BFIN,1,6620, bset,add,bran,1,mxb surf,on $vset,news,edge $bfin,3,vx, !SCRN, 0 8.0000 5.2650 !BFIN,3,335356, bset,add,bran,3001,mxb view reve replot surf,on $vset,news,edge $bfin,2,vx, !SCRN, 0 2.4724 8.0035 !BFIN,2,3632, bset,add,bran,4801,mxb surf,on $vset,news,edge $bfin,4,vx, !SCRN, 0 6.2870 6.9788 !BFIN,4,15772, bset,add,bran,7801,mxb rdef,1,cyclic 1,partial,regular,integral pdrop,6.28319,293 rdef,2,cyclic 1,partial,regular,integral pdrop,-6.28319,293 cymatch,1,2,6.28319,0,0,0.0001 rdef,3,cyclic 1,all,regular,integral rdef,4,cyclic 1,all,regular,integral cymatch,3,4,0,0,-3.14159,0.0001 bset none moni,9001 pres,1.e+05,9001

Spatial averaging of LES data

Version 4.02

! ====================================== ! Macro 16.2-2 - Spatially averaging LES data ! ====================================== ! The script produces 12 files: ! U.dat - Mean U against y/H ! V.dat - Mean V against y/H ! W.dat - Mean W against y/H ! VMAG.dat - Mean VMAG against y/H ! P.dat - Mean P against y/H ! VIST.dat - Mean VIST against y/H ! uu.dat - Mean u’u’ against y/H ! vv.dat - Mean v’v’ against y/H ! ww.dat - Mean w’w’ against y/H ! uv.dat - Mean u’v’ against y/H ! uw.dat - Mean u’w’ against y/H ! vw.dat - Mean v’w’ against y/H ! ======================================= ! Clear old .dat files syst rm -f U.dat 16-23

Tutorial 16.2



syst rm -f syst rm -f syst rm -f syst rm -f syst rm -f

V.dat W.dat VMAG.dat P.dat VIST.dat

!========================================================= load,channel_les.ccm oper,getc,SUMN,1 oper,getc,SVMN,2 oper,getc,SWMN,3 oper,vmag,4 oper,getc,PMN,5 oper,getc,VIMN,6 *set IC 0 10 *def noex cset none *set CC1 IC - 10 :lab ! Setting the current cell set to a layer in the geometry cset add cran CC1 + 9001 CC1 + 9010 1 *if CC1 ge 88800 + IC *goto done *endif *set CC1 CC1 + 600 *goto lab :done ! Total *get R1 *get R2 *get R3 *get R4 *get R5 *get R6

each rtot rtot rtot rtot rtot rtot

! Divide the *set R1 R1 / *set R2 R2 / *set R3 R3 / *set R4 R4 / *set R5 R5 / *set R6 R6 / ! Replace chan cset chan cset chan cset chan cset 16-24

variable in the cell set and store in registers 1-6 1 2 3 4 5 6 total NCX / NCX / NCX / NCX / NCX / NCX /

by the number of cells in the layer NCZ NCZ NCZ NCZ NCZ NCZ

register 1 ,,, 0.0 R1 ,,, 0.0 R2 ,,, 0.0 R3 ,,, 0.0 R4

with the new values for register 1 etc. 1 1 2 2 3 3 4 4 Version 4.02

Tutorial 16.2



chan cset ,,, 0.0 R5 5 5 chan cset ,,, 0.0 R6 6 6 *end *loo 1 NCY ! Make current cell set equal to 1 Y-column of cells cset none *set CC2 9001 10 *defi noex cset add clis CC2 *end *loo 0 NCY - 1 ! loads current cell set numbers into graph register 1 gloa 1 cell cset ! Loads the y values of cells corresponding to graph register 1 ! into graph register 2 gval 2 1 cell y 1 ! Operate on register 2 to make the data y/H rope add 2 2 ,, 1.0 / H ! Operate on y and add 1.0 to the value (shift to match DNS ! position) roper,add,2,2,0,1,1,, ! Load values from post register 1 (mean U) into graph register 3 gval 3 1 cell pst1 ! Operate on u velocity to make it positive !roper,add,3,3,3,1,0,absolute, gval gval gval gval gval

4 5 6 7 8

1 1 1 1 1

cell cell cell cell cell

pst2 pst3 pst4 pst5 pst6

sdat sdat sdat sdat sdat sdat

U.dat 2 2 1 V.dat 2 2 2 W.dat 2 2 3 VMAG.dat 2 2 4 P.dat 2 2 5 VIST.dat 2 2 6

clos clos clos clos clos clos

U.dat V.dat W.dat VMAG.dat P.dat VIST.dat

!======================================================= syst rm -f uu.dat syst Version 4.02

16-25

Tutorial 16.2



rm -f syst rm -f syst rm -f syst rm -f syst rm -f

vv.dat ww.dat uv.dat uw.dat

oper oper oper oper oper oper

vw.dat getc getc getc getc getc getc

SUP 1 SVP 2 SWP 3 UPVP 4 UPWP 5 VPWP 6

*set IC 0 10 *def noex cset none *set CC1 IC - 10 :lab cset add cran CC1 + 9001 CC1 + 9010 1 *if CC1 ge 88800 + IC *goto done *endif *set CC1 CC1 + 600 *goto lab :done *get *get *get *get *get *get *set *set *set *set *set *set chan chan chan chan chan chan *end *loo

R1 rtot 1 R2 rtot 2 R3 rtot 3 R4 rtot 4 R5 rtot 5 R6 rtot 6 R1 R1 / NCX / NCZ R2 R2 / NCX / NCZ R3 R3 / NCX / NCZ R4 R4 / NCX / NCZ R5 R5 / NCX / NCZ R6 R6 / NCX / NCZ cset ,,, 0.0 R1 * cset ,,, 0.0 R2 * cset ,,, 0.0 R3 * cset ,,, 0.0 R4 4 cset ,,, 0.0 R5 5 cset ,,, 0.0 R6 6

R1 1 1 R2 2 2 R3 3 3 4 5 6

1 NCY

cset none *set CC2 1 9010 *defi noex cset add clis CC2 16-26

Version 4.02

Tutorial 16.2


Macros Mean streamwise velocity profile

*end *loo 0 NCY - 1

Mean streamwise velocity profile

gval gval gval gval gval gval

3 4 5 6 7 8

1 1 1 1 1 1

cell cell cell cell cell cell

sdat sdat sdat sdat sdat sdat

uu.dat vv.dat ww.dat uv.dat uw.dat vw.dat

clos clos clos clos clos clos

uu.dat vv.dat ww.dat uv.dat uw.dat vw.dat

2 2 2 2 2 2

pst1 pst2 pst3 pst4 pst5 pst6 2 2 2 2 2 2

1 2 3 4 5 6

! ============================================== ! Macro 16.2-3 Producing a mean streamwise velocity profile ! ============================================== greset y ! Load mean u velocity gdata,U.dat,2,1,1,coded,1 roper multi,1,1,,395,,, ! Transform y axis to log scale roper,add,1,1,0,1,0,loge, !Load DNS data gdata,chan395.means,8,3,1,coded,1 ! Transform y axis to log scale roper,add,4,4,0,1,0,loge, !Plot the mean velocity in frame 1 frame,1,xreg,init, 1,4 frame,1,yreg,init, 2,5 frame,1,legend,10.2,5.0 12.5 6.5 Mean U frame,1,xrange,0,6 grlabel,1,1,on,,,5.0,1.5 ln(y+) grlabel,1,2,on,,,0.5,6.0 U+ symt,2,2,8,1$lint,2,2,2,1$rtab,2,y,y$bart,2,2,90,1 symt,5,4,8,1$lint,5,4,2,1$rtab,5,y,n rlabel,2,on $LES rlabel,5,on $DNS ! Reverse background colour clrm,reve

Version 4.02

16-27

Tutorial 16.2


Macros Reynolds stress profiles

gdraw,1

Reynolds stress profiles

! ============================================== ! Macro 16.2-4 Producing profiles of the Reynolds stresses ! ============================================== ! Reset graph parameters and set the number of registers at 40 greset y numr 40 ! Load fluctuating components for Cs = 0.01 gdata,uu.dat,2,1,1,coded,1 gdata,vv.dat,2,3,1,coded,1 gdata,ww.dat,2,5,1,coded,1 gdata,uv.dat,2,7,1,coded,1 gdata,uw.dat,2,9,1,coded,1 gdata,vw.dat,2,11,1,coded,1 !Load DNS RMS data gdata,chan395.reystress,8,15,1,coded,add ! GRAPH DATA frame 1 xreg init 1,15 frame 1 yreg init 2,17 gdraw 1 frame,1,legend,10.2,5.0 12.5 6.5 u’u’ frame,1,xrange,0,400 grlabel,1,1,on,,,5.0,1.5 y+ grlabel,1,2,on,,,0.5,6.0 u’u’ grlabel,1,3,on,,,0.5,5.9 ___ grlabel,1,4,on,,,0.5,5.5 ut^2 frame,1,xrange,0,1 symt,2,2,8,1$lint,2,2,2,1$rtab,2,y,y$bart,2,2,90,1 symt,17,4,8,1$lint,17,4,2,1$rtab,5,y,n rlabel,2,on $LES rlabel,17,on $DNS ! Reverse background colour clrm,reve ! GRAPH DATA frame 2 xreg init 3,15 frame 2 yreg init 4,18 gdraw 2 frame,2,legend,10.2,5.0 12.5 6.5 v’v’ frame,2,xrange,0,400 grlabel,2,1,on,,,5.0,1.5 y+ grlabel,2,2,on,,,0.5,6.0 v’v’

16-28

Version 4.02

Tutorial 16.2



grlabel,2,3,on,,,0.5,5.9 ___ grlabel,2,4,on,,,0.5,5.5 ut^2 frame,2,xrange,0,1 symt,4,2,8,1$lint,4,2,2,1$rtab,4,y,y$bart,4,2,90,1 symt,18,4,8,1$lint,18,4,2,1$rtab,18,y,n rlabel,4,on $LES rlabel,18,on $DNS ! Reverse background colour clrm,reve ! GRAPH DATA frame 3 xreg init 5,15 frame 3 yreg init 6,19 gdraw 3 frame,3,legend,10.2,5.0 12.5 6.5 w’w’ frame,3,xrange,0,400 grlabel,3,1,on,,,5.0,1.5 y+ grlabel,3,2,on,,,0.5,6.0 w’w’ grlabel,3,3,on,,,0.5,5.9 ___ grlabel,3,4,on,,,0.5,5.5 ut^2 frame,3,xrange,0,1 symt,6,2,8,1$lint,6,2,2,1$rtab,6,y,y$bart,6,2,90,1 symt,19,4,8,1$lint,19,4,2,1$rtab,19,y,n rlabel,6,on $LES rlabel,19,on $DNS ! Reverse background colour clrm,reve ! GRAPH DATA frame 4 xreg init 7,15 frame 4 yreg init 8,20 gdraw 4 frame,4,legend,10.2,5.0 12.5 6.5 u’v’ frame,4,xrange,0,400 grlabel,4,1,on,,,5.0,1.5 y+ grlabel,4,2,on,,,0.5,6.0 u’v’ grlabel,4,3,on,,,0.5,5.9 ___ grlabel,4,4,on,,,0.5,5.5 ut^2 frame,4,xrange,0,1 symt,8,2,8,1$lint,8,2,2,1$rtab,8,y,y$bart,8,2,90,1 symt,20,4,8,1$lint,20,4,2,1$rtab,20,y,n rlabel,8,on $LES rlabel,20,on $DNS ! Reverse background colour Version 4.02

16-29

Tutorial 16.2



clrm,reve ! GRAPH DATA frame 5 xreg init 9,15 frame 5 yreg init 10,21 gdraw 5 frame,5,legend,10.2,5.0 12.5 6.5 u’w’ frame,5,xrange,0,400 grlabel,5,1,on,,,5.0,1.5 y+ grlabel,5,2,on,,,0.5,6.0 u’w’ grlabel,5,3,on,,,0.5,5.9 ___ grlabel,5,4,on,,,0.5,5.5 ut^2 frame,5,xrange,0,1 symt,10,2,8,1$lint,10,2,2,1$rtab,10,y,y$bart,10,2,90,1 symt,21,4,8,1$lint,21,4,2,1$rtab,21,y,n rlabel,10,on $LES rlabel,21,on $DNS ! Reverse background colour clrm,reve ! GRAPH DATA frame 6 xreg init 11,15 frame 6 yreg init 12,22 gdraw 6 frame,6,legend,10.2,5.0 12.5 6.5 v’w’ frame,6,xrange,0,400 grlabel,6,1,on,,,5.0,1.5 y+ grlabel,6,2,on,,,0.5,6.0 v’w’ grlabel,6,3,on,,,0.5,5.9 ___ grlabel,6,4,on,,,0.5,5.5 ut^2 frame,6,xrange,0,1 symt,12,2,8,1$lint,12,2,2,1$rtab,12,y,y$bart,12,2,90,1 symt,22,4,8,1$lint,22,4,2,1$rtab,22,y,n rlabel,12,on $LES rlabel,22,on $DNS ! Reverse background colour clrm,reve

16-30

Version 4.02

Star CCM Tut

Recommend Documents