Workshop 1: Bubbly Flow in a Rectangular Bubble Column 14. 5 Release
Multiphase Flow Modeling In ANSYS CFX
Introduction •
•
•
•
•
This workshop models the dispersion of air bubbles bubb les in water in a rectangular bubble column. Gas is supplied through a sparger at the bottom of the bubble column and the rising action of bubbles bub bles provides agitation of the liquid. Although the boundary conditions are steady and the geometry is simple, there is a transient character charact er to the solution In this workshop, you will set up and a nd run a basic bubbly flow simulation. In the second workshop, you will add non-drag forces to the model.
Introduction •
•
•
•
•
This workshop models the dispersion of air bubbles bubb les in water in a rectangular bubble column. Gas is supplied through a sparger at the bottom of the bubble column and the rising action of bubbles bub bles provides agitation of the liquid. Although the boundary conditions are steady and the geometry is simple, there is a transient character charact er to the solution In this workshop, you will set up and a nd run a basic bubbly flow simulation. In the second workshop, you will add non-drag forces to the model.
Rectangular Bubble Column Geometry Vessel Details Height of column Width of column Depth of column
1.00 m 0.10 m 0.02 m
Height of sparger Length of sparger Width of sparger
0.01 m 0.01 m 0.02 m
•
•
Air inlet at the bottom via a sparger (porous aquarium stone) Air superficial velocity: 0.002 ... 0.03 m/s
.
Expected Behavior Measurements: •
•
High speed video camera: –
Gas velocity
–
Bubble size
Wire mesh sensor –
Gas volume fraction
–
Bubble sizes Bubbles dispersed across the column
Narrow plume of bubbles near the inlet
Computational Mesh outlet = opening
•
•
inlet (sparger)
Hexahedral mesh (ICEM-CFD Hexa) Mesh element size: x=y=z=0.005m
•
200204 cells
•
16,000 elements
•
21,105 nodes
Importing the Mesh •
•
Copy the file ICEM CFD mesh file rectangularcolumn.msh from the input files folder into a working directory. Start CFX-Pre from the ANSYS CFX Launcher after changing to this working directory and open a new case (File/New Case/General) Right-click on Mesh in the Outline and select Import Mesh/ICEM CFD and import rectangularcolumn.msh into the simulation, setting the Mesh Units to m.
Imported Mesh •
•
Hightlight the imported mesh in the Outline view. Right-click on it and select Mesh Statistics Note the dimensions of the imported mesh in the pop-up window, Note that the height of the vertical column ranges from a y-value of 0.0 [m] at the bottom and 1.0 [m] at the top
Defining Domain Fluids (Continuous Phase) •
•
Double-click the Default Domain created for your imported mesh to edit it (if a default domain was not created, create one). On the Basic Settings tab of the Details form for the domain: – Set the Domain Type to Fluid Domain – Highlight Fluid 1 in the Fluid and Particle Definition window and click on the Delete icon to remove it
– Click on the New icon in the Fluid and Particle definition window and insert a new fluid named water
– Select the predefined constant property material Water and set the Morphology Option to Continuous Fluid
Defining Domain Fluids (Dispersed Phase) •
Still on the Basic Settings tab of the Details form for the domain:
– Click on the New icon next to the Fluid and Particle Definition window and insert a new fluid definition named air
– For the new fluid air, select the predefined constant property material Air at 25 C and set the Morphology Option to Dispersed Fluid with a size of 0.003 [m]
Viewing the Fluid Densities •
•
Expand the Materials entry in the outline and double-click on the Material definitions for the Air at 25 C and Water materials used to define the fluid properties for this simulation and note the values of the constant densities set for these fluids (1.185 kg/m3 for Air at 25 C and 997 kg/m3 for Water) These values will be important in defining the reference density for the buoyancy settings for the domain as well as the hydrostatic head for the initial guess for the pressure
Setting the Buoyancy Properties •
•
•
•
Buoyancy effects are very important for gasliquid settings and therefore buoyancy properties must be defined for the domain On the Basic Settings form for the Domain under the Domain Models section, set the Buoyancy Option to Buoyant and enter the X,Y, and Z components of the gravity vector as [0, -9.81, 0] m/s2. Set the buoyancy reference density to the density of water [997.0 kg/m3] which is the continuous phase for this problem Set the Reference Location option for Buoyancy to Cartesian Coordinates and enter values consistent with the top surface of the domain [0 1 0 ] m
Fluid Domain: Fluid Models •
Left-Click the Fluid Models tab for the Domain. –
Leave the Homogeneous Model toggle unchecked
–
Set the Free Surface Model to None since this is a dispersed/continuous type of flow
–
Set Heat Transfer option to Isothermal with a Fluid temperature of 25 [C].
–
Set the Turbulence option to Fluid Dependent
Fluid Domain: Fluid Specific Models •
Click on the Fluid Specific Models tab on the Domain form and select air – Set the Fluid Buoyancy Model Option to Density Difference
– Set the Turbulence Model to Dispersed Phase Zero Equation •
Click on water and set: – Fluid Buoyancy Model Option to Density Difference
– Turbulence Model to Shear Stress Transport
– Buoyancy Turbulence Option to None
Fluid Pair Models •
Click on the Fluid Pair Models tab and: – Click on the Surface Tension Coefficient toggle and enter a value of 0.072 N/m (the surface tension force will not be modeled in this tutorial but the surface tension coefficient will be used in the Grace correlation for the drag)
– Set the Interphase Transfer Option to Particle Model
– Under Momentum Transfer, set the Drag Force Option to Grace
– Enable the Volume Fraction Correction Exponent and enter a value of 3. This value will help keep the drag law well behaved in the gas headspace region above the liquid
– Leave Non-drag forces unset and set the Turbulence Transfer Option to Sato Enhanced Eddy Viscosity •
Click OK to complete the domain definition
Flow Boundary Condition Strategy •
•
•
The bubble column modeled in this simulation is semi-batch where air flows continuously through a batch layer of liquid The sparger inlet at the bottom of the vessel has only air flowing through it (air volume fraction =1) The outlet at the top of the geometry will be a pressure specified opening through which either air or water could flow. To preserve the initial liquid loading set in the initial guess, an air headspace above the liquid will be specified in the initial guess for the volume fraction field. As long as convergence is reasonable, only air will leave this boundary and the initial amount of liquid will be preserved even for a steady simulation
Outlet Air Head Space
Batch Liquid
Air Inlet
Inlet Boundary Condition: inlet •
•
Insert an Inlet boundary named inlet and assign it to the location INLET On the Boundary details tab: –
–
–
–
Set the Mass and Momentum Option to Bulk Mass Flow Rate Click on the expression toggle next to the Mass Flow Rate entry box The mass flow rate of gas will be calculated based on its superficial velocity, the column cross-sectional area, and the gas density The superficial velocity, J SG, is defined as the volumetric gas flow rate divided by the cross-sectional area of the column: JSG=0.01 m/s CSA = 0.01 m x 0.2 m = 0.002 m 2 Air Density = 1.185 kg/m 3 Mass Flow Rate = 0.01 [m/s]*0.002 [m^2]*1.185 [kg/m^3]
–
Enter this expression for the Bulk Mass Flow Rate
Inlet Boundary Condition: Fluid Values •
•
On the Fluid Values tab: –
Highlight air and set the Volume Fraction to 1.0
–
Highlight water and set the Volume Fraction to 0.0
Click OK to create the boundary
Opening Boundary Condition: outlet •
•
•
Insert a boundary named outlet . Set the type to Opening and Location to OUTLET. For Boundary Details: –
Set the Mass and Momentum Option to Opening Pres. and Dirn.
–
Enter a Relative Pressure of 0.0 Pa
Click the Fluid Values tab (these are only applied if fluid is entrained at the outlet) –
Highlight air and set the Volume Fraction to 1.0
–
Highlight water and set the Volume Fraction to 0.0
Click OK to create the boundary
Default Wall Boundary Condition •
•
•
•
Double click the default boundary created for the domain (Default Domain Default for a domain named Default Domain) to bring up the Edit Boundary form On the Boundary details tab, set the Mass and Momentum Option to Fluid Dependent On the Fluid Values tab: –
Highlight air and set the Mass and Momentum Option to Free Slip Wall
–
Highlight water and set the Mass and Momentum Option to No Slip Wall
Click OK to update the wall boundary settings
Boundary Condition Summary •
Top Opening
•
Side and Bottom Walls
•
Sparger Inlet
Initial Condition •
•
The initial condition for this simulation will set up a gas headspace in the upper 10% of the domain (i.e. for y > 0.9 m)
Headspace
This will be implemented by using a step function for gas volume fraction that is zero for y < 0.9 m and 1 for y > 0.90 m. The air volume fraction expression will be: step((y - 0.90 [m])/1.0 [m])
•
We must also enter the correct hydrostatic pressure for this initial condition relative to the buoyancy reference density of 997 kg/m^3 and the buoyancy reference position (y = 1.0 m): P = (1.185 997)[kg/m^3]*g*(1.0[m] - y)* step((y - 0.9 [m])/1.0 [m]) –
This will be zero in the liquid region and hydrostatic in the gas * Note: g is a CFX system variable which is predefined as 9.81 [m/s^2]
Global Initialization •
•
•
Click the Global Initialization icon from the menu bar On the Global Settings tab, set the Static Pressure Option to Automatic with Value Enter the following expression for Relative Pressure which was given on the previous slide (be sure to click on the Equation toggle next to the Relative Pressure entry box): (1.185-997) [kg/m^3] *g* (1.0 [m] - y)* step((y-0.9 [m])/1.0 [m])
Global Initialization: Fluid Settings •
On the Fluid Settings tab, highlight air and set: – U, V, and W Cartesian Velocity Components to Automatic with Value with all at 0.0 [m/s]
– the Volume Fraction Option to Automatic with Value with the expression set to: step((y - 0.90 [m])/1.0 [m]) •
Highlight water and set: – U, V, and W Cartesian Velocity Components to Automatic with Value with all at 0.0 [m/s]
– Turbulence Option to Medium (Intensity = 5%) – the Volume Fraction Option to Automatic with Value with the expression set to: 1.0 - step((y - 0.90 [m])/1.0 [m]) •
Click OK to complete the Initialization
Solver Parameters •
•
Click on the Solver Control icon from the menu bar On the Basic Settings tab: –
Set the Advection Scheme Option to High Resolution
–
Set the Timescale Control to Physical Timescale and enter a Physical Timescale of 0.01 s
–
Set the Max. Iterations to 100
–
Enter 1e-4 for the Residual Target
–
Leave the other settings at their default values and click OK to apply the solver settings
Output Control: Monitor Point •
•
Click on the Output Control icon from the menu bar Click on the Monitor tab and: –
Enable the Monitor Options toggle
–
Under Monitor Points and Expressions, click on the New icon
–
Enter holdup as the name of the new monitor point
–
Set the Option for Holdup to Expression and enter the Expression Value as:: volumeAve(air.vf)@Default Domain
This gives the average volume fraction of air in the domain, commonly known as the gas hold-up. (If your domain name is not Default Domain, use that name in its place). Click OK to create the monitor
Write Solver File and Define Run •
Click the Define Run icon from the menu bar –
Enable the Quit CFX-Pre toggle and click Save to write the input file
–
Click Save and Quit when prompted to save the simulation file
Running the Solver •
•
When the Solver Manager Define Run form appears, click Start Run It should take about five minutes to solve 100 iterations
Monitoring the Residuals
Assessing Convergence •
•
•
•
After 100 iterations, the run has not converged very well in terms of the magnitudes of the residuals Browse the output file and check the imbalances for mass and the volume fraction of Air at 25 C. They are also still quite high. Click on the User Points tab of the Solver Manager to display the change in the computed gas phase holdup over time. The initial value near 0.10 corresponds to the initial headspace set in the initial guess Start CFX-Post and load the results file from your run
Post-Processing •
Select the -z view. Create a xy-plane for a z-value of 0.01 m and color it according to air.Volume Fraction. Clearly, the air volume fraction field is still evolving (The ANSYS CFX solver is time marching, even for a steady-state run). This is reflected in the high mass imbalances.
Continuing the Run
•
•
•
•
•
From the Solver Manager, click on Tools/Edit CFX Solver File and select the results file for your current run. Find the Solver Control section in the Definition File Editor and expand Convergence Control Double-click Physical Timescale and change it to 0.02 s. Double-click Maximum Number of Iterations and change it to 400 Click File/Save then File/Exit. Click the Restart icon to resume the run with the new settings
Solver Monitor •
The second run will require about 20 minutes to reach 400 iterations
Imbalance and Holdup
Continuation from First Run
•
Convergence and imbalances are still not great but we can examine the Results File in CFD-Post to look for causes
Post-Processing •
Start Post and load the current results file. Select the -z view. Create a XY-Plane for a z-value of 0.01 m and color it according to air.Volume Fraction. Next, clip the range by setting a user-specified range from 0 to 0.125. The bubble plume is unsteady which causes the wiggles in the convergence behavior.
Comparison to Experiment •
The current steady-state simulation results predict an oscillating relatively narrow plume of bubbles rising up the center of the column. The experimental pictures show that the length of the initial narrow plume of bubbles is much shorter than what the simulation predicts
Bubbles dispersed across the column
Narrow plume of bubbles near the inlet
Adding Non-Drag Forces •
•
One reason for the difference between the experimental bubble plume and the simulation prediction is the neglecting of several important non-drag forces including lift, turbulent dispersion, and wall lubrication. These will be included in the second workshop.
