Workshop 5.1 5 .1 14.5 Release
Load Mapping
Worked Example
We are going to create a simple box shaped model to demonstrate the load mapping process The structural model will include some simple stiffeners to show how to handle internal elements The Steps of the exercise include: •
Create Structural Geometry
•
Create Structural Model and Information
•
Create Hydrodynamic Geometry
•
Create Hydrodynamic Model and Information
•
Extract the Hydrodynamic Load Information (Load Mapping)
•
Include the Hydrodynamic loading to Structural model
•
Investigate the final results
Worked Example
We are going to create a simple box shaped model to demonstrate the load mapping process The structural model will include some simple stiffeners to show how to handle internal elements The Steps of the exercise include: •
Create Structural Geometry
•
Create Structural Model and Information
•
Create Hydrodynamic Geometry
•
Create Hydrodynamic Model and Information
•
Extract the Hydrodynamic Load Information (Load Mapping)
•
Include the Hydrodynamic loading to Structural model
•
Investigate the final results
Step 1: Create the Structural Geometry Open Workbench Create a Geometry instance and open DM for editing
...Create Structural geometry Create Hull •
Select length units as meters
•
Create box primitive
•
Set details of box
•
Generate
...Create Structural geometry Create a thin surface •
Set Selection Type to Bodies Only
•
Graphically select box for Geometry
•
Set thickness to 0m (acts as shell rather than solid)
...Create Structural geometry Create Stiffener •
•
We are going to generate a series of simple plate stiffeners First generate a new horizontal plane
...Create Structural geometry Create stiffener •
Use the new plane to slice the model
•
First Freeze the model to allow the slice
•
Slice all bodies using the plane created in the last step
...Create Structural geometry Create stiffener •
Create a second box that will be used to remove the interior of the plate to generate the desired stiffener
...Create Structural geometry Create stiffener •
•
Create the plate surface for the stiffener using the edges generated with the Slice command Edges are selected using the
...Create Structural geometry Create stiffener •
Remove interior of plate to create desired stiffener
– Use a Boolean operation (Subtract) – Target body is the plate generated in last step •
To select the plate use the layer selection image to step through the surfaces
– Tool body is the second box
...Create Structural geometry Generate copies of stiffener •
Use Pattern to create 5 copies of stiffener
– Linear pattern type with 5m offset – Geometry is the stiffener created in the last step
– Use the face normal of the stiffener surface to define direction.
– Note the use of the red and black arrows to define actual direction.
...Create Structural geometry
Resulting stiffener definition
...Create Structural geometry Complete stiffener connection •
• •
Stiffeners are not automatically connected to hull Use Joint command to make connections Select all surface bodies as Target Bodies. Can use Box Select mode to simplify selection.
...Create Structural geometry Create a single part •
Model currently has 8 bodies and 8 parts
•
To improve meshing create a single part
•
Rename the new Part to Hull
...Create Structural geometry
Geometry for structure is now complete Exit DesignModeler Now we need to create a structural meshed model for use in the load mapping stage
Step 2: Create Structural Model and Information Add Static Structural System to project, linking geometry to that created in DesignModeler. Double click on Model cell.
...Create Structural Model and Information Define plate thickness •
DesignModeler set plate thickness to 0.0
– Results in Geometry as ? – Set thickness for hull bodies to 32mm
– Set thickness for stiffener plate to 50mm
...Create Structural Model and Information Mesh •
Use default meshing for this model
...Create Structural Model and Information Define wetted surface •
•
•
Load transfer requires definition of wetted (external) surfaces Use dummy pressure case to define required geometry Select surfaces manually, or use named selections
...Create Structural Model and Information Model Interface definition •
AQWA WAVE requires structural model in ASAS format
•
ANSTOASAS command generates required data
•
In Workbench insert Commands in object tree
•
Add ANSTOASAS in Worksheet view
...Create Structural Model and Information Add Point Masses •
Masses represent ballast & storage
•
Associate mass with hull surface adjacent to position
•
First mass is at 5,5,-32.5
•
Mass value of 1000 tonnes
...Create Structural Model and Information Add Point Masses •
Add two more additional masses
– 1000 tonnes at 5,5,-27.5 – 1000 tonnes at 5,5,-22.5 •
Associate these masses to appropriate hull surfaces
...Create Structural Model and Information Disable weak springs •
ANSYS Mechanical defaults to including weak springs to remove rigid body motions
•
AQWA WAVE does not recognize the springs generated, so disable this feature
...Create Structural Model and Information Solve • •
In order to implement the ANSTOASAS command a Solve must be instigated. Can ignore any warnings and errors related to solution since results from this analysis are not used, only the generated ASAS interface file and mass information
...Create Structural Model and Information Mass Extraction •
•
The hydrodynamic model requires an accurate definition of the mass inertia information for the model. In the absence of better data this can be extracted from the structural model
Select Solution Information and review Worksheet for the mass data
...Create Structural Model and Information Review structural interface file •
The ANSTOASAS command generates a text file called file.asas
– This contains the structural definition in ASAS format •
Copy file.asas to a new directory where you will perform the load mapping
Step 3: Create Hydrodynamic Geometry
Structural definition model for AQWA WAVE is now complete Exit ANSYS Mechanical Now we need to create a hydrodynamic model for use in the load mapping stage
...Create Hydrodynamic Geometry Duplicate structural geometry created earlier. Rename system as Hydrodynamic Geometry and double click in the geometry cell of the new system
...Create Hydrodynamic Geometry The hydrodynamic geometry is much simpler, it is just the hull Suppress items in the tree that were used for the stiffener generation
...Create Hydrodynamic Geometry Modify Geometry •
AQWA requires model that is meshed up to water line
– Slice the model horizontally – Use XYPlane as the Base Plane (global Z is 0 for this) •
AQWA also requires one part for each vessel
– Form new part and name as Hull •
Close DesignModeler
Step 4: Create Hydrodynamic Model and Information Add a Hydrodynamic Diffraction to the Hydrodynamic Geometry Double click on Model
...Create Hydrodynamic Model and Information Add Point Mass •
•
Add a point mass and manually define the mass and inertia values obtained from structural model Ensure position of point mass is correctly defined (also obtained from structural model)
...Create Hydrodynamic Model and Information Generate Mesh •
In general the load mapping process requires a more refined hydrodynamic mesh than normally required for motions analysis
•
For this exercise, to reduce run time use maximum element size of 2.5m (and defeaturing tolerance of 1m)
...Create Hydrodynamic Model and Information Adjust the General Settings for Hydrodynamic Analysis •
To reduce run time for the exercise set the number of intermediate frequency values to 8
...Create Hydrodynamic Model and Information Check Hydrostatics •
Insert Hydrostatic Result to Solution
•
Solve Hydrostatics to check that we have a valid model
...Create Hydrodynamic Model and Information
Check Hydrostatics •
When solution has completed select Hydrostatic Report and review results
...Create Hydrodynamic Model and Information Solve •
Select Solve and review pressures using Pressures and Motions results object
•
Save AQWA files in the project directory to your load mapping directory
Step 5: Load Mapping
Hydrodynamic model for AQWA WAVE is now complete Exit AQWAWB Now we need to create a “steering information” data file for use in the load mapping stage
...Load Mapping AQWA WAVE Steering file •
•
•
•
Create a new *.dat file in the load mapping directory Copy the text in the slide to the *.dat file
* Standard lines for ASAS style data: SYSTEM DATA AREA 5000000 JOB NEW LINE PROJECT ANSY *At present ANSYS files default to project ANSY * Extension of the output files (*.txt) EXTENSION txt END * Define structural model (in this case output from anstoasas command) stru asas file.asas * Define hydrodynamic model hydr aqwa analysis
This file directs AQWA WAVE to the END appropriate structural and hydrodynamic information, and defines AQWAID * Following commands set target structural analysis system as ANSYS Mechanical load data required FELM For more information on the Steering file refer to AQWA WAVE Manual
FEPG ANSYS END LOAD * Load * Case CASE 0 CASE 0 CASE 0 CASE 0 END
information Current_ID Frequency_ID Direction_ID Wave_Height Phase 5 1 2.0 0 5 1 2.0 90 7 1 2.0 0 7 1 2.0 90
*Stop processing this file. STOP
...Load Mapping Run AQWA WAVE •
Running the program will bring up a dialogue box requesting the steering data file discussed on previous slide
...Load Mapping
AQWA WAVE creates (in this instance) 4 ANSYS APDL load files
Step 6: Include the Hydrodynamic loading to Structural model Create second structural model •
Create a second structural process by dragging the Static Structural system onto the first and sharing the first three cells (B2:B4)
...Include the Hydrodynamic loading to Structural model Apply generated loads • •
•
•
Open the second structural model In Analysis Settings set the number of steps to 4 In Workbench insert Commands in object tree of Static Structural 2 Use /INPUT command to reference the first of the loading files
! !
Commands inserted into this file will be executed just prior to the Ansys SOLVE command. These commands may supersede command settings set by Workbench.
!
Active UNIT system in Workbench when this object was created:
Metric (m, kg, N, s, V, A)
/INPUT,C:\ANSYS\TrainingWorkArea\LoadMapWorking_files\user_files\file_aqld1001.dat
...Include the Hydrodynamic loading to Structural model Apply generated loads •
• •
Set Step Selection Mode for the command object to By Number Set Step Number to 1 Repeat command insertion for the other three load cases, incrementing the step number by 1 each time
...Include the Hydrodynamic loading to Structural model Solve •
The standard load file generated by AQWAWAVE includes a SOLVE command for use in Mechanical APDL, not required for Workbench so comment out (or delete)
SFE, 1011, 2,PRES,0, 1.7681E+02, 1.9584E+02, 1.5090E+02, 1.3224E+02 SFE, 1012, 2,PRES,0, 2.2709E+02, 2.4616E+02, 1.9584E+02, 1.7681E+02 SFE, 1013, 2,PRES,0, 3.0239E+02, 3.0313E+02, 2.4616E+02, 2.2709E+02 SFE, 1014, 2,PRES,0, 2.4616E+02, 3.0313E+02, 3.0239E+02, 2.3488E+02 SFE, 1015, 2,PRES,0, -2.1617E+02, -2.0395E+02, -1.3253E+02, -1.3314E+02 SFE, 1016, 2,PRES,0, -1.3253E+02, -2.0395E+02, -2.1617E+02, -1.3811E+02 ACEL, 5.6327E-02, -5.7843E-07, 1.1702E-03 CGLOC, 5.0000E+00, 5.0000E+00, -2.4600E+01 DCGOMG, -2.8427E-08, 6.1327E-03, 3.6777E-08 ! SOLVE
•
Note this time we allow weak springs to be used
