OS-T: 1030 3D Inertia Relief Analysis
An existing finite element model is used in this tutorial to demonstrate how HyperMesh may be used to set-up an inertia relief analysis. The analysis is then performed using OptiStruct and post-processed in HyperView.
Figure 1 illustrates the structural model used for this tutorial.
![3d-inertia-1](../../../images/solvers/3d-inertia-1.png)
Launch HyperMesh and Set the OptiStruct User Profile
-
Launch HyperMesh.
The User Profile dialog opens.
-
Select OptiStruct and click
OK.
This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.
Open the Model
- Click .
- Select the ie_carm.hm file you saved to your working directory.
-
Click Open.
The ie_carm.hm database is loaded into the current HyperMesh session, replacing any existing data.
Apply Loads and Boundary Conditions
Create Load Collectors
-
In the Model Browser, right-click and select from the context menu.
A default load collector displays in the Entity Editor.
- For Name, enter static_loads.
- Click Color and select a color from the color palette.
-
Set Card Image to None and click
Close.
A new load collector, static_loads is created.
Figure 2. Creating the static_loads Load Collector
-
Create another load collector.
- For Name, enter SPCs.
- For Card Image, select None.
Create SUPORT1 Constraint
- From the menu bar, click to open the Constraints panel.
-
Create constraint 1.
-
Create constraint 2.
-
Create constraint 3.
Figure 4. Final Constraint Applied to Control Arm Model
- Click return to exit the panel.
Create Static Forces
- In the Model Browser, Load Collectors folder, right-click on static_loads and select Make Current to set it as the current load collector.
- From the menu bar, click to open the Forces panel.
-
Create force 1.
-
Create force 2.
- Click return and to exit the panel.
![3d-inertia-3](../../../images/solvers/3d-inertia-3.png)
Create Load Steps
- In the Model Browser, right-click and select from the context menu.
- For Name, enter linear.
- Set Analysis type to Linear Static.
-
Define LOAD.
- For LOAD, click to open Advanced Selection.
- In the dialog, select static_loads and click OK.
- In Subcase Options, select .
- For SUPORT1, click to open Advanced Selection.
- In the dialog, select SPCs and click OK.
An OptiStruct subcase has been created which references the forces in the load collector static_loads and the inertia relief support points in the load collector SPCs.
![](../../../images/solvers/os_1030_03.png)
Create Control Cards for Inertia Relief Analysis
- From the menu bar, click to open the Control Cards panel.
-
Click TITLE and enter a title for this inertia relief
analysis, then click return.
Tip: Use Next and Prev to browse through the different control card pages.
- Click PARAM, and enable INREL.
-
Under INREL_V1, toggle the selection to be -1.
This requests that an inertia relief analysis be performed.
- Click return twice to go to the main menu.
Submit the Job
-
From the Analysis page, click the OptiStruct
panel.
Figure 7. Accessing the OptiStruct Panel
- Click save as.
-
In the Save As dialog, specify location to write the
OptiStruct model file and enter
ie_carm for filename.
For OptiStruct input decks, .fem is the recommended extension.
-
Click Save.
The input file field displays the filename and location specified in the Save As dialog.
- Set the export options toggle to all.
- Set the run options toggle to analysis.
- Set the memory options toggle to memory default.
- Click OptiStruct to launch the OptiStruct job.
- ie_carm.html
- HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
- ie_carm.out
- OptiStruct output file containing specific information on the file setup, the setup of your optimization problem, estimates for the amount of RAM and disk space required for the run, information for each of the optimization iterations, and compute time information. Review this file for warnings and errors.
- ie_carm.h3d
- HyperView binary results file.
- ie_carm.res
- HyperMesh binary results file.
- ie_carm.stat
- Summary, providing CPU information for each step during analysis process.
View the Results
OptiStruct provides contour information for all of the loadsteps that were run. The following steps describe the process for viewing those results in HyperView.
View the Deformed Shape
-
When the message ANALYSIS COMPLETED is received in the Solver
View window, click Results.
HyperView is launched and the results are loaded.
-
Verify that the Animate Mode is set to Linear Animation Mode
.
-
Click the Deformed panel toolbar icon
.
- Set Result Type to Displacement(v).
-
Set Scale to Model units and enter a value of
10.
This means that the maximum displacement will be 10 model units and all other displacements will be proportional.
- Click Apply.
-
Set the toggle under Undeformed shape to Wireframe and
select Color as the Component.
A deformed plot of the model should be visible, overlaid on the original undeformed mesh.
View Deformed Animation of Loading Displacement
-
Verify that the Animate Mode is set to Linear Animation Mode
.
-
Click the Start/Pause Animation icon
to start the animation.
Note: Both the play speed and starting point of the animation can be controlled using the Animation Controls. -
With the animation running, use the lower slider bar in the Animation Controls
panel to adjust the speed of the animation.
Figure 8.
- Click the Start/Pause Animation icon, again, to stop the animation.
View a von Mises Stress Contour
-
On the Results toolbar, click
to open the Contour panel.
- Select Element Stresses (2D & 3D) as the Result type.
- Verify that the stress type is set to vonMises.
-
Click Apply.
Notice the graphical display of stresses
-
Once you are finished viewing, select HyperView.
to exit Note: Beginning with 8.0, there is a parameter PARAM, INREL, -2 that can activate inertia relief analysis without the need for a SUPORT/SUPORT1 entry. You can activate that parameter by clicking on the PARAM field on the Control Cards panel. In this tutorial, our intention was to show the steps in creating SUPORT1 cards; therefore the parameter was not used.
As an additional exercise, you could run this tutorial using the above mentioned parameter. In that case, you would not create SUPORT1 cards or choose that load collector in the subcase.