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.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Figure 1 illustrates the structural model used for this tutorial.


3d-inertia-1
Figure 1. Structural Model with Static Loads and Support Constraints Applied

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. 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

  1. Click File > Open > Model.
  2. Select the ie_carm.hm file you saved to your working directory.
  3. 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

  1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
    A default load collector displays in the Entity Editor.
  2. For Name, enter static_loads.
  3. Click Color and select a color from the color palette.
  4. Set Card Image to None.
    A new load collector, static_loads is created.


    Figure 2. Creating the static_loads Load Collector
  5. Create another load collector.
    1. For Name, enter SPCs.
    2. For Card Image, select None.

Create SUPORT1 Constraint

  1. From the menu bar, click BCs > Create > Constraints to open the Constraints panel.
  2. Create constraint 1.
    1. Set the entity selector to nodes, then select the node that sits in the middle of the multi-node rigid on the foremost attachment point of the control arm to the chassis.
      This can be seen in Figure 3 as 1st constraint.

      rd1030_constraint_bc
      Figure 3. Nodes to Select for Constraint Boundary Conditions
    2. Deselect the degrees of freedom dof4 through dof6 by right-clicking to uncheck each box.
    3. Set load types = to SUPORT1.
      The load type is modified to perform inertia relief analysis.
    4. Click create.
  3. Create constraint 2.
    1. Using the entity selector, select the node and the rearward attachment point of the control arm of the chassis.
      This can be seen in Figure 3 as 2nd constraint.
    2. Deselect dof1.
    3. Click create.
  4. Create constraint 3.
    1. Using the entity selector, select the top node in the rigid which would fasten the bottom of the shock assembly to the control arm.
      Tip: Switch to the Wireframe Elements Skin Only mode by clicking on the visualizationElementsWireframeSkinOnly-24 icon to view the rigid.
    2. Deselect dof2.
    3. Click create.

    rd1030_constraint_control_arm
    Figure 4. Final Constraint Applied to Control Arm Model
  5. Click return to exit the panel.

Create Static Forces

  1. In the Model Browser, Load Collectors folder, right-click on static_loads and select Make Current to set it as the current load collector.
  2. From the menu bar, click BCs > Create > Forces to open the Forces panel.
  3. Create force 1.
    1. Set the entity selector to nodes, then select the node on the top of the rigid at the end of the control arm.
      This can be seen in Figure 5.
    2. In the magnitude= field, enter -1e+05.
    3. Set the direction selector to x-axis.
    4. Click create.
  4. Create force 2.
    1. Set the entity selector to nodes, then select the node on the top of the rigid at the end of the control arm.
      This can be seen in Figure 5.
    2. In the magnitude= field, enter 3e+05.
    3. Set the direction selector to z-axis.
    4. Click create.
  5. Click return and to exit the panel.

3d-inertia-3
Figure 5. Application of Static Forces

Create Load Steps

  1. In the Model Browser, right-click and select Create > Load Step from the context menu.
  2. For Name, enter linear.
  3. Set Analysis type to Linear Static.
  4. Define LOAD.
    1. For LOAD, click Unspecified > Loadcol.
    2. In the Select Loadcol dialog, select static_loads and click OK.
  5. Define SUPORT1.
    1. For SUPORT1, click Unspecified > Loadcol.
    2. In the Select Loadcol 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.



Figure 6. Creating the linear Loadstep

Create Control Cards for Inertia Relief Analysis

  1. From the menu bar, click Setup > Create > Control Cards to open the Control Cards panel.
  2. 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.
  3. Click PARAM, and enable INREL.
  4. Under INREL_V1, toggle the selection to be -1.
    This requests that an inertia relief analysis be performed.
  5. Click return twice to go to the main menu.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.

    OS_1000_13_17
    Figure 7. Accessing the OptiStruct Panel
  2. Click save as.
  3. 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.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the ie_carm.fem was written. The ie_carm.out file is a good place to look for error messages that could help debug the input deck if any errors are present.
The default files written to the directory are:
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

  1. When the message ANALYSIS COMPLETED is received in the Solver View window, click Results.
    HyperView is launched and the results are loaded.
  2. Verify that the Animate Mode is set to Linear Animation Mode animationLinear-24.
  3. Click the Deformed panel toolbar icon resultsDeformed-24.
  4. Set Result Type to Displacement(v).
  5. 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.
  6. Click Apply.
  7. 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

  1. Verify that the Animate Mode is set to Linear Animation Mode animationLinear-24.
  2. Click the Start/Pause Animation icon animationStart-24 to start the animation.
    Note: Both the play speed and starting point of the animation can be controlled using the Animation Controls.
  3. With the animation running, use the lower slider bar in the Animation Controls panel to adjust the speed of the animation.

    animation_toolbar
    Figure 8.
  4. Click the Start/Pause Animation icon, again, to stop the animation.

View a von Mises Stress Contour

  1. On the Results toolbar, click resultsContour-16 to open the Contour panel.
  2. Select Element Stresses (2D & 3D) as the Result type.
  3. Verify that the stress type is set to vonMises.
  4. Click Apply.
    Notice the graphical display of stresses
  5. Once you are finished viewing, select File > Exit to exit HyperView.
    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.