Exercise 1: Linear Gap Analysis

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 rib.hm file you saved to your working directory.
  3. Click Open.
    The rib.hm database is loaded into the current HyperMesh session, replacing any existing data.

Create a Cylindrical Coordinate System

For gap elements with coincident nodes as is the case here, the gap coordinate system MUST be specified. For detailed information, refer to the Help section on CGAP.
  1. In the Model Browser, right-click and select Create > System Collector.
  2. For Name, enter cylindrical.
  3. Click Color and select a color from the color palette.
  4. In the Model Browser, hide all load collectors by right-clicking on Load Collector > Hide.
  5. In the Model Browser, click the Isolate Shown icon .
  6. Expand the Component list and select the Lug component.
    This isolates the display of only the Lug component.
  7. Click the XY Top Plane View icon viewAxisOrientationYXTop-24 to set the model view.
  8. Click Geometry > Create > Systems > Axis Direction to open the Systems panel.
  9. The cyan halo around the yellow nodes button indicates that it is the current option. Select the center node on the upper lug.
  10. Click origin and select the center node again.
  11. Click x-axis and select any node on the circumference.
  12. For xy plane, select any node on the plane of the lug, as shown in Figure 1:
    Figure 1. Nodes to Select for Creating Cylindrical Coordinate System

  13. Click the switch beside rectangular and select cylindrical.
  14. Click create.
    For cylindrical systems, the x-axis defines the radial direction (q= 0) and the xy plane defines the r-q plane.
  15. Repeat this process for the bottom lug (steps 9 through 12 of this sequence).
  16. Click return.
  17. Click on the Model Browser.
  18. Select only the gap component.
    With Isolate Shown still active this displays only the gap component.
  19. Click the Card Editor icon entityCards-24.
  20. Click the entity selection switch on the top left of the panel and select elems.
  21. Click elems >> by window from the pop-up menu.
  22. Select the gap elements that are connected to the top lug, as shown in Figure 2.
    Figure 2. Gap Elements Connected to Top Lug

  23. Click select entities.
  24. Click config= and select gap from the pop-up menu.
  25. Click edit.
  26. Click CID, and select the system that was created at the center of the top lug, as shown below.
    Figure 3.

  27. Click return twice to go back to the main menu.
  28. Repeat this process for the gap elements that are connected to the bottom lug.
    The gap elements have now been assigned with a cylindrical coordinate system.

Define a Property and Assign it to the Gap Elements

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter gap_prop.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select PGAP and click Yes to confirm.
  5. Make sure the check box next to U0_opts is checked. This way the initial gap opening is calculated automatically.
  6. Make sure the check box next to KA_opts is checked. This determines the value of KA for each gap element using the stiffness of surrounding elements automatically.
    Figure 4.

  7. Click Mesh > Create > 1D Elements > Gaps to open the Gaps panel.
  8. Select the update subpanel.
  9. Click elems >> by collector.
  10. Select gap by checking the box beside it.
  11. Click the green select button.
  12. Click property= and click on gap_prop.
  13. Click update.
  14. Check beside property.
  15. Click update.
    The gap elements have now been updated to the new property collector.
  16. Click return.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.
    Figure 5. Accessing the OptiStruct Panel

  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter rib_linear 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 rib_linear.fem was written. The rib_linear.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:
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
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.
HyperView binary results file.
HyperMesh binary results file.
Summary, providing CPU information for each step during analysis process.

Post-process the Results

  1. From the OptiStruct panel, click HyperView.
    This will launch HyperView and load the rib_linear.mvw file, reading the model and results.
  2. Click the Curves Attributes icon palette-24 and hide all components except the Web component.
    1. Activate the Auto apply mode check box
    2. Click on the components to turn off in the modeling window
    Figure 6.

  3. Go to the Contour panel resultsContour-16.
  4. Select the first pull-down menu below Result type and select Element Stresses (2D & 3D).
  5. Select the second pull-down menu below Result type and select vonMises.
  6. Above the Results Browser in the left hand panel are the Load Case and Simulation Selection drop-down menus. Select Subcase 1 (Coup_Vert) from the Load Case drop-down menu.
    Figure 7.

  7. Click the XY Top Plane View icon viewAxisOrientationYXTop-24 to display a top view of the Web.
  8. Click Apply.
    This should show the contour of stresses on the Web component under the coupled loading.
    Figure 8. Stress Results on the Web From Linear Gap Analysis

  9. Click Delete Page pageDelete-24 to end the HyperView session.