Exercise 2: Nonlinear Gap Analysis

Create a Load Collector Defining Parameters

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter nonlinear.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select NLPARM from the menu.
  5. Click NINC and enter 10.
    NINC denotes the number of load sub-increments. If NINC is blank, then the entire loading is applied at once. An NINC of 10 signifies that the load will be sub-divided into 10 equal increments.
  6. Click MAXITER and leave the default value of 25.
  7. The error tolerances EPSU, EPSP, and EPSW can be left at their default values.
    For details on these tolerances, read the section Nonlinear Quasi-static Gap and Contact Analysis in the online help.

    os_1320_04
    Figure 1.

Update the Load Steps

  1. Open the Load Step folder in the Model Browser.
  2. Click the Coup_Vert load step to open the Entity Editor.
  3. For NLPARM, click Unspecified > Loadcol.
  4. In the Select Loadcol dialog, select the nonlinear load collector and click OK.

    os_1320_05
    Figure 2.
  5. Repeat this process for the Pressure load step.

Submit the Job

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

    OS_1000_13_17
    Figure 3. 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_nonlinear 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_nonlinear.fem was written. The rib_nonlinear.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:
rib_nonlinear.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
rib_nonlinear.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.
rib_nonlinear.h3d
HyperView binary results file.
rib_nonlinear.res
HyperMesh binary results file.
rib_nonlinear.stat
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_nonlinear.h3d 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

    auto_apply
    Figure 4.
  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.

    rd2040_load_case
    Figure 5.
  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.

    1140results
    Figure 6. Stress Results on the Web From Nonlinear Gap Analysis
  9. Click Delete Page pageDelete-24 to end the HyperView session.