OS-T: 1040 3D Buckling Analysis

In this tutorial the steps required to perform a buckling analysis using OptiStruct are covered.

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.
Figure 1. Structural Model with Static Loads and Constraints Applied

1040_model

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

Apply Loads and Boundary Conditions

Create Load Collectors

Create two load collectors (SPC and Static load).
  1. Create the SPC load collector.
    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 SPC.
    3. Click Color and select a color from the color palette.
  2. Create another load collector named Static load.

Create Load Step Inputs

Create the load step input.
  1. In the Model Browser, right-click and select Create > Load Step Inputs from the context menu.
  2. For Name, enter Buckling load.
  3. For Config type, select Real Eigen value extraction.
  4. For Type, select EIGRL.
  5. For V1, enter 0.0.
  6. For ND, enter 2.
    This tells OptiStruct that you would like to extract the first two buckling modes.
Figure 2.


Create Loads and Boundary Conditions

  1. In the Model Browser, Load Collector folder, right-click on SPC and select Make Current from the context menu.
    Figure 3.

    rd_loadcollector_panel_11
  2. From the menu bar, click BCs > Create > Constraints to open the Constraints panel.
  3. Select all of the nodes on the bottom face of the beam.
    1. Click nodes > on plane.
    2. Verify that the N1 selector is active, then click any three nodes on the plane.
    3. Click select entities.
    All of the nodes on the plane are selected.
    Figure 4.

    104_nodes_const
  4. Deselect the degrees of freedom dof4 through dof6.
  5. Click create to create the necessary boundary constraints.
  6. Click return.
  7. In the Model Browser, Load Collector folder, right-click on Static load and select Make Current from the context menu.
  8. From the menu bar, click BCs > Create > Forces to open the Forces panel.
  9. Select all of the nodes on the top face of the beam.
    Figure 5. Nodes Selected for Application of Static Forces

    1040_nodes_static
  10. In the magnitude= field, enter -10000.
  11. Set the direction selector to z-axis.
  12. Click create.
    The forces display in the modeling window.
  13. Click return.

Create a Load Step

The last step in establishing boundary conditions is the creation of a subcase.
  1. Create the Linear load step.
    1. In the Model Browser, right-click and select Create > Load Step from the context menu.
      A default load step displays in the Entity Editor.
    2. For Name, enter Linear.
    3. Set Analysis type to Linear Static.
    4. For SPC, click Unspecified > Loadcol.
    5. In the Select Loadcol dialog, select SPC and click OK.
    6. For LOAD, click Unspecified > Loadcol.
    7. In the Select Loadcol dialog, select Static load and click OK.
    Figure 6.

    OS_1040_02
  2. Create the Buckling load step.
    1. In the Model Browser, right-click and select Create > Load Step from the context menu.
      A default load step displays in the Entity Editor.
    2. For Name, enter Buckling.
    3. Set Analysis type to Linear buckling.
    4. For METHOD(STRUCT), click Unspecified > Load Step Inputs.
    5. In the Select Load Step Inputs dialog, select Buckling load and click OK.
    6. For STATSUB(BUCKLING), click Unspecified > Loadcol.
      A STATSUB card allows for the selection of a linear static subcase for buckling analysis.
    7. In the Select Loadcol dialog, select Linear and click OK.
    Figure 7.

    OS_1040_03

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.
    Figure 8. Accessing the OptiStruct Panel

    OS_1000_13_17
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter buckling 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 buckling.fem was written. The buckling.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:
buckling.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
buckling.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.
buckling.h3d
HyperView binary results file.
buckling.res
HyperMesh binary results file.
buckling.stat
Summary, providing CPU information for each step during analysis process.

View the Results

OptiStruct gives you contour information for all of the loadsteps that were run. This section describes the process for viewing those results in HyperView.

View Linear Load Step Results

  1. From the OptiStruct panel, click the HyperView icon.
    HyperView launches with the buckling.hm file which contains the model and the results.
  2. Use the drop-down Subcase selector to change the analysis that you are reviewing in the current window.
    Figure 9.

    1040_subcase_analysis
  3. In the Results Browser, select Subcase 1 - Linear.
  4. On the Results toolbar, click resultsContour-16 to open the Contour panel.
  5. Select Element Stresses (2D and 3D) as the Result type and set the sub type to von Mises.
  6. Click Apply.
    This should show the contour of von Mises stress.

View Buckling Load Step Results

  1. Click Clear Contour from the Result display control panel.
  2. In the Results Browser, click Subcase 2 - Buckling and make sure the simulation is for Mode 1.
  3. Click the Deformed panel toolbar resultsDeformed-24.
  4. Under Deformed shape, enter a value of 10.
  5. Under Undeformed shape, for Show, select Wireframe from the drop-down list.
    Figure 10.

    rd1040_wireframe_11A
  6. Click the Start/Pause Animation icon animationStart-24 to view the animation.
  7. Similarly, check the results for the 2nd mode.