OS-HM-T: 1300 Direct Frequency Response Analysis of a Flat Plate

Tutorial Level: Beginner This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a finite element analysis on a flat plate.

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

The flat plate is subjected to a frequency-varying unit load excitation using the direct method. Post-processing is done in HyperView and HyperGraph to visualize deformations, mode shape response, and frequency-phase output characteristics.

The following exercises are included:
  • Set up the problem in HyperMesh
  • Submit the job
  • View the results in HyperView and HyperGraph

Launch HyperMesh

  1. Launch HyperMesh.
  2. In the New Session window, select HyperMesh from the list of tools.
  3. For Profile, select OptiStruct.
  4. Click Create Session.
    Figure 1. Create New Session


    This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

Import the Model

  1. On the menu bar, select File > Import > Solver Deck.
  2. In the Import File window, navigate to and select direct_response_flat_plate_input.fem you saved to your working directory.
  3. Click Open.
  4. In the Solver Import Options dialog, ensure the Reader is set to OptiStruct.
    Figure 2. Import Base Model in HyperMesh


  5. Accept the default settings and click Import.
    Tip: Alternatively, you can drag and drop the file from your file browser into the application window to open the model file.

Set Up the Model

Apply Loads and Boundary Conditions

In the following steps, the model is constrained at one edge. A unit vertical load is applied acting upwards in the positive z-direction at a point on a free edge corner of the plate.

First, the two load collectors (spcs and unit-load) are created.

  1. Click the Model tab to view the Model Browser.
    Tip: If you don’t see a Model Browser tab, you can open it by clicking View > Model Browser on the menu bar.
  2. In the Model Browser, right-click and select Create > Load Collector.
  3. For Name, enter unit-load.
  4. Click Color and select a color from the color palette.
  5. Set the Card Image to None.
    A new load collector, unit-load, is created.
  6. In the Model Browser, right-click and select Create > Load Collector.
  7. For Name, enter spcs.
  8. Click Color and select a different color from the palette.
  9. Set the Card Image to None.
    A new load collector, spcs, is created.

Create Constraints

  1. On the Analyze ribbon, select Constraints.
  2. For Entities, select Nodes.
  3. Left click and drag a small box over the left end of the plate (as in Top view) to select the 5 nodes as shown in Figure 3.
    Figure 3. Node selection


  4. Click to confirm the selection.
  5. In the Constraints dialog, clear the DOF6 check box and ensure all other DOF check boxes remain selected.
    The selected DOFs are constrained while unselected DOFs are free. DOFs 1, 2, and 3 are x, y and z translation degrees of freedom. DOFs 4, 5, and 6 are x, y and z rotational degrees of freedom.
  6. Click Create.
    The selected nodes are free to rotate about the z-axis since DOF6 was not selected.
  7. Click Close.
    Figure 4. Constrained Nodes


    Tip: To increase the size of the spc markers, click File > Preferences. Under HyperMesh, select , Appearance and increase the Size value for Boundary Conditions. To see the DOF labels, select Labels for Boundary Condition and Show load handle for Loads. Click OK.

Create a Unit Load at a Point on the Flat Plate

  1. In the Model Browser, right-click on the load collector unit-load and select Make Current.
  2. On the Analyze ribbon, click Excitations.
  3. For Type, select DAREA.
  4. Next to GSETID, click the hamburger menu and select Create.
  5. For Entities, verify selection is set to Nodes.
  6. Click Nodes > to open Advanced Selection.
  7. Select By ID.
  8. In the text box, enter, 19 and click OK.
  9. For Constraint Type, select DOF3 from the extended entity selection menu.
  10. For Am, enter 20.
  11. Click Close.
    Figure 5. Node Selection for Unit Vertical Load


Create a Frequency Range Table

  1. In the Model Browser, right-click and select Create > Curve.
  2. A new Curve Editor window opens.
  3. For name, enter tabled1.
  4. In the table, enter the following:
    x(1) = 0.0

    y(1) = 1.0

    x(2) = 1000.0

    y(2) = 1.0

  5. Close the window.
  6. In the Model Browser, double-click Curves.
  7. Select tabled1 to open the card.
  8. For Card Image, select TABLED1 from the drop-down menu.
  9. This provides a frequency range of 0.0 to 1000.0 with a constant 1.0 over this range.

Create a Frequency Dependent Dynamic Load

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter rload2.
  3. For Config Type, select Dynamic Load-Frequency Dependent from the drop-down list.
  4. For Type, select RLOAD2.
  5. For EXCITEID, click Unspecified.
    The load collector appears.
  6. Click the search tool.
  7. Select unit-load from the list of load collectors.
  8. Similarly, for TB, select the tabled1 curve.
    The type of excitation can be an applied load (force or moment), an enforced displacement, velocity or acceleration. The field Type in the RLOAD2 card image defines the type of load. The type is set to applied load by default.
  9. Click Close.

Create a Set of Frequencies for the Response Solution

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter freq1.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select FREQi from the drop-down menu.
  5. Select the FREQ1 option and verify the NUMBER_OF_FREQ1 field is set to 1.
  6. If needed, click and enter:
    F1 = 20.0

    DF = 20.0

    NDF = 49

    This provides a set of frequencies beginning at 20.0 incremented by 20.0 with 49 frequency increments.
  7. Click Close.

Create a Load Step

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter subcase1.
  3. For Analysis type, select Freq. resp (direct) from the drop-down menu.
  4. For SPC, open Advanced Selection and choose spcs from the dialog.
  5. Click OK.
  6. Similarly, for DLOAD, select rload2.
  7. For FREQ, select FREQ1.
    This creates an OptiStruct subcase that references the constraints in the spc load collector and the unit load in the rload2 load collector with a set of frequencies defined in the freq1 load collector.
  8. Click Close.

Create a Set of Nodes for Results Output

  1. In the Model Browser, right-click and select Create > Set.
  2. For Name, enter SETA.
  3. For Card Image, select Set_Grid from the drop-down menu.
  4. Verify Set Type is set to non-ordered type.
  5. For Entities, click Elements to expand the selection.
  6. Click Nodes.
  7. Select the By ID option and enter 15, 17, 19 in the text box.
  8. Click OK.
  9. Click Close.

Create a Set of Outputs and Mass Factors for Frequency Response Analysis

  1. In the Model Browser, right-click and select Create > Cards > Output.
  2. In the new window, select the DISPLACEMENT check box.
  3. In the DISPLACEMENT options, for FORM, select PHASE.
  4. For OPTION, select SID from the drop-down menu.
  5. For SID, click Unspecified.
  6. For Set, click Unspecified > to open Advanced Selection.
  7. In the dialog, select the By List option and choose SETA.
  8. Click OK.
    (1)SETA now appears in the SID field. This sets the output for only the nodes in SETA.
    Figure 6. Output for Nodes in SETA


  9. Click Close.
  10. In the Model Browser, right-click on Cards and select Create > More > FORMAT.
  11. In the new window, for number of formats, type 2 and press Enter.
  12. Next to Data Format_V1, click the table icon.
  13. Select OPTI for 1 and H3D for 2.
    Using OPTI generates OptiStruct ASCII result files like .disp, .strs, and so on once the run is complete. These files are used during post-processing.
  14. Click Close.
  15. In the Model Browser, right-click on Cards and select Create > PARAM.
  16. Scroll down and select the COUPMASS check box.
  17. For COUPM_V1, select YES.
    With this setting, the coupled mass matrix approach for eigenvalue analysis is used.
  18. Scroll down and select the G check box.
  19. For G_V1, enter 0.06.
    This value specifies a uniform structural damping coefficient and is obtained by multiplying the critical damping ratio by 2.0.
  20. Scroll down and select the WTMASS check box.
  21. For WTM_V1, enter 0.00259.
    This factor is used to input all mass entries in weight units. Using this PARAM multiplies all terms in the mass matrix by this factor.
  22. Click Close.
  23. In the Model Browser, right-click on Cards and select Create > OUTPUT.
  24. For KEYWORD, select HGFREQ.
    Using HGFREQ results in a frequency output presentation for HyperGraph.
  25. For FREQ, select ALL to choose all output results for all frequencies.
  26. Verify number_of_outputs is set to 1.

Submit the Job

Run OptiStruct.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    Figure 7. Select Run OptiStruct Solver


  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter flat_plate_direct_response.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. Click Export.
  6. For export options, toggle all.
  7. In the Altair Compute Console, click Run.
    If the job is successful, an "OptiStruct Job Completed" message appears in the Compute Console Solver View Message Log. New results files are in the directory where the model file was written. The flat_plate_direct_response.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 your directory are:
    flat_plate_direct_response.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.
    flat_plate_direct_response.h3d
    HyperView compressed binary results file.
    flat_plate_direct_response.stat
    Summary of analysis process, providing CPU information for each step during process.

Review the Results

This step describes how to view displacement results (.mvw file) in HyperGraph and also explains the displacement output (.disp file) from this run. The HyperView results (.h3d file) contains only the displacement results for the three nodes specified in the node set output.

  1. In the Compute Console Solver View window, click View.
  2. From the pull-down list, choose flat_plate_direct_response_freq.mvw.
    Figure 8. View Menu


    HyperGraph opens with the .mvw file loaded. The results for Subcase 1 (subcase 1) - Displacement of grid 15 are displayed.
    There are two sets of results on this page. The top graph shows Phase Angle verses Frequency. The bottom graph shows Magnitude versus Frequency.
    Figure 9. Frequency Response of Node 15


  3. In the Entities list, double click on p2 Subcase 1 (subcase1) - Displacement of grid 17 to see the graphs for displacement of grid 17.
    Figure 10. Frequency Response of Node 17


  4. Double click on Subcase 1 (subcase1) - Displacement of grid 19 to see the graphs for displacement of grid 19.
    Figure 11. Frequency Response of Node 19


    This concludes the HyperGraph results processing.

    The first field on the second line shows the iteration number, the second field shows number of data points, and the third field shows iteration frequency.

    The $DISP [MAG/PHASE] table shows node number, then x, y and z displacement magnitudes and x, y and z rotation magnitudes.

    In the line below the displacement magnitudes for each node, the x, y and z displacement phase angles and x, y and z rotation phase angles are listed.