OS-HM-T:1305 モーダル法による平板の周波数応答解析

チュートリアルレベル：初級本チュートリアルでは、既存の平板のFEモデルを読み込み、境界条件を与え、モーダル周波数応答解析を実行する方法について実際に示します。

開始する前に、このチュートリアルで使用するファイルを作業ディレクトリにコピーします。

平板は、モーダル法での周波数が変化する単位荷重の加振を受けます。ポスト処理では、HyperViewとHyperGraphでモードシェイプの応答と、周波数-位相の出力特性の可視化が行われます。

以下の演習が含まれます：
  • HyperMeshでの問題のセットアップ
  • ジョブのサブミット
  • HyperViewとHyperGraphでの結果確認

Launch HyperWorks

  1. Launch Altair HyperWorks.
  2. In the New Session window, select HyperMesh from the list of tools.
  3. For Profile, select OptiStruct.
  4. Click Create Session.
    図 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 modal_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.
    図 2. Solver Import Options


  5. Accept the default settings and click Import.

モデルのセットアップ

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.
    ヒント: 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. Colorをクリックし、カラーパレットから色を選択します。
  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 図 3.
    図 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. Closeをクリックします。
    図 4. Constrained Nodes


    ヒント: 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, double click on Collectors.
  2. Right-click on the load collector unit-load and select Make Current.
  3. On the Analyze ribbon, click Constraints.
  4. For Entities, select Nodes.
  5. Select the node at the lower right corner of the plate.
  6. Click to confirm the selection.
  7. Ensure the DOF3 check box remains selected and deselect all other DOFs.
  8. For DOF3, enter 1.
  9. For Load Type, select DAREA.
  10. Click Create.
    This applies a unit load to the selected node.
  11. Closeをクリックします。
    図 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. Closeをクリックします。

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. Colorをクリックし、カラーパレットから色を選択します。
  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. Closeをクリックします。

Create the Modal Method for Eigenvalue Analysis

Complete this step using the Lanczos method and specify the frequency range for eigenvalue extraction.

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter eigrl.
  3. Colorをクリックし、カラーパレットから色を選択します。
  4. For Config type, select Real eigen value extraction.
  5. For Type, select EIGRL.
  6. For V1, enter 0.0. For V2, enter enter 1000.0.
    This specifies a range of frequency between 0 Hz and 1000 Hz for eigenvalue extraction using the Lanczos method.
  7. Closeをクリックします。

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 (modal) from the drop-down menu.
  4. For METHOD(STRUCT) select Unspecified.
  5. Click the search tool.
  6. Select eigrl.
  7. Similarly, for SPC, select spcs.
  8. For DLOAD, select rload2.
  9. For FREQ, select FREQ1.
    This creates an OptiStruct subcase that references the constraints in the spc load collector, the unit load in the rload2 load collector with a set of frequencies defined in the freq1 load collector, and modal method defined in the eigrl load step input.

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. Closeをクリックします。

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. Click the search tool.
  7. Select SETA.
    (1)SETA now appears in the SID field. This sets the output for only the nodes in SETA.
  8. Click Close.
  9. In the Model Browser, right-click on Cards and select Create > PARAM.
  10. Scroll down and select the COUPMASS check box.
  11. For COUPM_V1, select YES.
    With this setting, the coupled mass matrix approach for eigenvalue analysis is used.
  12. Scroll down and select the G check box.
  13. For G_V1, enter 0.06.
    This value specifies a uniform structural damping coefficient and is obtained by multiplying the critical damping [C/C0] ratio by 2.0.
  14. Scroll down and select the WTMASS check box.
  15. For WTM_V1, enter 0.00259 and click Close.
  16. In the Model Browser, right-click on Cards and select Create > OUTPUT.
  17. In the number_of_outputs field, type 3 and press Enter.
    Three output KEYWORDs with OPTIONs appear.
  18. For the first KEYWORD, select HGFREQ.
    Using HGFREQ results in a frequency output presentation for HyperGraph.
  19. For FREQ under OUTPUT 1, select ALL.
  20. Set the second KEYWORD to OPTI.
  21. For FREQ under OUTPUT 2, select ALL.
  22. Set the third KEYWORD to H3D.
  23. For FREQ under OUTPUT 3, select ALL.
  24. Click Close.

Submit the Job

Run OptiStruct.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    図 6. Select Run OptiStruct Solver


    A browser window opens.
  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter flat_plate_modal_response.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. Click Export.
  6. For run options, toggle .
  7. Click Run.
    If the job is successful, you should see new results files in the directory in which flat_plate_modal_response.fem was run. The flat_plate_modal_response.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

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_modal_response_freq.mvw.
    図 7. 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.
    図 8. 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.
    図 9. 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.
    図 10. 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.