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

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

•	Setting up the problem in HyperMesh

•	Submitting the job

•	Viewing the results (HyperMesh and HyperGraph)

The following file found in the optistruct.zip file is needed to perform this tutorial. Refer to Accessing the Model Files.

direct_response_flat_plate_input.fem

Original ASCII OptiStruct input deck

Exercise

Step 1: Launch HyperMesh and set the OptiStruct User Profile

1.	Launch HyperMesh. A User Profiles dialog appears.

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.

Step 2: Import the Finite Element Model File

1.	Click File > Import > Solver Deck. An Import tab is added to your tab menu.

2.	For the File type:, select OptiStruct.

3.	Select the Files icon . A Select OptiStruct File browser opens.

4.	Select the direct_response_flat_plate_input.fem file from the optistruct.zip file. Refer to Accessing the Model Files.

5.	Click Open > Import.

6.	The direct_response_flat_plate_input.fem OptiStruct input file is loaded into the current HyperMesh session.

7.	Click Close to exit the tab.

Setting up the Problem in HyperMesh (Steps 3 - 11)

Step 3: Apply Loads and Boundary Conditions to the Model

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.

1.	Click the Model tab.

2.	In the Model browser, right-click and select Create > Load Collector.

3.	For Name, enter spcs.

4.	Click Color and select a color from the color palette.

5.	Set the Card Image to None. A new load collector, spcs is created.

6.	In the Model browser, right-click and select Create > Load Collector.

7.	For Name, enter unit-load.

8.	Click Color and select a different color from the color palette. A new load collector, unit-load is created.

Step 4: Create Constraints

1.	In the Model browser, expand Load Collector, right-click spcs > Make Current.

rd2000_spc_load_collector

2.	Click the Display Numbers icon .

3.	Click nodes >> displayed.

4.	Select on (green button). All of the node numbers on the flat plate should now be displayed.

5.	Click return to get to the main menu.

6.	Click BCs > Create > Constraints to open the Constraints menu.

7.	Click the entity selection switch and select nodes from the pop-up menu.

8.	Click nodes and select nodes 5, 29, 30, 31 and 32 (see figure).

os1100_pic1

Illustration of which nodes to select for applying single point constraints

9.	Constrain dof1, dof2, dof3, dof4 and dof5.

DOFs with a check will be constrained, while dofs without a check will be 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.

You need only to uncheck dof6.

10.	Click create. The selected nodes will be free to rotate about the z-axis since dof6 was not checked.

11.	Click return to return to the main menu.

Step 5: 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.	From the Analysis page, click load types.

3.	Select constraint = and select DAREA from the extended entity selection menu.

4.	Click return to exit the Load Types panel.

5.	Click BCs > Create > Constraints to open the Constraints menu.

6.	Select node number 19 on the plate by clicking on it (see figure).

os1100_pic2

Node selected for creating unit vertical load.

7.	Uncheck all the dof's; except dof3, and click the = to the right of dof3 and enter a value of 20.

8.	Click load types= and verify that DAREA is selected from the extended entity selection menu.

9.	Click create, and then click return.

Step 6: Create a Frequency Range Table

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter tabled1.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select TABLED1 from the drop-down menu.

5.	For TABLED1_NUM, input a value of 2 and press Enter.

6.	Click the Table icon below TABLED1_NUM and enter x(1) = 0.0, y(1) = 1.0, x(2) = 1000.0 and y(2) = 1.0 in the pop-out window.

7.	Click Close. This provides a frequency range of 0.0 to 1000.0 with a constant 1.0 over this range.

Step 7: Create a Frequency Dependent Dynamic Load

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter rload2.

3.	Click Color and select a color from the color palette.

4.	For Card Image, and select RLOAD2 from the drop-down list.

5.	For EXCITEID, click Unspecified > Loadcol.

6.	In the Select Loadcol dialog, select unit-load from the list of load collectors and click OK to complete the selection.

7.	Similarly select the tabled1 load collector for the TB field.

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.

Step 8: Create a Set of Frequencies to be used in 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.	Check the FREQ1 option and enter 1 in the NUMBER_OF_FREQ1 field.

6.	Click and enter F1= 20.0, DF = 20.0, NDF = 49, in the pop-out window.

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

Step 9: Create an OptiStruct Loadstep (also referred to as a subcase)

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, select spcs from the Select Loadcol pop-out window.

5.	For DLOAD, select rload2 from the Select Loadcol pop-out window.

6.	For FREQ, select freq1 from the Select Loadcol pop-out window.

An OptiStruct subcase has been created which references the constraints in the load collector spc and the unit load in the load collector rload2 with a set of frequencies defined in load collector freq1.

Step 10: Create a Set of Nodes for Output of Results

1.	In the Model browser, right-click and select Create > Set.

2.	For Name, enter SETA.

3.	For Card Image, select None.

4.	Leave the Set Type switch set to non-ordered type.

5.	For Entity IDs, select Nodes from the selection switch.

6.	Click Nodes and select nodes with IDs 15, 17 and 19.

7.	Click proceed.

Step 11: Create a Set of Outputs and Mass Factors Specific to Frequency Response Analysis

1.	Click Setup > Create > Control Cards to open the Control Cards panel.

2.	Select GLOBAL_OUTPUT_REQUEST and check the box next to DISPLACEMENT.

3.	Under FORM(1), select PHASE from the pop-up menu.

4.	Under OPTION(1), select SID from the pop-up menu. A new field appears in yellow.

5.	Double-click the SID(1) box and select SETA.

A value of 1 now appears below the SID field box. This sets the output for only the nodes in set 1.

rd2000_displacement

6.	Click return to exit the GLOBAL_OUTPUT_REQUESTS menu.

7.	From the Control Cards panel, select FORMAT. A new window appears in the work area screen.

8.	Click number_of_formats = and input a value of 2.

9.	On the extended menu in the work area, click on the first FORMAT_V1 field box and select OPTI from the pop-up menu.

Using OPTI generates OptiStruct ASCII result files like .disp, .strs, etc. as the output once the run is complete. These files are used during post-processing.

10.	Make sure the second field box is set to H3D.

11.	Click return to exit the Format menu and return to the Control Cards menu.

12.	Click next and select the PARAM subpanel.

13.	Scroll down the list using the arrow in the left corner and check the box next to COUPMASS. A new PARAM card appears in the work area screen.

14.	Click NO below COUPM_V1 and select YES from the pop-up menu selection.

Selecting YES uses the coupled mass matrix approach for eigenvalue analysis.

15.	Scroll down the list using the arrow in the left corner and check the box next to G. A new PARAM card appears in the work area screen.

16.	Click below G_V1 and input a value of 0.06 into the field box.

This value specifies a uniform structural damping coefficient and is obtained by multiplying the critical damping [] ratio by 2.0.

17.	Scroll down using the arrow in the left corner and check the box next to WTMASS.

A new window appears in the work area screen.

18.	Click below WTM_V1 and input a value of 0.00259 into the field box. Three PARAM statements now appear in the pop-up menu on the work screen.

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.

rd2000_param

19.	Click return to exit the PARAM menu.

20.	Select the OUTPUT subpanel.

21.	Verify that KEYWORD is set to HGFREQ.

Using HGFREQ results in a frequency output presentation for HyperGraph.

22.	Click on the box beneath FREQ and select ALL from the pop-up selection to choose all outputs results for all frequencies.

23.	Leave number_of_outputs set equal to 1.

24.	Click return to exit OUTPUT.

25.	Click return to exit the Control Cards panel.

Submitting the Job

Step 12: Run OptiStruct

1.	From the Analysis page, click OptiStruct.

2.	Click save as.

3.	Select the directory where you would like to write the OptiStruct model, enter the name flat_plate_direct_response.fem for the model in the File name: field, and click Save.

4.	Set the run options: toggle to analysis.

5.	Click OptiStruct. This launches the OptiStruct job.

If the job is successful, new result files can be seen in the director where the OptiStruct model file was written. The flat_plate_direct_response.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

The default files written to the directory are:

flat_plate_direct_response.html	HTML report of the analysis, giving a summary of the problem formulation and the analysis results.
flat_plate_direct_response.out	OptiStruct output file containing specific information on the file set up, the set up 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 the analysis process.

Viewing the Results (HyperMesh and HyperGraph)

Step 13: 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.	Click HyperView to launch HyperView.

2.	Click Close to close the Message Log window, if one appears.

3.	In the HyperView window, click File > Open > Session. The Open Session File window is displayed.

4.	Select the directory where the job was run and select the file flat_plate_direct_response_freq.mvw.

5.	Click Open.

6.	A warning appears asking whether to discard the existing contents. Click Yes.

Two graphs per page and a total of three pages are displayed.

The graph title shows Subcase 1 Displacement of grid 15 on page 1.

There are two sets of results on this page. The top graph shows Phase Angle verses Frequency (log). The bottom graph shows Magnitude versus Frequency (log) (see figure) for Displacement of grid 15.

rd2000_results

Frequency response of node 15.

7.	Click the Next Page icon .

This displayed page 2, which shows Subcase 1 (subcase1) - Displacement of grid 17 (see figure).

rd2000_results2

Frequency response of node 17.

8.	Select the Next Page icon again to display page 3 containing Subcase 1 (subcase1) - Displacement of grid 19 (see figure).

rd2000_results3

Frequency response of node 19.

This concludes the HyperGraph results processing.

9.	Open the displacement file (.disp) using a text editor.

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

Line 3, first field shows node number, then x, y, and z displacement magnitudes and x, y and z rotation magnitudes.

Line 4, first field shows node number, then x, y, and z displacement phase angles and x, y and z rotation angles.