OS-T: 1305 Modal Frequency Response Analysis of a Flat Plate

This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a modal frequency response analysis on a flat plate.

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

modal_response_flat_plate_input.fem

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

Launch HyperMesh and Set the OptiStruct User Profile

Launch HyperMesh.
The User Profile dialog opens.
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.

Import the Model

Click File > Import > Solver Deck.
An Import tab is added to your tab menu.
For the File type, select OptiStruct.
Select the Files icon .
A Select OptiStruct file browser opens.
Select the modal_response_flat_plate_input.fem file you saved to your working directory.
Click Open.
Click Import, then click Close to close the Import tab.

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.

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter spcs.
Click Color and select a color from the color palette.
For Card Image, set to None.
A new load collector, spcs is created.
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter unit-load.
Click Color and select a color from the color palette.
A new load collector, unit-load is created.
Click the Display Numbers icon to open the Numbers panel.
Click nodes > displayed.
Check the box next to display.
Select the green on button.
All of the node numbers on the flat plate should now be displayed.

Create Constraints

In the Model Browser, right-click the load collector spcs and select Make Current.

Figure 1.
Click BCs > Create > Constraints to open the Constraints panel.
Click the entity selection switch and select nodes from the pop-up menu.
Click nodes and select nodes 5, 29, 30, 31 and 32 (see Figure 2).

Figure 2. Illustration of Nodes to Select for Applying Single Point Constraints
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.
Click create.
The selected nodes will be free to rotate about the z-axis since dof6 was not checked.
Click return to go back to the main menu.

Create a Unit Load at a Point on the Flat Plate

In the Model Browser, right-click on the load collector unit-load and select Make Current.
Click BCs > Create > Constraints to open the Constraints menu.
Select node number 19 on the plate by clicking on it (Figure 3).

Figure 3. Node Selected for Creating Unit Vertical Load
Uncheck all the dof's except dof3 and click the = to the right of dof3 and enter a value of 1.
Click load types= and verify that DAREA is selected from the extended entity selection menu.
Click create, and then click return.
The unit load is applied to the selected node.

Create a Frequency Range Table

In the Model Browser, right-click and select Create > Curve.
A new window opens.
For Name, enter tabled1.
In the table, enter x(1) = 0.0, y(1) = 1.0, x(2) = 1000.0, y(2) = 1.0.
Close the Curve Editor window.
From Curves, select tabled1.
For Type, select TABLED1 from the drop-down menu.
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

In the Model Browser, right-click and select Create > Load Step Inputs.
For Name, enter rload2.
For Config type, select Dynamic Load – Frequency Dependent from the drop-down list.
For Type, and select RLOAD2 from the drop-down list.
For Excited, click Unspecified > Loadcol.
In the Select Loadcol dialog, select unit-load from the list of load collectors and click OK to complete the selection.
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 load step input defines the type of load. The type is set to applied load by default.

Create a Set of Frequencies

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter freq1.
Click Color and select a color from the color palette.
For Card Image, select FREQi from the drop-down menu.
Check the FREQ1 option and enter 1 in the NUMBER_OF_FREQ1 field.
Update the following fields in the pop-out window.
1. For F1, enter 20.0.
2. For DF, enter 20.0.
3. For NDF, enter 49.
Click Close.
This provides a set of frequencies beginning with 20.0, incremented by 20.0 and 49 frequencies increments.

Create the Modal Method for Eigenvalue Analysis

In the Model Browser, right-click and select Create > Load Step Inputs.
For Name, enter eigrl.
Click Color and select a color from the color palette.
For Config type, select Real Eigen Value Extraction.
For Type, select EIGRL.
Click V1 and enter a value 0.0, then click V2 and enter a value of 1000.0.
This specifies a range of frequency between 0 Hz and 1000 Hz for eigenvalue extraction using the Lanczos method.

Create a Load Step

In the Model Browser, right-click and select Create > Load Step.
A default load step template is now displayed in the Entity Editor below the Model Browser.
For Name, enter subcase1.
For Analysis type, select Freq.resp (modal) from the drop-down menu.
For METHOD(STRUCT), select Unspecified > Load step inputs.
From the Select Load Step Inputs dialog, select eigrl.
For SPC, select Unspecified > Loadcol.
From the Select Loadcol dialog, select spcs.
For DLOAD, select rload2 from the Select Load Step Inputs pop-out window.
For FREQ, click Unspecified > Loadcol
From the Select Loadcol dialog, select freq1.
An OptiStruct subcase is created which references the constraints in the load collector spc, the unit load in the load step input rload2 with a set of frequencies defined in load collector freq1 and modal method defined in the load step input eigrl.

Create a Set of Nodes

In the Model Browser, right-click and select Create > Set.
For Name, enter SETA.
For Card Image, select None.
Leave the Set Type switch set to non-ordered type.
For Entity IDs, select Nodes from the selection switch.
Click Nodes and select nodes with IDs 15, 17 and 19.
Click proceed.

Create a Set of Outputs and Mass Factors

Click Setup > Create > Control Cards to open the Control Cards panel.
Select GLOBAL_OUTPUT_REQUEST and check the box next to DISPLACEMENT.
Click the field box FORM(1) and select PHASE from the pop-up menu.
Click the field box OPTION(1) and select SID from the pop-up menu.
A new field appears in yellow.
Double-click the yellow SID box and select SETA from the pop-up selection on the bottom left corner.
A value of 1 now appears below the SID field box. This sets the output for only the nodes in set 1.
Click return to exit the GLOBAL_OUTPUT_REQUEST menu.
Click next and select the PARAM subpanel.
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.
Below COUPM_V1 click NO and select YES from the pop-up menu selection.
Selecting YES uses the coupled mass matrix approach for eigenvalue analysis.
Check the box next to G.
A new window appears in the work area screen.
Click below G_V1, and enter 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 [ $C / C_{0}$ ] ratio by 2.0.
Scroll down using the arrow to the left corner and check the box next to WTMASS.
A new window appears in the work area screen.
Click below WTM_V1, and enter a value of 0.00259 into the field box.
Three PARAM statements now appear in the pop-up menu on the work screen.
Click return to exit the PARAM menu.
Select the OUTPUT card.
A new window appears in the work area.
In the number_of_outputs field, enter 3.
Set the first KEYWORD to HGFREQ.
Using HGFREQ results in a frequency output presentation for HyperGraph.
Set the second KEYWORD to OPTI.
Set the third KEYWORD to H3D.
Double-click on the box beneath FREQ and select ALL from the pop-up selection for all keywords.
Selecting ALL will output all optimization iterations.
Click return to exit OUTPUT.
Click return to exit the Control Cards menu.

Submit the Job

From the Analysis page, click the OptiStruct panel.

Figure 4. Accessing the OptiStruct Panel
Click save as.
In the Save As dialog, specify location to write the OptiStruct model file and enter flat_plate_modal_response for filename.
For OptiStruct input decks, .fem is the recommended extension.
Click Save.
The input file field displays the filename and location specified in the Save As dialog.
Set the export options toggle to all.
Set the run options toggle to analysis.
Set the memory options toggle to memory default.
Click OptiStruct to launch the OptiStruct job.

If the job is successful, new results files should be in the directory where the flat_plate_modal_response.fem was written. 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.

The default files written to the directory are:

flat_plate_modal_response.html: HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
flat_plate_modal_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_modal_response.h3d: HyperView binary results file.
flat_plate_modal_response.res: HyperMesh binary results file.
flat_plate_modal_response.stat: Summary, providing CPU information for each step during analysis process.

Review the Results

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

From the OptiStruct panel, click HyperView.
HyperView is launched and the results are loaded. A message window appears to inform of the successful model and result files loading into HyperView.
Click Close to close the message window, if one appears.
In the HyperView window, click File > Open > Session.
An Open Session File window opens.
Select the directory where the job was run and select file flat_plate_modal_response_freq.mvw.
Click Open.
A discard warning appears.
Click Yes.
Two graphs per page and a total of three pages are displayed in HyperGraph. The graph title shows Subcase 1 (subcase 1) - Displacement of grid 15 on page 1.
Click the Axis toolbar icon . Select Logarithmic option and use the parameters shown below to make logarithmic plots of the results.

Figure 5.

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

Figure 6. Frequency response of node 15
Directly underneath the blue graph border, click the Next Page icon .
Page 2 displays, which shows Subcase 1 (subcase1) - Displacement of grid 17.

Figure 7. Frequency Response of Node 17
Click the Next Page icon again to display page 3 containing Subcase 1 (subcase1) - Displacement of grid 19.

Figure 8. Frequency Response of Node 19

This concludes the HyperGraph results processing.
Open the displacement file (.disp) using a text editor.
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.
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 phase angles.