OS-T: 1110 Modal Analysis Setup

In this tutorial, you continue to gain an understanding of the basic concepts for creating a OptiStruct input file. More specifically, learn how to set up a model for modal analysis, specify solver specific controls and also submit an input file to the solver from HyperMesh.

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

channel_brkt_modal.hm

To complete the setup of the model for a modal analysis with OptiStruct, you need to define a normal modes SUBCASE, containing METHOD and SPC statements.

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.

Open the Model

Click File > Open > Model.
Select the channel_brkt_modal.hm file you saved to your working directory.
Click Open.
The channel_brkt_modal.hm database is loaded into the current HyperMesh session, replacing any existing data.

Set Up the Model

Review and Edit the Materials

This step can be done from the Model Browser.

In the Model Browser, expand the Material folder to show the two materials in the model.
Click aluminum.
The material entry is displayed in the Entity Editor.
For RHO, enter 2.7e-9.
Repeat steps 1 to 3 to input an RHO value of 7.9e-9 for the steel entry.

Create modal Load Step Input

This can be done using the Load Step Inputs panel and the create subpanel.

In the Model Browser, right-click and select Create > Load Step Inputs.
For Name, enter modal.
Set Config type, select Real Eigen value extraction.
For Type, select EIGRL.
For ND, enter 10.
ND specifies the number of modes to extract.

Figure 2.

Create constraints Load Collector

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter constraints.
Set Card Image to None.

Apply Constraints (OptiStruct SPC) on the Channel

Expand the Component folder in the Model Browser.
Click the geometry icon next to the channel component to turn the geometry display on.
Click the Isometric View icon in the toolbar.
You are going to create the SPC constraints on the nodes along the lines on the perimeter of the channel's bottom surface, as shown in the image below.

Figure 3. Apply Constraints on the Channel
Click BCs > Create > Constraints to open the Constraints panel.
Switch the entity selector to lines.
Select the six lines on the perimeter of the channel's bottom surface.
To view the selected lines clearly, switch to Transparent Elements mode, as shown below:

Figure 4.
Activate degrees of freedom (DOF) 1 through 6.
- 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.
For size =, enter 10.
The display size of the constraints is reduced.
Click create > return to exit the panel.

Map the Constraints

Use the Load on Geom panel in this step.

From the Analysis page, click load on geom.
Click loadcols, and select constraints.
Click select to complete the selection of load collectors.
Click map loads.
A constraint is at each node associated to the geometry lines.
Click return to exit the panel.

Define the Load Step

Use the Load Step Entity Editor in this step. Define the loadstep to contain the load collectors constraints and modal.

In the Model Browser, right-click and select Create > Load Step.
For Name, enter normal_modes.
For Analysis type, select Normal modes.
For METHOD(STRUCT), select modal.
For SPC, select the load collector constraints.

Define the Formats of Result Files

In the Control Cards panel, use the OUTPUT card to add two output requests for the Altair H3D and HyperMesh .res formats.

Click Setup > Create > Control Cards to open the Control Cards panel.
Click next to go to the next panel menu of control cards.
Select the control card OUTPUT.
Notice in the card image the one OUTPUT line is set to a default value. This specifies OptiStruct to output the results to a HyperMesh command file.
Click the default value and select H3D from the pop-up menu.
For number_of_outputs =, enter 2.
A second OUTPUT line appears in the card image.
Click the default value again and select HM for the second output type.
This specifies OptiStruct to output results to a H3D file and a . res file, which can be viewed in HyperView Player. Also, an HTML report file is output and the H3D file is embedded in it.
Click return to return to the Control Cards panel.

Note: The OUTPUT button is green. This indicates the card is exported to the OptiStruct input file.
Click return to exit the panel.

Submit the Job

From the Analysis page, click the OptiStruct panel.

Figure 5. Accessing the OptiStruct Panel
Click save as.
In the Save As dialog, specify location to write the OptiStruct model file and enter modal_analysis 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 modal_analysis.fem was written. The modal_analysis.out file is a good place to look for error messages that could help debug the input deck if any errors are present.