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.
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.Figure 1.
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.
Notice: 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.
next to the channel component to turn the geometry display
on.
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.
