An existing finite element model will be used in this tutorial to demonstrate how HyperMesh may be used to set up a model to generate a flexible body for use in Altair MotionSolve. The model is then run in OptiStruct. The figure illustrates the structural model used for this tutorial.
The following exercises are included:
· Retrieving the .hm file
· Setting up the problem in HyperMesh
· Submitting the job
To load the OptiStruct user profile and retrieve the model:
Launch HyperMesh and choose the OptiStruct user profile in the User Profiles dialog.
User Profiles… can also be accessed from the Preferences pull-down menu on the toolbar.
Click the Files
panel toolbar button 
.
Select the hm file subpanel using the radio buttons on the left-hand side of the panel.
Click retrieve….
An Open file… browser window pops up.
Select the cms_carm.hm file, located in <install_directory>/tutorials/os/.
Click Open.
The cms_carm.hm database is loaded into the current HyperMesh session, replacing any existing data.
Click return to go to the main menu.
To create load collectors that will be used to conduct the flexible body reduction:
In this section, you will create two collectors; one for the ASET that defines the connecting degrees of freedom of the flexible body and the other for the method and parameters for the component mode synthesis.
Click the Collectors
toolbar button 
.
Select the create panel.
Click the collector type switch and choose load collectors.
Click the switch next to card image= and choose no card image.
For name =, type ASET, and click the create button on the right.
This load collector will be used to define connecting degrees of freedom of the flexible body to the multi-body system.
For name =, type CMS.
Change from no card image to card image.
Click card image = and select CMSMETH.
Click the create/edit button.
This creates the load collector used to define the component mode synthesis method and parameters. The card image can now be edited.
The Craig-Bampton (CB) method is selected by default. Either UB_FREQ (upper bound on frequency) or NMODES (number of modes) must be defined.
Under NMODES, enter 10.
Click return twice.
To modify the load types of constraint to ASET:
From the Analysis page, select the load types panel.
Click constraint = and select ASET.
Click return.
To create the ASETs required in the analysis:
Press g on the keyboard to activate the Global panel in HyperMesh.
Click loadcol =, select the load collector named ASET, and click return.
From the Analysis page, select the constraints panel.
Select the following degrees of freedom: dof1, dof2, and dof3.
Deselect any degree of freedom by right-clicking a checked (selected) box.
If nodes is not highlighted, click nodes.
Select the node that sits in the middle of the multi-node rigid on the foremost attachment point of the control arm to the chassis.
Click the create button.
Select dof2 and dof3 and verify that the nodes button remains active.
Choose the node and the reward attachment point of the control arm.
Click create.
Create the third constraint by selecting dof3 and choosing the top node in the rigid which would fasten the bottom of the shock assembly to the control arm. This can be seen in the next figure.
Click create.
Constraints applied to control arm model
Create the fourth constraint by selecting dof1, dof2, and dof3 and choosing the top node in the rigid on the boss to the right.
Click create.
Click return.
To create the OptiStruct subcase (also referred to as a loadstep):
From the Analysis page, select the subcase panel.
Click name = and enter flex-body.
Click the type: selection switch and select comp. mode synth..
Check the box preceding CMSMETH.
An entry field appears to the right of CMSMETH.
Click on the entry field and select CMS from the list of load collectors.
Click create.
Click return to go to the main menu.
To create a thin membrane skin for output purposes to reduce the flexible body data:
From the Tool page, select the faces panel.
Click comps.
Select nondesign and design from the list.
Click select.
Click find faces.
This creates a component of shell elements around the solid elements. The name of the component is ^faces.
We have to rename it and give it membrane properties.
Click return.
Enter the rename panel.
Click original name = and select ^faces from the list.
Click new name = and enter skin.
Click rename.
Click return.
Click the Collectors
toolbar button .
Select the update panel.
Click the switch and choose comps.
Click the yellow comps button.
Select skin from the list.
Click select.
Click card image= and choose PSHELL.
Fields for material = and thickness = will appear.
Enter a thickness of 0.0001.
A small thickness is selected since the purpose of the skin is only for visuals.
Click material = and select mat1.
Click update/edit.
Check the boxes beside MID2_opts and MID3_opts and use the switch for each to set both to BLANK in order to model a membrane.
Click return twice.
Now we want to create a property set (PSET) for selection in the output control to reduce the model and stress output to just use the skin elements.
Go to the Analysis page and enter the entity sets panel.
Click name = and enter skin.
For entity:, select comps.
Click comps and choose skin.
Click select.
Click create.
Click return.
To define a unit system, create a title, and create the output control for the component mode synthesis:
From the Analysis page, select the control cards panel.
Find DTI_UNITS to define the units system for the flex body output.
The units should correspond to the unit systems of your multi-body dynamics analysis. In this tutorial, we keep the standard SI units: kg, N, mm, s.
Click MODEL.
Click on the yellow ELSET field twice and select the property set skin.
This will reduce the output of the model to only the membrane skin. It is only for visualization in the final animation of the multi-body model.
Click return.
Click STRESS (on the last page of the control cards).
Click the button below STRESS_OPT and select PSID.
A new field for the selection of a property set will pop up.
Click on the yellow PSID field twice and select the property set skin.
This will reduce the stress output to only the membrane skin. It is only for visualization in the final animation of the multi-body model.
Click return.
Click TITLE and enter a title for this analysis.
Click return twice.
To run the component mode synthesis:
The OptiStruct panel accomplishes two things: it saves the current model with its settings to create the input file OptiStruct will use, and it allows you to select the type of analysis.
From the Analysis page, select the OptiStruct panel.
Set the export options: toggle at the bottom of the panel to all.
After input file: click save as….
For File name:, enter cms_carm.fem.
The file extension .fem is necessary for OptiStruct to recognize an input file.
Leave the memory options: toggle set to memory default.
Set the run options: switch to analysis.
Click OptiStruct.
This launches the OptiStruct job. If the job is successful, you should see new results files in the directory where HyperMesh was invoked. The cms_carm.out file is a good place to look for error messages that will help you debug your input deck if any errors are present.
The default files that will be written to your directory are:
|
cms_carm.h3d |
H3D file that contains the flexible body data for use in Altair MotionSolve. |
|
cms_carm.out |
ASCII-based output file of the model check run performed before the simulation begins which gives some basic information on the results of the run. |
|
cms_carm.stat |
Detailed breakdown on the CPU time used for each significant stage in the analysis. |
Go To