OS-T: 1930 Generate Flexible Body for use in MotionSolve

In this tutorial you will use an existing finite element model to generate a flexible body for use in MotionSolve. You will run the model in OptiStruct.

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

rd4030_flex_body
Figure 1.

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  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.

Open the Model

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

Set Up the Model

Create Load Collectors to Conduct the Flexible Body Reduction

In this step, two collectors will be created; 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.
  1. Create the ASET load collector.
    This load collector will be used to define connecting degrees of freedom of the flexible body to the multi-body system.
    1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
      A default load collector displays in the Entity Editor.
    2. For Name, enter ASET.
    3. Click Color and select a color from the color palette.
    4. Set Card Image to None.
  2. Create the CMS load collector.
    This load collector will be used to define the component mode synthesis method and parameters.
    1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
      A default load collector displays in the Entity Editor.
    2. For Name, enter CMS.
    3. Click Color and select a color from the color palette.
    4. Set Card Image to CMSMETH.
    5. Leave METHOD set to the default value, which is CB (Craig-Bampton).
    6. For NMODES (number of modes), enter 10.

Modify Load Types

  1. From the Analysis page, click the load types panel.
  2. Click constraint = > ASET.
  3. Click return.

Create the ASETs

  1. In the Model Browser, Load Collectors folder, right-click ASET and select Make Current from the context menu.
  2. From the menu bar, select BCs > Create > Constraints to open the Constraints panel.
  3. Create the first constraint.
    1. Select the following degrees of freedom: dof1, dof2, and dof3.
      Tip: Deselect degrees of freedom by right-clicking on a checked (selected) box.

      rd4030_aset
      Figure 2.
    2. Using the nodes selector, select the nodes that sit in the middle of the multi-node rigid on the primary attachment point of the control arm to the chassis.
    3. Click create.
  4. Create the second constraint.
    1. Select the degrees of freedom, dof2 and dof3.
    2. Using the nodes selector, select the node and the last attachment point of the control arm..
    3. Click create.
  5. Create the third constraint.
    1. Select the degree of freedom, dof3.
    2. Using the nodes selector, select the top node in the rigid which would fasten the bottom of the shock assembly to the control arm.
    3. Click create.
  6. Create the fourth constraint.
    1. Select the degrees of freedom, dof1, dof2, and dof3.
    2. Using the nodes selector, select the top node in the rigid on the boss to the right.
    3. Click create.

rd4030_control_arm
Figure 3. Constraints Applied to the Control Arm Model

Create Subcase

  1. From the , click Setup > Create > Control Cards to open the Control Cards panel.
  2. Click GLOBAL_CASE_CONTROL.
  3. Enable CMSMETH.
  4. Click CMSMETH and select the CMS load collector.
  5. Click return to return to the Control Cards panel.

Define Output Request

  1. From the menu bar, click Setup > Create > Control Cards to open the Control Cards panel.
  2. Define the units system for the flex body output.
    The units should be defined consistent with the material properties of the material defined for this model. This way, you will not need to take care of the units of Multibody Dynamics Analysis.
    1. Click DTI_UNITS.
      Tip: To check the material properties of your model, go to the Model Browser, Materials folder and click MAT1_1. In the Entity Editor, view the Elastic modulus (2.1e+05), Poisson's Ratio (0.3) and the Density of the material (7.9e-09). For this model, the material used is Steel. Since the values of the material properties provided are consistent with Megagram, Newton, Millimeter, Second, the MGG N MM S sequence is selected for this control card.
    2. The values of the material properties provided are consistent with Megagram, Newton, Millimeter, Second, therefore select the MGG N MM S sequence.
    3. Click return.
  3. Define the analysis type.
    1. Click GLOBAL_OUTPUT_REQUEST.
    2. Select STRESS.
    3. Select the options shown below.

      os_1930_01
      Figure 4.
    4. Click return.
  4. Create the output control for the component mode synthesis.
    1. Click OUTPUT.
    2. Select the options shown below.

      os_1930_02
      Figure 5.
    3. Click return.
  5. Create a title.
    1. Click TITLE.
    2. Enter a title for the analysis.
    3. Click return twice.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.

    OS_1000_13_17
    Figure 6. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter susp_sla for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the susp_sla.fem was written. The susp_sla.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:
susp_sla.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
susp_sla.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.
susp_sla.h3d
HyperView binary results file.
susp_sla.res
HyperMesh binary results file.
susp_sla.stat
Summary, providing CPU information for each step during analysis process.