OS-T: 1960 Define Point to Deformable Curve Joint

In this tutorial, a multibody dynamics analysis (simulation type: Transient Analysis) of a hook on a flexible cable are performed using OptiStruct.

Before you begin, copy the file(s) used in this tutorial to your working directory.
An existing finite element model is imported into HyperMesh. The rest of the setup (creation of joint, loading, etc.) is done in HyperMesh. HyperView is used to post-process the large deformations of the flexible cable model.

rd4060_hook
Figure 1. Hook Rolling on a Cable
You will learn how to create JOINTS (Fixed, PTDCV), a PFBODY, a PRBODY, a MBDCRV, and a multi-body dynamics subcase.

rd4060_HM_model
Figure 2. Model in HyperMesh

The flexible cable consists of 50 different CBAR elements (PFBODY) and the end of this flexible body is connected to ground (GROUND) using fixed joints.

The Hook (PRBODY) is an external graphic and is connected to the flexible cable by the PTDCV joint.

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 flex_cable.hm file you saved to your working directory.
  3. Click Open.
    The flex_cable.hm database is loaded into the current HyperMesh session, replacing any existing data.

Set Up the Model

Create Rigid Bodies (PRBODY)

  1. From the Analysis page, click the bodies panel.
  2. Select the create subpanel.
  3. In the body= field, enter Hook.
  4. Click type= and select PRBODY.
  5. Using the props selector, select Hook.
  6. Double-click nodes and select by id, then enter 14399.
  7. Click create.
  8. Click return.

Create Flex Bodies (PFBODY)

PFBODY is the Flexible Body Definition for Multibody Simulation. PFBODY defines a flexible body out of a list of finite element properties, elements, and grid points.
  1. From the Analysis page, click the bodies panel.
  2. Select the create subpanel.
  3. In the body= field, enter Cable.
  4. Click type= and select PFBODY.
  5. Using the props selector, select Cable.
  6. Double-click nodes and select by id, then enter 1, 2.
  7. Set CMS Method to Craig-Bampton.
  8. Verify frequency upper bound is set to upper bound default.
  9. Toggle number of modes to nmodes=, and enter 15.


    Figure 3.
  10. Click create.
  11. Click return.

Create GROUND Bodies (GROUND)

Note: The selection of a property is not required when defining a ground body.
  1. From the Analysis page, click the bodies panel.
  2. Select the create subpanel.
  3. In the body= field, enter Ground.
  4. Click type= and select GROUND.
  5. Double-click nodes and select by id, then enter 14397, 14398.
  6. Click create.

Define the Deformable Curve

  1. In the Model Browser, right-click and select Create > Set.
    A default set template displays in the Entity Editor.
  2. For Name, enter deform_curve.
  3. Set Card Image to MBDCRV.
  4. Verify Set Type is set to ordered.
  5. Select entity IDs.
    1. For Entity IDs, click 0 Nodes > Nodes.
    2. In the panel area, click node list > by path.
    3. Select the nodes at two ends of the flexible cable made up by CBAR elements.
      All of the nodes are automatically selected on the cable.
    4. Click proceed.

OS_1960_01
Figure 4.

Create Joints

You will create all the necessary joints including the PTDCV joint.

Three joints for the model are needed. Two fixed joints between the Cable ends to the Ground, and one PTDCRV between the Hook and the Cable.
  1. Create the component, joints.
    1. In the Model Browser, right-click and select Create > Component from the context menu.
      A default component template displays in the Entity Editor.
    2. For Name, enter joints.
  2. From the menu bar, click Mesh > Create > 1D Elements > Joints.
    The Joints panel opens.
  3. Create a fixed joint between one end of the Cable and Ground.
    1. Set joint type to fixed.
    2. Select node ID 1 as the first terminal and select node ID 14397 as the second terminal.
      Tip: Nodes 1 and 14397 are coincident. Use coincident node picking in the options panel > graphics subpanel to help you select these coincident nodes in the modeling window.
    3. Click create.
  4. Create the fixed joint between the other end of the Cable and Ground.
    1. Set joint type to fixed.
    2. Select node ID 2 as the first terminal and select node ID 14398 as the second terminal.
    3. Click create.
  5. Create the PTDCV joint.
    1. Set joint type to ptdcv.
    2. Select node ID 14399 as the first terminal.
    3. Click set= and select deform_curve.
      The deform_curve entity set is defined as MBDCRV.
    4. Click create.

    os_1960_05
    Figure 5.
  6. Click return.

Create Load Collectors

In this step you will create the gravity force that applies to the model and MBSIM Bulk Data card, which is to specify the parameter for multibody simulation.

  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 gravity.
  3. Click Color and select a color from the color palette.
  4. Set Card Image to GRAV.
  5. Input the values as illustrated below.


    Figure 6.
  6. Create another load collector.
    1. For Name, enter SIM.
    2. For Card Image, select MBSIM.
    3. Input the values as illustrated below.


      Figure 7.

Create Load Steps

  1. In the Model Browser, right-click and select Create > Load Step from the context menu.
  2. For Name, enter Dynamic.
  3. Set Analysis type to Multi-body dynamics.
  4. Define MLOAD.
    1. For MLOAD, click Unspecified > Loadcol.
    2. In the Select Loadcol dialog, select gravity and click OK.
  5. Define MBSIM.
    1. For MBSIM, click Unspecified > Loadcol.
    2. In the Select Loadcol dialog, select SIM and click OK.

Submit the Job

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

    OS_1000_13_17
    Figure 8. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter flex_cable 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 flex_cable.fem was written. The flex_cable.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:
flex_cable.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
flex_cable.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.
flex_cable.h3d
HyperView binary results file.
flex_cable.res
HyperMesh binary results file.
flex_cable.stat
Summary, providing CPU information for each step during analysis process.

View the Results

In this step you will view the results in HyperView, which will be launched from within the OptiStruct panel of HyperMesh.

HyperView is a complete post-processing and visualization environment for finite element analysis (FEA), multibody system simulation, video and engineering data.

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

    The path and filename for flex_cable.h3d appears in the fields to the right of Load model and Load results. This is fine because the .h3d format contains both model and results data.

    The model and results are loaded in the current HyperView window.

  2. Click the Contour panel toolbar icon resultsContour-16.
  3. Under Results type: select Displacement(v).
  4. Click Apply.
  5. Start/stop the animation using the Animation Controls in the panel next to the playback controls.

    animation_toolbar
    Figure 9.
    1. Verify Animate Mode is set to animationTransient-24 (Transient).
    2. Click the Start/Pause Animation icon to start the animation.
    3. With the animation running, use the bottom slider bar to adjust the speed of the animation.
    4. Click the Start/Pause Animation icon again to stop the animation.