HM-4450: Introduction to HyperBeam

In this tutorial, you will learn how to couple degrees of freedom and to assign a standard beam section using the Section and HyperBeam panels.

Before you begin, copy chapter3.hm from <hm.zip>/interfaces/ansys/ to your working directory.
Figure 1 and Figure 2 are pictorial representations of the original model. The model can be simplified in such a way that you can extract represent the entire model with a set of shell elements representing the plate part of the model and two lines indicating the beam.


Figure 1.


Figure 2.

Load the ANSYS User Profile

In this step, you will load the ANSYS user profile in HyperMesh.

  1. Start HyperWorks.
  2. From the menu bar, click File > Solver Interface > Ansys.

Retrieve the Model File

In this step, you will retrieve and open the model file in HyperMesh.

  1. From the menu bar, click File > Open > HyperMesh Model.
  2. In the Open File dialog, select chapter3.hm.
    This model contains a plate collector which includes shell elements. The plate component is updated with the necessary element type, real constant, and material properties.


    Figure 3.
    The model displays in the graphics area.
  3. Optional: If your model's elements and mesh lines are not shaded, click on the View Controls toolbar then select .

Create Collectors and Attach Element Types and Materials

In this step, you will create collectors and attach element types and materials to the collectors.

  1. In the Model Browser, right-click and select Create > Component from the context menu.


    Figure 4.
    HyperMesh creates and opens a component in the Entity Editor.
  2. For Name, enter beam_std.
  3. Click the Color icon and select a color.


    Figure 5.
  4. For Property, right-click Unspecified and select Create.
  5. In the embedded Entity Editor, set the card image to SECTYPE then expand Mat-ET Type.
  6. For MAT, click Unspecified > Material.
  7. Click the search icon.
  8. In the Select Material dialog, select Steel.
  9. For SECTION, right-click Undefined and select Create.
  10. In the new Entity Editor, verify that the config is set to BEAM then click Previous.
  11. For TYPE, right-click Undefined and select Create/Edit.
  12. In the new Entity Editor, set the element type to BEAM188 then click Previous.


    Figure 6.
  13. In the Model Browser, right-click and select Create > Component from the context menu.
    HyperMesh creates and opens a component in the Entity Editor.
  14. For Name, enter beam_asec.
  15. Click the Color icon and select a new color.


    Figure 7.
  16. Repeat steps 4-12 for beam_asec.


    Figure 8.

Create a Beam Element

In this step, you will create a Beam element in HyperMesh.

In the Model Browser, notice that the current component is beam_asec.


Figure 9.
  1. From the panel area, click 1D > Bars.
    The Bars panel opens.
  2. Edit settings within the bar2 subpanel.
    1. Open the bar2 subpanel.
    2. Set orientation to plane.
    3. Set Beam Y Axis to parallel to XY.


      Figure 10.
  3. Use the node A and node B selectors to select the two nodes that form the ends of the Arbitary_Beam_Section line as indicated in Figure 11.


    Figure 11.
    Note: Arbitary_Beam_Section is shown as a tag in the graphics area.
    HyperMesh creates a BEAM188 element.
  4. In the Component Browser, right-click on beam_std and select Make Current from the context menu.
  5. Use the node A and node B selectors to select the two nodes that form the ends of the Std_circular_Beam_sec line as indicated in Figure 12.
    Figure 12.
    HyperMesh creates a BEAM188 element.
  6. Click return to exit the bar2 subpanel.

Create Coupled DOF - Rigid Elements

In this step, you will create coupled DOF and rigid elements.

  1. From the panel area, click 1D > Rigids.
    The Rigids panel opens.
  2. Set the dependent selector to multiple nodes.
  3. Select each of the dof checkboxes as indicated in Figure 13.


    Figure 13.
  4. Set elem types to CERIG.
  5. In the Component Browser, right-click on beam_asec and select Make Current from the context menu.
  6. Activate the independent selector set to node.
  7. On Arbitary_Beam_Section, select the independent node at the end of the beam element as indicated in Figure 14.


    Figure 14.
  8. Click dependent: nodess > by path.
  9. On the plate component, select the dependent nodes indicated in Figure 15.


    Figure 15.
  10. Click create.


    Figure 16.
  11. In the Component Browser, right-click on beam_std and select Make Current from the context menu.
  12. Activate the independent selector set to node.
  13. On Std_circular_Beam_sec, select the independent node at the end of the beam element as indicated in Figure 17.


    Figure 17.
  14. Click dependent: nodes > by path.
  15. On the plate component, select the dependent nodes indicated in Figure 18.


    Figure 18.
  16. Click create.


    Figure 19.
  17. Click return to exit the Rigids panel.

Create and Attach a Standard Circle Property

In this step, you will create and then attach a standard circle property to a component in HyperMesh.

  1. In the Model Browser, right-click and select Create > Sections from the context menu.
  2. Set config to BEAM.
  3. Set Subtype to CSOLID.
  4. Under SECDATA, enter 15 for R.
  5. In the Component Browser, click beam_std.
    The Entity Editor opens and displays the component's corresponding data.
  6. Right-click on property and select Create/Edit from the context menu.
    The Create Properties dialog opens.
  7. For Name, enter Circular_Sec.
  8. Set card image to SECTYPE.
  9. Click the Section selector then click the three dots.
  10. In the Advanced Selection dialog, select section1 then click OK.
  11. Click Close.
    HyperMesh assigns the property Circular_Sec to the beam_std component.

Create an Arbitrary Property

In this step, you will create an arbitrary property in HyperMesh.

  1. In the Model Browser, right-click and select Create > Property from the context menu.
    HyperMesh creates and opens a property in the Entity Editor.
  2. For Name, enter arbi_sec.
  3. Set card image to SECTYPE.
  4. In the Component Browser, click next to beam_std, beam_asec, and Plate to turn off the display of their elements.
    Note: You should only see geometric entities in the graphics area.


    Figure 20.
  5. In the panel area, click 1D > HyperBeam.
    The HyperBeam panel opens.
  6. Open the solid section subpanel.
  7. Set the entity selector to lines.
  8. Select all of the lines (displayed in pink as indicated in Figure 21) that form the Arbitrary_Beam_Section.


    Figure 21.
  9. Set section base node to centroid.


    Figure 22.
  10. Click create.
    The HyperBeam Data Model dialog opens, meshes the area enclosed by the selected lines with quadrilateral elements, and calculates the properties using these elements.


    Figure 23.
  11. In the Properties Browser, click arbi_sec.
    The Entity Editor opens and displays the beam section's corresponding data.
  12. For Hyper beam section [OPTIONAL], click Unspecified > Beamsection, then select the three dots.


    Figure 24.
  13. In the Advanced Selection dialog, select solid_section.0 and then click OK.

Update the Component Collector with the Beam Section

In this step, you will update the component collector with the beam section.

  1. In the Component Browser, click beam_asec.
    The Entity Editor opens and displays the component's corresponding data.
  2. For Property, click Unspecified > Property, then select the three dots.
  3. In the Advanced Selection dialog, select arbi_sec and then click OK.
    HyperMesh attaches this property to the component.
  4. Click on the View Controls toolbar, then select All.
    All entity types are displayed in the graphics area as indicated in Figure 25.


    Figure 25.

Save your Work

In this step, you will save your work as a model in HyperMesh.

  1. From the menu bar, click File > Save As > HyperMesh Model.
  2. In the Save File As dialog, navigate to your working directory and save your file.

Export the Deck to ANSYS *.cdb Format

In this step, you will export your model within HyperMesh.

  1. Click File > Export > Solver Deck from the menu bar.
  2. Set File type to Ansys.
    Note: If you are in the ANSYS user profile, HyperMesh automatically sets the File type to Ansys and loads ANSYS as the default Template.
  3. Navigate to your working directory and save the file as 4450_export.cdb.
  4. In the Solver Export Options dialog, click Export.