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 HyperMesh Desktop.
  2. In the User Profile dialog, set the user profile to 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 > Model.
  2. In the Open Model dialog, open the chapter3.hm file.
    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 Visualization toolbar.

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.
  4. Right-click on Type and select Create from the context menu.


    Figure 5.
    The Create Sensors dialog opens.
  5. Set Element Type to BEAM188.


    Figure 6.
  6. Click Close.
  7. For Material, click Unspecified > Material.
  8. In the Select Material dialog, select Steel and then click OK.


    Figure 7.
  9. In the Model Browser, right-click and select Create > Component from the context menu.
    HyperMesh creates and opens a component in the Entity Editor.
  10. For Name, enter beam_asec.
  11. Click the Color icon, and select a new color.
  12. For Type, click Unspecified > Sensor.


    Figure 8.
  13. In the Select Sensor dialog, select sensor1 (BEAM188) and then click OK.


    Figure 9.
  14. For Material, click Unspecified > Material.
  15. In the Select Material dialog, select Steel and then click OK.

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 10.
  1. From the menu bar, click Mesh > Create > 1D Elements > 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 11.
  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 12.


    Figure 12.
    Note: Arbitary_Beam_Section is shown as a tag in the graphics area.
    HyperMesh creates a BEAM188 element.
  4. In the Component folder of the Model 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 13.
    Figure 13.
    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 menu bar, click Mesh > Create > 1D Elements > Rigids.
    The Rigids panel opens.
  2. Set the dependent selector to multiple nodes.
  3. Select each of the dof checkboxes as indicated in Figure 14.


    Figure 14.
  4. Set elem types to CERIG.
  5. In the Component folder of the Model 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 15.


    Figure 15.
  8. Click dependent: nodess > by path.
  9. On the plate component, select the dependent nodes indicated in Figure 16.


    Figure 16.
  10. Click create.


    Figure 17.
  11. In the Component folder of the Model 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 18.


    Figure 18.
  14. Click dependent: nodes > by path.
  15. On the plate component, select the dependent nodes indicated in Figure 19.


    Figure 19.
  16. Click create.


    Figure 20.
  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 Component folder of the Model Browser, click beam_std.
    The Entity Editor opens and displays the component's corresponding data.
  2. Right-click on property and select Create from the context menu.
    The Create Properties dialog opens.
  3. For Name, enter Circular_Sec.
  4. Set SUBTYPE to CSOLID.
  5. Under SECDATA, enter 15 for R.
  6. 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 folder of the Model 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 21.
  5. From the menu bar, click Properties > 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 22) that form the Arbitrary_Beam_Section.


    Figure 22.
  9. Set section base node to centroid.


    Figure 23.
  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 24.
  11. In the Model Browser, select .
  12. In the Properties folder of the Model Browser, click arbi_sec.
    The Entity Editor opens and displays the beam section's corresponding data.
  13. For Hyper beam section [OPTIONAL], click Unspecified > Beamsection.


    Figure 25.
  14. In the Select Beamsection 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 folder of the Model Browser, click beam_asec.
    The Entity Editor opens and displays the component's corresponding data.
  2. For Property, click Unspecified > Property.
  3. In the Select Property dialog, select arbi_sec and then click OK.
    HyperMesh attaches this property to the component.
  4. In the Model Browser, click to display all of the entities in the graphics area.
    All of the entities are displayed in the graphics area as indicated in Figure 26.


    Figure 26.

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 > Model.
  2. In the Save Model 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.
    The Export tab opens.
  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. In the File field, navigate to your working directory and save the file as 4450_export.cdb.
  4. Click Export.