HyperBeam Sections

1. In the Section Browser, right-click and select Create > Shell Section or Solid Section from the context menu.
2. In the Create dialog define parameters and click Create.
   1. In the Thickness field, enter the default thickness for each new part created.
      Part thicknesses can be edited later.
   2. In the Canvas size field, enter the initial length and width of the sketching area.
   3. In the Grid size field, enter the default size of the background grids.
      This can be altered in the Parameters pull-down menu.
   4. In the Snap size field, enter the smallest interval at which you can define a vertex by clicking while sketching.
      This is also the snap size while moving existing vertices.
   5. In the Point size field, enter the size of the vertices in the graphics area.
      Tip: Increasing the point size makes it easier to select an existing grid point when you are creating a part.

   
   
   Figure 1.

3. Once the defaults are set, the canvas will appear and you can start creating parts with the shell part / solid perimeter tool ().
   Once clicked, the button remains highlighted until you move the mouse off of the canvas.

   • Left-click to create a new vertex.
   • Right-click to remove vertices in the reverse order they were created.
   • Once the part is complete, move the mouse off of the canvas to finalize it.

   Note: Each part has only one thickness, and it is common to have a section with multiple connecting parts.

   
   
   Figure 2.

4. Use the Move vertex / Adjust Dimension tool () to click and drag vertices to snap points for shell and solid sections, or to adjust parameters such as shell thicknesses or standard section parameters.

   
   
   Figure 3.

5. After the parts are created and assembled it is sometimes necessary to revise the connectivity or change the part thicknesses.

   This can be done in the part editor shown above. Each part is listed with its part name, thickness and connectivity, and as each part is selected it will highlight yellow on the canvas.

   The connectivity order is simply the order in which the vertices are drawn for a given part. Remember to leave a space between each vertex when editing the connectivity order.

6. Redefine the local axis location and angle using the Reorient tab in the Edit shell section dialog.
   This becomes useful when comparing HyperBeam shell section properties (results) to more rigidly-defined sections. Note that changing the local axis in HyperBeam is not the same as using element offsets in a finite element model.

   
   
   Figure 4.

The same toolset can be applied to sketching solid sections as well. You can start by right-clicking the browser on the left-hand side, creating a new solid section, and defining defaults for Canvas, Grid and Snap sizes.

The Shell part / Solid perimeter tool can now be used to trace the outline of a solid shape.

Figure 5.

As before, once the outline is sketched, move the mouse out of the canvas area to finalize the part. Unlike shell sections, solid sections can only have one part defined, although the same tool can be used to sketch out a cavity within the solid section.

Note: Only one cavity can be defined per section.

Figure 6.

As before, the Move vertex / Adjust dimension tool can be used to move vertices of solid sections. Each vertex movement requires a re-mesh of the solid section, so take care when moving vertices of complicated parts.

Create and assign a standard section to an OptiStruct PBARL property.

Before you begin, load the OptiStruct user profile and open the standard_section.hm model, located in <installation_directory>\tutorials\hm.

Figure 7. . The grey elements in the image to the left represent a structure that needs to be stiffened by adding I-beams down the length of it. The image to the right is the 3D visualization of 1D bar elements running along five separate node paths.

1. In the Model Browser, click to activate the HyperBeam view.
2. Create a Standard Section by right-clicking on the browser and selecting Create > Standard Section > OptiStruct > I from the context menu.
3. Define the parameters as shown below:

   
   
   Figure 8.

Once HyperBeam solves the cross sectional properties, it is necessary to attach the beam section to a PBARL card image. This can be done by creating a component and assigning it a property that references the PBARL card image and beam section.

4. In the Model browser, right-click and select Create > Component from the context menu.
   A new component is created, and opens in the Entity Editor.
5. In the Entity Editor, right-click on the Property field and select Create from the context menu.
6. Define the property in the Create Properties dialog and then click Close.
   1. In the Name field, enter pbarl.
   2. For Card Image, select PBARL.
   3. For Beam Section, click <Unspecified> > Beamsection.
   4. In the Select Beamsection dialog, select standard I and click OK.

   
   
   Figure 9.

7. After the new component and property are created with the beam section attached, the bar element can be defined in the bars panel in the 1D menu-page.

   
   
   
   
   Figure 10. Bars Panel

   Bar element alignment using HyperBeam sections is very straightforward since standard sections are defined using an absolute y-direction. The direction specified in the Bars panel defines the alignment of the beamsection’s y-direction. In this case, the positive z-direction in the Bars panel will align with the y-direction of the HyperBeam section. Since the centerline of a 1D beam element is defined about the section’s shear center, elemental offsets are frequently required. In this case, we have added z-offsets at both ends of each element to align the I-beams flush with the plate.

   To fully visualize the 1D element in HyperMesh, find the display option in the Visualization toolbar ().

Create and assign a shell section to an OptiStruct PBAR property.

Before you begin, load the OptiStruct user profile and open the shell_section.hm model from <installation_directory>\tutorials\hm.

Figure 11. . The blue lines are plot elements denoting the beam section. Elements or lines can be used to describe a beam cross section. The purple lines are plot elements used to align the section within HyperBeam.

1. From the 1D page, select the HyperBeam panel, shell section subpanel.
2. Set the selector type to use elems, and then select the blue plot elements.
3. Under cross section plane, toggle to the plane and vector selector.

   
4. Select N1, N2, and N3 locations.

   
   
   Figure 12.

   The vector created by N1 to N2 describes the local y-axis used in HyperBeam. N3 describes the positive sense of the z-axis. It is important to note the alignment of the local axes at this point. Later, it will be necessary to know this when the beam section is aligned for bar elements.

5. Set section base node to shear center.
6. Click create.
   HyperBeam View is invoked.

   
   
   Figure 13.

Once selected solves the cross-sectional properties, it is necessary to attach the beam section to a PBAR card image. This can be done by creating a component and assigning it a property that references the PBAR card image and beam section.

7. In the Model browser, right-click and select Create > Component from the context menu.
   A new component is created, and opens in the Entity Editor.
8. In the Entity Editor, right-click on the Property field and select Create from the context menu.
9. Define the property in the Create Properties dialog and then click Close.
   1. In the Name field, enter pbar.
   2. For Card Image, select PBAR.
   3. For Beam Section, click <Unspecified> > Beamsection.
   4. In the Select Beamsection dialog, select shell_section.0 and click OK.

   
   
   Figure 14.

10. After the new component and property are created with the beamsection attached, the bar element can be defined in the bars panel in the 1D menu-page.

    
    
    
    
    Figure 15.

    Bar element alignment using HyperBeam sections is very straightforward if the section has been defined using an absolute y-direction. The direction specified in the Bars panel defines the alignment of the beamsection’s y-direction. In this case, the positive y-direction in the Bars panel will align with the y-direction of the HyperBeam section.

    To fully visualize the 1D element in HyperMesh, find the display option in the Visualization toolbar ().