HM-3320: Penetration Check

In this tutorial you will learn strategies for penetration checking.

Use the following guidelines for conducting checks:
  • Checks can be run on both 2D and 3D elements, 2D elements only, or 3D elements only.
  • Select include self interference to include components that bend and pass through themselves. This occurs rarely and is expensive when running the check. By default, this checkbox is cleared.
  • By default the check is set to all interferences, meaning both intersection and penetration. The intersections only option and the penetrations only option are also available.
  • Select allowable interference depth to ignore penetrations and intersections that are less than the value specified. By default, this checkbox is cleared.
  • Select uniform thickness to assign a global thickness to all components.
  • Select thickness multiplier to multiply the existing thicknesses in the model.

When the penetration check is invoked, a new penetration tab opens in the browser area.

The results are split into intersections and penetrations with the number of components that are clashing in brackets. In the example below, two components are intersecting and eleven components have material penetration. Expand each section for more detail as to which components have failed.

The ID, Elems, Depth, and Comps columns provide information on which components' IDs are involved, the number of failed elements, the depth of penetration (not applicable for intersections), and the number of components affected in the penetration/intersection. Each of the columns can be sorted by clicking the column header.

Figure 1.

The fixing of penetrations and intersections falls into two categories: automatic and manual. These capabilities will be discussed in more detail in the tutorial.

Open the Model File

In this step you will open the model file,

  1. Start HyperMesh Desktop.
  2. In the User Profile dialog, select LS-DYNA.
    Note: This model is a LS-DYNA model; therefore, it is important to select the appropriate user profile so that HyperMesh can access the actual thickness values of the shell components. The thickness values are required for material penetration check.
  3. Click OK.
  4. From the menu bar, click File > Open > Model.
  5. In the Open Model dialog, open the file. The model appears.
  6. On the Visualization toolbar, click to shade the model's elements and mesh lines.
  7. Observe the model using various visualization options available in HyperMesh, such as rotation and zooming.

Run the Penetration Check

In this step you will run the penetration check.

  1. Open the Penetration panel by clicking Tools > Penetration Check from the menu bar.
  2. In the Entity Editor, in the Entity Type field, select Components.
  3. In the Selection field, click the entry 0 Components and then click Components again.

    Figure 2.
  4. At the bottom of the Select Components dialog, click Select All and then click the OK button.

    Figure 3.
  5. Back in the Entity Editor, click the Check button.
    Once the check is complete, the Penetration tab populates with one intersection and 15 penetrations.

    Figure 4.

Review the Intersection Results

In this step you will review the intersection results.

  1. View intersections by expanding Intersections in the Penetration tab, if there are more than one.
    Note: Based on which mode is chosen, certain components are displayed on the screen.

    Figure 5.
  2. Select (Display Components with Failed Elements) and (Fit View to Failed Elements).
  3. Under Intersections, select the Rocker Inner Panel RH component.
    HyperMesh automatically fits the screen to the failed intersecting elements.

    Figure 6.
  4. Review other visualization modes by clicking (Review Failed Elements). The contour and vector displays are only applicable to intersections. The intersecting elements display as follows:

    Figure 7.

Fix Intersection Results

In this step you will fix the intersection results.

To fix intersections manually:

  1. Under Intersections, select the Rocker Inner Panel RH component.
  2. Ensure that the intersecting entities can be fixed by clicking (Manual Fix Tools).
    Note: Additional tools display for intersection fixing.
  3. Click (Elements from Tree Selection).
    Note: You will not pick any additional elements.
  4. Click (Move in Normal Direction) for the direction of movement.
  5. For the distance value, type 2.

    Figure 8.
  6. Click twice.
    HyperMesh moves the selected elements in the chosen direction.
    Note: After the elements have been moved by a value of 4, they no longer intersect.
  7. Click (Recheck).

    To fix intersections automatically,

  8. Reload the file,
  9. Re-select all components.
  10. Click check. Once the check is complete, the Penetration tab populates with one intersection and 15 penetrations.
  11. Click the Automatic Pentration/Intersection Fix button ().

Interrogate the Penetration Results

In this step you will interrogate the penetration results.

  1. Expand Penetrations.
  2. Select the component, C-Pillar Bot Inner Panel RH. The penetration results look similar to the following image.

    Figure 9.
  3. View different types of display results for penetration by clicking the following visualization options: .
    Remember that the columns can be sorted. For example, if you were only interested in the worst offending penetrations then sorting by the depth column will reorganize the tree structure, while still retaining the parent/child relationship.

Fix Penetration Results

In this step you will fix the penetration results.

Within the checking tool there is an automatic penetration fix that will remove the penetrations within the model. This works by physically moving the failed nodes to new locations to remove the material penetration.

In some circumstances, there may be the need to lock or freeze a component that cannot be adjusted or moved by the fixing tool. To achieve this, right-click on the component and select Lock Component from the context menu. Once a component is locked, a symbol will appear by the folder indicating that the component is locked.

In the previous example, you locked the component, C-Pillar Bot Inner Panel RH. The lock symbol appears multiple times to correspond with the multiple references to the same component. To unlock the component, right-click again on the locked component and select Unlock Component from the context menu. For the purpose of this tutorial you will not be using the lock functionality.

In the Penetrations tab, click on Penetrations and then click the Automatic Penetration/Intersection Fix button.
All penetrations should be fixed.