Penetration Check

Tutorial Level: Beginner In this tutorial, you will learn strategies for penetration checking.

Use the following guidelines for conducting checks:
  • Settings for running the checks is accessed through the menu on the guide bar of the Penetration tool.
  • Checks can be run on both 2D and 3D elements, 2D elements only, or 3D elements only.
  • The check method can be used to select Embedded algorithm (default) and Solver output reader (only for LS-DYNA Interface) to check the penetrations and intersections.
  • By default, the check type is set to intersection and penetration. The intersections only option and the penetrations only option are also available.
  • Select allowable penetration depth to ignore penetrations and intersections that are less than the value specified. By default, the value is 0.
  • Select Thickness method to consider thickness of components for checking. You can select Component / element thickness. 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, the guide bar is displayed for entities selection and the Penetration Browser opens to showcase penetration check results.

The results are split into intersections and penetrations with the number of components that are clashing in brackets. In Figure 1, two components are intersecting and 11 components have material penetration. You can expand each section for more detail as to which components have failed. The ID, Elements, Depth, and Comps columns provide information on which component 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 this tutorial.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Open Model File

  1. Start HyperMesh.
  2. In the Startup dialog, select LsDyna for profile.
    Note: The model used in this tutorial is an LS-DYNA model; therefore, it is important to select the appropriate solver profile so that HyperMesh can access the actual thickness values of the shell components. The thickness values are required for material penetration check.
  3. Select your working directory and click Create Session.
  4. From the menu bar, click File > Open > HyperMesh Model.
  5. Browse to your working directory, select penetration_check.hm, and click Open.
    The model opens in the modeling window.
  6. On the View control toolbar, click on and then click on .
  7. Observe the model using various visualization options available in HyperMesh, such as rotation and zooming.

Run Penetration Check

  1. From the Validate ribbon, select the Penetration too.
    Figure 2.


  2. From the guide bar, verify Components is selected.
  3. Select all components in the model by completing one of the following options:
    • In the modeling window, right-click and select Select > All from the context menu.
    • From the guide bar, click to open Advanced selection, and select all components in the list.
  4. From the guide bar, click Check.
Once the check is complete, the Penetration Browser is populated with one intersection and 10 penetrations.
Figure 3.


Review the Intersection Results

In the Penetration Browser, expand the Intersection section and select the intersection pair.
Only the components with the intersection display in the modeling window.
Figure 4.


Note: The legends under the guide bar provide view options like penetration vectors, contour depth, highlight failed elements, and only elements options. By default, components are displayed with failed elements and the penetration vectors legend on. Review these visualizations modes by toggling them.
Figure 5.


Fix the Intersection Results

You can fix the intersection results manually (step 1) or automatically (step 2). For this tutorial, you only have complete one of the two steps. If you would like to fix the intersection results manually and automatically, you must complete Open Model File and Run Penetration Check again prior to moving on to step 2.

  1. Manually fix the intersection.
    1. In the Penetration Browser, right-click the Rocker Inner Panel RH component under Intersection and select Manual Fix from the context menu.
      Figure 6.


      In the modeling window, the collision entity is displayed with nodes which intersect with the components. The graphic manipulator opens.
    2. In the graphic manipulator, select the Y direction.
    3. Move the nodes manually in the direction shown by penetration vectors or enter -4 in the microdialog for Y.
      Figure 7.


    4. On the guide bar, click Recheck.
      The Intersection pair is removed from the Penetration Browser as a result of the removal of the intersected nodes.
  2. Automatically fix the intersection by completing one of the following options:
    • In the Penetration Browser, right-click the Rocker Inner Panel RH component under Intersection and select Auto Fix from the context menu.
    • From the guide bar, click Fix all to fix all penetrations and intersections simultaneously.

Interrogate the Penetration Results

  1. In the Penetration Browser, expand Penetrations.
  2. Select the C-Pillar Bot Inner Panel RH component.
    The penetration result is isolated in the modeling window.
    Figure 8.


  3. Use the legends under the guide bar to review different types of display results, like highlight failed, contour depth, penetration vectors, or only elements.
    Tip: You can change the penetration vector size by clicking on the guide bar. Penetration vector visualization can be set to fixed size or scaled size.
    Tip: In the Penetration Browser, the columns can be sorted. For example, if you were interested in only 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

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 entity from the context menu. Once a component is locked, a symbol will appear indicating that the component is locked.

To lock or unlock a component, right-click on component and select Lock Entity or Unlock entity from the context menu to prevent the component nodes from being moved when removing penetrations or intersections For the purpose of this tutorial you will not be using the lock functionality.

In the Penetration Browser, right-click Penetrations and select Auto fix from the context menu.
Similarly, penetrations can be fixed manually by clicking on the guide bar. Collision will then be selected on the guide bar and you can manually fix the penetrations.
Figure 9.


Use and on the guide bar to browse between collision entities in the modeling window.

Selection of a collision entity is synchronized with the Penetration Browser entity pair selection. For each penetration pair, an Entity Editor list of penetrated nodes is presented by default.
Figure 10.


You can follow the same process as described in step 1 of Fix the Intersection Results to manually remove penetrations. After completing the manual removal, you can recheck the penetration again to confirm.