Check for Element Penetrations/Intersections

Penetration is defined as the overlap of the material thickness of shell elements, while intersection is defined as elements that actually pass completely through one another.

Figure 1. Penetration and Intersection
Restriction: Penetration checking is supported by all of the impact solver interfaces, such as LS-DYNA, Radioss and PAM-CRASH, and works best with a solver interface that supports thickness data for modeled shell elements. The default HyperMesh solver interface does not support modeled element thickness, but the penetration checking tools can still be used to specify a uniform thickness when performing a check.
  • You can only set up and initiate the check in the Penetration panel; the majority of the checking tool actually resides in a special tab that opens in the tab area. However, this tab only displays after you complete the panel and run an initial check.
  • When the penetration check runs, it automatically masks (hides) everything in your model except for the penetrating or intersecting elements. It then fits the view to these elements’ components. You can show or hide additional elements using toolbar buttons located in the Penetration tab, and you can make other entity types, such as ellipsoids, visible again via the Display panel or the Mask panel.
  • Solid entities never register penetrations between each other; instead, any overlap between solids registers as intersections, because one or more of each the solid’s faces intersect. A solid that is completely contained within another solid will not be detected as an intersection or penetration, because its faces will not intersect any of the larger (containing) solid’s faces. In addition, only surface elements register penetrations; the tool cannot find penetrations between internal, that is, tetra- or hexa-, elements.

    Figure 2. Intersections Found

    Figure 3. No Intersections
  • Solids can register penetrations with respect to adjacent shell elements, based on the thickness of the shell elements.
  1. From the Tools page, click Penetration.
  2. Use the entity selector to select entities to be checked for penetrations or intersections.
    In any case, the penetrating elements will be found; for example, picking two components locates elements from each component that penetrate elements of the other.
  3. Select the type of interferences to check for.
    Choose all interferences, intersections only, or penetrations only.
    Note: Solid entities only register penetrations in conjunction with shell elements. With other solids, they only register intersections.
  4. Select the type of elements to check.

    Choose 2D and 3D elements, 2D only elements, or 3D only elements.

    If you choose 2D only elements or 3D only elements, HyperMesh only checks elements of the specified type for penetration. Elements in the selected entities which are not of that dimensional type will be ignored, even if they penetrate or intersect another entity.

  5. To enter a tolerance for penetration checking, select the allowable interference depth checkbox.

    For example, if you check a model of a part measured in millimeters, and are not concerned about penetrations of less than a tenth of a millimeter, you could set this field to a value of 0.1. The penetration tool would then ignore any elements that penetrated each other by 1/10 of a millimeter or less, but still locate and highlight elements with a penetration depth greater than 1/10 mm.

    Some solvers will not permit direct, adjacent contact between elements, for example a penetration depth of exactly zero, with no space between elements. For such solvers, you should set this field to any negative value, such as -0.1. This allows the penetration tool to locate and display elements that are exactly adjacent to one another as if they were penetrating each other, so that you can use the penetration fixing tools to add some space between them.

  6. Select a method adjusting thickness.
    Not available when you run the check on groups, because a group’s thickness is defined by its control card.
    • Choose Component thickness to use the thickness value specified in a component’s property card for each element within that component.
    • Choose thickness multiplier to enter a value to multiply the selected entities’ thickness by for purposes of the penetration check. Fractional numbers are acceptable, but negative ones are not.
    • Choose uniform thickness to enter a thickness value.

      This can be used to work around the lack of thickness information in the default HyperMesh user profile, or when working with models that do not have a thickness specified.

      You can also use this option to determine the proximity between non-penetrating parts by specifying a thickness greater than the minimum distance between the selected elements.

  7. To check for components that intersect or penetrate themselves, for instance, due to high curvature in the component, select the include self interference checkbox.
    This option is computationally intensive, therefore it is not recommend that you use it when checking large numbers of elements for penetration.
  8. Click check.

The selected components, elements, or groups are checked for penetration and/or intersection. A message in the status bar displays the percentage progress of each step in the check.

If for some reason you wish to abort a check, you can do so by right-clicking in the graphics area and holding the button down. The exact length of time that you must hold the button depends on the size and complexity of the check you are running; the check will cancel once its completion percentage increments. When the check aborts, the status bar turns red and displays a message stating that the check was canceled.

Once the penetration/intersection check is complete, view the results of the check and make adjustments.