Manage Penetrations/Intersections

Check components or groups for element penetrations and intersections using the Penetration Check tool.

Penetration and intersection can be used individually or collectively. Penetration is defined as the overlap of the material thickness of shell elements, while intersection is defined as elements passing completely through one another.

  1. From the menu bar, click Tools > Penetration Check.
    Restriction: Only available in the Radioss, LS-DYNA, and PAM-CRASH user profiles.
    The Penetrations browser opens.
  2. Set up the Penetration Check and check for intersections/penetrations.
    1. In the Penetrations browser, click to invoke the collision setup widget.
    2. In the Check type field, select the type of collision to check.
    3. In the Entity type field, select the type of entity to be checked for intersections and/or penetrations.
    4. In the Selection field, select contacts (groups), components, or elements to check.
      Selecting one of more contacts will perform the penetration check according to the rules enforced by the solver. In any case, the penetrating elements will be found, and the results will display in the Penetration Browser. Results will be listed by pairs of components regardless of the entity type that was used to select penetration candidates.
    5. Use Minimum penetration depth to filter out penetrations with lower penetration depth values.
    6. Select a Thickness option.
      Restriction: Only available for Component checks.
      • Choose Component/Elements thickness to apply no adjustments as it uses the thickness value specified in a component’s property card for each element within that component.
      • Choose Thickness multiplier to multiply the selected entities' thickness by the value entered in the Thickness multiplier field for purposes of the penetration check. Fractional values are acceptable, but negative values are not.
      • Choose Uniform thickness to ignore the existing component's thickness, and instead uses the value entered in the Uniform Thickness field for all of the components in the model.
        Note: Use Uniform thickness as a workaround to the lack of thickness information in the default HyperMesh user profile, or when working with models that do not have a thickness specified.
    7. Select a Thickness > size option.
      Restriction: Only available for Component checks.
      • Ignore self-penetrations when thickness > elem size
      • Consider self-penetrations when thickenss > elem size
    8. To consider edge penetrations, select the Consider edge penetrations checkbox.
    9. Select a treatment algorithm for the boundary shell edge.
      • Choose Flat edges to consider external borders of the components flat.


        Figure 1. Flat Edges
      • Choose Rounded edges to extend external borders of the component by a cylinder having the diameter of the component thickness.


        Figure 2. Rounded Edges
    10. Click Check.
      Once the check is complete, the browser populates with detected intersections and/or penetrations.


      Figure 3.
  3. Review the penetrations/intersections using the view controls in the browser.


    Figure 4.
  4. Fix the penetrations/intersections.
    To fix Do this
    Manually
    1. Select groups/components to fix in the browser.
    2. Click on the collision toolbar. Additional tools display.


      Figure 5.
    3. Select the elements or nodes to move.
    4. Move and/or translate the selected elements/nodes.
    5. Click to recheck that the intersection/penetration no longer remains.
    Automatically
    1. Select groups/components to fix in the browser.
    2. Click on the collision toolbar.
    Tip:
    • If a component is intersecting with another, right-click on the component and select Find Matching Penetrating Component Pair from the context menu to find the same pair of components in the penetrations list. If the pair does not penetrate, a message will display.
    • To keep a specific component from changing when performing de-penetration fixes, right-click on that component and select Lock Component from the context menu. A red padlock displays on the component name in the browser to indicate that it has been locked. The nodes in a locked component cannot be moved by the Collision tool. To unlock, right-click a locked component and select Unlock Component from the context menu.


      Figure 6.
    • Sort the columns in the browser by clicking the column headings. For example, clicking the Violations heading sorts the parent components according to their number of violations. A small triangular arrow in the column heading indicates whether the components are sorted in ascending or descending order; repeated clicks toggle between these two options.

Penetration Check Browser

Overview of the Penetration Check Browser user interface.

Collision Toolbar

Option Description
Invokes the collision setup widget, which can be used to setup the Penetration Check and check for intersections/penetrations.
Reruns the collision check. This is recommended when you modify any attributes that control the collision check, or when a mesh modification has occurred.
Automatically attempts to fix the intersections/penetrations you have selected in the browser, based on the settings found in the Options dialog.

You can perform a fix on all of the intersections/penetrations listed in the browser, but it is highly recommended that all intersections are resolved before any automatic penetration fix is executed.

Enables you to manually fix intersections/penetrations. When selected, additional tools display in the browser that can be used to perform manual, rather than automatic, penetration fixes.
Exports the result of the collision run to a .txt or .csv file.

Nodes and nodes + element pairs are supported.

When multiple collisions are displayed in graphics area, click this button to identity the collision pairs in the collision browser after making a seletion in the graphics area.
Displays a node List for selected penetration that reports penetration depth (thickness minus residual distance), thickness, relative penetration, (penetration divided by thickness) and residual distance for all penetrating nodes.

View Controls

Button Action
Highlights all elements that caused penetrations or intersections when you select a component in the browser.
Makes all elements transparent (wireframe) except for the interacting elements of the component that you selected in the browser, which display in a solid color.
Displays a color gradient of the penetrating elements in the selected component, which indicates the severity (degree) of penetration for the interacting elements.

This mode is not available for intersections because their depth cannot be determined.
Displays a color gradient of relative penetrating elements.
Displays individual vectors for each penetrating element in the component that you select in the browser. These vectors indicate the direction and depth of penetration for both the selected component and its interacting components.

This mode is not available for intersections because their depth cannot be determined.
Fits the failed elements to the display.

In large models, this can be very helpful in finding and viewing small areas of minor penetration. Note that while this option is active, the view automatically fits to the penetrating elements of any component that you click in the browser. Click the option again to deactivate the fit mode.
Displays all elements, by unmasking all elements in the model, but not other masked entities such as model geometry.
Masks everything in the model except for components with penetrations or intersections. Note that this option only applies to components for which you have run the current penetration check; other components may be interacting, but if you have not run a check on them they do not appear as interacting, and they will be masked.
Masks everything in the model, including the interacting components, except for the specific elements that penetrate or intersect.


Masks everything in the model, including the interacting components, except for the specific elements and neighbors that penetrate or intersect.

Manual Fix Tools

Button Action
Select Elements By Tree. When enabled, clicking the lowest-level component in the browser selects all of its failed elements.
Select Elements Manually. When enabled, you can click each desired element belonging to the lowest-level component in the browser. This includes the ability to select non-failed elements or a sub-set of the failed elements.
Select Nodes By Tree. When enabled, clicking the lowest-level component in the browser selects all of the penetrating nodes in its failed elements. This differs from Select Elements By Tree in that individual nodes can be moved to fix a penetration, thus changing the shape of a failed element, instead of moving entire elements.
Select Nodes Manually. When enabled, you can click each desired node belonging to the lowest-level component in the browser. This includes the ability to select individual nodes of non-failed elements, or a sub-set of nodes belonging to the failed elements.
Determines the direction that you wish to manually move the selected nodes or elements. Click the small triangle, in the bottom corner, to select one of the following:
Move along the average normal of the selected elements, or related elements in the case of selected nodes.
Move along a fixed vector.
Move along the X axis.
Move along the Y axis.
Move along the Z axis.
Move along an already-existing vector entity in your model that you select.
Move along nodes in your model that you select to define the direction vector. If you pick two nodes, they define the direction. If you pick three nodes, the direction is the normal of the plane that these three nodes define (picking more than three nodes uses only the last three picked.)
Moves the selected nodes/elements by the negative amount specified in the numeric text box.
Moves the selected nodes/elements by the positive amount specified in the numeric text box.