Check contacts, components, or groups for element penetrations and intersections
using the Penetration 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.
From the Validate ribbon, click the Penetration
tool.
Figure 1.
The guide bar and
Penetrations browser opens.
Set up the Penetration Check and check for intersections/penetrations using the
embedded algorithm.
From the guide bar, click and select
Embedded Algorithm for Check method.
Restriction: This is only for the LS-DYNA profile.
For Check type, select the type of collision to check.
From the guide bar, select the type of entity to
be checked for intersections and/or penetrations.
You can select Groups (contacts), Components, Elements, or
Parts.
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.
From the guide bar, click and adjust the
Minimum Penetration depth to filter out penetrations with lower
penetration depth values.
Select a Thickness option.
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.
Select a Thickness>Size option.
Select the Consider edge penetrations checkbox
to consider edge penetrations.
For Boundary shell edge treatment, select a treatment algorithm for the
boundary shell edge.
Choose Flat edges to consider external
borders of the components flat.Figure 2. Flat Edges
Choose Rounded edges to extend external
borders of the component by a cylinder having the diameter of
the component thickness.Figure 3. Rounded Edges
From the guide bar, click Check.
Once the check is complete, the browser
populates with detected intersections and/or penetrations.Figure 4.
Review the penetrations/intersections using the view controls legend.
Figure 5.
Highlight failed: Highlights all elements that caused penetrations or
intersection when you select a component pair the browser.
Contour depth: Displays a color gradient of the penetrating elements in
the selected component pair, which indicates the severity (degree) of
penetration for the interacting elements. This mode is not available for
intersections because their depth cannot be determined.
Penetration Vectors: Displays individual vectors for each penetrating
element in the component that you select in the browser. These vectors
indicate the direction and depth of the penetration for both the
selected component and its interacting components.
Note: If you want to
view the vectors in a fixed size of his choice, you must adjust the
Penetration vector size from the guide bar
under .
This mode
is not available for intersections because their depth cannot be
determined.
Only elements: Masks everything in the model, including the interacting
components, except for the specific elements that penetrate or
intersect.
Fix the penetrations/intersections.
To fix
Do this
Manually
Select groups/components/parts to fix in the Penetration
Browser.
Right-click on the pair, and select Manual
Fix from the context menu.
Note: You can also select the pair in the Penetration
Browser and click on the
guide bar.
Nodes list from
the penetrations are automatically selected. The Manual Fix move
tool opens and will be used to manipulate nodes, elements to
remove the penetrations, or intersections.
From the guide bar, select Recheck to recheck that the
intersection/penetration no longer remains.
Automatically
Select groups/components/parts to fix in the Penetration
Browser.
On the guide bar, click Fix all.
Note: You can also right-click
the pair in the Penetration Browser and select
Auto fix from the context menu.
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.
Set up the Penetration Check and check solver output files for penetrations
using the Solver output file reader method.
Restriction: This capability is only for the LS-DYNA profile. It reads the LS-DYNA message or d3hsp file containing the contact
penetrations information and populates those penetrations in the Penetration
Browser.
From the guide bar, click .
In the Check Method field, select the Solver output file
reader method.
In the Selection field, select contacts (groups) that need to be
checked for penetrations.
If no contact is selected, all penetrations for all contacts written
in the solver output file will be displayed in the browser.
In the Solver output directory, browse and select the path in which the
solver output files are located.
Use Minimum penetration depth to filter out penetrations with lower
penetration depth values.
Select the Create sets of failed entities check
box to automatically generate solver set containing the penetrating
nodes and penetrated segments.
Click Check to read the solver output file and
populate the penetrations in the browser.
Fix the penetrations using automatic or manual methods.
Overview
The Penetration Check tool in HyperMesh is designed to
mimic the respective Finite Element solver on hand to the maximum extent possible. This way,
identified initial penetrations are almost identical to those detected by the solvers
themselves.
Most Finite Element solvers encounter two types of collisions: penetrations and
intersections.
Penetrations
Penetrations themselves are broadly divided into two categories: Node to Segment and
Edge to Edge penetrations. Most commercial Finite Element solvers offer interfaces
that are Node to Segment only, or Edge to Edge only, or more often than not, a
combination of Node to Segment and Edge to Edge.
Node to Segment Penetrations
A node to segment penetration is encountered when a secondary node is
spatially located within the thickness of a main segment:Figure 7.
Such penetrations are usually reported by solvers as “node to surface”
penetrations. During penetration checks, a secondary node is a sphere
with its diameter numerically equal to the maximum thickness of all
secondary segments it is attached to.
The "Gap" used for detection of penetration = (Secondary node thickness / 2)
+ (Main segment thickness / 2)
Figure 8.
In order to accurately identify nodal penetrations at segment boundaries,
like most commercial Finite Element solvers, the Penetration Check tool adds
virtual cylinders to the edges of segment boundaries as shown below:Figure 9.
Penetrations are also encountered when secondary nodes impact virtual
cylindrical edges of main segments:
Some solvers report such penetrations separately as “node to edge,” while
others bundle them together with “nodes to surface” penetrations.
Flat boundary shell edges treatment: During nodes to surface penetration
checks, some modern contact interfaces provide parameters to disable the
addition of virtual cylinders on free/boundary edges of shell elements
(along free edges of shell components).
With this, it is possible to identify ‘true’ penetrations at free edges of
shell components since the checks are now performed on geometries that
accurately represent the physical model.
For such modern interfaces in the Penetration Check tool:
No virtual cylinders are added to the free/boundary edges of main
shell elements.
For secondary nodes of shell elements, the portion of the secondary
node spheres that lie outside the material of the shell elements are
ignored.Figure 10.
Note: A secondary node sphere should not be attached to more than two
free/boundary shell edges. If attached to more than two, the secondary
node sphere will be retained fully.
Edge to Edge Penetrations
Edge to edge penetrations are those that occur when two distinct virtual
edge cylinders of segments (that do not share a common node) interfere
with each other.Figure 11.
Most solvers identify and report such penetrations distinctly as "Edge to
Edge" penetrations.
Special Use Case
Self-penetrations due to extremely thick segments. Some interfaces contain
segments with large thicknesses (when compared to segment edge lengths).
Depending on the type of penetration check performed, you might encounter
penetrations within the same component.
In a node to surface check, the secondary node sphere of one element
penetrates the virtual cylinder of the neighboring main segment.Figure 12.
In an edge to edge check, two virtual cylinders on opposite edges of the
same segment penetrate each other.Figure 13.
Some solvers offer one or both of the following remedies to deal with the
above issues when they are encountered during Node to Surface checks:
Ignore penetrations within the neighborhood of a secondary node.
Penetrations between a secondary node and main segments in its
immediate neighborhood within the same component are ignored. In
Radioss, this method can be
activated for /INTER/TYPE7 type interfaces by setting 'IREM_GAP =
2'. This method, if activated in the Penetration Check tool, will
impose significant computation overhead, thereby impacting the
performance of the tool.
Reduce thickness of main segments by a specified factor. This can be
seen in LS-DYNA single surface contacts,
where the thickness is reduced to 40% of the minimum edge length of
the segment.
Intersections
Intersections are formed when an edge of an element crosses the mid surfaces/faces of
other shell elements/solid elements, respectively. Figure 14.
Intersection checks are not a function of solver parameters and are, therefore,
user-profile agnostic.
Intersections are not reported by most solvers. However, their presence will lead to
severe issues during analyses, and should therefore be avoided at all costs.
Supported Solver Contacts and Parameters
In this section you will find contact and parameter information for the LS-DYNA, PAM-CRASH, and Radioss solver cards.
After performing penetration checks, detailed information regarding penetrating
secondary nodes can be viewed in the node list for selected penetrations.
Figure 15.
The list contains information on all penetrating secondary nodes from the Components
Pair(s)/Group(s) selected in the Penetrations Check browser. The five columns in the
table contain the following information:
Node ID
IDs of the penetrating secondary nodes.
Pene. Depth
The maximum penetration depth for each secondary node listed.
Thickness
The gap (or thickness) value corresponding to the maximum of all penetration
depths for each secondary node listed.
Rel. Pene
The relative penetration value for each secondary node listed. Relative
Penetration = Penetration Depth / Thickness.
Res. Dist
The residual distance (or physical distance) between the mid-plane of the
main segment and the center of the secondary node sphere.
If a secondary node impacts multiple segments (from a "Node to Surface" check) and/or
belongs to an edge that impacts multiple edges (from an "Edge to Edge" check):
The secondary node is listed only once (despite multiple penetrations of
multiple entities)
The information listed against it corresponds to the maximum of all its
penetration depths
and select
Embedded Algorithm for Check method.
Restriction: This is only for the LS-DYNA profile.
Check.
Once the check is complete, the browser populates with detected intersections and/or penetrations.
on the
guide bar.
