Detecting interference and clearance issues between meshes

Use the Interference Check command to check your model for areas where 2D and 3D elements physically interfere with each other. You can use the Interference Check command to check for elements that penetrate or intersect (cross) other elements, or elements that penetrate or intersect themselves.

• Element penetration occurs when two or more elements interfere within their defined element thickness values.

• Element intersection occurs when two or more elements physically intersect each other.

• Element self-interference occurs when elements that are assigned to the same mesh collector penetrate or intersect each other. Elements that share a mesh collector have the same element family, such as 2D or 3D, and have the same material, physical, and display properties.

The following example shows how the Interference Check tool identifies a location where element penetration occurs between two shell meshes. One mesh has an element thickness of 30mm, and the other has an element thickness of 35mm.

Element penetration	Detailed view of the penetrating elements

Checking for interference in FEM, assembly FEM, and Simulation files

The capabilities of the Interference Check command differ slightly, depending on whether you are working in a FEM, an assembly FEM, or a Simulation file.

• In a FEM file and a Simulation file, you can identify and repair element intersection or penetration between selected meshes.

• In an assembly FEM file, you can identify and repair element intersection or penetration between selected meshes or between selected components.

• In a Simulation file, you can identify and repair interference between contact definitions as well between meshes.

Checking for interference between meshes or mesh collectors

In FEM and assembly FEM files, you can use the Interference Check command to check for element interference and penetration between:

• 2D meshes and other 2D meshes

• 2D meshes and 3D meshes

• 3D meshes and other 3D meshes

Checking for interference between contact definitions

In Simulation files, you can use the Interference Check command to check for element penetration and intersection in Contact definitions. In the Interference Set dialog box, when you select Contact Definition from the Selection Type list, you can select any contact definitions either from the graphics window or the Simulation Navigator. The software checks all elements included in the contact definition for interference.

Defining the interference set

You can use the Interference Set options in the Interference Set dialog box to select the meshes that you want the software to check. After you run the Interference Check command, the software lists all interference sets in the Interference Check Navigator. When you select a set in the Interference Check Navigator, you can use the right-click Edit option to add or remove meshes from the set and re-run the check.

Specifying thickness information

2D elements may not physically interfere with each other until you apply any element thickness data. You can use options in the Interference Check dialog box to specify the source of the elements' thickness data and specify a Thickness Factor that the software uses to scale the elements' actual thickness values. You can specify a value between 0.1 and 3. For example, if the elements' assigned thickness is 10mm and you specify a Thickness Factor of 0.8, then the software uses applies a thickness value of 8mm during the interference check calculations.

In the LS-DYNA environment, there are multiple settings that you can use to apply thickness values to elements in contact. When you use the Interference Check command to check for intersections and penetrations between contact definitions in LS-DYNA models, the software examines these settings to compute the appropriate thickness value to apply to the elements. For information on contact thickness calculations for LS-DYNA models, see Contact interference in LS-DYNA models.

Understanding the 2D Element Boundary Treatment

You can use the Shell Element Boundary Treatment option to control how Pre/Post treats element edges on the outer boundary of the mesh during the interference computations. This setting is particularly important when you check for intersection between meshes that include T-type intersections.

Certain explicit solvers, such as LS-DYNA or Radioss, use rounded edges on 2D elements on the outer boundary because they help smooth forces between contact segments. For example, in LS-DYNA, all *CONTACT_AUTOMATIC type contacts include a virtual contact cylinder around each element edge.

Sharp element boundary edges	Rounded element boundary edges

Controlling the distance tolerance for the interference calculations

When you click OK in the Interference Check dialog box, the software calculates whether the selected meshes, mesh collectors, or contact definitions physically interfere within a proximity tolerance. You can use the distance Tolerance value in the Customer Defaults to modify this tolerance value, if necessary.

Working with the Interference Check Navigator

The software reports the results of the Interference Check command in the Interference Check Navigator. You can use different options in the Interference Check Navigator to view or try to repair the intersections or penetrations that the software identifies.

• For more information on the Interference Check Navigator, see Working with the Interference Check Navigator.

• For more information on repairing interference issues, see Repairing interference and clearance issues between elements.

Where do I find it?

Interference Check command

Application	Pre/Post
Prerequisite	A FEM, assembly FEM, or Simulation file active
Command Finder	Interference Check

Proximity Tolerance default

Menu	File→Utilities→Customer Defaults
Location in dialog box	Simulation→Pre/Post→General→Environment tab Tolerance group

Learn more

Working with the Interference Check Navigator

Repairing interference and clearance issues between elements

Contact interference in LS-DYNA models

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Detecting interference and clearance issues between meshes, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });