Structural Contact (ANSYS)

In the ANSYS environment, you can use the Structural Contact command to analyze structural contact between surfaces and edges in ANSYS structural analyses.

In Pre/Post, you use the Structural Contact dialog box to define the contacting surfaces, either manually or automatically. When you export or solve your ANSYS input file, ANSYS automatically creates the necessary contact and target elements.

Contact surface and target elements are created automatically

ANSYS uses special surface elements and target elements to define the contacting and target faces in a contact analysis.

• Contact elements (CONTA172, CONTA174, CONTA175, and CONTA177) overlay the existing 2D or 3D structural elements. The contact elements are those elements which are potentially in contact with the target surface.

• Target elements (TARGE169 and TARGE170) overlay the existing 2D or 3D structural elements on the specified target surface in the contact definition.

Defining source and target surfaces for contact

In the ANSYS environment in Pre/Post:

• You must specify both a source and a target region for contact. You cannot analyze contact with a free thermal surface (contact without a target surface).

• Both the source and target regions must be deformable. In Pre/Post, you cannot analyze contact with a rigid target surface and pilot nodes.

Type of contact is determined by the geometry selected

The type of contact you define is determined by the type of geometry you specify for the source and target regions.

• If you select Manual from the Type list in the Structural Contact dialog box, you use Simulation Regions to define the source and target geometry. With the Manual option, the type of geometry that you specify in each Simulation Region determines the type of contact. You can define:Surface-to-surface contact (CONTA174/TARGE170 pair).Line-to-surface contact (CONTA177/TARGE170 pair).Point-to-surface contact (CONTA175/TARGE170 pair).Line-to-line contact using the edges of planar elements (CONTA172/TARGE169 pair) in either structural analyses or axisymmetric structural analyses.Point-to-line contact using the edges of planar elements (CONTA175/TARGE169 pair).Note: With line-to-line and point-to-line thermal contact, you should use PLANE182 or PLANE183 elements as the underlying structural elements.Note: Although you can create and export these different types of contact in Pre/Post, currently only surface-to-surface (CONTA174/TARGE170) is supported for import into Pre/Post.

• If you select Automatic Pairing from the Type list in the Structural Contact dialog box, the software only searches for appropriate source and target surfaces. Therefore, only surface-to-surface contact (CONTA174/TARGE170 pair) is supported with Automatic Pairing.

Defining the properties and options that control the contact analysis

In the Structural Contact dialog box, after you define the contacting surfaces, you must define:

• A CONTA174 ET modeling object that controls how ANSYS performs the contact analysis.

• A CONTA174 Real Constants modeling object that controls the contact properties used in the analysis.

Note:

The CONTA174 ET and CONTA174 Real Constants modeling objects apply to all ANSYS contact elements, not just CONTA174 elements.

Controlling the contact algorithm through contact element keyopts

In ANSYS, KEYOPT(1) for contact elements controls whether the contact is structural or thermal. In ANSYS Structural environment in Pre/Post , when you use the Structural Contact command to define contact between surfaces, KEYOPT(1) is automatically set to 0 (structural contact) when you export or solve your ANSYS input file. You cannot control the setting of KEYOPT(1) in the user interface.

In the CONTA174 ET dialog box, you can specify the values for the other CONTA172, CONTA174, and CONTA175 KEYOPTs. For example, you can control:

• The points during the analysis at which ANSYS updates the contact stiffness.

• The type of contact, such as rough or sliding.

• Whether to include the effects of shell thickness in the contact analysis.

For example, if you set KEYOPT(2) Contact Algorithm to (2) Multipoint constraint, you can use the Structural Contact definition as a multi-point constraint to connect separate bodies.

Defining contact properties

After you use the Structural Contact dialog box to define the contacting surfaces, you can use the CONTA174 Real Constants dialog box to specify options that control the contact behavior, such as:

• The penetration tolerance factor.

• The limits on the amount of allowable initial penetration.

• The amount of allowable elastic slip.

Additional information

For more information, see:

• The ANSYS Contact Technology Guide.

• CONTA174 in the ANSYS Elements Reference.

• Set the Real Constants and Element KEYOPTS in the Surface-to-Surface Contact chapter of the ANSYS Contact Technology Guide.

Where do I find it?

Application	Pre/Post
Prerequisite	An active Simulation file with ANSYS as the specified solverStructural or Axisymmetric Structural as the specified analysis type
Command Finder	Structural Contact
Simulation Navigator	Under the active solution, right-click Simulation Objects→New Simulation Object→Structural Contact

How do I

Define surface-to-surface contact

Learn more

Surface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS)

Creating ANSYS rigid bodies

Thermal Contact (ANSYS)

Automatic face pairing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Structural Contact (ANSYS), 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 } });