Creating simulation regions in the ANSYS environment

In the ANSYS environment, you can use the Simulation Region command to create a reusable region that you can use to define the source and target regions in structural and thermal contact definitions. A region is a collection of homogenous entities, such as polygon faces.

When you export or solve your model, the software writes out a single instance of the region to your solver input file, even if that region is referenced by multiple glue or contact definitions.

Creating line regions

You can create a line region for ANSYS contact analyses by using the Selection Filter to select either polygon edges or element edges.

Note:

If you define line contact using element edges, you must select the edges of planar elements.

You can use a line region as the source or target region for:

• Line-to-line contact

• Point-to-line contact

When you export or solve a model that contains a line region, the type of contact elements that the software creates depends upon whether you use the region to define the source or target region in a contact definition.

• If you use a line region as the source region, the software creates CONTA172 elements if the underlying structural elements are planar (either PLANE182 or PLANE183 elements for structural contact, or PLANE55 or PLANE77 elements in thermal contactNote: The planar elements must lie in the X-Y plane.

• If you use a line region as the source region, the software creates CONTA177 elements if the underlying structural elements are not planar.

• If you use a line region as the target region, the software creates TARGE169 elements if the underlying structural elements are planar. ANSYS does not support line regions as target regions if the underlying elements are not planar.

Creating surface regions

You can create a surface region for ANSYS contact analyses by using the Selection Filter to select either polygon faces or element faces.

When you export or solve a model that contains a surface region, the type of contact elements that the software creates depends upon whether you use the region to define the source or target region in a contact definition.

• If you use a surface region as the source region, the software creates CONTA174 elements.

• If you use a surface region as the target region, the software creates TARGE170 elements.

Creating point regions

You can create a point region for ANSYS contact analyses by using the Selection Filter to select only nodes.

Note:

You can only use a point region as a source region in a contact definition.

When you export or solve a model that contains a point region, the software creates CONTA175 elements.

Understanding the ESURF option

In the Region dialog box, the setting for the Use ESURF option controls how the software creates the contact elements in your model.

• If you select Yes, the software uses the ANSYS ESURF command to automatically create the ANSYS contact elements.

• If you select No, the software creates the ANSYS contact elements in your ANSYS input file when you export or solve your model. If you select this option, the software uses the CMBLOCK coded database file command to write out the group of nodes that define the region and used the ESURF command to create the ANSYS contact elements.For more information, see the Programmer's Manual for ANSYS.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file active with ANSYS as the specified solver environment
Command Finder	Simulation Region

Learn more

Automatic face pairing

Working with reusable regions

Creating cross section regions (LS-DYNA)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Creating simulation regions in the ANSYS environment, 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 } });