Modeling cohesive zones with ANSYS interface elements

You can create interface elements in the ANSYS environment to define cohesive zones. Interface elements are specialized 3D elements with zero thickness that you can use to model delamination and progressive failure at the interface of two materials. You can create interface elements between two structural elements that have identical faces with coincident nodes.

ANSYS interface elements are designed to represent the cohesive zone between components and to account for the separation across the interface.

To model a cohesive zone in ANSYS, the interface elements and structural elements must have the same characteristics.

Supported ANSYS interface element	Topology	ANSYS structural elements
INTER204	3D, 16-node solid element	SOLID186 and SOLID187 elements.
INTER205	3D, 8-node solid element	SOLID185, SOLSH190

Note:

This software does not support the ANSYS INTER202 and INTER203 interface elements.

For more information on cohesive zones in ANSYS, see Interface Delamination and Failure Simulation in the ANSYS Structural Analysis Guide.

Creating interface elements

Typically, you create a single layer of interface elements between two sets of 2D elements or between the faces of two sets of 3D elements.

• You can use the 3D Swept Mesh command with the Type list set to Manual Between to create one layer of interface elements between specified source and target faces. If the source and target faces are coincident, the software generates interface elements with a thickness value of zero.Note: The software does not check the generated interface elements for possible degenerative elements.

• You can use the Element Extrude command with the Type list set to Element Faces to create interface elements.Note: The software does not check the generated interface elements for elements that have a length of zero.

Defining a cohesive exponential behavior material

Currently, this software supports only the ANSYS exponential material model for cohesive materials. In this software, you use the Cohesive Zone Material option in the appropriate Cohesive Collector dialog box to specify a table field that defines the temperature values and the coefficients, C1, C2, and C3, for each temperature value. These coefficients characterize the separation behavior at the interface.

C1 (σmax)	Maximum normal traction at the interface
C2 (δn)	Normal separation across the interface where the maximum normal traction is attained
C3 (δt)	Shear separation where the maximum shear traction is attained

Checking the quality of interface elements

The Element Quality command supports the following quality checks for INTER204 and INTER205 elements:

• Aspect ratio

• Parallel deviation

• Maximum corner angle

Note:

Warp and Jacobian ratio checks do not apply to ANSYS INTER204 and INTER205 elements.

Where do I find it?

3D Swept Mesh or Element Extrude

Application	Pre/Post
Prerequisite	A FEM file as the work part and displayed partANSYS as the specified solverStructural as the specified analysis type
Command Finder	3D Swept Mesh Element Extrude

Cohesive Collector

Application	Pre/Post
Prerequisite	A Simulation file with ANSYS as the work part and displayed partANSYS as the specified solverStructural as the specified analysis type
Command Finder	Mesh Collector
Location in dialog box	Collector Type→Cohesive Collector

Element Quality

Application	Pre/Post
Prerequisite	A Simulation file with ANSYS as the work part and displayed partANSYS as the specified solverStructural as the specified analysis type
Command Finder	Element Quality

How do I

Create an ANSYS KEYOPT table

Learn more

ANSYS environment

Specifying user defined KEYOPTs for ANSYS

Requesting output for ANSYS analyses

Previewing ANSYS solver syntax

Customizing ANSYS input files with user defined text

Look up more details

Using ANSYS high performance computing options

ANSYS boundary conditions

Modeling cohesive zones with ANSYS interface elements, 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 } });