Mechanical APDL Structural Analysis Guide

12.2.1. Analyzing Interface Delamination

An interface delamination analysis with interface elements involves the same general steps that are in-
volved in any nonlinear analysis procedure. Most of these steps, however, warrant special consideration
with regard to behavior at the cohesive zone.

Following is the general procedure, with special considerations indicated, along with links to applicable
sections where more detailed information is available:

1. Build or import the model.There are no special considerations for building or importing the model for
   an interface delamination analysis. You perform this step as you would in any typical analysis. See
   Building the Model in the Basic Analysis Guide. For further details on building the model, see the Modeling
   and Meshing Guide.


2. Define element type.To properly simulate the cohesive zone, you must define structural element types
   and corresponding interface element types. See Element Selection (p. 399) in this chapter for more details
   on this topic.


3. Define material. Use TB,CZM with TBOPT = EXPO or BILI to define the cohesive zone material that
   characterizes the separation behavior at the interface. You then input the sets of data using the TBDATA
   commands, as applicable.


4. Mesh the model. Use the AMESH or VMESH commands to mesh the structural elements, and use the
   CZMESH command to mesh the cohesive zone element interface along the layers. Special restrictions
   apply to the CZMESH command in terms of matching the source and target. Also, the order in which
   you execute these commands is critical. You can only use CZMESH after the underlying solid model has
   been meshed. You can also generat e interface elements directly using theEGEN command. Each of these
   commands involves special consideration for interface elements. See Meshing and Boundary Condi-
   tions (p. 401) in this chapter for more details on this topic.


5. Solve.There are special solving consideration when you perform an interface delamination analysis.
   These are primarily concerned with the interface element stiffness loss or softening. Care should be taken
   to avoid the numerical instability that may be caused by the delamination and failure of the interface.


6. Review Results.You can print or plot your cohesive zone output items using the PRESOL,PRNSOL,
   PLESOL,PLNSOL, or ESOL commands. See Reviewing the Results in this chapter for more details on this
   topic.

12.2.2. Interface Elements

Four element types are available for simulating interface delamination and failure:

• INTER202 - 2-D, 4-node, linear element.


• INTER203 - 2-D, 6-node, quadratic element.


• INTER204 - 3-D, 16-node, quadratic element.


• INTER205 - 3-D, 8-node, linear element

The 2-D elements,INTER202 and INTER203, use a KEYOPT to define various stress state options.

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

Interface Delamination and Failure Simulation