Mechanical APDL Structural Analysis Guide

• Use the CZMESH command to generat e the interface. You must either define the model into two
  components or groups of elements (between which the cohesive zone interface elements will reside),
  or specify a coordinate value for the line or plane that will divide the model.


• Use the E command to directly generat e interface elements from a set of nodes.


• For generating interface elements directly from a pattern, use the EGEN command.

12.2.4.2. Boundary Conditions

The interface delamination and failure process involves the stiffness softening and complete loss of the
interface stiffness, which in turn will cause numerical instability of the solution.You should therefore
apply your constraints as boundary conditions. Using forces or pressures will generally cause rigid body
motion after the fracture, and will result in other solution difficulties.

12.2.5. Solution Procedure and Result Output.

Interface traction-separation behavior is highly nonlinear. The full Newton-Raphson solution procedure
(the standard ANSYS nonlinear method), is the default method for performing this type of analysis.
Other solution procedures for interface analyses are not recommended.

Like most nonlinear problems, convergence behavior of an interface delamination analysis depends
strongly on the particular problem to be solved. ANSYS has provided a comprehensive solution control
strategy, therefore it is always recommended that you use the ANSYS default solution options, unless
you are sure about the benefits of any changes.

Some special considerations for solving an interface delamination problem:

• When the element breaks apart under external loading, it will lose its stiffness and may cause numerical
  instability.


• It is always a good practice to place the lower and upper limit on the time step size using the DELTIM or
  NSUBST commands, and to start with a small time step, then subsequently ramp it up. This ensures that
  all of the modes and behaviors of interest will be accurat ely included and that the problem is solved ef-
  fectively.


• When interface elements are under tension, the normal stiffness is exponentially related to the separation.
  That is, the greater the separation, the lower the normal stiffness of the elements.


• When interface elements are under compression, you can align contact elements with the interface elements
  to obtain better penetration control.

A convergence failure can indicat e a physical instability in the structure, or it can merely be the result
of some numerical problem in the finite element model.

12.2.6. Reviewing the Results

Results from an interface delamination analysis consist mainly of displacements, stresses, strains and
reaction forces of the structural components and the cohesive zone layer information (interface tension,
separation, etc.). You can review these results in POST1, the general postprocessor, or in POST26, the
time-history postprocessor. See the Output Data sections of the element descriptions for any of the
interface elements (for example INTER202) for a description of the available output components.

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

Interface Delamination and Failure Simulation