A set of four interface elements is available for modeling interface delamination at the interface of two materials. The elements are capable of representing the cohesive zone between the interface and can account for the separation across the interface.
The following related topics are available:
Also see Modeling Interface Delamination with Contact Elements (Debonding).
An interface delamination analysis with interface elements involves the same general steps involved in any nonlinear analysis. Most of these steps, however, require special consideration with regard to behavior at the cohesive zone:
Build or import the model.
No special considerations apply when building or importing a model for an interface delamination analysis.
See Building the Model in the Basic Analysis Guide. For more information about building the model, see the Modeling and Meshing Guide.
Define the element types.
Define structural element types and corresponding interface element types. See Element Selection for more information.
Define the CZM material.
Define the cohesive zone material (CZM) characterizing the separation behavior at the interface (TB,CZM with
TBOPT= EXPO or BILI) . Input the necessary data (TBDATA).Mesh the model.
Mesh the structural elements (AMESH or VMESH), then mesh the cohesive zone element interface along the layers (CZMESH).
Restrictions apply to CZMESH with regard to matching the source and target. Also, the order in which the commands execute is critical. Issue CZMESH only after the underlying solid model has been meshed.
You can also generate interface elements directly (EGEN).
Each command involves special considerations for interface elements. See Meshing and Boundary Conditions for more information.
Solve.
Special solver considerations apply when performing an interface delamination analysis, primarily involving interface element-stiffness loss or softening. Numerical instability can occur due to delamination and failure of the interface.
Review the Results.
You can print or plot the cohesive zone output items (PRESOL, PRNSOL, PLESOL, PLNSOL, or ESOL). See Reviewing the Results for more information.
Four element types are available for simulating interface delamination and failure:
The 2D elements, INTER202 and INTER203, use a KEYOPT to define various stress state options.
An interface element is composed of bottom and top surfaces. Figure 205.1: INTER205 Geometry in the Element Reference shows the geometry of a 3D 8-node interface element. The element midplane can be created by averaging the coordinates of node pairs from the bottoms and top surfaces of the element. The numerical integration of the interface elements is performed in the element midplane. The Gauss integration scheme is used for the numerical integrations.
The simulation of an entire assembly, consisting of the cohesive zone and the structural elements on either side of the cohesive zone, requires that the interface elements and structural elements have the same characteristics. When you issue the CZMESH command, the appropriate interface element(s) is selected automatically, depending on the adjacent structural elements. You can also manually specify your interface elements. Use the following table as a guideline for choosing interface and structural elements that have the same characteristics:
| For elements with these characteristics: | ... use this interface element: | ... with one of these structural elements: |
|---|---|---|
| 2D, linear | INTER202 | PLANE182 |
| 2D, quadratic | INTER203 | PLANE183 |
| 3D, quadratic | INTER204 | SOLID186, SOLID187 |
| 3D, linear | INTER205 | SOLID185, SOLSH190, SOLID272, SOLID273, SOLID285 |
Proper element type is chosen based on the stress states of interest and structural element types used.
Element selection is done by the element type command, ET, for example,
ET,1,205
defines element type 1 as element INTER205.
The following material-definition topics are available for modeling interface delamination with interface elements:
The TB,CZM command defines interface separation behavior with interface elements. The interface is represented by a single element set of these elements. The interface deformation is characterized by a traction separation law (see below), with the deformation occurring only within the interface elements (the cohesive zone).
The tension or shear deformations within this zone are of primary interest.
The surface behavior of the material depends on the type of CZM model specified
(TB,CZM,,,,TBOPT, where
TBOPT = EXPO or BILI). Unloading behavior is not
addressed in the CZM with exponential law (TB,CZM,,,,EXPO).
The surface behavior of the material is highly nonlinear in either case, and the resulting softening or loss of stiffness changes character rapidly as the element separation increases. Unloading behavior is not addressed in this configuration.
The cohesive zone model
(TB,CZM,,,,EXPO) uses a
traction-separation law, defined as:
for normal traction at the interface, and
for shear traction at the interface, where:
The material constants σmax, 
, and 
are input as C1, C2, and C3. The input format is
TB,CZM,,,, TBDATA,1,C1,C2,C3
This CZM material option must be used with interface elements INTER202, INTER203, INTER204, and INTER205.
The cohesive zone model (TB,CZM,,,,BILI) uses bilinear traction-separation laws, defined as:
where
The material constants are input via the TBDATA command:
| Constant | Meaning | Property |
|---|---|---|
| C1 | σmax | Maximum normal traction |
| C2 |
| Normal displacement jump at the completion of debonding |
| C3 | τmax | Maximum tangential traction |
| C4 |
| Tangential displacement jump at the completion of debonding |
| C5 | α | Ratio of  to  , or ratio of
 to 
Note:
|
| C6 | β | Non-dimensional weighting parameter |
For more information about defining a cohesive zone material in an interface delamination analysis, see Bilinear Cohesive Zone Material for Interface Elements and Contact Elements in the Material Reference.
The cohesive zone material (CZM) model supports viscous regularization (TB,CZM,,,,VREG) for stabilizing interface delamination. For more information, see Cohesive Material Law in the Material Reference and Viscous Regularization in the Mechanical APDL Theory Reference.
There are three options available for meshing interface elements:
Use the CZMESH command to generate 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 generate interface elements from a set of nodes.
For generating interface elements directly from a pattern, use the EGEN command.
For most cases, Ansys, Inc. recommends using linear elements.
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.
Interface traction-separation behavior is highly nonlinear. The full Newton-Raphson solution procedure (the standard Mechanical APDL nonlinear method), is the default method for performing this type of analysis. Other solution procedures for interface analyses are not recommended.
As with most nonlinear problems, convergence behavior of an interface delamination analysis depends on the given problem to be solved. Mechanical APDL offers a comprehensive solution-control strategy; therefore, it is always best to use the 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 (DELTIM or NSUBST), 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 accurately included and that the problem is solved effectively.
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 indicate a physical instability in the structure, or it can merely be the result of some numerical problem in the finite element model.
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 the results in POST1, the general postprocessor, or in POST26, the time-history postprocessor. The results file (Jobname.RST) must be available.
The following topics are available:
For a description of the available output components, see the Output Data sections of the element descriptions for any of the interface elements (for example, INTER202).
In POST1, only one substep can be read in at a time, and that the results from that substep should have been written to Jobname.RST. (The load step option command OUTRES controls which substep results are stored on Jobname.RST.) A typical POST1 postprocessing sequence is described below.
To review results in POST1, the database must contain the same model for which the solution was calculated.
Verify from your output file (Jobname.out) whether or not the analysis converged at all load steps.
If not, you probably won't want to postprocess the results, other than to determine why convergence failed.
If your solution converged, then continue postprocessing.
Enter POST1. If your model is not currently in the database, issue RESUME.
Command(s): /POST1GUI:Read in results for the desired load step and substep, which can be identified by load step and substep numbers or by time.
Command(s): SETGUI:Display the results using any of the following options. Note that cohesive zone element results, such as tension and separation, are always displayed and listed in the local coordinate system.
Option: Display Deformed Shape
Command(s): PLDISPGUI:Option: Contour Displays
Use these options to display contours of stresses, strains, or any other applicable item. When displaying the interface tension distribution, if other structural mating components are not included, Mechanical APDL plots the geometry of those components in gray. To have a better visualization of an interface tension plot, it is better for you to select the interface elements only.
Option: Tabular Listings
Option: Animation
You can also animate interface results over time:
Many other postprocessing functions are available in POST1. See The General Postprocessor (POST1) in the Basic Analysis Guide for details. Load case combinations usually are not valid for nonlinear analyses.
You can also review the load-history response of a nonlinear structure using
POST26, the time-history postprocessor. Use POST26 to compare one Mechanical APDL
variable against another. For example, you might graph the interface separation
vs. interface tension, which should correspond to the material behavior defined
by TB,CZM. You might also graph the displacement at a node
versus the corresponding level of applied load, or you might list the interface
tension at a node and the corresponding TIME value. A
typical POST26 postprocessing sequence for an interface delamination analysis is
the same as the sequence for a typical nonlinear analysis. See steps 1 through 4
in Reviewing Results in POST26 in the Structural Analysis Guide.