Delamination
By adding a Delamination node, you can model interfacial failure between the layers in a laminate.
The formulation of the delamination models is essentially identical to the decohesion model used in contact simulations. See also:
•
Including Adhesion and Decohesion, and The Decohesion Node in the Structural Mechanics Modeling chapter.
•
Decohesion in the Structural Mechanics Theory chapter.
Interface Selection
Select the interface or interfaces for which this delamination model is to be added.
Table 6-20: Interface Selections; Delamination.
Selection
Apply To
Selection of Individual Interfaces
Boundary
When added: Interior interfaces.
The choice All interfaces is equivalent to Interior interfaces.
When Selected Interfaces is selected.
Only internal interfaces between layers selected in the physics interface can be selected.
If the same interface is selected in two Delamination nodes being active on the same boundary, the second definition will override the previous.
For a general description of layer and interface selections, see The Shell Properties and Interface Selection Sections.
Coordinate System Selection
The interface stresses are defined as boundary tractions with respect to the selected coordinate system. The selection is limited to boundary systems. Make sure that the tangents of the selected boundary system are well defined.
Initial State
Select an initial state for the interface, Bonded or Delaminated. If the state is delaminated, the effect of this node is only to act as a contact condition between the two delaminated layers. In this case, only the Contact section of the settings is displayed.
Adhesion
In this section, you specify the stiffness of the adhesive layer in the normal and tangential directions. The adhesive normal stiffness is used in tension only; in compression the penalty factor is always used.
The default is to set Adhesive stiffness to User defined. For this setting you enter each component of the stiffness vector kA individually.
When Adhesive stiffness is set to Use material data, the stiffness vector kA is computed from material data and layer thickness. From the Specify list, select a pair of elastic properties — Young’s modulus and Poisson’s ratio, Young’s modulus and shear modulus, or Bulk modulus and shear modulus. For the chosen properties, select from the applicable list to use the value From material or enter a User defined value or expression. In order to use From material, you must have assigned a material to the selected boundaries.
Enter a Thickness, ds, to specify the physical thickness of the adhesive layer.
Delamination
Select a Cohesive zone model — Displacement-based damage or Energy-based damage to choose the type of variable that controls the damage process.
Select a Traction separation law — Linear, Exponential, Polynomial, or Multilinear. The definition of these differ between the two cohesive zone models, and the last option is available only for Displacement-based damage.
For the displacement-based damage models, enter:
•
Tensile strength, σt. This is the peak stress in pure tension.
•
Shear strength, σs. This is the peak stress in pure shear.
•
Tensile energy release rate, Gct. This is the energy released during the whole delamination process in a state of pure tension.
•
Shear energy release rate, Gcs. This is the energy released during the whole delamination process in a state of pure shear.
For Multilinear separation, also enter the Shape factor, λ.
When the traction separation law is Linear, Exponential, or Polynomial select the Mixed mode criterion to be either Power law or Benzeggagh-Kenane. In either case, enter the Mode mixity exponent α. The mixed mode criterion determines how normal and shear components are combined into a single scalar failure criterion. For the Multilinear separation law, the mixed mode criterion is always linear (equivalent to a power law with  α= 1.)
For the energy-based damage models, enter:
•
Tensile damage threshold, G0t. This is the elastic energy at the onset of damage in pure tension.
•
Shear damage threshold, G0s. This is the elastic energy at the onset of damage in pure shear.
•
Tensile energy release rate, Gct. This is the energy released during the whole delamination process in a state of pure tension.
•
Shear energy release rate, Gcs. This is the energy released during the whole delamination process in a state of pure shear.
•
Mode mixity exponent, damage initiation, α0. The value determines how normal and shear components are combined into a single scalar criterion for damage initiation.
•
Mode mixity exponent, αc. The value determines how normal and shear components are combined into a single scalar failure criterion.
•
Smoothening parameter, N. This parameter adjusts the shape of the traction separation law. It is only available for the Exponential and Polynomial options. By default, N = 1; a smaller value gives a smoother behavior.
In the Regularization list it is possible to add a viscous delay to the damage growth for time-dependent studies. Do this by selecting Delayed damage and enter a value for the Characteristic time, τ.
Contact
In this section you specify the Penalty factor used to minimize the overclosure of the two layers during compression in the normal direction. The default is to use From adhesive stiffness, in which case the normal component of the stiffness vector kA is used.
When Penalty factor is set to User defined, enter the Contact pressure penalty factor pn. The default value is <phys>.Eequ/<phys>.d_ad.
Advanced
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
Maximum damage determines the residual stiffness of the adhesive layer after delamination. By default, dmax = 1, which means that no residual stiffness remains. Enter a value smaller than 1 to introduce some residual stiffness.
Select Compute damage dissipation energy to compute and store to the energy dissipated by damage.
Location in User Interface
Context Menus
Layered Shell>Material Models>Delamination
Ribbon
Physics tab with Layered Shell selected in the Model Builder tree:
Boundaries>Delamination