Defining the constitutive response of cohesive elements using a continuum approach | ||
| ||
ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE
Behavior of cohesive elements with conventional material models
The implementation of the conventional material models (including user-defined models) in Abaqus for cohesive elements is based on certain assumptions regarding the state of the deformation in the cohesive layer. Two different classes of problems are considered: modeling of an adhesive layer of finite thickness and modeling of gaskets.
Modeling of damage with cohesive elements for these classes of problems can be carried out in both Abaqus/Standard and Abaqus/Explicit (see About progressive damage and failure for details regarding the damage models). You may need to alter the damage model for an adhesive material to account for the fact that the failure of an adhesive bond may occur at the interface between the adhesive and the adherend rather than within the adhesive material.
When used with conventional material models in Abaqus, cohesive elements use true stress and strain measures. When used with a material model that is based on a traction-separation description (see Defining the constitutive response of cohesive elements using a traction-separation description for details on this approach), cohesive elements use nominal stress and strain measures.
The frequency characteristics of cohesive elements are accounted for by the algorithms to automatically choose the time increment in Abaqus/Explicit (Explicit dynamic analysis). In many applications involving adhesives or gaskets cohesive elements may be quite thin compared to the other elements, which tends to decrease the stable time increment. See Stable time increment in Abaqus/Explicit for further discussion on this topic, including suggestions on how to avoid significant reductions in the stable time increment when using cohesive elements.
Modeling of an adhesive layer of finite thickness
For adhesive layers with finite thickness it is assumed that the cohesive layer is subjected to only one direct component of strain, which is the through-thickness strain, and to two transverse shear strain components (one transverse shear strain component for two-dimensional problems). The other two direct components of the strain (the direct membrane strains) and the in-plane (membrane) shear strain are assumed to be zero for the constitutive calculations. More specifically, the through-thickness and the transverse shear strains are computed from the element kinematics. However, the membrane strains are not computed based on the element kinematics; they are simply assumed to be zero for the constitutive calculations. These assumptions are appropriate in situations where a relatively thin and compliant layer of adhesive bonds two relatively rigid (compared to the adhesive) parts. The above kinematic assumptions are approximately correct everywhere inside the cohesive layer except around its outer edges.
An additional linear elastic transverse shear behavior can be defined to provide more stability to cohesive elements, particularly after damage has occurred. The transverse shear behavior is assumed to be independent of the regular material response and does not undergo any damage.
Input File Usage
Use the following options (the second option is needed only to define uncoupled transverse shear response):
COHESIVE SECTION, RESPONSE=CONTINUUM TRANSVERSE SHEAR STIFFNESS
Abaqus/CAE Usage
Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Continuum
Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections.
Modeling of gaskets and/or small adhesive patches
The modeling of gaskets and/or small adhesive patches involves situations where there are no lateral constraints on the cohesive layer. Hence, the layers are free to expand in the lateral direction in a stress-free manner. Application areas include individual spot welds and gaskets. The constitutive calculations assume only one direct stress component, which is the through-thickness normal stress. All other stress components, including the transverse shear stress components, are assumed to be zero.
The gasket modeling capability that is offered with this option has some advantages compared to the family of gasket elements in Abaqus/Standard. The cohesive elements are fully nonlinear (the element kinematics properly account for finite strains as well as finite rotations), can contribute mass and damping in a dynamic analysis, and are available in Abaqus/Explicit. The gasket response modeled in the above manner is similar to modeling using the special-purpose gasket elements in Abaqus/Standard with thickness-direction behavior only (see Including gasket elements in a model).
Uncoupled, linear-elastic transverse shear behavior, if desired, can be defined. The transverse shear behavior may either define the response of the gasket and/or adhesive patch or provide stability after damage has occurred in the response in the thickness direction. There is no damage associated with the transverse shear response.
Input File Usage
Use the following options (the second option is needed only to define uncoupled transverse shear response):
COHESIVE SECTION, RESPONSE=GASKET TRANSVERSE SHEAR STIFFNESS
Abaqus/CAE Usage
Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Gasket
Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections.
Output
All standard output variables in Abaqus (Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers) are available for cohesive elements that are used with conventional material models. The stresses due to the additional transverse shear response are reported separately using the output variables TSHR13 and (in three dimensions) TSHR23. These stresses are not added to the usual material point stresses reported using the output variable S.