Defining the constitutive response of cohesive elements using a traction-separation description

To define the constitutive response of the cohesive element directly in terms of traction versus separation, you choose a traction-separation response when defining the section behavior of the cohesive elements.

COHESIVE SECTION, RESPONSE=TRACTION SEPARATION

Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Traction Separation

The available traction-separation model in Abaqus assumes initially linear elastic behavior (see Defining elasticity in terms of tractions and separations for cohesive elements) followed by the initiation and evolution of damage. The elastic behavior is written in terms of an elastic constitutive matrix that relates the nominal stresses to the nominal strains across the interface. The nominal stresses are the force components divided by the original area at each integration point, while the nominal strains are the separations divided by the original thickness at each integration point. The default value of the original constitutive thickness is 1.0 if traction-separation response is specified, which ensures that the nominal strain is equal to the separation (i.e., relative displacements of the top and bottom faces). The constitutive thickness used for traction-separation response is typically different from the geometric thickness (which is typically close or equal to zero). See Specifying the constitutive thickness for a discussion on how to modify the constitutive thickness.

The nominal traction stress vector, $\mathbf{t}$, consists of three components (two components in two-dimensional problems): $t_n$, $t_s$, and (in three-dimensional problems) $t_t$, which represent the normal (along the local 3-direction in three dimensions and along the local 2-direction in two dimensions) and the two shear tractions (along the local 1- and 2-directions in three dimensions and along the local 1-direction in two dimensions), respectively. The corresponding separations are denoted by ${\delta }_n$, ${\delta }_s$, and ${\delta }_t$. Denoting by $T_o$ the original thickness of the cohesive element, the nominal strains can be defined as

The elastic behavior can then be written as

The elasticity matrix provides fully coupled behavior between all components of the traction vector and separation vector and can depend on temperature and/or field variables. Set the off-diagonal terms in the elasticity matrix to zero if uncoupled behavior between the normal and shear components is desired.

Optionally, for the uncoupled traction behavior a compression factor can be specified; this ensures that the compressive stiffness is equal to the specified factor times the tensile stiffness, $E_{nn}$. This factor affects only the traction response for separation in the normal direction; the shear behavior is not affected.

ELASTIC, TYPE=TRACTION

ELASTIC, TYPE=TRACTION, COMPRESSION FACTOR=f

ELASTIC, TYPE=COUPLED TRACTION

Property module: material editor: MechanicalElasticityElastic: Type: Traction

Property module: material editor: MechanicalElasticityElastic: Type: Coupled Traction

The material parameters, such as the interfacial elastic stiffness, for a traction-separation model can be better understood by studying the equation that represents the displacement of a truss of length L, elastic stiffness E, and original area A, due to an axial load P:

This equation can be rewritten as

where $S=P/A$ is the nominal stress and $K=E/L$ is the stiffness that relates the nominal stress to the displacement. Likewise, the total mass of the truss, assuming a density $\rho$, is given by

The above equations suggest that the actual length L may be replaced with 1.0 (to ensure that the strain is the same as the displacement) if the stiffness and the density are appropriately reinterpreted. In particular, the stiffness is $K=\left(E/L\right)$ and the density is $\overline{\rho }=\left(\rho L\right)$, where the true length of the truss is used in these equations. The density represents mass per unit area instead of mass per unit volume.

These ideas can be carried over to a cohesive layer of initial thickness $T_c$. If the adhesive material has stiffness $E_a$ and density ${\rho }_c$, the stiffness of the interface (relating the nominal traction to the nominal strain) is given by $E_c=\left(E_a/T_c\right)T_o$ and the density of the interface is given by $\overline{{\rho }_c}=\left({\rho }_c{T}_c\right)$. As discussed earlier, the default choice of the constitutive thickness $T_o$ for modeling the response in terms of traction versus separation is 1.0 regardless of the actual thickness of the cohesive layer. With this choice, the nominal strains are equal to the corresponding separations. When the constitutive thickness of the cohesive layer is “artificially” set to 1.0, ideally you should specify $E_c$ and $\overline{{\rho }_c}$ (if needed) as the material stiffness and density, respectively, as calculated with the true thickness of the cohesive layer.

The above formulae provide a recipe for estimating the parameters required for modeling the traction-separation behavior of an interface in terms of the material properties of the bulk adhesive material. As the thickness of the interface layer tends to zero, the above equations imply that the stiffness, $E_c$, tends to infinity and the density, $\overline{{\rho }_c}$, tends to zero. This stiffness is often chosen as a penalty parameter. A very large penalty stiffness is detrimental to the stable time increment in Abaqus/Explicit and may result in ill-conditioning of the element operator in Abaqus/Standard. Recommendations for the choice of the stiffness and density of an interface for an Abaqus/Explicit analysis such that the stable time increment is not adversely affected are provided in Stable time increment in Abaqus/Explicit.

Time domain viscoelasticity can be used in Abaqus/Explicit to model rate-dependent behavior of cohesive elements with traction-separation elasticity. The evolution equation for the normal and two shear nominal tractions take the form:

where $t_n^0\left(t\right)$, $t_s^0\left(t\right)$, and $t_t^0\left(t\right)$ are the instantaneous nominal tractions at time t in the normal and the two local shear directions, respectively. The functions $g_R\left(t\right)$ and $k_R\left(t\right)$ represent the dimensionless shear and normal relaxation moduli, respectively. See Defining viscoelastic behavior for traction-separation elasticity in Abaqus/Explicit for additional details and usage information.

You can also combine time domain viscoelasticity with the models for progressive damage and failure described in the next sections. This combination allows modeling rate-dependent behavior both during the initial elastic response (prior to damage initiation), as well as during damage progression.

Both Abaqus/Standard and Abaqus/Explicit allow modeling of progressive damage and failure in cohesive layers whose response is defined in terms of traction-separation. By comparison, only Abaqus/Explicit allows modeling of progressive damage and failure for cohesive elements modeled with conventional materials (Defining the constitutive response of cohesive elements using a continuum approach). Damage of the traction-separation response is defined within the same general framework used for conventional materials (see About progressive damage and failure). This general framework allows the combination of several damage mechanisms acting simultaneously on the same material. Each failure mechanism consists of three ingredients: a damage initiation criterion, a damage evolution law, and a choice of element removal (or deletion) upon reaching a completely damaged state. While this general framework is the same for traction-separation response and conventional materials, many details of how the various ingredients are defined are different. Therefore, the details of damage modeling for traction-separation response are presented below.

The initial response of the cohesive element is assumed to be linear as discussed above. However, once a damage initiation criterion is met, material damage can occur according to a user-defined damage evolution law. Figure 1 shows a typical traction-separation response with a failure mechanism. If the damage initiation criterion is specified without a corresponding damage evolution model, Abaqus will evaluate the damage initiation criterion for output purposes only; there is no effect on the response of the cohesive element (i.e., no damage will occur). The cohesive layer does not undergo damage under pure compression.

Figure 1. Typical traction-separation response.

As the name implies, damage initiation refers to the beginning of degradation of the response of a material point. The process of degradation begins when the stresses and/or strains satisfy certain damage initiation criteria that you specify. Several damage initiation criteria are available and are discussed below. Each damage initiation criterion also has an output variable associated with it to indicate whether the criterion is met. A value of 1 or higher indicates that the initiation criterion has been met (see Output for further details). Damage initiation criteria that do not have an associated evolution law affect only output. Thus, you can use these criteria to evaluate the propensity of the material to undergo damage without actually modeling the damage process (i.e., without actually specifying damage evolution).

In the discussion below, $t_n^o$, $t_s^o$, and $t_t^o$ represent the peak values of the nominal stress when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. Likewise, ${\epsilon }_n^o$, ${\epsilon }_s^o$, and ${\epsilon }_t^o$ represent the peak values of the nominal strain when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. With the initial constitutive thickness $T_o=1$, the nominal strain components are equal to the respective components of the relative displacement—${\delta }_n$, ${\delta }_s$, and ${\delta }_t$—between the top and bottom of the cohesive layer. The symbol $⟨⟩$ used in the discussion below represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a pure compressive deformation or stress state does not initiate damage.

The damage evolution law describes the rate at which the material stiffness is degraded once the corresponding initiation criterion is reached. The general framework for describing the evolution of damage in bulk materials (as opposed to interfaces modeled using cohesive elements) is described in Damage evolution and element removal for ductile metals. Conceptually, similar ideas apply for describing damage evolution in cohesive elements with a constitutive response that is described in terms of traction versus separation; however, many details are different.

A scalar damage variable, D, represents the overall damage in the material and captures the combined effects of all the active mechanisms. It initially has a value of 0. If damage evolution is modeled, D monotonically evolves from 0 to 1 upon further loading after the initiation of damage. The stress components of the traction-separation model are affected by the damage according to

where ${\overline{t}}_n$, ${\overline{t}}_s$ and ${\overline{t}}_t$ are the stress components predicted by the elastic traction-separation behavior for the current strains without damage.

To describe the evolution of damage under a combination of normal and shear deformation across the interface, it is useful to introduce an effective displacement (Camanho and Davila, 2002) defined as

You have control over how Abaqus treats cohesive elements with severe damage. By default, the upper bound to the overall damage variable at a material point is $D_{max}=1.0$. You can reduce this upper bound as discussed in Controlling element deletion and maximum degradation for materials with damage evolution. You can control what happens to the cohesive element when the damage reaches this limit, as discussed below.

By default, once the overall damage variable reaches $D_{max}$ at all of its material points and none of its material points are in compression, the cohesive elements, except for the pore pressure cohesive elements, are removed (deleted). See Controlling element deletion and maximum degradation for materials with damage evolution for details. This element removal approach is often appropriate for modeling complete fracture of the bond and separation of components. Once removed, cohesive elements offer no resistance to subsequent penetration of the components, so it may be necessary to model contact between the components as discussed in Defining contact between surrounding components.

Alternatively, you can specify that a cohesive element should remain in the model even after the overall damage variable reaches $D_{max}$. In this case the stiffness of the element in tension and/or shear remains constant (degraded by a factor of 1 − $D_{max}$ over the initial undamaged stiffness). This choice is appropriate if the cohesive elements must resist interpenetration of the surrounding components even after they have completely degraded in tension and/or shear (see Defining contact between surrounding components). In Abaqus/Explicit it is recommended that you suppress bulk viscosity in the cohesive elements by setting the scale factors for the linear and quadratic bulk viscosity parameters to zero using section controls (see Section controls).

An optional linear elastic transverse shear behavior can be defined to provide additional 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.

COHESIVE SECTION, RESPONSE=TRACTION SEPARATION
TRANSVERSE SHEAR STIFFNESS

Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of viscous regularization of the constitutive equations, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments.

The traction-separation laws can be regularized in Abaqus/Standard using viscosity by permitting stresses to be outside the limits set by the traction-separation law. The regularization process involves the use of a viscous stiffness degradation variable, $D_v$, which is defined by the evolution equation:

where $\mu$ is the viscosity parameter representing the relaxation time of the viscous system and D is the degradation variable evaluated in the inviscid backbone model. The damaged response of the viscous material is given as

Using viscous regularization with a small value of the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscous system relaxes to that of the inviscid case as $t/\mu \to \mathrm{\infty }$, where t represents time. You can specify the value of the viscosity parameter as part of the section controls definition (see Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard). If the viscosity parameter is different from zero, output results of the stiffness degradation refer to the viscous value, $D_v$. The default value of the viscosity parameter is zero so that no viscous regularization is performed. Use of viscous regularization for improving the convergence behavior of delamination and debonding problems is discussed in Delamination analysis of laminated composites and Analysis of skin-stiffener debonding under tension.

The approximate amount of energy associated with viscous regularization over the whole model or over an element set is available using output variable ALLCD.