Damage Evolution and Element Removal for Ductile Metals

When material damage occurs, the stress-strain relationship no longer accurately represents the material's behavior. Continuing to use the stress-strain relation introduces a strong mesh dependency based on strain localization, such that the energy dissipated decreases as the mesh is refined. A different approach is required to follow the strain-softening branch of the stress-strain response curve. Hillerborg's (1976) fracture energy proposal is used to reduce mesh dependency by creating a stress-displacement response after damage is initiated. Using brittle fracture concepts, Hillerborg defines the energy required to open a unit area of crack, $G_f$, as a material parameter. With this approach, the softening response after damage initiation is characterized by a stress-displacement response rather than a stress-strain response.

The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length, L, associated with an integration point. The fracture energy is then given as

This expression introduces the definition of the equivalent plastic displacement, ${\overline{u}}^{pl}$, as the fracture work conjugate of the yield stress after the onset of damage (work per unit area of the crack). Before damage initiation ${\dot{\overline{u}}}^{pl}=0$; after damage initiation ${\dot{\overline{u}}}^{pl}=L{\dot{\overline{\epsilon }}}^{pl}$.

The definition of the characteristic length depends on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic length is used because the direction in which fracture occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which they crack: some mesh sensitivity remains because of this effect, and elements that have aspect ratios close to unity are recommended. Alternatively, this mesh dependency could be reduced by directly specifying the characteristic length as a function of the element topology and material orientation in user subroutine VUCHARLENGTH (see Defining the Characteristic Element Length at a Material Point in Abaqus/Explicit).

Each damage initiation criterion described in Damage Initiation for Ductile Metals may have an associated damage evolution law. The damage evolution law can be specified in terms of equivalent plastic displacement, ${\overline{u}}^{pl}$, or in terms of fracture energy dissipation, $G_f$. Both of these options take into account the characteristic length of the element to alleviate mesh dependency of the results.

The overall damage variable, D, captures the combined effect of all active mechanisms and is computed in terms of individual damage variables, $d_i$, for each mechanism. You can choose to combine some of the damage variables in a multiplicative sense to form an intermediate variable, $d_{\mathrm{mult}}$, as follows:

Then, the overall damage variable is computed as the maximum of $d_{\mathrm{mult}}$ and the remaining damage variables:

In the above expressions $N_{\mathrm{mult}}$ and $N_{max}$ represent the sets of active mechanisms that contribute to the overall damage in a multiplicative and a maximum sense, respectively, with $N_{\mathrm{act}}=N_{\mathrm{mult}}\cup N_{max}$.

You can specify the damage variable directly as a tabular function of equivalent plastic displacement, $d=d\left({\overline{u}}^{pl}\right)$, as shown in Figure 2(a).

Different definitions of damage evolution based on plastic displacement: (a) tabular, (b) linear, and (c) exponential.

Assume a linear evolution of the damage variable with effective plastic displacement, as shown in Figure 2(b). You can specify the effective plastic displacement, ${\overline{u}}_f^{pl}$, at the point of failure (full degradation). Then, the damage variable increases according to

This definition ensures that when the effective plastic displacement reaches the value ${\overline{u}}^{pl}={\overline{u}}_f^{pl}$, the material stiffness will be fully degraded ($d=1$). The linear damage evolution law defines a truly linear stress-strain softening response only if the effective response of the material is perfectly plastic (constant yield stress) after damage initiation.

Assume an exponential evolution of the damage variable with plastic displacement, as shown in Figure 2(c). You can specify the relative plastic displacement at failure, ${\overline{u}}_f^{pl}$, and the exponent $\alpha$. The damage variable is given as

Assume a linear evolution of the damage variable with plastic displacement. You can specify the fracture energy per unit area, $G_f$. Then, once the damage initiation criterion is met, the damage variable increases according to

where the equivalent plastic displacement at failure is computed as

and ${\sigma }_{y0}$ is the value of the yield stress at the time when the failure criterion is reached. Therefore, the model becomes equivalent to that shown in Figure 2(b). The model ensures that the energy dissipated during the damage evolution process is equal to $G_f$ only if the effective response of the material is perfectly plastic (constant yield stress) beyond the onset of damage.

Assume an exponential evolution of the damage variable given as

The formulation of the model ensures that the energy dissipated during the damage evolution process is equal to $G_f$, as shown in Figure 3(a). In theory, the damage variable reaches a value of 1 only asymptotically at infinite equivalent plastic displacement (Figure 3(b)). In practice, Abaqus/Explicit will set d equal to one when the dissipated energy reaches a value of $0.99G_f$.

Energy-based damage evolution with exponential law: evolution of (a) yield stress and (b) damage variable.

The default setting of $D_{\max }$ depends on whether elements are to be deleted upon material failure. For the default case of element deletion and in all cases for cohesive elements, $D_{\max }=1.0$; otherwise, $D_{\max }=0.99$. Output variable SDEG contains the value of $D\mathrm{.}$ No further damage is accumulated at an integration point once $D$ reaches $D_{\max }$ (except, of course, any remaining stiffness is lost upon element deletion).

A material point is assumed to fail upon reaching maximum degradation. Except for cohesive elements with traction-separation response (see Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description), Abaqus applies damage to all stiffness components equally at material points during the progressive damage process. At any given time during the analysis, the stress tensor in the material is given by the scalar damage equation

where $\overline{\mathit{\sigma }}$ is the effective (or undamaged) stress tensor computed in the current increment. By default, an element is deleted (or removed) from a mesh upon material failure. Details for element deletion driven by material failure are described in Material Failure and Element Deletion. The status of a material point and an element can be determined by requesting output variables STATUSMP and STATUS, respectively.

In a heat transfer analysis the thermal properties of the material are not affected by the damage status of the material stiffness until the element deletion condition is reached; at this point, the thermal contribution of the element is also removed.

Optionally, you may choose not to remove the element from the mesh, except in the case of three-dimensional beam elements. With element deletion turned off, the overall damage variable is enforced to be $D\le D_{\max }$. The default value is $D_{\max }=0.99$ if element deletion is turned off, which ensures that elements will remain active in the simulation with a residual stiffness of at least 1% of the original stiffness. The dimensionality of the stress state of the element affects which stiffness components can become damaged, as discussed below.

In a heat transfer analysis the thermal properties of the material are not affected by damage of the material stiffness.

You can overcome some of the convergence difficulties associated with softening and stiffness degradation by using the viscous regularization scheme, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments.

In this regularization scheme a viscous damage variable is defined by the evolution equation:

where $\eta$ is the viscosity coefficient representing the relaxation time of the viscous system and d is the damage variable evaluated in the inviscid base model. The damaged response of the viscous material is computed using the viscous value of the damage variable. 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 $t/\eta \to \mathrm{\infty }$, where t represents time.

In Abaqus/Standard you can specify the viscous coefficients as part of a section controls definition. For more information, 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.

In general, if any of the ductile evolution models is used, the material Jacobian matrix will be nonsymmetric. To improve convergence, it is recommended that the unsymmetric equation solver is used in this case.