Applying Cohesive Material Concepts to XFEM-Based Cohesive Behavior

Linear Elastic Traction-Separation Behavior

The available traction-separation model in Abaqus assumes initially linear elastic behavior followed by the initiation and evolution of damage. The elastic behavior is written in terms of an elastic constitutive matrix that relates the normal and shear stresses to the normal and shear separations of a cracked element.

The nominal traction stress vector, $t$ , consists of the following components: $t_{n}$ , $t_{s}$ , and (in three-dimensional problems) $t_{t}$ , which represent the normal and the two shear tractions, respectively. The corresponding separations are denoted by $δ_{n}$ , $δ_{s}$ , and $δ_{t}$ . The elastic behavior can then be written as

t = {\begin{matrix} t_{n} \\ t_{s} \\ t_{t} \end{matrix}} = [\begin{matrix} K_{n n} & 0 & 0 \\ 0 & K_{s s} & 0 \\ 0 & 0 & K_{t t} \end{matrix}] {\begin{matrix} δ_{n} \\ δ_{s} \\ δ_{t} \end{matrix}} = K δ .

The normal and tangential stiffness components will not be coupled: pure normal separation by itself does not give rise to cohesive forces in the shear directions, and pure shear slip with zero normal separation does not give rise to any cohesive forces in the normal direction.

The terms $K_{n n}$ , $K_{s s}$ , and $K_{t t}$ are calculated based on the elastic properties for an enriched element. Specifying the elastic properties of the material in an enriched region is sufficient to define both the elastic stiffness and the traction-separation behavior. For simplicity, we assume that $K_{n n} = K_{s s} = K_{t t}$ .

Input File Usage

Alternatively, the elastic stiffness can be specified directly by using one of the following options:

SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=LINEAR
SURFACE BEHAVIOR, PENALTY
SURFACE BEHAVIOR, AUGMENTED LAGRANGE

Specifically, if a user-defined material is used, you must define the elastic stiffness using one of the options above.

Abaqus/CAE Usage

Interaction module: contact property editor: MechanicalNormal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Linear; Penalty (Standard); or Augmented Lagrange (Standard)

Damage Modeling

Damage modeling allows you to simulate the degradation and eventual failure of an enriched element. The failure mechanism consists of two ingredients: a damage initiation criterion and a damage evolution law. The initial response is assumed to be linear as discussed in the previous section. However, once a damage initiation criterion is met, damage can occur according to a user-defined damage evolution law. Figure 1 shows a typical linear and a typical nonlinear traction-separation response with a failure mechanism. The enriched elements do not undergo damage under pure compression.

Damage of the traction-separation response for cohesive behavior in an enriched element is defined within the same general framework used for conventional materials (see About Progressive Damage and Failure). However, unlike cohesive elements with traction-separation behavior, you do not have to specify the undamaged traction-separation behavior in an enriched element.

Crack Initiation and Direction of Crack Extension

Crack initiation refers to the beginning of degradation of the cohesive response at an enriched element. The process of degradation begins when the stresses or the strains satisfy specified crack initiation criteria. Crack initiation criteria are available based on the following Abaqus/Standard built-in models:

the maximum principal stress criterion,
the maximum principal strain criterion,
the maximum nominal stress criterion,
the maximum nominal strain criterion,
the quadratic traction-interaction criterion,
the quadratic separation-interaction criterion, and
the three-dimensional LaRC05 criterion.

In addition, a user-defined damage initiation criterion can be specified in user subroutine UDMGINI.

An additional crack is introduced or the crack length of an existing crack is extended after an equilibrium increment when the fracture criterion, f, reaches the value 1.0 within a given tolerance:

1.0 \leq f \leq 1.0 + f_{t o l} .

You can specify the tolerance $f_{t o l}$ . If $f > 1 + f_{t o l}$ , the time increment is cut back such that the crack initiation criterion is satisfied. The default value of $f_{t o l}$ is 0.05. To improve performance, a separate tolerance $f_{t o l}^{g}$ can be specified to control the crack growth of an existing crack while $f_{t o l}$ is used to control the nucleation of an additional crack. If it is not specified, the growth tolerance, $f_{t o l}^{g},$ is set equal to $f_{t o l} .$

Input File Usage

DAMAGE INITIATION, TOLERANCE= $f_{t o l}$ , GROWTH TOLERANCE= $f_{t o l}^{g}$

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Tolerance:  $f_{t o l}$

Fracture of Multiple Elements in an Unstable Crack Growth Analysis

For an unstable crack growth problem, sometimes it is more efficient to allow multiple elements at and ahead of a crack tip to fracture without excessively cutting back the increment size when the fracture criterion is satisfied. Abaqus/Standard activates this capability automatically if you specify an unstable growth tolerance, $f_{t o l}^{u}$ . In this case if the fracture criterion, f, is within the given unstable growth tolerance:

1.0 + f_{t o l} \leq f \leq 1.0 + f_{t o l}^{u},

where

f_{t o l}

is the tolerance described earlier in this section, Abaqus/Standard immediately reduces the time increment size by default to a very small value,

β ▵ t_{\min} .

Reducing the time increment size allows more elements to fracture until

f < 1

for all the elements ahead of the crack tip. You can, however, optionally specify the maximum number of cutbacks allowed,

n

, to be controlled by the regular tolerance,

f_{t o l}

, prior to the activation of the unstable growth tolerance in an increment. After this limit the time increment size is recovered automatically to a larger value,

α ▵ t_{p r e}

, where:

$▵ t_{\min}$: Minimum time increment allowed
$▵ t_{p r e}$: Time increment size prior to the unstable crack growth
$α$ (default 0.5), $β$ (default 2.0), and $n$ (default 0): Scaling parameters

If you do not specify a value for the unstable growth tolerance, the default value is infinity. In this case the fracture criterion, f, for unstable crack growth is not limited by any upper bound value in the above equation.

Input File Usage

Use both of the following options:

DAMAGE INITIATION, UNSTABLE GROWTH TOLERANCE= $f_{t o l}^{u}$ 
CONTROLS, TYPE=NO CUTBACK SCALING

Abaqus/CAE Usage

Use the following option to specify an unstable crack growth tolerance:

Interaction module: Interaction Property Create : Contact: Mechanical Fracture Criterion , Toggle on Specify tolerance for unstable crack propagation, select Specify value

Specifying the Crack Direction

When the maximum principal stress or the maximum principal strain criterion is specified, the newly introduced crack is always orthogonal to the maximum principal stress/strain direction when the fracture criterion is satisfied. However, when one of the other Abaqus/Standard built-in crack initiation criteria is used, you have to specify if the newly introduced crack will be orthogonal to the element local 1-direction or orthogonal to the element local 2-direction (see Conventions) when the fracture criterion is satisfied. By default, the crack is orthogonal to the element local 1-direction. If a user-defined damage initiation criterion is specified, the normal direction to the crack plane or the crack line can be defined in user subroutine UDMGINI.

Input File Usage

Use one of the following options to specify the crack direction when the maximum nominal stress, the maximum nominal strain, the quadratic traction-interaction, or the quadratic separation-interaction criterion is specified:

DAMAGE INITIATION, NORMAL DIRECTION=1 (default)

DAMAGE INITIATION, NORMAL DIRECTION=2

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Direction relative to local 1-direction (for XFEM): Normal or Parallel

Maximum Principal Stress Criterion

The maximum principal stress criterion can be represented as

f = {\frac{⟨ σ_{m a x} ⟩}{σ_{m a x}^{o}}} .

Here, $σ_{m a x}^{o}$ represents the maximum allowable principal stress. The symbol $⟨ ⟩$ represents the Macaulay bracket with the usual interpretation (that is, $⟨ σ_{m a x} ⟩ = 0$ if $σ_{m a x} < 0$ and $⟨ σ_{m a x} ⟩ = σ_{m a x}$ if $σ_{m a x} \geq 0$ ). The Macaulay brackets are used to signify that a purely compressive stress state does not initiate damage. Damage is assumed to initiate when the maximum principal stress ratio (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=MAXPS

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxps Damage

Maximum Principal Strain Criterion

The maximum principal strain criterion can be represented as

f = {\frac{⟨ ε_{m a x} ⟩}{ε_{m a x}^{o}}} .

Here, $ε_{m a x}^{o}$ represents the maximum allowable principal strain, and the Macaulay brackets signify that a purely compressive strain does not initiate damage. Damage is assumed to initiate when the maximum principal strain ratio (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=MAXPE

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxpe Damage

Maximum Nominal Stress Criterion

The maximum nominal stress criterion can be represented as

f = \max {\frac{⟨ t_{n} ⟩}{t_{n}^{o}}, \frac{t_{s}}{t_{s}^{o}}, \frac{t_{t}}{t_{t}^{o}}} .

The nominal traction stress vector, $t$ , consists of three components (two in two-dimensional problems). $t_{n}$ is the component normal to the likely cracked surface, and $t_{s}$ and $t_{t}$ are the two shear components on the likely cracked surface. Depending on what you specify (see Specifying the Crack Direction above), the likely cracked surface will be orthogonal either to the element local 1-direction or to the element local 2-direction. Here, $t_{n}^{o}$ , $t_{s}^{o}$ , and $t_{t}^{o}$ represent the peak values of the nominal stress. The symbol $⟨ ⟩$ represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a purely compressive stress state does not initiate damage. Damage is assumed to initiate when the maximum nominal stress ratio (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=MAXS

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxs Damage

Maximum Nominal Strain Criterion

The maximum nominal strain criterion can be represented as

f = \max {\frac{⟨ ε_{n} ⟩}{ε_{n}^{o}}, \frac{ε_{s}}{ε_{s}^{o}}, \frac{ε_{t}}{ε_{t}^{o}}} .

Damage is assumed to initiate when the maximum nominal strain ratio (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=MAXE

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxe Damage

Quadratic Nominal Stress Criterion

The quadratic nominal stress criterion can be represented as

f = {\frac{⟨ t_{n} ⟩}{t_{n}^{o}}}^{2} + {\frac{t_{s}}{t_{s}^{o}}}^{2} + {\frac{t_{t}}{t_{t}^{o}}}^{2} .

Damage is assumed to initiate when the quadratic interaction function involving the stress ratios (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=QUADS

Abaqus/CAE Usage

Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quads Damage

Quadratic Nominal Strain Criterion

The quadratic nominal strain criterion can be represented as

f = {\frac{⟨ ε_{n} ⟩}{ε_{n}^{o}}}^{2} + {\frac{ε_{s}}{ε_{s}^{o}}}^{2} + {\frac{ε_{t}}{ε_{t}^{o}}}^{2} .

Damage is assumed to initiate when the quadratic interaction function involving the nominal strain ratios (as defined in the expression above) reaches a value of one.

Input File Usage

DAMAGE INITIATION, CRITERION=QUADE

Abaqus/CAE Usage

Property module: material editor: : Damage for Traction Separation Laws: Quade Damage

Larc05 Three-Dimensional Criterion

The LaRC05 three-dimensional criterion can be applied generally to polymer-matrix fiber-reinforced composites. This criterion considers four different damage initiation mechanisms: matrix cracking, fiber kinking, fiber splitting, and fiber tension. For detailed information on the damage initiation criterion, see LaRC05 Criterion.

The initiation criterion that first reaches a value of 1.0 determines the damage initiation.

Input File Usage

DAMAGE INITIATION, CRITERION=LARC05

Abaqus/CAE Usage

The LaRC05 damage initiation criterion is not supported in Abaqus/CAE.

User-Defined Damage Initiation Criterion

User subroutine UDMGINI provides a general capability for implementing a user-defined damage initiation criterion.

You can define several damage initiation mechanisms in user subroutine UDMGINI. You represent each damage initiation mechanism by a fracture criterion, $f_{i n d e x i}$ , and its associated normal direction to the crack plane or the crack line. Although you can define several damage initiation mechanisms, the actual damage initiation for an enriched element is governed by the most severe damage initiation mechanism:

f = \max {f_{i n d e x 1}, f_{i n d e x 2}, \dots f_{i n d e x n}} .

Damage is assumed to initiate when f, as defined in the expression above, reaches a value of one.

You must specify any material constants that are needed in user subroutine UDMGINI as part of a user-defined damage initiation criterion definition.

Input File Usage

Use the following option to define a user-defined damage initiation criterion:

DAMAGE INITIATION, CRITERION=USER

Use the following option to specify the total number of failure mechanisms in the user-defined damage initiation criterion:

DAMAGE INITIATION, CRITERION=USER, FAILURE MECHANISMS= $n$

Use the following option to define properties for a user-defined damage initiation criterion:

DAMAGE INITIATION, CRITERION=USER, PROPERTIES=number_of_constants

Abaqus/CAE Usage

Defining a user-defined damage initiation criterion is not supported in Abaqus/CAE.

Limiting the Crack Propagation Direction

When the maximum principal stress, maximum principal strain, or user-defined damage initiation criterion is specified, you can limit the new crack propagation direction to within a certain angle (in degrees) of the previous crack propagation direction. The default is 85°.

Input File Usage

Use the following option to set the maximum allowed change in the crack propagation angle (in degrees):

DAMAGE INITIATION, ANGLEMAX=max_angle

Abaqus/CAE Usage

Limiting the crack propagation direction is not supported in Abaqus/CAE.

Local Calculations of the Stress and Strain Fields Ahead of the Crack Tip

An accurate and efficient evaluation of the stress/strain fields ahead of the crack tip is important for both evaluating the crack initiation criterion and computing the crack propagation direction when needed. Abaqus/Standard offers several options for computing these fields.

Centroidal Values of Stress and Strain

By default, the stress/strain computed at the element centroid ahead of the crack tip is used to determine if the damage initiation criterion is satisfied and to determine the crack propagation direction. See Figure 2.

Input File Usage

DAMAGE INITIATION, POSITION=CENTROID (default)

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Position Centroid

Computing the Stress and Strain Fields at the Crack Tip

With a sufficiently refined mesh, the centroidal approximation is accurate and economical. However, if the finite element mesh in the vicinity of the crack tip is coarse relative to the gradients in the stress/strain fields, the default centroidal approximation may not be sufficient. In such cases you can use the stress/strain extrapolated to the crack tip to determine if the damage initiation criterion is satisfied and to determine the crack propagation direction. See Figure 2.

Input File Usage

DAMAGE INITIATION, POSITION=CRACKTIP

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Position Crack tip

Combining Crack Tip and Centroidal Calculations

You can also choose to combine the two previous alternatives: you can use the stress/strain values extrapolated to the crack tip to determine if the damage initiation criterion is satisfied, and you can use the stress/strain values at the element centroid to determine the crack propagation direction.

Input File Usage

DAMAGE INITIATION, POSITION=COMBINED

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Position Combined

Nonlocal Averaging of the Stress/Strain Fields and Smoothing of the Crack Surface Normals to Improve the Accuracy of Crack Propagation Directions

The three options for evaluating the stress and strain fields discussed above are local calculations in the sense that the evaluated fields are local to the single element ahead of the crack tip. In the case of coarse and/or unstructured meshes a nonlocal averaging of the stress and strain fields ahead of the crack tip can lead to a more accurate evaluation of those fields, which can improve the accuracy of the computed propagation directions. In addition, a moving least-squares approximation by polynomials is used by default to obtain more accurate crack propagation directions. The least-squares approximation further smooths out the normals of the individual crack facets in elements along the crack front that satisfy the damage initiation criterion.

Input File Usage

DAMAGE INITIATION, POSITION=NONLOCAL

Abaqus/CAE Usage

Nonlocal averaging of the stress/strain fields and smoothing of the crack surface normals are not supported in Abaqus/CAE.

Specifying the Region of the Model Used for Nonlocal Averaging and Smoothing

To control the range of elements used for nonlocal averaging and smoothing in the crack direction calculations, you can specify a radius, $r_{c}$ , within which the elements ahead of the crack tip are included (see Figure 3). The default radius is three times the typical element characteristic length in the enriched region.

Input File Usage

DAMAGE INITIATION, R CRACK DIRECTION= $r_{c}$

Abaqus/CAE Usage

Specifying the range of the model for nonlocal averaging and smoothing is not supported in Abaqus/CAE.

Smoothing the Stress/Strain Fields before Averaging

To further improve the nonlocal averaging, you can request an initial smoothing of the stress/strain fields ahead of the crack. In this case Abaqus/Standard averages the field values to element nodes and then interpolates the smoothed fields to the integration points. Once smoothing is complete, the nonlocal averaging is applied. No smoothing is applied by default.

Input File Usage

Use one of the following options:

DAMAGE INITIATION, SMOOTHING=NONE (default)
DAMAGE INITIATION, SMOOTHING=NODAL

Abaqus/CAE Usage

Smoothing the stress/strain fields before averaging is not supported in Abaqus/CAE.

Weighting Schemes for Nonlocal Averaging

Abaqus/Standard offers a number of weighting schemes for field smoothing that provide additional control over nonlocal averaging. For example, you may want to give a higher weighting to elements close to the crack tip. You can specify a weight function, $ω$ , to compute the average stress/strain based on the distance from the element integration points to the crack tip, $r$ . By default, a uniform weighting is applied to all elements used for averaging; alternatively, you can use a Gaussian function or a cubic spline function. You can also define a weight function with a user subroutine.

The Gaussian function is represented by:

ω (r) = \frac{1}{{(2 π)}^{3 / 2} r_{c}^{3}} e x p (\frac{- r^{2}}{2 r_{c}^{2}})

The cubic spline function is represented by:

ω (r) = {\begin{matrix} 4 (\frac{r}{r_{c}} - 1) {(\frac{r}{r_{c}})}^{2} + \frac{2}{3}, & 0 < r < \frac{r_{c}}{2} \\ \frac{4}{3} {(1 - - \frac{r}{r_{c}})}^{3}, & \frac{r_{c}}{2} \leq r \leq r_{c} \\ 0, & otherwise \end{matrix}

Input File Usage

Use one of the following options:

DAMAGE INITIATION, WEIGHTING METHOD=UNIFORM (default)
DAMAGE INITIATION, WEIGHTING METHOD=GAUSS 
DAMAGE INITIATION, WEIGHTING METHOD=CUBIC SPLINE 
DAMAGE INITIATION, WEIGHTING METHOD=USER

Abaqus/CAE Usage

Specifying a weighting scheme for nonlocal averaging is not supported in Abaqus/CAE.

Smoothing the Normals of Individual Crack Facets Using Least-Squares Approximation

After the predicted crack propagation direction is obtained based on the nonlocal stress/strain averaging, a moving least-squares approximation by polynomials is used by default to further smooth out the crack normals. The least-squares approximation is applied to the normals of the individual facets in elements along the crack front that satisfy the damage initiation criterion, as highlighted in Figure 4. This approximation provides a smoother crack surface (as shown in Figure 5), leading to a more accurate crack propagation direction.

You can use linear, quadratic, or cubic polynomial approximation for the moving least-squares approximation to smooth out the crack normals. You specify the number of terms in the polynomial. You can also suppress the least-squares approximation. In this case, the predicted crack propagation direction is determined based only on the nonlocal stress/strain averaging.

Input File Usage

Use one of the following options:

DAMAGE INITIATION, NPOLY=4
DAMAGE INITIATION, NPOLY=7 (default)
DAMAGE INITIATION, NPOLY=10
DAMAGE INITIATION, NPOLY=0 (suppress)

Abaqus/CAE Usage

Using the least-squares approximation to smooth out the crack normals is not supported in Abaqus/CAE.

Limiting the Elements Involved in Crack Normal Smoothing

At the beginning of the analysis, you can choose to include or exclude the preexisting crack facets in elements from the moving least-squares approximation to obtain the crack propagation direction. During the analysis, you can also limit the elements involved in the least-squares approximation. You can set the maximum allowed difference (in degrees) below which the normals of the crack facets are included in the moving least-squares approximation. The default is 70°.

Input File Usage

Use the following option to include the normals of preexisting crack facets:

DAMAGE INITIATION, INISMOOTH=YES (default)

Use the following option to exclude the normals of preexisting crack facets:

DAMAGE INITIATION, INISMOOTH=NO

Use the following option to limit the elements involved by setting a maximum allowed difference (in degrees):

DAMAGE INITIATION, ANGSMOOTH=angle

Abaqus/CAE Usage

Limiting the elements involved in crack normal smoothing is not supported in Abaqus/CAE.

Damage Evolution

The damage evolution law describes the rate at which the cohesive stiffness is degraded once the corresponding initiation criterion is reached. The general framework for describing the evolution of damage is conceptually similar to that used for damage evolution in surface-based cohesive behavior (Contact Cohesive Behavior).

A scalar damage variable, D, represents the averaged overall damage at the intersection between the crack surfaces and the edges of cracked elements. 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 normal and shear stress components are affected by the damage according to

t_{n} = {\begin{matrix} (1 - D) T_{n}, & T_{n} \geq 0 \\ T_{n}, & otherwise (no damage to compressive stiffness); \end{matrix}

t_{s} = (1 - D) T_{s},

t_{t} = (1 - D) T_{t},

where $T_{n}$ , $T_{s}$ , and $T_{t}$ are the normal and shear stress components predicted by the elastic traction-separation behavior for the current separations without damage.

To describe the evolution of damage under a combination of normal and shear separations across the interface, an effective separation is defined as

δ_{m} = \sqrt{{⟨ δ_{n} ⟩}^{2} + δ_{s}^{2} + δ_{t}^{2}} .

Input File Usage

Use the following option to specify a damage evolution law:

DAMAGE EVOLUTION

The combination option DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=EXPONENTIAL is not recommended to be used with XFEM.

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Maxpe Damage or Maxps Damage: Suboptions Damage Evolution

Use with User-Defined Damage Initiation Criterion

A separate damage evolution law should be specified for each damage initiation criterion defined in user subroutine UDMGINI. Each combination of a damage initiation criterion and a corresponding damage evolution law is referred to as a failure mechanism. Damage will accumulate for only one failure mechanism per element, corresponding to the mechanism whose damage initiation criterion was achieved first.

Input File Usage

Use the following options to specify damage evolution laws for multiple user-defined damage initiation criteria:

DAMAGE INITIATION, CRITERION=USER, FAILURE MECHANISMS= $n$ 
DAMAGE EVOLUTION, FAILURE INDEX=1
DAMAGE EVOLUTION, FAILURE INDEX=2
...
DAMAGE EVOLUTION, FAILURE INDEX= $n$

Abaqus/CAE Usage

Defining a user-defined damage initiation criterion is not supported in Abaqus/CAE.

Use with LaRC05 Criterion

You can specify four separate damage evolution laws, one for each of the four initiation mechanisms. Alternatively, you can specify fewer than four damage evolution laws. In this case, the initiation mechanisms that do not have a corresponding evolution law use the specified damage evolution law with the smallest failure index. Damage accumulates for only one failure mechanism per element, corresponding to the mechanism whose damage initiation criterion was achieved first.

Input File Usage

Use the following options to specify damage evolution laws for the LaRC05 damage initiation criterion:

DAMAGE INITIATION, CRITERION=LARC05
DAMAGE EVOLUTION, FAILURE INDEX=1
DAMAGE EVOLUTION, FAILURE INDEX=2
DAMAGE EVOLUTION, FAILURE INDEX=3
DAMAGE EVOLUTION, FAILURE INDEX=4

FAILURE INDEX=1, 2, 3, and 4 correspond to matrix cracking, fiber kinking, fiber splitting, and fiber tension, respectively.

Abaqus/CAE Usage

Defining the LaRC05 damage initiation criterion is not supported in Abaqus/CAE.

Viscous Regularization in Abaqus/Standard

Models exhibiting various forms of softening behavior and stiffness degradation often lead to severe convergence difficulties in Abaqus/Standard. Viscous regularization of the constitutive equations defining cohesive behavior in an enriched element can be used to overcome some of these convergence difficulties. Viscous regularization damping causes the tangent stiffness matrix to be positive definite for sufficiently small time increments.

The approximate amount of energy associated with viscous regularization over the whole model is available using output variable ALLVD.

Input File Usage

Use the following option to specify viscous regularization:

DAMAGE STABILIZATION

Abaqus/CAE Usage

Property module: material editor: Mechanical Damage for Traction Separation Laws : Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Suboptions Damage Stabilization Cohesive

Output

Whole element variables:

STATUSXFEM: Status of the enriched element. (The status of an enriched element is 1.0 if the element is completely cracked and 0.0 if the element contains no crack. If the element is partially cracked, the value of STATUSXFEM lies between 1.0 and 0.0.)

Surface variables (available only for propagating cracks modeled with first-order solid continuum elements):

CRKDISP: Crack opening and relative tangential motions on cracked surfaces in enriched elements.
CSDMG: Damage variable on cracked surfaces in enriched elements.
CRKSTRESS: Remaining residual pressure and tangential shear stresses on cracked surfaces in enriched elements.