Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method

Modeling Approach

Modeling stationary discontinuities, such as a crack, with the conventional finite element method requires that the mesh conforms to the geometric discontinuities. Creating a conforming mesh can be quite difficult. Modeling a growing crack is even more cumbersome because the mesh must be updated continuously to match the geometry of the discontinuity as the crack progresses.

The extended finite element method (XFEM) alleviates the need to create a conforming mesh. The extended finite element method was first introduced by Belytschko and Black (1999). It is an extension of the conventional finite element method based on the concept of partition of unity by Melenk and Babuska (1996), which allows local enrichment functions to be easily incorporated into a finite element approximation. The presence of discontinuities is ensured by the special enriched functions in conjunction with additional degrees of freedom. However, the finite element framework and its properties such as sparsity and symmetry are retained. XFEM does not alleviate the need for sufficient mesh refinement in the vicinity of the crack tip.

Introducing Nodal Enrichment Functions

For the purpose of fracture analysis, the enrichment functions typically consist of the near-tip asymptotic functions that capture the singularity around the crack tip and a discontinuous function that represents the jump in displacement across the crack surfaces. The approximation for a displacement vector function $u$ with the partition of unity enrichment is

\begin{matrix} u \end{matrix} = \overset{N}{\sum_{I = 1}} N_{I} (x) [u_{I} + H (x) a_{I} + \overset{4}{\sum_{α = 1}} F_{α} (x) b_{I}^{α}],

where $N_{I} (x)$ are the usual nodal shape functions; the first term on the right-hand side of the above equation, $u_{I}$ , is the usual nodal displacement vector associated with the continuous part of the finite element solution; the second term is the product of the nodal enriched degree of freedom vector, $a_{I}$ , and the associated discontinuous jump function $H (x)$ across the crack surfaces; and the third term is the product of the nodal enriched degree of freedom vector, $b_{I}^{α}$ , and the associated elastic asymptotic crack-tip functions, $F_{α} (x)$ . For more details, see Nodal enrichment functions.

Accurately modeling the crack-tip singularity requires constantly keeping track of where the crack propagates and is cumbersome because the degree of crack singularity depends on the location of the crack in a nonisotropic material (see Nodal enrichment functions). Therefore, we consider the asymptotic singularity functions only when modeling stationary cracks in Abaqus/Standard. Moving cracks are modeled using one of the two alternative approaches described below.

Modeling Moving Cracks with the Cohesive Segments Method and Phantom Nodes

One approach for modeling moving cracks within the framework of XFEM is based on traction-separation cohesive behavior. This approach is used in Abaqus/Standard to simulate both crack initiation and propagation. This is a very general interaction modeling capability, which can be used for modeling brittle or ductile fracture. Other non-XFEM–based approaches for modeling crack initiation and propagation capabilities available in Abaqus/Standard are based either on cohesive elements (Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description) or on surface-based cohesive behavior (Contact Cohesive Behavior). Unlike these non-XFEM–based methods, which require that the cohesive surfaces align with element boundaries and the cracks propagate along a set of predefined paths, the XFEM-based cohesive segments method can be used to simulate both crack initiation and propagation along an arbitrary, solution-dependent path in the bulk materials, since the crack propagation is not tied to the element boundaries in a mesh. In this case the near-tip asymptotic singularity is not needed, and only the displacement jump across a cracked element is considered. Therefore, the crack has to propagate across an entire element at a time to avoid the need to model the stress singularity.

The cohesive segments approach is based on the use of so-called phantom nodes, which are superposed on the original real nodes, and are introduced to represent the discontinuity of the cracked elements (see Figure 1). When the element is intact, each phantom node is completely constrained to its corresponding real node. When the element is cut through by a crack, the cracked element splits into two parts. Each part is formed by a combination of some real and phantom nodes depending on the orientation of the crack. Each phantom node and its corresponding real node are no longer tied together and can move apart. For more details, see Phantom node method.

See Applying Cohesive Material Concepts to XFEM-Based Cohesive Behavior for more information.

Modeling Hydraulically Driven Fracture

The cohesive segments method in conjunction with phantom nodes discussed above can also be extended to model hydraulically driven fracture. In this case additional phantom nodes with pore pressure degrees of freedom are introduced on the edges of each enriched element to model the fluid flow within the cracked element surfaces in conjunction with the phantom nodes that are superposed on the original real nodes to represent the discontinuities of displacement and fluid pressure in a cracked element. The phantom node at each element edge is not activated until the edge is intersected by a crack. The flow patterns of the pore fluid in the cracked elements are shown in Figure 2. The fluid is assumed to be incompressible. The fluid flow continuity, which accounts for both tangential and normal flow within and across the cracked element surfaces as well as the rate of opening of the cracked element surfaces, is maintained. The fluid pressure on the cracked element surfaces contributes to the traction-separation behavior of the cohesive segments in the enriched elements, which enables the modeling of hydraulically driven fracture.

Optionally, phantom nodes with pore pressure, temperature, and slurry concentration degrees of freedom can be introduced on the edges of each enriched element, and phantom nodes with displacement, pore pressure, and temperature degrees of freedom can be superposed on the original real nodes. The temperature degrees of freedom are necessary to model heat transfer due to thermal conduction and radiation across the cracked element surfaces, as well as thermal convection within the cracked element surfaces. The slurry concentration degrees of freedom are necessary to model proppant transport and placement within the cracked surfaces. The temperature and/or slurry degrees of freedom will be activated automatically if thermal and/or slurry material properties are specified for the fluid flow within the cracked element surfaces.

Multiple fluid injections can also be performed in a single analysis.

See Defining the Constitutive Response of Fluid Flow within the Cracked Element Surfaces and Modeling Slurry Flow for more information.

Modeling Moving Cracks Based on the Principles of Linear Elastic Fracture Mechanics (LEFM) and Phantom Nodes

An alternative approach to modeling moving cracks within the framework of XFEM is based on the principles of linear elastic fracture mechanics (LEFM). Therefore, it is more appropriate for problems in which brittle crack propagation occurs either on reaching a critical value of a fracture criterion or associated with fatigue crack growth; for more discussion of fracture criteria and fatigue crack growth using the Paris law, see Fatigue Crack Growth Criterion, Linear Elastic Fatigue Crack Growth Analysis, and Low-Cycle Fatigue Analysis Using the Direct Cyclic Approach. The XFEM-based LEFM approach can be used to simulate crack propagation along an arbitrary, solution-dependent path in the bulk material.

Similar to the XFEM-based cohesive segments method described above, the near-tip asymptotic singularity is not considered, and only the displacement jump across a cracked element is considered. Therefore, the crack has to propagate across an entire element at a time to avoid the need to model the stress singularity. The strain energy release rate at the crack tip is calculated based on the modified Virtual Crack Closure Technique (VCCT), which has been used to model delamination along a known and partially bonded surface (see Crack Propagation Analysis).

Another similarity is the introduction of phantom nodes to represent the discontinuity of the cracked element when the fracture criterion is satisfied (for more details. see Phantom node method). The real node and the corresponding phantom node will separate when the equivalent strain energy release rate exceeds the critical strain energy release rate at the crack tip in an enriched element. The traction is initially carried as equal and opposite forces on the two surfaces of the cracked element. The traction is ramped down linearly over the separation between the two surfaces with the dissipated strain energy equal to either the critical strain energy required to initiate the separation or the critical strain energy required to propagate the crack depending on whether the VCCT or the enhanced VCCT criterion is specified.

See Applying the VCCT Technique to the XFEM-Based LEFM Approach for more information.

Using the Level Set Method to Describe Discontinuous Geometry

A key development that facilitates treatment of cracks in an extended finite element analysis is the description of crack geometry, because the mesh is not required to conform to the crack geometry. The level set method, which is a powerful numerical technique for analyzing and computing interface motion, fits naturally with the extended finite element method and makes it possible to model arbitrary crack growth without remeshing. The crack geometry is defined by two almost-orthogonal signed distance functions, $ϕ$ and $ψ$ , as illustrated in Figure 3. For more details, see Level set method.

Defining an Enriched Feature and Its Properties

An enriched feature is a region of a model, specified with an element set, in which the finite element interpolation functions are enhanced to include discontinuities. In other words, an enriched feature is a region in the model where you can use the extended finite element method (XFEM) to model a crack. You must specify an enriched feature and its properties to use XFEM. Because there is a computational cost associated with modeling discontinuities, limiting the extent of an enriched feature can enhance computational performance.

An enriched feature can model a stationary crack or a propagating crack, but not both. You must decide during model setup whether a particular enriched feature models a stationary crack or a propagating crack. For a stationary crack, the enrichment functions include the asymptotic elastic crack-tip fields (see Introducing Nodal Enrichment Functions). If you model a propagating crack, you must ensure that the enriched feature is large enough to include all areas of the part where the crack could potentially propagate. You should not include areas where the crack is unlikely to propagate in the enriched feature (if this information is known ahead of time). Including these areas increases the computational cost without having any impact on the accuracy of the model. Additional details regarding the criteria for initiation and propagation of a crack are discussed in Crack Initiation and Direction of Crack Extension.

The default XFEM implementation in Abaqus does not support interactions among multiple cracks or branching of a single crack. It is best suited for problems where only a single crack is modeled within an enriched feature. Real applications often require modeling multiple cracks within a single part. A part can contain no preexisting cracks or one or more preexisting cracks; it can also contain one or more cracks that initiate during the analysis. For such applications, you can use multiple enriched features within a part (one for each crack) or use a single enriched feature to model more than one crack, although the latter approach has limitations.

The choice of one approach versus the other depends on the ease of specifying multiple enrichment features at the time of model setup. This, in turn, depends on the proximity of the cracks to one another at initiation and during growth. You can choose a single enriched feature in situations where you do not have any prior knowledge regarding the potential locations of multiple cracks or when it is not straightforward to separate out two or more distinct enriched features in a complex part. The following paragraphs provide some guidelines to help you judge what types of situations you can model and to select the correct modeling approach for your problem, starting with the important concept of a level set conflict.

As discussed in Using the Level Set Method to Describe Discontinuous Geometry, an XFEM crack is represented in terms of nodal values of a level set function. A requirement of the level set representation is that the level set function at any given node must have a unique value. This requirement is violated when more than one crack cuts through a single element or adjacent elements of a given node, resulting in an attempt to assign multiple values of the level set function at the node. Such a condition is referred to as a level set conflict. If a level set conflict occurs during an analysis, the analysis ends with an error. Without any kind of prior experimental data, paths of propagating cracks are often difficult to predict. This can cause uncertainty prior to a simulation as to whether a level set conflict will occur if you model multiple cracks in a single enriched feature.

If there are multiple preexisting cracks in a part, you can define them within a single enriched feature as long as these cracks are relatively far away from one another to begin with and do not come close to one another during the crack growth process. This restriction ensures that a level set conflict does not occur at any node. Mesh refinement can help avoid a level set conflict.

By default, crack initiation exhibits the following behavior to avoid level set conflicts:

Crack initiation in an enriched feature cannot occur until all existing cracks propagate through the enriched feature boundary. As illustrated in Figure 4, Crack 2 does not initiate until Crack 1 propagates through the enriched feature boundary.
Crack initiation cannot occur near a preexisting crack (because this immediately causes a level set conflict).
More than one crack can initiate at nonpredetermined locations within an enriched feature only if two or more nonadjacent elements satisfy the damage initiation criterion in the same time increment and one of the following conditions is satisfied:
- There are no preexisting cracks in the enriched feature.
- All preexisting cracks in the enriched feature have propagated through the feature boundary.
A level set conflict occurs if the elements in which cracks initiate share nodes.
A newly initiated second crack cannot approach or enter an already cracked element.

You can use one of the following methods to change the default behavior described above:

Use multiple enriched features.
Use a single enriched feature that is capable of initiating more than one crack at different locations and at different time increments before existing cracks propagate through the feature boundary.

The sections that follow outline these two approaches.

Multiple Enriched Features

To use multiple enriched features, you must define the element sets belonging to each feature at the time of model setup. In other words, you must be able to determine the boundaries among multiple enriched features at the time of model setup. Figure 5 shows a part with two holes that result in stress concentrations. For the loading shown, two cracks would initiate and grow near these holes. For this part, it is easy to define multiple enriched features during model setup. If both cracks in Figure 6 are preexisting cracks and do not come close to each other as they grow, you can also use a single enriched feature. However, with a single enriched feature, performance suffers if most of the enriched feature remains uncracked. From a performance point of view, the better choice might still be to use two separate enriched features in the areas where the cracks grow.

Single Enriched Feature Capable of Initiating Multiple Cracks before Existing Cracks Propagate through the Feature Boundary

You might not be able to clearly define two or more enriched features at the time of model setup in all situations. Figure 6, which shows a plate with two closely spaced holes, illustrates an example of this situation. The potential crack initiation and growth paths are difficult to anticipate ahead of time. It might take some experience and modeling iterations to properly choose the boundaries that separate multiple enriched features. Using a single enriched feature might be more appropriate for this situation. XFEM cannot model cases in which cracks should coalesce during a simulation.

Another example where a clear separation of enriched features is difficult (maybe impossible) involves a composite panel with a hole and with +45/−45 plies. In this panel many parallel matrix cracks could nucleate and propagate in each ply, as illustrated in Figure 7. A single enriched feature per ply is more appropriate for this problem.

For the examples shown in Figure 6 and Figure 7, it is recommended that you use a single enriched feature (per ply), but activate the capability to initiate more than one crack at different locations and at different time increments even before preexisting cracks propagate through the feature boundary. This nondefault approach has fewer limitations compared to the default approach discussed earlier. During the model setup phase in this nondefault approach, you explicitly specify that multiple cracks can initiate within a single enriched feature. You also specify a small relative radius, $r_{s}$ , to define a crack initiation suppression zone near a crack tip within which the initiation of another crack is not allowed (to prevent a level set conflict). Multiple cracks are allowed to initiate in an enriched feature, but only outside the crack initiation suppression zone for each individual crack tip (see Activating and Deactivating the Enriched Feature). However, a level set conflict could still occur if two cracks propagate close to each other during the crack growth. If this happens, further mesh refinement in the region where the cracks approach each other might help run the analysis to completion.

Specifying the Enrichment

Abaqus activates the enriched degrees of freedom only when a crack cuts through an element. You can associate only stress/displacement, displacement/pore pressure, displacement/temperature, or displacement/pore pressure/temperature solid continuum elements with an enriched feature.

Input File Usage

ENRICHMENT

Abaqus/CAE Usage

Interaction module: SpecialCrackCreateXFEM

Defining the Type of Enrichment

You can choose to model an arbitrary stationary crack or a discrete crack propagation along an arbitrary, solution-dependent path. The former requires that the elements around the crack tips are enriched with asymptotic functions to catch the singularity and that the elements intersected by the crack interior are enriched with the jump function across the crack surfaces. The latter infers that crack propagation is modeled with either the cohesive segments method or the linear elastic fracture mechanics approach in conjunction with phantom nodes. However, the options are mutually exclusive and cannot be specified simultaneously in a model.

Input File Usage

Use the following option to specify a crack propagation analysis (default):

ENRICHMENT, TYPE=PROPAGATION CRACK

Use the following option to specify an analysis with stationary cracks:

ENRICHMENT, TYPE=STATIONARY CRACK

Abaqus/CAE Usage

Use the following input to specify a crack propagation analysis:

Interaction module: crack editor: toggle on Allow crack growth

Use the following input to specify an analysis with stationary cracks:

Interaction module: crack editor: toggle off Allow crack growth

Assigning a Name to the Enriched Feature

You must assign a name to an enriched feature, such as a crack. This name can be used in defining the initial location of the crack surfaces, in identifying a crack for contour integral output, in activating or deactivating the crack propagation analysis, and in generating cracked element surfaces.

Input File Usage

ENRICHMENT, NAME=name

Abaqus/CAE Usage

Interaction module: SpecialCrackCreate: XFEM: Name: name

Identifying an Enriched Region

You must associate the enrichment definition with a region of your model. Only degrees of freedom in elements within these regions are potentially enriched with special functions. The region should consist of elements that are presently intersected by cracks and those that are likely to be intersected by cracks as the cracks propagate.

Input File Usage

ENRICHMENT, ELSET=element set name

Abaqus/CAE Usage

Interaction module: SpecialCrackCreate: XFEM: Select the crack domain: select region

Defining a Crack Surface

As a crack propagates through the model, a crack surface representing both facets of cracked elements is generated on those enriched elements that are intersected by a crack during the analysis. You must associate the name of an enriched feature with the surface (see Assigning a Name to the Enriched Feature above).

Input File Usage

SURFACE, TYPE=XFEM

Abaqus/CAE Usage

An XFEM-based crack surface is not supported in Abaqus/CAE.

Defining Contact Interaction of Enriched Cracked Element Surfaces

Contact interaction of cracked element surfaces, including thermal interaction and pore fluid interaction, is allowed based on a small-sliding formulation or on a finite-sliding formulation within the general contact framework.

See Contact Interaction of Cracked Element Surfaces for more information.

Applying Distributed Pressure Loads and Heat Fluxes to Cracked Element Surfaces

When an element is cut by a crack during the analysis, a XFEM-based crack surface is generated during the analysis (see #simaanl-c-enrichment-t-DefiningAnEnrichedFeatureAndItsProperties-sma-topic6__simaanl-c-enrichment-surf). You can apply a distributed pressure load or heat flux to the cracked element surfaces.

Input File Usage

Use the following option to apply a distributed pressure load to a crack surface:

DSLOAD
surface name, P or PNU, magnitude

Use the following option to apply a distributed heat flux to a crack surface:

DSFLUX
surface name, S or SNU, magnitude

Abaqus/CAE Usage

An XFEM-based crack surface is not supported in Abaqus/CAE.

Specifying the Initial Location of an Enriched Feature

Because the mesh is not required to conform to the geometric discontinuities, the initial location of a preexisting crack must be specified in the model. The level set method is provided for this purpose. Two signed distance functions per node are generally required to describe a crack geometry. The first describes the crack surface, while the second is used to construct an orthogonal surface so that the intersection of the two surfaces gives the crack front (see Initial Conditions).

The first signed distance function must be either greater or less than zero and cannot be equal to zero. If an initial crack has to be defined at the boundaries of an element, a very small positive or negative value for the first signed distance function must be specified.

Input File Usage

Use the following option to specify the initial location of an enriched feature:

INITIAL CONDITIONS, TYPE=ENRICHMENT

Abaqus/CAE Usage

Interaction module: crack editor: Crack location: Select: select region

Activating and Deactivating the Enriched Feature

You can activate or deactivate the crack propagation capability within the step definition.

You can specify a small relative radius, $r_{s}$ , around the crack tip (as shown in Figure 8) to define a crack initiation suppression zone within which the elements in the enriched feature are excluded from crack nucleation. However, multiple crack nucleations are allowed to occur when the damage initiation criterion is satisfied in the elements lying outside the crack initiation suppression zone in the enriched feature. The default radius value is five times the typical element characteristic length in the enriched region.

Input File Usage

Use the following option to activate the crack propagation capability within the step definition:

ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=ON  (default)

Use the following option to deactivate the crack propagation capability within the step definition:

ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=OFF

Use the following option to deactivate the crack propagation capability automatically once all the preexisting cracks (or if there are no preexisting cracks, all the allowable newly nucleated cracks) have propagated through the boundary of the given enriched feature within the step definition:

ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=AUTO OFF

Use the following option to activate the crack propagation capability for a given enriched feature with the possibility of multiple crack nucleations within the step definition:

ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=MULTICRACKS, CRACK INITIATION RADIUS= $r_{s}$

Abaqus/CAE Usage

To modify the status of the crack propagation capability in a step, you must first create an XFEM crack growth interaction:

Interaction module: Create Interaction: select initial step: XFEM Crack Growth: select crack: Interaction manager: select interaction in step: Edit: toggle on/off Allow crack growth in this step

Activating the crack propagation capability for a given enriched feature with the possibility of multiple crack nucleations is not supported in Abaqus/CAE.

Contour Integral

When you evaluate the contour integrals using the conventional finite element method (Contour Integral Evaluation), you must define the crack front explicitly and specify the virtual crack extension direction in addition to matching the mesh to the cracked geometry. Detailed focused meshes are generally required and obtaining accurate contour integral results for a crack in a three-dimensional curved surface can be cumbersome. The extended finite element in conjunction with the level set method alleviates these shortcomings. The adequate singular asymptotic fields and the discontinuity are ensured by the special enrichment functions in conjunction with additional degrees of freedom. In addition, the crack front and the virtual crack extension direction are determined automatically by the level set signed distance functions.

Input File Usage

Use one of the following options to obtain contour integrals for a named enriched feature with the extended finite element method:

CONTOUR INTEGRAL, XFEM=DOMAIN, CRACK NAME=name

CONTOUR INTEGRAL, XFEM=LINE (default), CRACK NAME=name

Abaqus/CAE Usage

Step module: history output request editor: Domain: Crack: crack name

Specifying the Enrichment Radius

Although XFEM has alleviated the shortcomings associated with defining the conforming mesh in the neighborhood of the crack front, you must still generate a sufficient number of elements around the crack front to obtain path-independent contours, particularly in a region with high crack-front curvature. The group of elements within a small radius from the crack front are enriched and become involved in the contour integral calculations. The default enrichment radius is six times the typical element characteristic length of those elements along the crack front in the enriched area. You must include the elements inside the enrichment radius in the element set used to define the enriched region. Elements with a large aspect ratio should be avoided along the crack front.

Input File Usage

Use the following option to specify an enrichment radius:

ENRICHMENT, ENRICHMENT RADIUS

Abaqus/CAE Usage

Interaction module: crack editor: Enrichment radius: Analysis default or Specify

Procedures

Modeling discontinuities as an enriched feature can be performed using any of the following:

static analysis (see Static Stress Analysis);
implicit dynamic analysis (see Implicit Dynamic Analysis Using Direct Integration);
low-cycle fatigue analysis using the direct cyclic approach (Low-Cycle Fatigue Analysis Using the Direct Cyclic Approach);
fatigue crack growth analysis (see Linear Elastic Fatigue Crack Growth Analysis);
fully coupled thermal-stress analysis (see Fully Coupled Thermal-Stress Analysis);
quasi-static analysis (see Quasi-Static Analysis);
geostatic stress field analysis (see Geostatic Stress State); or
coupled pore fluid diffusion/stress analysis (see Coupled Pore Fluid Diffusion and Stress Analysis).

Initial Conditions

Initial conditions to identify initial boundaries or interfaces of an enriched feature can be specified (see Initial Conditions).

Boundary Conditions

Boundary conditions can be applied to any of the displacement, temperature, or pore pressure degrees of freedom (see Boundary Conditions).

Loads

The following types of loading can be prescribed in a model with an enriched feature:

Concentrated nodal forces can be applied to the displacement degrees of freedom (1–3) or the pore pressure degree of freedom (8); see Concentrated Loads.
Distributed pressure forces or body forces can be applied; see Distributed Loads. The distributed load types available with particular elements are described in Abaqus Elements Guide.
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Node-based film and radiation conditions.
Average-temperature radiation conditions.
Element- and surface-based film and radiation conditions.

For more information on heat fluxes, film conditions, and radiation conditions, see Thermal Loads.

Predefined Fields

The following predefined fields can be specified in a model with an enriched feature, as described in Predefined Fields:

Nodal temperatures (although temperature is not a degree of freedom in stress/displacement elements). The specified temperature affects temperature-dependent critical stress and strain failure criteria.
The values of user-defined field variables. The specified value affects field-variable-dependent material properties.

Material Options

Any of the mechanical constitutive models in Abaqus/Standard, including user-defined materials (defined using user subroutine UMAT) can be used to model the mechanical behavior of the enriched element in a crack propagation analysis. See Abaqus Materials Guide. The inelastic definition at a material point must be used in conjunction with the linear elastic material model (Linear Elastic Behavior), the porous elastic material model (Elastic Behavior of Porous Materials), or the hypoelastic material model (Hypoelastic Behavior). Only isotropic elastic materials are supported when evaluating the contour integral for a stationary crack.

Elements

Only the following elements can be associated with an enriched feature:

First-order solid continuum stress/displacement elements.
First-order displacement/pore pressure solid continuum elements.
First-order displacement/temperature solid continuum elements.
First-order displacement/pore pressure/temperature solid continuum elements.
Second-order stress/displacement tetrahedral elements.

For propagating cracks these include

bilinear plane strain and plane stress elements,
bilinear axisymmetric elements,
linear brick elements,
linear tetrahedral elements, and
second-order tetrahedral elements.

For stationary cracks, these include

linear brick elements,
linear tetrahedral elements, and
second-order tetrahedral elements.

For an incompatible mode element, Abaqus/Standard discards the contribution due to the incompatible deformation mode immediately after the element is fractured under a tensile loading. Therefore, the stress level at the cracked element may not return completely to its originally unloaded state even when this cracked element is unloaded completely and the contact of the cracked element surfaces is reestablished.

Output

In addition to the standard output identifiers available in Abaqus (Abaqus/Standard Output Variable Identifiers), the following nodal, whole element, and surface variables have special meaning for a model with an enriched feature.

Nodal variables:

PHILSM: Signed distance function to describe the crack surface.
PSILSM: Signed distance function to describe the initial crack front.

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.)
LOADSXFEM: Distributed pressure loads applied to the crack surface.

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.

Use of Unsymmetric Matrix Storage and Solution

When the pore pressure degrees of freedom are activated in the enriched elements, matrices are unsymmetric; therefore, unsymmetric matrix storage and solution may be needed to improve convergence (see Matrix Storage and Solution Scheme in Abaqus/Standard).

Visualization

A crack can be visualized through the iso-surface for the signed distance function PHILSM.

If a crack cuts through a very tiny corner of an enriched element, the displacements along the crack front in the enriched element may be distorted in rare cases in the Visualization module of Abaqus/CAE (Abaqus/Viewer) when displaying the contours. The distortion, however, is not present when viewing only the deformed shape.

When an element is cut through by a crack, the cracked element splits into two parts, each part formed by a real domain and a phantom domain, as illustrated in Figure 1. Contour plot integration point values for cracked elements consider contributions from only the real domains in both parts of the cracked elements. However, when you probe cracked elements, only the contribution from the part of the elements containing the real domain $Ω_{0}^{-}$ and the phantom domain $Ω_{p}^{+}$ is reported.

When evaluating the contour integrals in a stationary crack, additional integration stations are introduced internally in the elements enriched with singular asymptotic crack-tip fields. However, visualization of the element output variables in those additional integration points is not supported in the Visualization module of Abaqus/CAE (Abaqus/Viewer).

Limitations

The following limitations exist with an enriched feature:

An enriched element cannot be intersected by more than one crack.
A crack is not allowed to turn more than 90° in one increment during an analysis.
Only asymptotic crack-tip fields in an isotropic elastic material are considered for a stationary crack.
Adaptive remeshing is not supported.
Composite solid elements are not supported.
Import analysis is not supported.

Input File Template

The following is an example of modeling crack propagation with the XFEM-based cohesive segments method:

HEADING
...
NODE, NSET=ALL
...
ELEMENT, TYPE=C3D8, ELSET=REGULAR
ELEMENT, TYPE=C3D8, ELSET=ENRICHED
...
SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR
SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED

ENRICHMENT, TYPE=PROPAGATION CRACK, ELSET=ENRICHED, 
NAME=ENRICHMENT, INTERACTION=INTERACTION
SURFACE, TYPE=XFEM, NAME=SURF_NAME
Data lines to specify the names of enriched features
MATERIAL, NAME=STEEL1
...
MATERIAL, NAME=STEEL2
DAMAGE INITIATION, CRITERION=MAXPS, TOLERANCE=0.05
DAMAGE EVOLUTION, TYPE=ENERGY
Data lines to specify the failure mechanism
...
SURFACE INTERACTION, NAME=INTERACTION
SURFACE BEHAVIOR
Data lines to specify the contact of cracked element surfaces
...
STEP
STATIC
...
END STEP
STEP
STATIC
...

ENRICHMENT ACTIVATION, TYPE=PROPAGATION CRACK, 
NAME=ENRICHMENT, ACTIVATE=OFF
...
END STEP

The following is an example of modeling crack propagation with the XFEM-based LEFM approach:

HEADING
...
NODE, NSET=ALL
...
ELEMENT, TYPE=C3D8, ELSET=REGULAR
ELEMENT, TYPE=C3D8, ELSET=ENRICHED
...
SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR
SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED

ENRICHMENT, TYPE=PROPAGATION CRACK, ELSET=ENRICHED, 
NAME=ENRICHMENT, INTERACTION=INTERACTION
MATERIAL, NAME=STEEL1
...
MATERIAL, NAME=STEEL2
DAMAGE INITIATION, CRITERION=MAXPS, TOLERANCE=0.05
Data lines to specify the crack nucleation mechanism
...
SURFACE INTERACTION, NAME=INTERACTION
SURFACE BEHAVIOR
FRACTURE CRITERION, TYPE=VCCT, TOLERANCE=0.05,VISCOSITY=0.00001
Data lines to specify the crack propagation criterion
...
END STEP

The following is an example of calculating contour integrals in stationary cracks with the extended finite element method:

HEADING
...
NODE, NSET=ALL
...
ELEMENT, TYPE=C3D8, ELSET=REGULAR
ELEMENT, TYPE=C3D8, ELSET=ENRICHED
...
SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR
SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED

ENRICHMENT, TYPE=STATIONARY CRACK, ELSET=ENRICHED, 
NAME=ENRICHMENT, ENRICHMENT RADIUS
MATERIAL, NAME=STEEL1
...
MATERIAL, NAME=STEEL2
...
STEP
STATIC
...
CONTOUR INTEGRAL, CRACK NAME=ENRICHMENT, XFEM
END STEP

References

Belytschko, T., and T. Black, “Elastic Crack Growth in Finite Elements with Minimal Remeshing,” International Journal for Numerical Methods in Engineering, vol. 45, pp. 601–620, 1999.
Melenk, J., and I. Babuska, “The Partition of Unity Finite Element Method: Basic Theory and Applications,” Computer Methods in Applied Mechanics and Engineering, vol. 39, pp. 289–314, 1996.