The extended finite element method (XFEM)

You can study the onset and propagation of cracking in quasi-static problems using the extended finite element method (XFEM). XFEM allows you to study crack growth along an arbitrary, solution-dependent path without needing to remesh your model. XFEM is available only for three-dimensional solid and two-dimensional planar models; three-dimensional shell models are not supported. You can use XFEM to study a crack in parts containing geometry, orphan mesh elements, or a combination of the two. You can choose to study a crack that grows arbitrarily through your model or a stationary crack. You define an XFEM crack in the Interaction module. You can specify the initial location of the crack. Alternatively, you can allow Abaqus to determine the location of the crack during the analysis based on the value of the maximum principal stress or strain calculated in the crack domain. For more information, see Modeling discontinuities as an enriched feature using the extended finite element method. Examples of XFEM models created in Abaqus/CAE are provided in Modeling discontinuities using XFEM.

To perform an XFEM crack analysis, you must specify the following:

Crack domain

To define the crack domain, you can select one or more cells from three-dimensional parts or one or more faces from two-dimensional planar parts. If you are defining the crack domain on an orphan mesh or a part containing both orphan and native mesh elements, you can select elements. The crack domain includes regions that contain any existing cracks and regions in which a crack might be initiated and into which a crack might propagate.

After you define the initial crack location, you can reduce the size of the crack domain by indicating that you want to use only elements in the vicinity of the crack geometry. You specify the number of element layers to include to prescribe a minimal enrichment zone automatically. The crack domain is defined using the elements intersected by the crack location. These elements are the initial set. The enrichment zone is built of elements in the neighborhood of the initial crack using the number of element layers that you specify. You can highlight the elements in the viewport and, if desired, save the highlighted elements to a set.

Crack growth

You can allow the crack to propagate along an arbitrary, solution-dependent path, or you can specify that the crack is stationary.

Initial crack location

To define the initial crack location, you can select faces from a three-dimensional solid or edges from a two-dimensional planar model. The initial crack location must be contained within the crack domain. A selected face can be a face of the solid, a face created by a partition, or a planar part instance. Similarly, a selected edge can be an edge of the solid, an edge created by a partition, or a wire part instance; you should not select a seam crack. You should not mesh the faces or edges that you selected to define the initial crack location. Figure 1 shows examples of the crack domain and the crack location for two- and three-dimensional geometry and orphan meshes.

Figure 1. Defining a crack for XFEM.

Alternatively, you can choose not to define the initial crack location. Regardless of whether you define the initial crack location, Abaqus initiates the creation of cracks during the simulation by searching for regions that are experiencing principal stresses and/or strains greater than the maximum damage values specified by the traction-separation laws.

Enrichment radius

The enrichment radius is a small radius from the crack tip within which the elements will be used for calculating crack singularity for a stationary crack. Elements within the enrichment radius must be included in the cells or faces that you chose to represent the crack domain. You can allow Abaqus to calculate the radius (three times the typical element characteristic length in the enriched area), or you can specify its value.

Contact interaction property

You can choose to associate a contact interaction property with the XFEM crack that defines the contact of cracked element surfaces. For detailed information, see Specifying a contact interaction property for XFEM.

Damage initiation

You must specify the conditions that will initiate a crack by specifying damage initiation criteria in the material definition. You can specify a criterion based on either maximum principal stress or maximum principal strain. For more information, see Maximum principal stress or strain damage.

Analysis procedure

You can include an XFEM crack in a static analysis procedure. Alternatively, you can include an XFEM crack in an implicit dynamic analysis procedure to simulate the fracture and failure in a structure under high-speed impact loading. The XFEM-based crack propagation simulated in an implicit dynamic procedure can also be preceded or followed by a static procedure to model the damage and failure throughout the loading history.

For detailed instructions, see Creating an XFEM crack.