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 (six 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.
