You can use the Special menu in the Interaction module to create an extended finite element method (XFEM) crack. For more information, see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1 of the Abaqus Analysis User's Guide.
To create an XFEM crack:
From the main menu bar in the Interaction module, select Special
CrackCreate.
From the Create Crack dialog box that appears, select XFEM.
Enter the name of the crack, and click Continue to close the dialog box.
From the model in the viewport, select the entities representing the crack domain. You can select cells from a three-dimensional part instance or faces from a two-dimensional part instance. If you have an orphan mesh or an instance containing both orphan mesh and native mesh elements, you can select elements to represent the crack domain. You should select the entities that contain an existing crack along with any entities into which a crack might propagate.
Click mouse button 2 to indicate that you have finished selecting the crack domain.
The Edit Crack dialog box appears.
Do either of the following:
Toggle on Allow crack growth to define a crack that grows along an arbitrary path through your model as the solution progresses.
Toggle off Allow crack growth to define a stationary crack that cannot grow.
If you chose to allow crack growth, you can do either of the following to specify the crack location:
Toggle off Crack location, indicating that you will allow Abaqus to determine the location of the crack based on the damage initiation criterion that you specified.
Toggle on Crack location and click 
to specify the crack location by selecting interior faces from a three-dimensional model or edges from a two-dimensional planar part. You should not select a seam crack.
If you chose to prevent crack growth, do the following:
Click to specify the crack location by selecting interior faces from a three-dimensional model or edges from a two-dimensional planar part. You should not select a seam crack.
To specify the enrichment radius, do either of the following:
Choose Analysis default, to allow Abaqus to determine the enrichment radius. The default radius is three times the typical element characteristic length in the enriched area.
Choose Specify and enter a value. The value should be the radius from the crack tips within which the elements are used to calculate the crack singularity.
Choose the type of XFEM analysis:
By default, Abaqus will use the traction-separation cohesive behavior approach. You can select or create a contact interaction property that specifies the compressive and frictional behavior of the cracked faces based on a small-sliding contact formulation. For more information, see “Defining surface-to-surface contact,” Section 15.13.7.
If you create a fracture criterion contact interaction property, Abaqus will use the linear elastic fracture mechanics (LEFM) approach. For more information, see “Specifying fracture criterion properties for crack propagation” in “Defining a contact interaction property,” Section 15.14.1.
Click OK to configure the XFEM crack and to close the editor.
Abaqus displays green crosses to represent the crack domain and the crack location.
To view the crack growth in the Visualization module, you must use the Field Output Request editor in the Step module and request that Abaqus writes the signed distance function PHILSM to the output database during the analysis. For more information, see “Viewing an XFEM crack,” Section 31.3.3, and “Modifying field output requests,” Section 14.12.2.
