31.2.2 Defining the crack front

The first step in the procedure to configure a contour integral is to define the crack front by selecting entities from the assembly. The crack front is the forward part of the crack. Abaqus uses the crack front to compute the first contour integral using all of the elements inside the crack front and one layer of elements outside the crack front. You can request output for more than one contour integral, in which case Abaqus/CAE adds a single layer of elements to the group of elements that were used to calculate the previous contour integral. Figure 31–4 illustrates how Abaqus/CAE computes successive contour integrals for a two-dimensional model by adding layers of elements.

Figure 31–4 Successive contour integrals are calculated by adding a layer of elements.

If your part is three-dimensional, Abaqus computes contour integrals at each node along the crack line, as shown in Figure 31–5. For more information, see “Defining the crack front” in “Contour integral evaluation,” Section 11.4.2 of the Abaqus Analysis User's Guide.

Figure 31–5 Abaqus computes the contour integral at each node along the crack line.

The entities from which you can select depend on whether the crack front is located in geometry or an orphan mesh and on the modeling space of the part.

Geometry

When you are defining the crack front on geometry, the entities that you can select depend on the modeling space of the part.

Two-dimensional geometry

If you are defining the crack front on two-dimensional geometry, you can select the following:

A single vertex
Connected edges
Connected faces

Figure 31–6 shows the entities from which you can select when defining a crack front on two-dimensional geometry.

Figure 31–6 Selecting the crack front from two-dimensional geometry.

Three-dimensional geometry

If you are defining the crack front on three-dimensional geometry, you can select the following:

Connected edges
Connected faces
Connected cells

Figure 31–7 shows the entities from which you can select when defining a crack front on three-dimensional geometry.

Figure 31–7 Selecting the crack front from three-dimensional geometry.

Mesh

When you are defining the crack front on an orphan mesh, you can select the elements or element edges or faces that define the crack front. Alternatively, you can select the nodes from the corresponding region. When you are defining the crack front on an orphan mesh, the entities that you can select depend on the modeling space of the part.

Two-dimensional orphan mesh

If you are defining the crack front on a two-dimensional orphan mesh, you can select the following:

A single node
Connected element edges
Connected elements

Figure 31–8 shows the entities from which you can select when defining a crack front on a two-dimensional orphan mesh.

Figure 31–8 Selecting the crack front from a two-dimensional orphan mesh.

Three-dimensional orphan mesh

If you are defining the crack front on a three-dimensional orphan mesh, you can select the following:

Connected element edges
Connected element faces
Connected elements

Figure 31–9 shows the entities from which you can select when defining a crack front on a three-dimensional orphan mesh.

Figure 31–9 Selecting the crack front from a three-dimensional orphan mesh.