Meshing the crack region and assigning elements

Large stress concentrations occur at the crack tip. As a result, you should create a refined mesh around the crack tip to get accurate results for stresses and strains. In contrast, because the J-integral is an energy measure, you can obtain accurate J-values with a relatively coarse mesh. However, if the material becomes more nonlinear, you must create a finer mesh at the crack tip to maintain the accuracy of the J-values. You can control the density of the mesh at the crack tip by partitioning the region and by assigning mesh seeds to the resulting edges. For more information, see Understanding seeding.

For a large-strain analysis during which Abaqus will allow for nonlinear geometry, you should mesh the contour integral region with quadrilateral or hexahedral elements. For more information, see Constructing a fracture mechanics mesh for finite-strain analysis with the conventional finite element method.

However, for a small-strain analysis that does not allow for nonlinear geometry, you must allow for the singularity at the crack tip or crack line by meshing the region that defines the crack front with a ring of triangles or wedges. For more information, see Controlling the singularity at the crack tip for a small-strain analysis.

You must use the swept meshing technique to create wedge elements; however, there are limitations on the regions that Abaqus/CAE can mesh using the swept meshing technique, as described in Swept meshing of three-dimensional solids. As a result, if you cannot use the swept meshing technique, you cannot create wedge elements, and you cannot allow for the singularity at the crack line. In most cases you can ignore the singularity if your mesh is sufficiently refined to model the deformation around the crack tip or crack line and the resulting high strain gradients. You can also ignore the singularity if you are interested in only the contour integral output.