The geometry of the first example is shown in Figure 1. The plane strain structure is a section of a plate with symmetric edge cracks at its
centerline, leaving an uncracked ligament of half the plate's width. The specimen is loaded
in Mode I by uniform tension applied to its top and bottom surfaces. When the conventional
finite element method is used, symmetry about x = 0 and about
y = 0 can be used to model only the top right-hand quadrant of the
plate. The mesh used for the quarter model is shown in Figure 2. Second-order elements (8-node quadrilaterals, 20-node bricks) are used. In the case of
the full-model seam crack, left and right contour integrals are defined in Abaqus/CAE, as shown in Figure 3. Either the normal to the crack extension or the q vectors can be
used to define the crack extension direction.
One advantage of using second-order elements with the conventional finite element method is
that they can be used to model the desired singularity at the crack tip. To obtain a
singularity term, the following conditions must be met:
-
The elements around the crack tip must be focused on the crack tip. One edge of each
element must be collapsed to zero length (as shown in Figure 2) so that the nodes of this zero length edge are located at the crack tip.
-
The “midside” nodes of the edges radiating out from the crack tip of each of the
elements attached to the crack tip must be placed at one-quarter of the distance from
the crack tip to the other node of the edge.
The region around the crack tip can be partitioned as shown in Figure 4 and swept meshed with elements having a quad-dominated shape. The node connectivity table
is adjusted internally by Abaqus/CAE to create the degenerate quadrilateral elements.
If the coincident nodes at the crack tip are constrained to displace together, the only
singularity term in strain is
; if the crack-tip nodes are free to displace independently, the crack-tip
singularity in strain includes a
term in addition to the
term. These methods of creating singularities in standard isoparametric
elements are explained in detail by Barsoum (1976).
The material type determines the singularity at the crack tip. A linear elastic material
exhibits a
singularity in strain at a sharp crack tip, whereas a perfectly plastic
material exhibits a
singularity in strain. The singularity in strain for a plastic hardening
material lies somewhere between
and
.
Frequently the need for meshing simplicity with a preprocessor is greater than the need for
extreme accuracy of contour integral results. The contour integral results often will be
adequate as long as some singularity is included. For example, a
singularity is introduced if the element edges are collapsed, the nodes at
the crack tip are free to displace independently, and the midside nodes are not moved to the
quarter points (they remain at the midside points). This singularity is often quite adequate
for elastic-plastic problems.
The model in this example problem uses a linear elastic material and, thus, should be
modeled with only a
singularity term.
For the quarter model of the double-edged notch specimen, symmetry is used for calculating
the contour integral results. Thus, the results for the contour integrals are multiplied by
two before being output. The three-dimensional model uses the same mesh with one layer of
20-node bricks, as shown in Figure 5. The loading applied is either a uniform edge load in two dimensions or a uniform surface
pressure (of negative magnitude) in three dimensions.
When the extended finite element method is used, the mesh is not required to match the
cracked geometry. The presence of a crack is ensured by the special enriched functions in
conjunction with additional degrees of freedom. This approach also removes the requirement
to explicitly define the crack front or to specify the virtual crack extension direction
when evaluating the contour integral. The data required for the contour integral will be
determined automatically based on the level set signed distance functions at the nodes in an
element. First-order brick elements with both full integration and reduced integration are
used for this example. The mesh is shown in Figure 6.
The axisymmetric model corresponds to a penny-shaped crack in a round bar. The model is
shown in Figure 7 and is loaded in Mode I by uniform tension applied to the top and bottom surfaces.
Symmetry about r = 0 and z = 0 allows you to model
only the top right-hand quadrant with a mesh, as shown in Figure 8. Second-order elements (CAX8 and
CAX8R) are used.
The third example is a single-edged notch specimen under Mode I tension, as shown in Figure 9. This specimen contains a crack in the symmetry plane in a homogeneous linear elastic
material. This example has been studied using both the conventional finite element method
and the extended finite element method. Due to symmetry only the top half-plane is modeled
for the specimen when used with the conventional finite element method. The complete body is
modeled when used with the extended finite element method. Second-order elements
CPE8 and
CPS8 are used with the conventional finite
element method, while first-order brick elements
C3D8 and first-order tetrahedral elements
C3D4 are used with the extended finite element
method.
The last example is also a single-edged notch specimen under Mode I tension, as shown in
Figure 9. This specimen contains a crack lying along the interface between two dissimilar elastic
materials. The complete body is modeled for the specimen with an interface crack.
Second-order elements CPE8 and
CPS8 are used for this example.
The J-integral, stress intensity factors, and
T-stress should be path independent, and Abaqus provides for its evaluation on as many contours as you request. The first contour is
normally at the crack tip, and subsequent contours are generated automatically as contours
passing through the nearest neighboring elements, moving out from the crack tip. The mesh
used in this case has several rings of elements surrounding the crack tip and as many
contours as the number of rings that can be requested. The contour integral should be path
independent, so the variation of values between contours can be taken as an indicator of the
quality of the mesh for determining the fracture parameters. Path independence of the
contour integral values is sufficient to indicate mesh convergence for stress, strain, or
displacements.