1.15.5 Fully plastic J-integral evaluation

Product: ABAQUS/Standard  

This example illustrates fully plastic J-integral evaluation using deformation theory plasticity, as is used in the “engineering fracture mechanics” methodology developed by Kumar, et al. (1981). In this type of analysis elastic and fully plastic J-integral values are first obtained for the geometry of concern and are then combined, using a simple formula, to obtain approximate values of the J-integral at all load levels up to the limit load. The method offers a simple technique for flaw evaluation, provided the fully plastic J-integral values are readily available. ABAQUS contains a Ramberg-Osgood deformation plasticity theory model for this purpose. This example demonstrates the standard method provided in ABAQUS to obtain such fully plastic results.

In many cases the user may prefer to evaluate the J-integral at each load level using incremental or deformation theory, thus providing a direct computation of the J-integral value at each load level. The “engineering fracture mechanics” approach used in this example is generally used when tabulations of values are required for standard geometries, loadings, and materials.

Problem description

Material

The material model is the deformation theory, Ramberg-Osgood model provided in ABAQUS for such applications. This plasticity model is nonlinear at all stress levels, although the initial response up to the reference stress and strain values is almost linear. Various hardening exponents are of practical interest, the most commonly needed values being from 3 to 10. For this reason several different values are studied in this example.

Loading

The load is far-field tension applied to the top edge of the model. This is accomplished by applying negative pressure to the edges of the elements along the top of the model.

Solution development

The deformation theory solutions are not path dependent (the deformation theory plasticity model used here is entirely equivalent to a nonlinear elasticity model), so any technique that will provide the fully plastic solution in a numerically efficient manner is satisfactory. The most effective approach in ABAQUS for this purpose is usually the standard technique of incrementation and iteration, gradually increasing the load magnitude until the fully plastic solution is obtained. A general static analysis is done. Simultaneously, a region is monitored to become fully plastic, thus monitoring the progress of such a deformation theory solution. In this problem a set named Monitor is created that contains all of the elements in the focused part of the mesh and the first layer of elements above that region. In ABAQUS/CAE such a region is created by partitioning. ABAQUS will stop incrementing the load when all points in all elements in the specified set Monitor are in the fully plastic range (defined by the equivalent plastic strain being 10 times the offset yield strain), at which time the desired solution has been obtained.

Automatic incrementation is used, so the only control value that is needed is the suggested initial increment size. This can be estimated from knowledge of the limit load for the problem (available in Kumar, et al., 1981). The initial increment is suggested as 40% of the limit load value. This choice is not very critical in this case since the automatic incrementation algorithm will quickly find a suitable increment size, provided the suggestion is not grossly wrong.

Results and discussion

Submodeling of the crack tip

In Contour integral evaluation: two-dimensional case, Section 1.15.1, the submodeling capability is used to obtain more accurate near-tip stress fields in the linear elastic problem. In this example the submodeling capability is used to analyze the crack-tip region when the material is elastic-plastic. When small-scale yielding conditions exist, the far-field elastic region is not affected by the plastic zone around the crack tip. This will be true if the plastic zone size is less than about 10% of any characteristic length in the problem. The crack length serves as the characteristic length in this case. The loads in the problem are chosen so that the plastic zone is sufficiently small.

The problem is first solved with a relatively coarse mesh, as an elastic problem. The boundary of the submodel is chosen sufficiently far away from the crack tip so that the displacements on the boundary will not be affected by the plastic zone. The coarse mesh used is shown in Figure 1.15.5–2 (left). Plane strain conditions are modeled with CPE8RH elements, and a focused mesh is used (see jintegralplastic_global.inp). The value of the far-field loading for the global problem is chosen so that the small-scale yielding conditions at the crack-tip field are met in the elastic-plastic material case. A region of 508 mm (20 in) by 254 mm (10 in) is used for the submodel. The driven boundary is sufficiently far from the crack tip so the stress field near this boundary is not influenced by the plastic zone. The submodel has six rings of CPE8RH elements around the crack tip. The elastic-perfectly plastic material properties can be found in the corresponding files for the submodel. Figure 1.15.5–3 shows the geometry for the double-edged notch submodel and its deformed shape with a magnification factor of 169.

The J-integral values for the submodel should match the J-values for the global elastic mesh provided small-scale yielding conditions are met. Results are given in Table 1.15.5–3 for an analysis in which the plastic zone is entirely contained within the first two rings of elements surrounding the crack tip. The corresponding Mises stress contours are shown in Figure 1.15.5–4.

Submodeling could equally be used with a Ramberg-Osgood deformation plasticity model.

Python scripts

Input files

References

Tables

Table 1.15.5–1 Fully plastic results for double-edged cracked plate in plane stress. values for double-edged cracked plate in tension; (crack depth/half ligament) = 0.5.

Hardening exponent
ABAQUSKumar, et al. (1981)
31.37–1.381.38
51.17–1.181.17
71.011.01
90.90not given
100.850.845

Table 1.15.5–2 Fully plastic results for double-edged cracked plate in plane strain. values for double-edged cracked plate in tension; (crack depth/half ligament) = 0.5.

Hardening exponent
ABAQUSKumar, et al. (1981)
Coarse meshFiner mesh
32.55–2.592.55–2.582.48
52.59–2.622.58–2.592.43
72.55–2.582.55–2.562.32
102.39–2.432.46–2.472.12

Table 1.15.5–3 J-integral comparison for global and submodel analyses.

ContourGlobal elastic analysisSubmodel elastic-plastic analysis
 
1294.783281.524
2293.176284.562
3293.177288.742
4292.966288.782
5288.797
6288.790


Figures

Figure 1.15.5–1 Geometry for double-edged notch specimen.

Figure 1.15.5–2 Coarse (left) and finer (right) meshes for double-edged notch specimen.

Figure 1.15.5–3 Geometry for double-edged notch submodel and its deformed shape shown with magnification factor of 169.

Figure 1.15.5–4 Contour of the Mises stress around the crack tip of the elastic-plastic submodel.