Product: ABAQUS/Standard
This example illustrates fully plastic 
-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 -integral values are first obtained for the geometry of concern and are then combined, using a simple formula, to obtain approximate values of the -integral at all load levels up to the limit load. The method offers a simple technique for flaw evaluation, provided the fully plastic -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 -integral at each load level using incremental or deformation theory, thus providing a direct computation of the -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.
The example uses the same double-edged notch specimen geometry used in “Contour integral evaluation: two-dimensional case,” Section 1.15.1 (where linear elastic -integral evaluation is illustrated), except that the length of the specimen has been extended somewhat to ensure that the results are effective for an infinitely long plate. Plane stress and plane strain cases are both analyzed. Results for these cases are available in Kumar, et al. (1981), so that the example provides verification of the fully plastic -integral results.
The geometry is shown in Figure 1.15.5–1. The specimen half-length has been extended to 2.54 m (100 in) to ensure that the far-field tension load is applied at a sufficient distance from the crack tip. The meshes for the 1/4 model are shown in Figure 1.15.5–2. Both a coarse mesh and a fine mesh are used. The fine mesh is similar to the coarse mesh, but with more elements. This mesh is used only in the plane strain case, because the incompressibility assumption in the material model makes that case more difficult. Shih and Needleman (1984) discuss this issue and point out that it is essential that the mesh should be able to model the fully plastic flow field accurately. For this reason mesh convergence studies are essential in such applications—see the discussion in the “Results” section below. Second-order elements are used. For the plane stress case the element type is CPS8R (the reduced integration, 8-node quadrilateral element). For the plane strain case element type CPE8RH is used; this element is a “hybrid” (mixed) formulation element and is used in this case because the material behavior is fully incompressible at the limit load and the mixed method can handle the incompressibility constraint. Acceptable results can also be obtained by using element type CPE8R, since the use of reduced integration avoids excessive constraint with incompressible response.
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.
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.
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.
Kumar, et al. (1981) provide tables of values of the nondimensional parameter 
, which defines the fully plastic -integral for the geometry as
, 
, and 
are the material parameters in the Ramberg-Osgood model; 
/
; 
is the half-width of the remaining ligament; 
is the half-width of the specimen; 
is the total load on the specimen; and 
is the limit load. For plane strain
Table 1.15.5–1 and Table 1.15.5–2 summarize the values of obtained in this example (calculated from the -integral values provided in the ABAQUS output, using the equation above) and compare them to the values published by Kumar, et al. (1981). The plane stress case causes little difficulty, and the differences between -integral values calculated on different contours are small, indicating that the results are fairly accurate. The agreement between these results and the values published by Kumar, et al. (1981) is quite good. In the plane strain case Table 1.15.5–2 shows considerable scatter in the results obtained with the coarse mesh, indicating inaccuracy. The finer mesh results show only a small scatter between the different contours (six contours are available in this mesh, and Table 1.15.5–2 shows the minimum and maximum values obtained). These finer mesh values are all close to the values obtained with the coarse mesh. These observations suggest that the finer mesh results are reliable. However, they do not agree closely with those tabulated by Kumar, et al. (1981). It has been established that some of the plane strain results presented by Kumar, et al. (1981) are inaccurate; Shih and Needleman (1984) reanalyzed the single-edge cracked specimen for this reason. They point out the need for fine, carefully designed meshes to obtain accurate and reliable -integral values, especially in such cases where incompressibility constrains the deformation. They also discuss consistency checks. One of these is the comparison of numerical values of the -integral obtained from different contours around the crack tip. The -integral should be path independent; therefore, any variation in -integral values calculated on different contours implies inaccuracy. Table 1.15.5–2 shows the range of -integral values obtained in this example; as mentioned above, there is very little scatter in the values calculated with the fine mesh, so they satisfy this consistency check. The other consistency check discussed by Shih and Needleman (1984) requires the evaluation of -integral values at different crack depths so that the slope of the -versus-crack-depth variation can be calculated. In this example only one value of crack depth has been investigated, so this check cannot be applied. The discrepancy between the values reported here and those tabulated by Kumar, et al. (1981) must remain unexplained until further analysis, including the second consistency check, is done.
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 -integral values for the submodel should match the -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.
Symmetric two-dimensional double-edged notch specimen coarsely meshed using reduced-integration plane stress elements
Run the 2DDoubleEdPlCoarseCPS8R_model.py script to create the model. Then run the 2DDoubleEdPlCoarseCPS8R_job.py script to analyze the model. In this model a hardening exponent of 5 is used. The other coarse mesh cases reported in the tables are available by changing the hardening exponent in the material definition.
Symmetric two-dimensional double-edged notch specimen coarsely meshed using hybrid reduced-integration plane strain elements
Run the 2DDoubleEdPlCoarseCPE8RH_model.py script to create the model. Then run the 2DDoubleEdPlCoarseCPE8RH_job.py script to analyze the model. In this model a hardening exponent of 5 is used. The other coarse mesh cases reported in the tables are available by changing the hardening exponent in the material definition.
Symmetric two-dimensional double-edged notch specimen finely meshed using hybrid reduced-integration plane strain elements
Run the 2DDoubleEdPlFineCPE8RH_model.py script to create the model. Then run the 2DDoubleEdPlFineCPE8RH_job.py script to analyze the model. In this model a hardening exponent of 5 is used. The other fine mesh cases reported in the tables are available by changing the hardening exponent in the material definition.
Submodel analysis of a symmetric two-dimensional double-edged notch specimen using an elastic-perfectly plastic material and meshed using hybrid reduced-integration plane strain elements
The analysis is done in two stages:
Run the 2DDoubleEdPlasGlCPE8RH_model.py script to create the global model. Then run the 2DDoubleEdPlasGlCPE8RH_job.py script to analyze the model and to create the output database (.odb) file that will drive the submodel.
Run the 2DDoubleEdPlasSubCPE8RH_model.py script to create the submodel. Then run the 2DDoubleEdPlasSubCPE8RH_job.py script to analyze the submodel using the output database file from the global model to drive it.
The input files listed below are provided for users who prefer to use the ABAQUS keyword interface instead of ABAQUS/CAE. The meshes created in these input files are different from those created by using the Python scripts; however, the results are of similar accuracy.
Typical input data for one case (plane stress, = 5). The other coarse mesh cases reported in the tables are available by changing the element type for plane strain and/or by changing the exponent in the material definition.
Typical input data for a finer mesh study in plane strain; the other cases are available by changing the value of .
Submodel data for an elastic-perfectly plastic material. The file jintegralplastic_global.inp contains the global model used.
Coarse mesh in plane strain, global model used for submodeling.
Kumar, V., M. D. German, and C. F. Shih, “An Engineering Approach for Elastic-Plastic Fracture Analysis,” Report NP–1931, Electric Power Research Institute, Palo Alto, California, 1981.
Shih, C. F., and A. Needleman, “Fully Plastic Crack Problems,” Parts I and II, ASME Journal of Applied Mechanics, vol. 51, pp. 48–64, 1984.
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 | | |
|---|---|---|
 | ABAQUS | Kumar, et al. (1981) |
| 3 | 1.37–1.38 | 1.38 |
| 5 | 1.17–1.18 | 1.17 |
| 7 | 1.01 | 1.01 |
| 9 | 0.90 | not given |
| 10 | 0.85 | 0.845 |
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 | | ||
|---|---|---|---|
| ABAQUS | Kumar, et al. (1981) | ||
| Coarse mesh | Finer mesh | ||
| 3 | 2.55–2.59 | 2.55–2.58 | 2.48 |
| 5 | 2.59–2.62 | 2.58–2.59 | 2.43 |
| 7 | 2.55–2.58 | 2.55–2.56 | 2.32 |
| 10 | 2.39–2.43 | 2.46–2.47 | 2.12 |
