Product: Abaqus/Standard
For the two-dimensional case an edge crack of length 1 m is modeled in a linear elastic specimen. The results are effectively for an infinitely long plate. The geometry is symmetric about the crack line, so only the top half is modeled. The geometry is meshed using CPE8R elements. The crack faces are loaded in five steps. In the first step a load of constant magnitude 1 MPa is applied. In all subsequent steps the load is zero at the surface of the specimen and has magnitude 1 MPa at the crack tip. The load varies linearly in Step 2, quadratically in Step 3, cubically in Step 4, and quartically in Step 5.
For the three-dimensional case the model from 3DDoubleEdgedNotchC3D20_model.py in “Contour integral evaluation: two-dimensional case,” Section 1.16.1, is modified to apply a uniform crack-face loading via user subroutine DLOAD.
Results for the two-dimensional and three-dimensional analyses are discussed in the following sections.
Abaqus results are compared with the results taken from page 8.8 of The Stress Analysis of Cracks Handbook by H. Tada, P. C. Paris, and G. R. Irwin. The crack-face loading is given by 
MPa. Results for the J-integral in Pa are presented in Table 1.16.7–1.
The results should be the same as those shown in “Contour integral evaluation: two-dimensional case,” Section 1.16.1. The results are within a difference of 0.1%.
Nonuniform crack face loading on a two-dimensional model
Run the 2DEdgeCrackCPE8R_model.py script to create the model. Then run the 2DEdgeCrackCPE8R_job.py script to analyze the model. User subroutine DLOAD (2DEdgeCrackCPE8R.for) is used to apply the nonuniform loading on the crack face.
Uniform crack face loading on a three-dimensional model via user subroutine DLOAD
Run the 3DCrackC3D20_model.py script to create the model. Then run the 3DCrackC3D20_job.py script to analyze the model. User subroutine DLOAD (3DCrackC3D20.for) is used to apply the uniform loading on the crack face.
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 the same accuracy.
Checks the nonuniform loads applied to plane strain elements via user subroutine DLOAD.
User subroutine DLOAD used in pjinnu2d.inp.
Uses subroutine DLOAD and, therefore, “nonuniform” load types, to apply a uniform load to the crack faces.
User subroutine DLOAD used in pjinnu3d.inp.
