If desired, you can modify the entities that you selected to define the crack front, the crack tip, and the crack extension direction that will be used to define a contour integral. You can also specify that the crack front is defined on a symmetry plane that models only half of the structure. For more information, see “Symmetry” in “Contour integral evaluation,” Section 7.10.2 of the ABAQUS Analysis User's Manual.
To define a crack to be used in a contour integral analysis:
Display the Crack editor using one of the following methods:
To configure a new contour integral, follow the instructions in “Defining data for contour integrals,” Section 20.1.11.
To edit an existing contour integral, select Special
CrackEditcrack name from the main menu bar in the Interaction module.
Toggle on On symmetry plane (half-crack model) to specify that the crack front is defined on a symmetry plane that models only half of the structure. ABAQUS doubles the change in potential energy calculated from the virtual crack front advance to compute the correct contour integral values.
If desired, click Edit to modify your selection of entities that define the crack front, crack tip, or crack line. If ABAQUS/CAE selected the crack tip or crack line region to be the same as the crack front, you cannot edit the selection.
If desired, change the method for defining the crack extension direction. You can also click Edit to modify your selection of entities that define the crack extension direction.
Click OK to configure the contour integral and to close the editor.
ABAQUS displays green crosses on the region to represent the crack front.
You must use the History Output Request editor in the Step module to include the contour integral data in the output database generated by the analysis. For more information, see “Contour integral output,” Section 20.1.6, and “Modifying history output requests,” Section 14.11.3.