You can use the Special menu in the Interaction module to define the data for contour integrals. For more information, see “Fracture mechanics,” Section 7.10 of the ABAQUS Analysis User's Manual.
The entities that you select to define the contour integral depend on whether the part is two- or three-dimensional and whether you are defining the part using geometry from an ABAQUS native part or using elements and nodes from an orphan mesh part.
To define the data for contour integrals:
From the main menu bar in the Interaction module, select Special
CrackCreate.
The Create Crack dialog box appears.
Enter the name of the crack, and click Continue to close the dialog box.
From the model in the viewport, select the entities representing the crack front region. For a description of the entities to select, see “Defining the crack front,” Section 20.1.2.
Click mouse button 2 to indicate that you have finished selecting the crack front region.
From the model in the viewport, select the entities representing the crack-tip region. In some cases, depending on the modeling space of your model and the entities that you selected to define the crack front, ABAQUS/CAE selects the crack tip for you and skips to Step 7. For more information, see “Defining the crack tip or crack line,” Section 20.1.3.
From the prompt line, toggle on Select mesh entities to select entities from an orphan mesh part.
Click mouse button 2 to indicate that you have finished selecting the crack-tip region.
From the prompt area, choose the method for defining the crack extension direction.
Normal to crack plane
Select Normal to crack plane to specify the normal to the crack plane, and select points representing the start and end of the normal.
q vectors
Select q vectors to specify the crack extension direction directly, and select points representing the start and end of the vector.
ABAQUS/CAE displays a red arrow indicating the crack extension direction and displays the Edit Crack dialog box.
Use the Edit Crack dialog box to configure the parameters that control a contour integral analysis.
Click the General tab of the dialog box to do the following:
Specify that the crack front is defined on a symmetry plane that models only half of the structure.
Change the entities that define the crack front or crack tip/line.
Change the method for defining the crack extension direction. You can also change the entities that define the crack extension direction.
Click the Singularity tab of the dialog box to model a singularity of the strain field at the crack tip. For more information, see “Controlling the singularity at the crack tip,” Section 20.1.10.
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.
