To request contour integral output:

Enter the Step module.

From the main menu bar, select OutputHistory Output RequestCreate.

ABAQUS/CAE displays the Create History dialog box.

From the Create History dialog box, enter the name of the output request and the step in which it will be created. Click Continue to close the dialog box.

ABAQUS/CAE displays the History Output Requests editor.

From the Domain field, select Contour integral, and select the desired contour integral.

From the fields that appear in the History Output Requests editor, enter the output frequency.

Select the type of contour integral calculation to perform. You can select from the following:

J-integral

You use the J-integral in rate-independent quasi-static fracture analysis to characterize the energy release associated with crack growth. The J-integral can be related to the stress-intensity factor if the material response is linear. For more information, see “The J-integral” in “Contour integral evaluation,” Section 11.4.2 of the ABAQUS Analysis User's Manual.

-integral

You use the -integral for time-dependent creep behavior, where it characterizes creep crack deformation under certain creep conditions, including transient crack growth. For more information, see “The C_t-integral” in “Contour integral evaluation,” Section 11.4.2 of the ABAQUS Analysis User's Manual.

T-stress

You use the T-stress component to represent a stress parallel to the crack front. For more information, see “The T-stress” in “Contour integral evaluation,” Section 11.4.2 of the ABAQUS Analysis User's Manual.

Stress intensity factors

You use the stress intensity factors , , and in linear elastic fracture mechanics to characterize the local crack-tip stress and displacement fields. For more information, see “The stress intensity factors” in “Contour integral evaluation,” Section 11.4.2 of the ABAQUS Analysis User's Manual.

If you request a contour integral calculation using stress intensity factors, ABAQUS also computes the crack propagation direction at initiation. You must choose one of the following to indicate the crack initiation criteria:

Maximum tangential stress

Maximum energy release rate



For more information, see “The crack propagation direction” in “Contour integral evaluation,” Section 11.4.2 of the ABAQUS Analysis User's Manual.

Enter the number of contours to evaluate. ABAQUS/CAE computes the next contour integral by adding a single layer of elements to the region defined by the previous domain, as described in Figure 20–2. Each contour generates a value or a group of values for the contour integral.

Click OK to configure the contour integral analysis and to close the editor.

For examples of how ABAQUS names history output variables in the output database for each contour integral that it calculates, see “Contour integral output,” Section 20.1.6.