Enter the Step module. From the main menu bar, select . 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 Crack, and select the desired XFEM crack. Select the frequency at which the history output will be generated. 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. Each contour generates a value or a group of values for the contour integral. If desired, toggle on Step for residual stress initialization values and select the step from which Abaqus will use the stress data in the last available increment to extract the residual stresses. If you select the initial step, the residual stresses are defined by the specified initial conditions. You cannot select a step that occurs after the step in which the history output request is created. For more information, see Including the effect of a residual stress field on J-integral evaluation. 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.
- -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 Ct-integral.
- T-stress
You use the T-stress component to represent a stress parallel to the crack front. For more information, see The T-stress.
- 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.
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:
For more information, see The crack propagation direction.
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.
|