Performing the Fracture Analysis
In this section, a crack is inserted and then propagated. First, we read the local .inp file that was created in Section 2. Start FRANC3D and then Open File, switching the File Filter to ABAQUS inp Files, and then select the appropriate .inp file. We wish to retain all of the material properties; we will select the mesh facets to retain as well as selecting the contact/constraint surfaces, Figure 4. We select the two surfaces that represent the ends of the piece of weld and we retain the mesh facets for these surfaces (middle panel of Figure 4). We select the four constraint surfaces (right panel of Figure 4) without retaining the mesh; note that two of these surfaces have already been selected in the previous panel.
The above selections allow us to insert the crack in the weld and remesh around it while maintaining a record of the surfaces that are involved in the original *Tie definitions. The resulting model with retained mesh facets for one end of the weld is shown in Figure 5.
Figure 4: FE Mesh File select items to retain dialogs.
Figure 5: Local portion of weld with mesh facets retained on the ends.
We will insert a through crack, Figure 6, which is 2 mm wide and penetrates the weld. The template radius is set to 0.1, Figure 7, so that the template mesh fits within the bottom narrow surface of the weld geometry. ABAQUS is used to do the volume meshing.
Figure 6: Through crack dimension and position/orientation dialogs.
Figure 7: Through crack template radius dialog along with the meshing parameter dialog.
The resulting cracked and remeshed model is shown in Figure 8. Note that ends of the weld have the original mesh facets retained while the surfaces that were tied to the frame and the flange have been remeshed.
Figure 8: Final meshed crack model.
We will perform a ‘static’ analysis using ABAQUS. Choose Analysis and Static Crack Analysis from the menu bar. Provide a file name (weld_step_000.fdb) and choose ABAQUS as the finite element analysis program. The analysis options are shown in Figure 9. We select the global model .inp file to connect to this local portion, and then select Next.
Figure 9. Static analysis options for ANSYS.
The next dialog box provides the user with options for connecting the local and global portions. We will use the existing *Tie definitions. When we select this radio button, the Merge Parts/Instances check box, Figure 10, is automatically selected. Select Finish to start the ABAQUS analysis of the combined local/global model.
Figure 10: Static analysis ABAQUS local/global model connection dialog.
Once ABAQUS has finished running, we can compute the SIFs; choose Cracks and Compute SIFs from the menu. In the dialog that is presented, Figure 11, select M-integral and then select Finish to plot the SIFs, Figure 12. Note that there are two crack fronts, so two plots will be displayed and the SIFs vary along the crack front as identified by the red A – B on the plot.
ABAQUS should automatically write the results to a .fil file that FRANC3D automatically reads. You can view the deformed shape, Figure 13, or other field variables using ABAQUS by reading the .odb file that ABAQUS should generate.
Figure 11: Compute SIFs dialog.
Figure 12: M-Integral based SIFs.
Figure 13: Compute SIFs dialog.