A blade/disk assembly is modeled using ABAQUS, Figure 1. A .cae and .inp file were supplied to FAC.
Figure 1. ABAQUS blade/disk model in CAE
A typical crack growth simulation involves only a small portion of the full model. For this blade/disk model, we separate the blade from the disk and write two .inp files. The .inp files that ABAQUS generates from CAE are typically ‘messy’ making them a little unfriendly for a novice to read/edit. After writing the two files, dove_top.inp and dove_bottom.inp, we manually edited the files to make them simpler to work with in FRANC3D. We also redefined some of the node/element sets and surfaces.
Cracking will be limited to the dove_bottom (disk) portion. This .inp file is read into FRANC3D. It is necessary that we retain node sets corresponding to the nodes with boundary conditions so that the *Transform command works properly. The displacement constraints act in a rotated coordinate system, and this must be carried forward after crack insertion and remeshing. The initial wizard panels showing the selected/retained items upon initial import of the dove_bottom.inp file are shown in Figure 2. Note that one node set is retained in the third panel; this corresponds with the boundary conditions on the outer surfaces (see Figure 1).
There are no “cut-surfaces” in this model because we will remesh the entire disk portion after crack insertion/growth. This simplifies later merging of the cracked/remeshed disk portion with the blade portion because we only have to redefine the contact conditions and do not need to do node-merging of model portions (although this could be done as well).
One node set (dove_bottom_contact) is selected in the fourth panel as the contact surface; the mesh for this surface is not retained. We regenerate the node set for the contact surface after crack insertion and remeshing.
Figure 2. Wizard panels showing selected/retained items for dove_bottom.inp
Once the model is read into FRANC3D, before we insert the crack, we use the Edges Wizard in the Advancedmenu. The Angle Threshold for the Kink Angle Edges is increased from the default 151 to 156 degrees. This causes the upper surfaces to be broken into several pieces, Figure 3.
Figure 3. Edges wizard used to change the angle threshold for edges.
The initial crack can now be inserted into the disk portion. We start with a 0.5 unit radius crack oriented as shown in the left panel of Figure 4. The crack front template mesh is shown in the right panel of Figure 4. Selecting Finishon this panel causes the crack to be inserted and the model to be remeshed.
Figure 4. Crack insertion wizard panels.
Once the cracked model is remeshed, we can perform the analysis. At present, we do a series of static crack analyses. From the Analysis menu, we select the Static Crack Analysis option and then provide a file name for the .fdb (and related files) – do not overwrite the original uncracked .inp file.
The series of wizard panels shown in Figure 5 indicate the selections that we make. The important thing to note is that we combine with dove_top.inp (as the global model – see the second panel) using contact conditions – see the third panel. The sets/surfaces that we choose for the contact-pair include the remesh_contact set for the local cracked portion and the top_contact_surf set for the blade portion.
Contact in ABAQUS is defined using SURFACE TO SURFACE or NODE TO SURFACE conditions. We use NODE TO SURFACE and define the remesh_conctactto be a node-based surface, and thus, require that the other surface be element-based; FRANC3D attempts to generate all of this data automatically.
The fifth panel allows us to choose whether we run ABAQUS immediately from FRANC3D or simply write the .inp files. Note that two .inp files are written, one for the remeshed portion and one for the combined remeshed and top pieces; the latter is the file that ABAQUS uses. Note that you should verify that ABAQUS is running by looking at the FRANC3D-CMD window; ABAQUS pre.exe and standard.exe should be executed without error.
Figure 5. Static analysis wizard panels – combine local cracked disk portion with the blade portion using contact conditions.
Once the ABAQUS analysis has been completed, FRANC3D automatically reads the .fil file, which contains the results, including the displacements. Stress intensity factors (SIFs) can be computed and displayed, Figure 6.
Figure 6. SIF dialog and SIF plot.
Crack growth can then be performed; select Grow Crack from the Cracksmenu. Figure 7 shows the three panels for crack growth. We predict growth by specifying an extension for the point on the crack front with the median value of SIF – see first panel.
The second panel shows the predicted new crack front and provides options for fitting a smooth curve through the computed front points. Initially, a fixed 3rd order polynomial with 5-10% extrapolation is adequate. As the crack grows, this simple polynomial fit might need to be adjusted.
The final panel shows the crack front mesh template along the new crack front. The template must intersect the model surface for this crack; the program tries to ensure this, but the user should check.
Figure 7. Crack growth wizard panels.
Preliminary discrete crack growth simulations have been completed, starting from the initial corner crack. Twelve steps of crack growth have been completed, with the crack growth predominantly along the axis of the dovetail, Figure 8. The SIF history is shown in Figure 9, which shows the Mode I SIF values for the thirteen crack fronts and the SIF history along a path through the crack fronts.
Figure 8. Deformed shape for initial crack and steps 3, 6, 9 and 12 at 25x magnification.
Figure 9. SIF history data for corner crack in blade/disk ABAQUS model.