Fracture Analysis Workflows

This section describes the typical workflow for computing fracture parameters in the static structural analysis that contains cracks. The typical workflows are shown below:


Note:  For all workflows, the static structural analysis supports imported thermal loads from both steady-state thermal or transient thermal analysis by linking the set up cell of the static structural analysis to the upstream steady-state thermal or transient thermal analysis.


Define Crack Location using the Semi-Elliptical Crack Object

The steps shown below describe setting up the fracture analysis when using the Semi-Elliptical crack object.


Note:  You can also use these steps to compute fracture parameters in a Transient Structural analysis that contains cracks.


  1. In ANSYS Workbench, insert a Static Structural analysis in the project schematic.

  2. Input geometry.

  3. Locate a coordinate system with a graphic pick point, coordinates, or topology. The coordinate system must be located on the surface.

  4. Align the axes of the coordinate system of the crack. The specified coordinate system's y-axis must be pointing in the direction normal to the crack surface. For cracks lying on curved surfaces, ensure that the coordinate system's x-axis is pointing normal to the surface of the body at the coordinate system location. See Creating a Coordinate System Based on a Surface Normal for details on how to orient such a coordinate system on a curved surface.

  5. Insert a Fracture folder in the Tree Outline.

  6. Insert a Semi-Elliptical Crack object under the Fracture folder.

  7. Specify the Semi-Elliptical crack object details.

  8. Generate the mesh by right-clicking the Fracture folder and selecting Generate All Crack Meshes.

  9. Apply loads and boundary conditions. As needed, apply pressure on the crack face using a Nodal Pressure. Nodal pressure can be scoped using the automatically generated crack face Named Selection created under the crack object.

  10. Ensure the Fracture setting under Fracture Controls in the Analysis Settings is turned On.

  11. Solve.

  12. Add the Fracture tool and Fracture Result.

  13. Post process the Fracture Result.

  14. Export to Excel or copy/paste from the chart if necessary.

Define an Arbitrary Crack using a Surface Body

The steps shown below describe how to set up a fracture analysis using the Arbitrary Crack object during a Static Structural analysis. You can follow same steps to set up fracture analysis for a Transient Structural Analysis.

  1. From ANSYS Workbench, insert a Static Structural analysis into the Project Schematic.

  2. Input the geometry, which has a surface body (and will represent crack surface). The crack surface must intersect with one face of a solid body and must not be embedded inside of the solid body.

  3. Create a coordinate system. The Y axis must be directed towards the normal of the crack's top face and the X axis helps to determine the crack extension direction.

  4. Insert a Fracture folder in to the tree Outline.

  5. Using the Fracture Toolbar or the context menu (right-click the folder), insert an Arbitrary Crack object into the Fracture folder.

  6. Specify the properties of the Arbitrary Crack object.

  7. Right-click the Fracture folder and selecting Generate All Crack Meshes to generate the mesh.

  8. Apply loads and boundary conditions. As needed, apply pressure on the crack face using the Nodal Pressure boundary condition. You can scope this boundary condition using the automatically generated crack-face Named Selection created under the object.

  9. Make sure that the Fracture property under the Fracture Controls of the Analysis Settings is turned to On.

  10. Solve.

  11. Add the Fracture Tool and scope it to the Arbitrary Crack object and add Fracture Result.

  12. Post process the Fracture Result.

  13. Export to Excel or copy/paste from the chart if necessary.

Imported Crack Mesh

This workflow describes using the Pre-Meshed crack object for the computation of fracture parameters in 2D and 3D analysis using imported crack mesh. You can follow same steps to set up a Fracture analysis for a Transient Structural Analysis.

  1. In ANSYS Workbench, insert a Static Structural analysis in the project schematic.

  2. Input the mesh through FE Modeler. The imported mesh contains the crack mesh and its definition.

  3. Create a coordinate system with a Y axis perpendicular to the crack faces.

  4. Insert a Fracture folder in the Tree Outline.

  5. Insert a Pre-Meshed Crack object under the Fracture folder.

  6. Specify the crack object details.

  7. Associate the Pre-Meshed Crack object with the created coordinate system.

  8. Apply load and boundary conditions.


    Note:  You cannot apply Pressure loads to the crack face. You can only apply Nodal Pressures on a structured mesh via node-based Named Selections for the nodes defining the crack face.


  9. Ensure the Fracture setting under Fracture Controls in the Analysis Settings is turned On.

  10. Solve.

  11. Add the Fracture tool and Fracture Result.

  12. Post process the Fracture Result.

  13. Export to Excel or copy/paste from the chart if necessary.


Note:  In 2D, you can draw the crack in the same model using DesignModeler and generate the crack mesh using the mesh connection feature.



Release 18.2 - © ANSYS, Inc. All rights reserved.