A Fracture analysis can be performed in two stages:
- 1. Defining a crack and computing fracture parameters.
Fracture parameters help to design engineering structures within limits of catastrophic failure. You can define a crack and compute the needed fracture parameters using the following methods:
- 2. Analyze/study the crack growth.
You can study the crack growth phenomenon using the SMART Crack Growth object. This object provides the following crack growth options:
: Use this option to model structures subjected to cyclic loading. Fatigue crack growth model used is Paris’ law.
: For this option, crack growth modeling is based on selected fracture parameters (SIFS or J-Integral) and criteria.
For additional technical information, refer to the Understanding Crack-Growth Mechanics section in the Mechanical APDL Fracture Analysis Guide.
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 any Analytical Crack Object
The steps shown below describe setting up the fracture analysis when using a Semi-Elliptical Crack, Elliptical Crack, Ring Crack, Corner Crack, Edge Crack, Through Crack, and/or a Cylindrical Crack.
Note: You can also use these steps to compute fracture parameters in a Transient Structural analysis that contains cracks.
In Ansys Workbench, insert a Static Structural analysis in the project schematic.
Select a geometry.
Launch Mechanical.
Define a coordinate system location for the crack you will define. Note the following:
For semi-elliptical and edge cracks, the specified coordinate system must be located on one of the surfaces of a solid body.
For elliptical, through, cylindrical, and ring cracks, the specified coordinate system must be located inside of a solid body.
For corner cracks, the specified coordinate system can be located on the corner edge or close to corner of a solid body.
Align the axes of the coordinate system of the crack such that the direction of the specified coordinate system's Y-Axis is normal to the crack surface
For Semi-Elliptical cracks lying on curved surfaces, ensure that the coordinate system's X-Axis is 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.
Insert a Fracture folder in the Outline.
Note: If you have an import base mesh that is hex-dominant, set Re-mesh Hex-dominant to Tetrahedral property of the Fracture folder to . This setting automatically re-meshes an imported hex-dominant base mesh, on the solid body of an analytical crack object, to a tetrahedral mesh. The resulting mesh is used to generate the initial crack mesh for the fracture parameters calculation and SMART Crack Growth.
Insert any analytical crack, such as a Semi-Elliptical Crack, object under the Fracture folder.
Specify the properties of the specified crack.
Generate the mesh by right-clicking the Fracture folder and selecting Generate All Crack Meshes.
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.
Ensure the Fracture setting under Fracture Controls in the Analysis Settings is turned .
Solve the simulation.
Insert the Fracture Tool and specify the desired crack using the Crack Selection property.
Insert desired fracture results under the Fracture Tool.
Post-process the fracture results.
Export to Excel or copy/paste from the chart if necessary.
Supplementary Steps to Define an Analytical Crack Object on Imported Base Mesh
Use the following steps to configure your simulation on the Project Schematic in order to specify an analytical crack object on a mesh imported from External Model or Mechanical Model.
- External Model
From Ansys Workbench, insert an External Model system into the Project Schematic.
Open the Setup cell of the External Model tab and select the desired .cdb-based mesh that contains a solid body with tetrahedron/hex-dominant mesh. Return to the Project page and update the system.
Insert a Static Structural analysis.
Connect the fully-defined External Model upstream system to the downstream Static Structural analysis.
Launch Mechanical from the Static Structural system and then follow the steps from the above Define Crack Location using any Analytical Crack Object topic, beginning with Step 4.
- Mechanical Model
From Ansys Workbench, insert a Mechanical Model system into the Project Schematic.
Using the Geometry cell, specify solid body/bodies needed to define the crack.
Open the Model cell of the Mechanical Model system and mesh the solid bodies with either tetrahedron/hex-dominant mesh.
Return to the Project page and update the Mechanical Model system.
Insert a Static Structural analysis.
Connect the fully-defined Mechanical Model upstream system to the downstream Static Structural analysis.
Launch Mechanical from the Static Structural system and then follow the steps from the above Define Crack Location using any Analytical Crack Object topic, beginning with Step 4.
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.
From Ansys Workbench, insert a Static Structural analysis into the Project Schematic.
Input the geometry, which has a surface body (and will represent crack surface).
Launch Mechanical.
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.
Insert a Fracture folder in to the tree Outline.
Note: If you have an import base mesh that is hex-dominant, set Re-mesh Hex-dominant to Tetrahedral property of the Fracture folder to . This setting automatically re-meshes an imported hex-dominant base mesh, on the solid body of a Arbitrary Crack object, to a tetrahedral mesh. The resulting mesh is used to generate the initial crack mesh for the fracture parameters calculation and SMART Crack Growth.
Using the Fracture Context Tab or the context menu (right-click the folder), insert an Arbitrary Crack object into the Fracture folder.
Specify the properties of the Arbitrary Crack object.
Right-click the Fracture folder and select to generate the mesh.
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.
Make sure that the Fracture property under the Fracture Controls of the Analysis Settings is turned to .
Solve.
Add the Fracture Tool and scope it to the Arbitrary Crack object and add desired fracture results.
Post process the fracture results.
Export to Excel or copy/paste from the chart if necessary.
Supplementary Steps to Define Arbitrary Crack on Imported Base Mesh
Use the following steps to configure your simulation on the Project Schematic in order to specify an Arbitrary Crack on a mesh imported from External Model.
From Ansys Workbench, insert an External Model system into the Project Schematic.
Open the External Model tab and select the desired .cdb-based mesh that contains a solid body (that may also contain a surface body to define the crack shape) with tetrahedron mesh. Return to the Project page and update the system.
Note: If the imported .cdb- based mesh file contains a surface body that can be used to define the crack shape, you can jump to Step 6.
Insert a Mechanical Model system.
Note: If the imported .cdb-based mesh doesn't contain a surface body, then the Mechanical Model system is required to import the surface body (including its mesh) individually for later use when defining the Arbitrary Crack surface.
Using the Geometry cell of the Mechanical Model system, specify a surface body. This surface body represents crack surface. The crack surface must intersect with at least one face of the solid body specified in the External Model system and must not be embedded inside of the solid body.
Update the Mechanical Model system
Insert a Static Structural analysis.
Connect the fully-defined External Model and Mechanical Model (if defined above) upstream systems to the downstream Static Structural analysis.
Launch Mechanical from the Static Structural system and then follow the steps from the above Define an Arbitrary Crack using a Surface Body topic, beginning with Step 4.
Important:Arbitrary Crack mesh generated on an imported base mesh could affect the existing mesh (nodal and element) based Named Selection objects.
When you have an Arbitrary Crack specified on an imported base mesh, the application of imported loads or constraints is not supported because the Arbitrary Crack mesh generation could affect the existing mesh (nodes) during remeshing.
Imported Crack Mesh (Pre-Meshed Crack)
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.
From Ansys Workbench, insert an External Model system into the Project Schematic.
Open the External Model tab and select the desired .cdb-based mesh that contains the crack mesh and its definition. Return to the Project page and update the system.
Insert a Static Structural analysis in the Project Schematic.
Connect the Setup cell of the External Model system to Model cell of the Static Structural system.
Launch Mechanical.
Create a Coordinate System with a Y axis perpendicular to the crack faces.
Insert a Fracture folder in the Outline.
Insert a Pre-Meshed Crack object under the Fracture folder.
Specify the Pre-Meshed Crack object details.
Associate the Pre-Meshed Crack object with the newly created Coordinate System.
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.
Ensure the Fracture setting under Fracture Controls in the Analysis Settings is turned .
Solve.
Add the Fracture Tool and desired fracture results.
Post process the fracture results.
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.