Defining a Pre-Meshed Crack

A Pre-Meshed Crack is based on a previously-generated mesh and uses a node-based named selection to analyze crack fronts. In addition to cracks modeled in CAD and meshed manually in the Mechanical Application, this feature is also useful when you have a pre-existing mesh generated from an external source and imported to the existing database using FE Modeler. The referenced named selection must contain references only to nodes.

Selecting the named selection is done through the Details view of the Pre-Meshed Crack object by selecting from the list of valid named selections in the Crack Front (Named Selection) property. Named selections that contain only nodes are offered as choices.


Note:  Before defining a pre-meshed crack, you must have defined at least one node-based named selection. For more information on named selections, see Specifying Named Selections in the Mechanical Application. As an alternative, a geometric based named selection can be converted into a node-based based named selection using the Worksheet. For more information, see Specifying Named Selections using Worksheet Criteria.


To define a pre-meshed crack:

  1. Select the Model object in the Tree Outline.

  2. Insert a Fracture object into the Tree by right-clicking the Model object and selecting Insert > Fracture.


    Note:  Only one Fracture object is valid per Model.


  3. Insert a Pre-Meshed Crack object into the Tree by right-clicking the Fracture object and selecting Insert > Pre-Meshed Crack.

  4. In the Details View:

    • For 2D analysis, for Crack Tip (Named Selection), select the node-based named selection to which the crack definition will be scoped.

    • For 3D analysis, for Crack Front (Named Selection), select the node-based named selection to which the crack definition will be scoped.


    Note:  For a complete Pre-Meshed Crack definition, you must have previously defined the scoped node-based named selection and generated all crack meshes.


  5. To further define the crack, use the following controls in the Details View.

    • Coordinate System: Specifies the coordinate system that defines the position and orientation of the crack. The Y axis of the specified coordinate system defines the crack surface normal. The origin of the coordinate system represents the open side of the crack. You can select the default coordinate system or a local coordinate system that you have defined. The default is the Global Coordinate System. The valid coordinate system must be of type Cartesian.

    • Solution Contours: Specifies the number of contours for which you want to compute the fracture result parameters.

    • Symmetry: Specifies the crack symmetry about a line (in 2D analysis) or about a plane (in 3D analysis). The default is No.

    • Suppressed: Toggles suppression of the Pre-Meshed Crack object. The default is No.


      Note:  The Pre-Meshed Crack object is suppressed automatically if the scoped body is suppressed.



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