- Define the crack-tip node component and the crack-plane normal.
This approach applies for both 2-D crack geometry and 3-D flat crack surfaces. It offers a simple way
to define a 3-D stress-intensity-factors calculation, as you need only define the crack-tip (front) node
component and the normal of the crack plane. Use this method when the crack plane is flat.- Define the crack-extension node component and crack-extension direction.
This approach applies for 3-D curve crack planes, where a unique normal may not exist. However,
you must define the crack-extension node component and the crack-extension direction at each
crack-tip node location. Use this method when the crack plane is not flat, or when a set of nodes
form the crack tip, as in the case of a collapsed crack-tip mesh.The auxiliary crack-tip field is based on the crack-extension direction. To ensure the accuracy of the
stress-intensity factors calculation, it is crucial that you correctly define the crack-extension definition.
Define the Crack-Tip Node Component and Crack-Plane Normal
For 2-D crack geometry, define a crack-tip node component (usually a node located at the crack tip).
You can also define a group of nodes around the crack tip, including the node at the crack tip. The
program uses this group of nodes as the starting nodes to form the necessary information for the
contour integration automatically.
For 3-D flat crack geometry, you must define a crack-tip node component that includes all of the nodes
along the crack front. At each node location, however, only one node can exist. All nodes in the crack-
tip node component must be connectable, and they must form a line based on the element connectivity
associated with it.This line is the crack front. ANSYS uses it to automatically determine the elements
for the contour integration. The procedure is similar to 2-D crack geometry, and is done through all the
nodes along the crack front.
The command syntax is:
CINT,CTNC,Par1,Par2,Par3where Par1 is the crack-tip node component name,Par2 defines the crack-extension direction calcu-
lation-assist node (any node on the open side of the crack), and Par3 is crack front’s end-node crack-
extension direction-override flag.
The Par2 and Par3 values help to identify the crack-extension direction. Although the program
automatically calculates the local coordinate system at crack tip for stress-intensity factors calculations,
it is usually best to Par2 to define a crack face node to help align the ext ension directions of the crack-
tip nodes. By default, the program uses the external surface to determine the crack-extension direction
and normal when the crack-tip node hits the free surface; however, you can use Par3 to override this
default with the calculated coordinate system.
After the crack-tip node component is defined, use the CINT command's NORM option to define the
normal of the crack plane. The program automatically converts it into the crack-extension vector q,
based on the element information. The crack-extension vector is taken along the perpendicular direction
to the plane formed by the crack-plane normal and the tangent direction of the crack-tip node, and is
normalized to a unit vector.
The command syntax is:
CINT,NORM,Par1,Par2Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationNumerical Evaluation of Fracture Mechanics Parameters