Two approaches for evaluating stress-intensity factors (SIFs) are available:
Interaction integral method -- The program performs the SIF calculation at solution and stores the results to the result file for postprocessing.
Displacement extrapolation method -- The program performs the SIF calculation during postprocessing.
For a list of supported elements, see Table 2.1: Element Support for Fracture-Parameter Calculation.
Stress-intensity evaluation supports the following material behavior:
Linear isotropic elasticity
Similar to the domain integral method for J-integral evaluation, the interaction integral method for stress-intensity factors calculation applies area integration for 2-D problems and volume integration for 3-D problems. In comparison to the traditional displacement extrapolation method, the interaction integral method offers better accuracy, fewer mesh requirements, and ease of use.
The following topics are available:
The interaction integral is defined as:
where:
|
|
|
|
| and |
If thermal and initial strains exist in the structure and the surface tractions act on crack faces, the interaction integral is expressed as:
where:
|
|
|
|
For higher-order elements (such as
PLANE183 and SOLID186),
the vector, temperature values and initial strains at midside
nodes takes the averaged values from the corresponding corner nodes.
The interaction integral is associated with the stress-intensity factors as
where:
| |
| |
| E* = E for plane stress and E* = E / (1 - ν2) for plane strain |
| E = Young’s modulus |
| ν = Poisson’s ratio |
| μ = shear modulus |
Mechanical APDL calculates the stress-intensity factors via interaction integral evaluation at the solution phase of the analysis, and then stores the values to the results file.
The CINT command's SIFS option initiates the stress-intensity factors calculations. Similar to the J-integral calculation, CINT is also used to specify the parameters necessary for the calculation. For element type and material behavior support for CINT, see Material Behavior.
Following is the general process for calculating the stress-intensity factors:
To start a stress-intensity factors calculation, issue the CINT command twice, as follows:
CINT,NEW,n
CINT,TYPE,SIFS
where n is the number identifying this
stress-intensity factors calculation.
CINT,NEW,1 ! initiate a new calculation as #1 CINT,TYPE,SIFS ! specify stress-intensity factor calculations
Similar to the J-integral calculation, the crack-tip node component and the crack-extension direction are both necessary for the stress-intensity factors calculation. Two methods, both involving the CINT command, are available for specifying the values:
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.
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,Par3
where Par1 is the crack-tip node component
name, Par2 defines the crack-extension
direction calculation-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 extension 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,Par2
where Par1 is the coordinate system number
and Par2 is the axis of coordinate system
Par1.
! local coordinate system LOCAL,11,0,,,, ! select nodes located along the crack front and ! define it as crack front/tip node component NSEL,S,LOC,X,Xctip NSEL,R,LOC,Y,Yctip CM,CRACK_TIP_NODE_CM ! Define a new stress-intensity factors calculation CINT,NEW,1 CINT,TYPE,SIFS CINT,CTNC,CRACK_TIP_NODE_CM CINT,NORM,11,2
! select nodes located along the crack front and ! define it as crack front/tip node component LSEL,,,, NSLL CM,CRACK_FRONT_NODE_CM,NODE CINT,NEW,1 CINT,TYPE,SIFS CINT,CTNC,CRACK_FRONT_NODE_CM,
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:
Define a node component consisting of one or more nodes forming the crack tip.
The node component can have one or more nodes.
Example:
CINT,CENC, CMName
Identify the crack-tip node separately if the node component has more than one node.
If a crack-tip node is not identified, the first node of the node component is taken to be the first node.
Example:
CINT,CENC,
CMName,Node1
Define the crack-extension direction.
Identify the local coordinate system associated with the crack under consideration.
Identify the local axis (for the above CS) along which the crack is supposed to extend.
Example:
CINT,CENC, CMName,Node1,11,2
Alternatively, define the crack-extension direction by directly specifying the global X Y and Z components of the crack-extension vector.
Example:
CINT,CENC,
CMName,Node1,,,compx,compy,compz
Repeat this method for all node locations along the crack front. Although the program automatically calculates the local coordinate system at the crack tip to determine stress-intensity factors, it is usually best to use the NORM option to help align the calculated normals of the crack-tip nodes.
! local coordinate systems local,11,0,,,, local,12,0,,,, ! … local,n,0,,,, NSEL,S,LOC,X,Xctip1 NSEL,R,LOC,Y,Yctip1 NSEL,R,LOC,Z,Zctip1 CM,CRACK_FRONT_NODE_CM1 NSEL,S,LOC,X,Xctip2 NSEL,R,LOC,Y,Yctip2 NSEL,R,LOC,Z,Zctip2 CM,CRACK_FRONT_NODE_CM2 ! … NSEL,S,LOC,X,Xctipn NSEL,R,LOC,Y,Yctipn NSEL,R,LOC,Z,Zctipn CM,CRACK_FRONT_NODE_CMn CINT,NEW,1 CINT,TYPE,SIFS CINT,CENC,CRACK_FRONT_NODE_CM1,,11,2 CINT,CENC,CRACK_FRONT_NODE_CM2,,12,2 ! … CINT,CENC, CRACK_FRONT_NODE_Cn,,n,2
! Crack-extension node component and ! crack-extension direction specification using vectors NSEL,S,LOC,X,Xctip1 NSEL,R,LOC,Y,Yctip1 NSEL,R,LOC,Z,Zctip1 CM,CRACK_FRONT_NODE_CM1 NSEL,S,LOC,X,Xctip2 NSEL,R,LOC,Y,Yctip2 NSEL,R,LOC,Z,Zctip2 CM,CRACK_FRONT_NODE_CM2 ! … NSEL,S,LOC,X,Xctipn NSEL,R,LOC,Y,Yctipn NSEL,R,LOC,Z,Zctipn CM,CRACK_FRONT_NODE_CMn CINT,NEW,1 CINT,TYPE,SIFS CINT,CENC,CRACK_FRONT_NODE_CM1,,,,Vx1,Vy1,Vz1 CINT,CENC,CRACK_FRONT_NODE_CM2,,,,Vx2,Vy2,Vz2 ! … CINT,CENCOMP,CRACK_FRONT_NODE_Cn,,,,Vxn,Vyn,Vzn
Local Crack-Tip Coordinate System
The auxiliary crack-tip field is based on the local crack-tip coordinate systems. To ensure the accuracy of the stress-intensity factors calculation, it is crucial to have a correct local crack-tip coordinate system in which the local x axis is pointed to the crack extension, the local y axis is pointed to the normal of the crack surfaces or edges, and the local z-axis pointed to the tangential direction of the crack front.
The local coordinate systems must be consistent across all nodes along the crack front. A set of inconsistent coordinate systems results in no path dependency of the calculated stress-intensity factors and irregular behavior of the stress-intensity factor distribution along crack front. The program automatically calculate the local coordinate systems based on the input crack front nodes and the normal of the crack surface or extension directions; however, because there may be not enough information to determine a set of consistent coordinate systems, ANSYS, Inc. recommends using the CINT command's CTNC option to define a crack-face node to help identify the coordinate systems, or use the NORM option with the CENC option to define the coordinate systems.
The interaction integral, and thus the stress-intensity factors, have the same contour-independent behavior as the J-integral. You can specify the number of contours for the interaction integral evaluation, as follows:
CINT,NCON,n
where n is the number of contours.
For 3-D crack geometry, every node along the crack front has the same number of contours.
CINT,NEW,1 CINT,TYPE,SIFS CINT,CTNC,CRACK_FRONT_NODE_SET,NODE CINT,NCON,6
In general, there is no crack symmetry condition for a mixed-mode crack. When a crack symmetry condition is defined, however, stress-intensity factor KII and KIII are both set to zero. The calculated interaction integral is timed by a factor of two and is used to calculate the stress-intensity factor KI.
The command syntax for defining a symmetric condition is:
CINT,SYMM,ON
CINT,NEW,1 CINT,TYPE,SIFS CINT,SYMM,ON ! crack #1 is a symmetrical crack
Similar to the J-integral calculation, Mechanical APDL calculates the stress-intensity factors during the solution phase of the analysis and stores it to the results file for postprocessing. Stress-intensity factors output uses all the defaults from the OUTRES command. The command OUTRES,ALL includes CINT command results. However, you can issue an OUTRES,CINT command to control the specific output for stress-intensity factors results only.
CINT,NEW,1 CINT,TYPE,SIFS CINT,CTNC,CRACK_TIP_NODE_CM CINT,SYMM,ON CINT,NCON,5 OUTRES,CINT,10 ! output CINT results every 10 substeps
The POST1 postprocessing KCALC command () calculates the mixed-mode stress-intensity factors KI, KII, and KIII. The command is limited to linear elastic problems with a homogeneous, isotropic material near the crack region.
To calculate stress-intensity factors using the displacement extrapolation method, follow these steps within the POST1 postprocessor:
The X axis must be parallel to the crack face (perpendicular to the crack front in 3-D models) and the Y axis perpendicular to the crack face (as shown in Figure 1.5: Crack Tip and Crack Front).
This coordinate system must be the active model coordinate system (CSYS) and results coordinate system (RSYS) when KCALC executes.
The first node on the path should be the crack-tip node. For a half-crack model, two additional nodes are required, both along the crack face. For a full-crack model, where both crack faces are included, four additional nodes are required: two along one crack face and two along the other.
The following figure illustrates the two cases for a 2-D model.
The KPLAN field on the KCALC command specifies whether the model is plane-strain or plane-stress. Except for the analysis of thin plates, the asymptotic or near-crack-tip behavior of stress is usually thought to be that of plane strain. The KCSYM field specifies whether the model is a half-crack model with symmetry boundary conditions, a half-crack model with antisymmetry boundary conditions, or a full-crack model.