2.3. Stress-Intensity Factor (SIF) Calculation

Two approaches for evaluating stress-intensity factors (SIFs) are available:

For a list of supported elements, see Table 2.1: Element Support for Fracture-Parameter Calculation.

2.3.1. Material Behavior

Stress-intensity evaluation supports the following material behavior:

  • Linear isotropic elasticity

2.3.2. SIF Calculation via Interaction Integrals

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.

2.3.2.1. Understanding Interaction Integral Formulation

The interaction integral is defined as:

where:

= stress, strain and displacement (respectively)
= stress, strain and displacement (respectively) of the auxiliary field
and = crack-extension vector

If thermal and initial strains exist in the structure and the surface tractions act on crack faces, the interaction integral is expressed as:

where:

= thermal and initial strains (respectively)
= traction on crack surfaces

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:

(i = 1,2,3) = mode I, II, and III stress-intensity factors
(i = 1,2,3) = auxiliary mode I, II and III stress-intensity factors
E* = E for plane stress and E* = E / (1 - ν2) for plane strain
E = Young’s modulus
ν = Poisson’s ratio
μ = shear modulus

2.3.2.2. Calculating the Stress-Intensity Factors

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.

2.3.2.2.1. Step 1: Initiate a Stress-Intensity Factors Calculation

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.

Example 2.15:  Initiating a Stress-Intensity Factors Calculation
CINT,NEW,1       ! initiate a new calculation as #1 
CINT,TYPE,SIFS   ! specify stress-intensity factor calculations 

2.3.2.2.2. Step 2: Define Crack Information

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.

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,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.

Example 2.16:  Defining the Crack-Tip Node Component and Crack-Plane Normal
! 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

Example 2.17:  Defining the Crack-Tip Node Component and Crack-Plane Normal
! 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,

Define the Crack-Extension Node Component and Crack-Extension Direction

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:

  1. 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

  2. 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

  3. 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.

Example 2.18:  Defining the Crack-Extension Node Component and Crack-Extension Direction
! 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

Example 2.19:  Defining the Crack-Extension Node Component and Crack-Extension Direction
! 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.

2.3.2.2.3. Step 3: Specify the Number of Contours

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.

Example 2.20:  Specifying the Number of Contours
CINT,NEW,1
CINT,TYPE,SIFS
CINT,CTNC,CRACK_FRONT_NODE_SET,NODE
CINT,NCON,6

2.3.2.2.4. Step 4: Define a Crack Symmetry Condition

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

Example 2.21:  Defining a Crack Symmetry Condition
CINT,NEW,1
CINT,TYPE,SIFS
CINT,SYMM,ON    ! crack #1 is a symmetrical crack

2.3.2.2.5. Step 5: Specify Output Controls

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.

Example 2.22:  Specifying Output Controls
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

2.3.3. SIF Calculation via Displacement Extrapolation

The POST1 postprocessing KCALC command (Main Menu> General Postproc> Nodal Calcs> Stress Int Factr) 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:

2.3.3.1. Step 1: Define a Local Crack-Tip or Crack-Front Coordinate System

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.

Command(s): LOCAL (or CLOCAL, CS, CSKP, etc.
GUI: Utility Menu> WorkPlane> Local Coordinate Systems> Create Local CS> At Specified Loc

2.3.3.2. Step 2: Define a Path Along the Crack Face

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.

Command(s): PATH (or PPATH)
GUI: Main Menu> General Postproc> Path Operations> Define Path

The following figure illustrates the two cases for a 2-D model.

Figure 2.3:  Typical Crack Face Path Definitions

Typical Crack Face Path Definitions

(a) half-crack model and (b) full-crack model


2.3.3.3. Step 3: Calculate KI, KII, and KIII

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.

Command(s): KCALC
GUI: Main Menu> General Postproc> Nodal Calcs> Stress Int Factr

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