2.1. J-integral Calculation

The J-integral evaluation is based on the domain integral method by Shih[5]. The domain integration formulation applies area integration for 2-D problems and volume integration for 3-D problems. Area and volume integrals offer much better accuracy than contour integral and surface integrals, and are much easier to implement numerically. The method itself is also easy to use.

The following topics concerning J-integral calculation are available:

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

2.1.1. Understanding the Domain Integral Representation of the J-integral

For a 2-D problem, the domain integral representation of the J-integral is given by:

where:

= stress tensor
= displacement vector
= strain energy density
= Kronecker delta
= local coordinate axis
= crack-extension vector
= coefficient of thermal expansion
= initial strain tensor
= crack face traction
= integration domain
= crack faces upon which tractions act

The direction of is the x axis of the local coordinate system ahead of the crack tip. The q vector is chosen as zero at nodes along the contour Γ, and is a unit vector for all nodes inside Γ except the midside nodes, if there are any, that are directly connected to Γ. The program refers to these nodes with a unit vector as virtual crack-extension nodes.

For higher-order elements (such as PLANE183 and SOLID186), the vector at midside nodes takes the averaged values from the corresponding corner nodes.

For a 3-D problem, domain integral representation of the J-integral becomes a volume integration, which again is evaluated over a group of elements.

2.1.1.1. Virtual Crack-Extension Nodes and J-integral Contours

Virtual crack-extension nodes are one of the most important input data elements required for J-integral evaluation. It is also referred to as the crack-tip node component.

For a 2-D crack problem, the crack-tip node component usually contains one node which is also the crack-tip node. The first contour for the area integration of the J-integral is evaluated over the elements associated with the crack-tip node component. The second contour for the area integration of the J-integral is evaluated over the elements adjacent to the first contour of elements. This procedure is repeated for all contours. To ensure correct results, the elements for the contour integration should not reach the outer boundary of the model (with the exception of the crack surface).

For a 3-D crack problem, the crack-tip node component consists of the nodes along the crack front. The crack-tip node component is not required to be sorted. The 3-D J-integral contour follows a procedure similar to that of the 2-D contour.

2.1.1.2. Material Behavior

J-integral evaluation supports the following material behaviors:

  • Linear isotropic elasticity

  • Isotropic Plasticity

2.1.2. Performing the J-integral Calculation

The program calculates the J-integral at the solution phase of the analysis after a substep has converged, then stores the value to the results file.

The CINT command initiates the J-integral calculation and also specifies the parameters necessary for the calculation.

2.1.2.1. Step 1: Initiate a New J-integral Calculation

To start a J-integral calculation, use the CINT command's NEW option and provide a number to identify the input information for the J-integral calculation.

The command syntax is:

CINT,NEW,n

where n is the number identifying this J-integral calculation.

Example 2.1:  Initiating a J-integral Calculation
CINT,NEW,1   ! initiate a new J-integral calculation as # 1 

2.1.2.2. Step 2: Define Crack Information

The crack-tip node component and the crack-extension direction are both necessary for a J-integral calculation. Two methods using 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 J-integral 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.

2.1.2.2.1. 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. ANSYS 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,ComponentName

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 2.2:  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 J-integral calculation
CINT,NEW,1
CINT,CTNC,CRACK_TIP_NODE_CM
CINT,NORM,11,2

Example 2.3:  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,CTNC,CRACK_FRONT_NODE_CM,

2.1.2.2.2. 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,ComponentName

  2. Identify the crack-tip node separately if the node component has more than one node. If a crack-tip node is not identified, then the first node of the node component is taken to be the first node.

    Example: CINT,CENC,ComponentName,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,ComponentName,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,ComponentName,Node1,,,compx,compy,compz

Repeat this method for all node locations along the crack front.

Example 2.4:  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,CENC,CRACK_FRONT_NODE_CM1,,11,2
CINT,CENC,CRACK_FRONT_NODE_CM2,,11,2
! …
CINT,CENC,CRACK_FRONT_NODE_CM2,,n,2

Example 2.5:  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,CENC,CRACK_FRONT_NODE_CM1, , , ,Vx1,Vy1,Vz1
CINT,CENC,CRACK_FRONT_NODE_CM2, , , ,Vx2,Vy2,Vz2
! …
CINT,CENC,CRACK_FRONT_NODE_CM2, , , ,Vxn,Vyn,Vzn

2.1.2.3. Step 3: Specify the Number of Contours

Specify the number of contours for the J-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 2.6:  Specifying the Number of Contours
CINT,NEW,1
CINT,CTNC,CRACK_FRONT_NODE_SET,NODE
CINT,NCON,6

2.1.2.4. Step 4: Define a Crack Symmetry Condition

If the crack is located along a symmetry plane, and only a half model is created, define a symmetric condition so that ANSYS can account for it:

CINT,SYMM,ON

Example 2.7:  Defining a Crack Symmetry Condition
CINT,NEW,1
CINT,SYMM,ON   ! crack 1 is a symmetrical crack

2.1.2.5. Step 5: Specify Output Controls

Mechanical APDL calculates the J-integral at the solution level and stores it to the results file for postprocessing. J-integral 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 J-integral results only.

Example 2.8:  Specifying Output Controls
CINT,NEW,1
CINT,CTNC,CRACK_TIP_NODE_CM
CINT,SYMM,ON
CINT,NCON,5
OUTRES,CINT,10  
! output J-integral every 10 substeps


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