2.5. Material Force Calculation

The material force method determines the vectorial force-like quantities conjugated to the configurational change; that is, the method evaluates the material node point forces corresponding to the Eshelby stress and the material body forces.

The following topics concerning material force calculation are available:

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

2.5.1. Understanding the Material Force Approach

For a general 2-D problem (in the absence of body forces, thermal strain and dynamic loads), the nodal material forces are defined as:

The Eshelby stress (Σ) is introduced in small-strain elasticity as:

In finite strain elasticity, the Eshelby stress yields:

In the following figure, the directions of e1 and e2 correspond to the local coordinate system at the crack tip:

Figure 2.4:  Domain Enhancement via Nodal Vectors

Domain Enhancement via Nodal Vectors

Here, e1 is the tangential component of the local coordinate system with respect to the crack surface, while e2 represents the normal component of the local coordinate system. The tangential component of the material force vector Fmat, which is in the direction of e1, represents the scalar crack-driven force. In the numerical evaluation of material force, the material force is calculated based on the resultant of all the material force vectors in a user-defined domain β surrounding the crack tip.

If the plastic deformations exist in the structure, the material body forces acting on the domain are expressed as:

where B is the material body forces:

Here, Bp is the material body forces via plasticity, whereas Bt is the material body forces via thermal stress. Then, the material body forces via plasticity are expressed as:

If thermal strains exist in the structure, the nodal material body force vectors are:

For hyperelastic material, the material force is:

The Eshelby stress () is defined as:

where is the hyperelastic potential.

For a 3-D problem, integral representation of the nodal material forces becomes a volume integration, which again is evaluated over a group of elements. The principal is similar to the 2-D problem. After nodal material forces are evaluated, however, they are divided by a distance quantity through the thickness.

2.5.1.1. Virtual Crack-Extension Nodes and Material Force Contours

Virtual crack-extension nodes are critical input data elements required for material force evaluation. The program uses virtual crack-extension node input to evaluate tangential (crack-driven force) and non-tangential components to the crack surface of the material force vectors. The crack-extension nodes are typically grouped together as crack-tip node components.

For a 2-D crack problem, the crack-tip node component typically contains one node, which is also the crack-tip node. The first contour for the area integration of the material force is evaluated over the elements associated with the crack-tip node component. The first contour gives nodal material force. The second contour for the area integration of the material force approach is evaluated over the elements adjacent to the first contour of elements. The 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. It is not necessary for the crack-tip node component to be sorted. The 3-D material force contour uses a procedure similar to that of the 2-D contour.

2.5.1.2. Material Behavior

Material force evaluation supports the following material behaviors:

  • Linear isotropic elasticity

  • Isotropic hardening plasticity

  • Kinematic hardening plasticity

  • Isotropic hyperelasticity

2.5.2. Calculating Material Force

The program calculates the material forces during the solution phase of the analysis after a substep has converged, then stores the values to the results file.

The CINT command initiates the material force calculation and specifies the necessary parameters.

2.5.2.1. Step 1: Initiate a New Material Force Calculation

To start a material force calculation, issue the CINT command twice, as follows:

CINT,NEW,n

CINT,TYPE,MFOR

where n is the material force calculation ID number.

Example 2.24:  Initiating a New Material Force Calculation
CINT,NEW,1       ! initiate a new material force calculation as #1 
CINT,TYPE,MFOR   ! set calculation type to material force

2.5.2.2. Step 2: Define Crack Information

The crack-tip node component and the local crack direction are both necessary for a material force calculation. Two methods using the CINT command are available for specifying the values:

  • Define the crack-tip node component and crack-plane normal.

    This approach applies to both 2-D crack geometry and 3-D flat crack surfaces. It offers a simple way to define a 3-D material force 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 to 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.

2.5.2.2.1. Define the Crack-Tip Node Component and Crack-Plane Normal

For 2-D crack geometry, you can 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. The program uses it to automatically determine the elements for the contour integration. The procedure is similar to 2-D crack geometry, and is performed through all nodes along the crack front.

The command syntax is:

CINT,CTNC,ComponentName

where ComponentName is the crack-tip node component name.

After defining the crack-tip node component, define the normal of the crack plane:

CINT,NORM,Par1,Par2

where Par1 is the coordinate system number and Par2 is the axis of that coordinate system.

The program automatically converts the crack plane normal into the local crack coordinate system, based on the element information. The local coordinate system is evaluated 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.

Example 2.25:  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 material force calculation
CINT,NEW,1
CINT,CTNC,CRACK_TIP_NODE_CM
CINT,NORM,11,2

Example 2.26:  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,

2.5.2.2.2. 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: Example: CINT,CENC,ComponentName,NODE1

  3. Define the crack-extension direction.

    ComponentName

    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 2.27:  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,,12,2
…
CINT,CENC,CRACK_FRONT_NODE_CM2,,n,2

Example 2.28:  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

2.5.2.3. Step 3: Specify the Number of Contours

Specify the number of contours for the material force evaluation:

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 2.29:  Specifying the Number of Contours
CINT,NEW,1
CINT,CTNC,CRACK_FRONT_NODE_SET,NODE
CINT,NCON,6

2.5.2.4. 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 the program can account for it:

CINT,SYMM,ON

Example 2.30:  Defining a Crack Symmetry Condition
CINT,NEW,1
CINT,SYMM,ON     ! crack 1 is a symmetrical crack

2.5.2.5. Step 5: Specify Output Controls

The program calculates the nodal material forces at the solution level and stores it to the results file for postprocessing.

The output for the material force approach uses all OUTRES command defaults. The command OUTRES,ALL includes CINT command results. However, you can issue an OUTRES,CINT command to control the specific output for material force results only.

Example 2.31:  Specifying Output Controls
CINT,NEW,1
CINT,CTNC,CRACK_TIP_NODE_CM
CINT,SYMM,ON
CINT,NCON,5
OUTRES,CINT,10     ! output material forces every 10 substeps


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