**CINT**, * Action*,

`Par1`

`Par2`

`Par3`

`Par4`

`Par5`

`Par6`

`Par7`

Compatible Products: – | – | – | Enterprise | Ent PP | Ent Solver | –

`Action`

Specifies action for defining or manipulating initial crack data:

**NEW**—

**CTNC**—

**CENC**—

Define the crack-extension node component, the crack-tip node, and the crack extension direction.

**TYPE**—

**DELE**—

**NCON**—

Specify the number of contours to calculate in the contour-integral calculation.

**SYMM**—

Indicate whether the crack is on a symmetrical line or plane.

**NORM**—

**UMM**—

**EDIR**—

**PLOT**—

**CXFE**—

Define the crack-tip element or crack-front element set. Valid for XFEM-based crack-growth analysis only.

**RADIUS**—

Define the radius at which the given value is to be evaluated. Valid for XFEM-based crack-growth analysis only.

**RSWEEP**—

Define the minimum and maximum sweep angle from existing crack direction. Valid for XFEM-based crack-growth analysis only.

`Action`

`Par1`

`Par2`

`Par3`

--`Par1`

Crack-tip node component name.

--`Par2`

Crack-extension direction calculation-assist node. Any node on the open side of the crack.

--`Par3`

Crack front’s end-node crack-extension direction override flag:

**0 --**Align the extension direction with the edges attached at the two end nodes of the crack front (default).

**1 --**Align the extension direction to be perpendicular to the crack front.

`Action`

`Par1`

`Par2`

`Par3`

`Par4`

`Par5`

`Par6`

`Par7`

--`Par1`

Crack extension node component name (

**CM**).--`Par2`

Crack-tip node. The crack-tip node defaults to the first node of the crack extension node component.

,`Par3`

--`Par4`

Coordinate system number (

) and the number of the axis that is coincident with the crack direction (`Par3`

). When these parameters are defined,`Par4`

,`Par5`

and`Par6`

are ignored.`Par7`

,`Par5`

,`Par6`

--`Par7`

Global x, y, and z components of the crack extension direction vector. (

and`Par3`

must be blank.)`Par4`

`Action`

`Par1`

--`Par1`

Type of calculation to perform:

**JINT --**Calculate J-integral (default).

**MFOR --**Calculate material forces.

**SIFS --**Calculate stress-intensity factors.

**TSTRESS --**Calculate T-stress.

**VCCT --**Calculate energy-release rate using the VCCT method.

**CSTAR --**Calculate C*-integral.

**PSMAX --**Calculate circumferential stress at the location where when sweeping around the crack tip at the given radius. Valid in an XFEM-based crack-growth analysis only.

**STTMAX --**Calculate maximum circumferential stress when sweeping around the crack tip at the given radius. Valid in an XFEM-based crack-growth analysis only.

`Action`

`Par1`

--`Par1`

**OFF, 0,***or*NO --Deactivate Unstructured Mesh Method (UMM).

**ON, 1,***or*YES --Activate .

`Action`

`ITYPE`

`Par1`

`Par2`

`Par3`

`Par4`

--`ITYPE`

Input type for the crack-assist extension direction. Valid values are CS (coordinate system number) or COMP (component x or y extension direction).

--`Par1`

If

= CS, the coordinate system number.`ITYPE`

If

= COMP, the x component of the crack-assist extension direction.`ITYPE`

--`Par2`

If

is CS, the axis representing the crack-assist extension direction.`ITYPE`

If

= COMP, the y component of the crack-assist extension direction.`ITYPE`

--`Par3`

For

= CS, this value is not specified.`ITYPE`

For

= COMP, the z component of the crack-assist extension direction.`ITYPE`

--`Par4`

A reference node on the crack front attached to the crack-assist extension direction. To accurately calculate and flip the crack extension directions, the crack-assist extension direction defined at this node is rotated as the tangent along the crack front rotates. This capability is useful when the crack-extension directions vary by more than 180 degrees along the crack front.

`Action`

`Par1`

`Par2`

--`Par1`

Crack ID.

--`Par2`

0 -- Disable plotting of crack-tip coordinate system.

1 -- Enable plotting of crack-tip coordinate system (default).

Color codes are white for crack-extension direction, green for crack normal, and red for the direction tangential to the crack front. To clear or delete the plots, issue the

**/ANNOT**command.

Initiate a new calculation via the * Action* = NEW parameter. Subsequent

The simplest method is to define crack information using
* Action* = CTNC; however, this method limits you to only one node for a
given location along the crack front. Use the CTNC option only when all nodes that define the
crack front lie in a single plane.

To define crack information at multiple locations along the crack front, use
* Action* = CENC. You can issue

`Par1`

Although you can vary the sequence of your definitions, all specified crack-tip nodes must be at the crack front, and no crack-tip node can be omitted.

You can define the crack extension direction directly by specifying either
* Action* = CENC or

`Action`

The crack-assist extension direction (* Action* = EDIR) provides a
generic extension direction when

`Action`

For * Action* = UMM, the default value can be OFF or ON depending on the element type. The

For an XFEM-based crack-growth analysis:

= CTNC, CENC, NCON, SYMM, UMM, or EDIR have no effect.`Action`

= CXFE, RADIUS, or RSWEEP are XFEM-specific and invalid for any other type of crack-growth analysis.`Action`

For

**CINT**,TYPE, only= PSMAX or STTMAX are valid. Other`Par1`

values have no effect.`Par1`

The stress-intensity factors calculation (**CINT**,TYPE,SIFS) applies only to
isotropic linear elasticity. Use only one material type for the crack-tip elements that
are used for the calculations.

When calculating energy release rates (**CINT**,TYPE,VCCT), do not restrict the
results from being written to the database (**/CONFIG**,NOELDB,1) after
solution processing; otherwise, incorrect and potentially random results are
possible.

The **CINT** command supports only strain data for
initial state (**INISTATE**,SET,DTYP,EPEL). Other initial state
capabilities are not supported.

For more information about using the **CINT** command, including supported
element types and material behavior, see Evaluation of Fracture Mechanics Parameters in the Mechanical APDL Fracture Analysis Guide.