CINT

CINT, Action, Par1, Par2, Par3, Par4, Par5, Par6, Par7
Defines parameters associated with fracture-parameter calculations.

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

Action

Specifies action for defining or manipulating initial crack data:

NEW

 — 

Initiate a new calculation and assign an ID.

CTNC

 — 

Define the crack-tip node component.

SURF

 — 

Define the crack-surface node components.

CENC

 — 

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

TYPE

 — 

Define the type of calculation to perform.

DELE

 — 

Delete the CINT object associated with the specified ID.

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

 — 

Define the crack-plane normal.

UMM

 — 

Enable or disable the unstructured-mesh method (UMM).

EDIR

 — 

Crack-assist extension direction.

PLOT

 — 

Plot the crack-front and crack-tip coordinate system.

LIST

 — 

List the CINT commands issued, or the elements used, in fracture-parameter calculations.

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.

INIT

 — 

SMART crack-initiation ID.

CSFL

 — 

Convert initial-stress data to crack-surface traction loading.

SMOOTH

 — 

Smooth the calculated fracture-parameter results.

Command Specification for Action = NEW

CINT, NEW, Par1

Par1 –

CINT ID number.

Command Specifications for Action = CTNC

CINT, CTNC, Par1, Par2, Par3

Par1 –

Crack-tip node component name (must be 32 characters or less).

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.

Command Specifications for Action = SURF

CINT, SURF, Par1, Par2

Par1 –

Crack-surface node component 1 (top or bottom crack face). (Component name must be 32 characters or less.)

Par2 –

Crack-surface node component 2 (top or bottom crack face, but the opposite of Par1). (Component name must be 32 characters or less.)

Command Specifications for Action = CENC

CINT, CENC, Par1, Par2, Par3, Par4, Par5, Par6, Par7

Par1 –

Crack-extension node component name (CM). (Must be 32 characters or less.)

Par2 –

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

Par3, Par4 –

Coordinate system number (Par3) and the number of the axis that is coincident with the crack direction (Par4). When these parameters are defined, Par5, Par6 and Par7 are ignored.

Par5, Par6, Par7 –

Global x, y, and z components of the crack-extension direction vector. (Par3 and Par4 must be blank.)

Command Specifications for Action = TYPE

CINT, TYPE, Par1, Par2

Par1 –

Type of calculation to perform:

JINT – Calculate J-integral (default).
SIFS – Calculate stress-intensity factors.
TSTRESS – Calculate T-stress.
MFOR – Calculate material forces.
CSTAR – Calculate C*-integral.
VCCT – Calculate energy-release rate using the VCCT method.
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.
Par2 –

Auxiliary stress fields and strategy for 3D stress-intensity factors (Par1 = SIFS) calculations:

0 – The plane-strain auxiliary fields are used at the interior nodes along the crack front. The stress-intensity factors at the end nodes of the crack front are set to copy the stress-intensity factors at the adjacent nodes (default).
1 – The plane-stress auxiliary fields are used over the entire crack front.
2 – The plane-strain auxiliary fields are used over the entire crack front.

Command Specifications for Action = DELE

CINT, DELE, Par1

Par1 –

CINT ID (default = ALL).

Command Specifications for Action = NCON

CINT, NCON, Par1

Par1 –

Number of contours to be calculated.

Command Specifications for Action = SYMM

CINT, SYMM, Par1

Par1 –

OFF, 0, or NO – No symmetry (default).

ON, 1, or YES – Symmetric about the crack line/plane.

Command Specifications for Action = UMM

CINT, UMM, Par1

Par1 –

OFF, 0, or NO – Disable the unstructured-mesh method (UMM) (default).

ON, 1, or YES – Enable the UMM.

Command Specifications for Action = NORM

CINT, NORM, Par1, Par2

Par1 –

Coordinate system number (default = 0, global Cartesian).

Par2 –

Axis of coordinate system (default = 2, global Cartesian Y-axis).

Command Specifications for Action = EDIR

CINT, EDIR, ITYPE, Par2, Par3, Par4, Par5

ITYPE –

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

Par2 –

If ITYPE = CS, the coordinate system number.

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

Par3 –

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

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

Par4 –

For ITYPE = CS, this value is not specified.

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

Par5 –

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.

Command Specifications for Action = PLOT

CINT, PLOT, 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 the crack-extension direction, green for the crack normal, and blue for the direction tangential to the crack front. To clear or delete the plots, issue /ANNOT.

Command Specifications for Action = LIST

CINT, LIST, CRACKID, Par2, Par3, Par4

CrackID –

Crack ID. Default = ALL.

Par2 –

No value – List the CINT commands issued for the crack. Par3 and Par4 are ignored.

ELEM – List the elements used in the fracture-parameter calculation.

Par3 –

Node number on the crack front/tip. Default = ALL. Valid only when Par2 =ELEM.

Par4 –

Contour number around the crack front/tip. Default = ALL. Valid only when Par2 =ELEM.

Command Specifications for Action = CXFE

CINT, CXFE, Par1

Par1 –

Crack-tip element number or crack-front component name. (Component name must be 32 characters or less.)

Command Specifications for Action = RADIUS

CINT, RADIUS, Par1

Par1 –

Radius at which a value is evaluated (used with CINT,TYPE,PSMAX or CINT,TYPE,STTMAX only).

Command Specifications for Action = RSWEEP

CINT, RSWEEP, Par1, Par2, Par3

Par1 –

Number of intervals for the sweep.

Par2 –

Minimum angle of the sweep.

Par3 –

Maximum angle of the sweep.

Command Specifications for Action = INIT

CINT, INIT, Par1

Par1 –

ADPCI ID number. The data associated with the ADPCI ID is connected to the CINT data set to define crack-initiation analysis details (such as crack location and shape, initiation criteria, etc.).

Command Specifications for Action = CSFL

CINT, CSFL, INIS, STRE

Initial-stress data (mesh-independent) are converted to a traction load acting on the crack-surfaces (specified via CINT,SURF). The traction is applied as a step load for all substeps.

The initial-stress data points are specified at various spatial locations in the global Cartesian coordinate system (CSYS). The data is required in the vicinity of the crack surfaces only. The program interpolates the initial stress at the centroid of each element face of the crack surfaces, then determines the equivalent traction at the element face based on its orientation.

For more information, see Table 2.2: Material and Load Support for Fracture-Parameter Calculation and Superposition Principle: Initial Stress vs. Crack-Face Traction in the Fracture Analysis Guide

Command Specifications for Action = SMOOTH

CINT, SMOOTH, Par1, Par2, Par3

Par1 –

FPAR – Fracture parameters.

Par2 –

OFF – Turn off fracture-parameter smoothing.

MLS – Moving least-squares algorithm for fracture-parameter smoothing.

Par3 –

For Par2 = MLS, this value is the number of divisions of crack-front nodes for the fracture-parameter data smoothing.

Notes

Initiate a new calculation via the Action = NEW parameter. Subsequent CINT commands (with parameters other than NEW) define the input required for the fracture-parameter calculations.

The simplest method is to define crack information via 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.

For Action= SURF, Par1 and Par2 can be the top or bottom crack-face node component. No order is required, provided that if one value the top crach-face node component, the other must be the bottom, and vice-versa. This option is valid only with CGROW for crack-growth simulation.

To define crack information at multiple locations along the crack front, use Action = CENC. You can issue CINT,CENC, Par1, etc. multiple times to define the crack-extension node component, the crack tip, and the crack-extension directions at multiple locations along the crack front.

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 = NORM.

The crack-assist extension direction (Action = EDIR) provides a generic extension direction when Action = CTNC. It helps to define crack-extension directions based on the connectivity of the crack-front elements. For a 2D case when the crack tangent cannot be calculated, the program uses the provided crack-assist extension direction directly.

For an XFEM-based crack-growth analysis:

  • Action = 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.

  • For CINT,TYPE, only Par1 = PSMAX or STTMAX are valid. Other Par1 values have no effect.

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.

Fracture-parameter calculations based on domain integrations such as stress-intensity factors, J-integral, or material force are not supported when contact elements exist inside the domain. The calculations may become path-dependent unless the contact pressure is negligible.

For Action = UMM, the default value can be OFF or ON depending on the element type. The CINT command overrides the default setting for the given element.

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

The Action = SMOOTH option applies to fracture-parameter types such as JINT, SIFS, TSTRESS, MFOR, and CSTAR when there are more than five crack-front nodes total. When you use a CINT parameter in SMART crack-growth calculation, the default option is MLS,5.

For more information about using the CINT command, including supported element types and material behavior, see Calculating Fracture Parameters in the Fracture Analysis Guide.

Menu Paths

This command cannot be accessed from a menu.