cint#

SpecialPurpose.cint(action='', par1='', par2='', par3='', par4='', par5='', par6='', par7='', **kwargs)#

Defines parameters associated with fracture-parameter calculations.

Mechanical APDL Command: CINT

Parameters:
actionstr

Specifies action for defining or manipulating initial crack data:

par1str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par2str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par3str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par4str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par5str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par6str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

par7str

The description of the argument is missing in the Python function. Please, refer to the command documentation for further information.

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.

For more information about using the cint command, including supported element types and material behavior, see Calculating Fracture Parameters

Command Specifications#

Command Specification for Action= NEW

  • Par1 - cint ID number.

Command Specifications for Action= CTNC

  • 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

  • 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

  • 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

  • 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 C2-integral.

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

    • PSMAX - Calculate circumferential stress at the location where \(equation not available\) 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

<https://ansyshelp.ansys.com/Views/Secured/corp/v232/en/ans_frac/frac_parmcalctypes.html#strcalcSIFs>`_ ( 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

  • Par1 - cint ID (default = ALL).

Command Specifications for Action= NCON

  • Par1 - Number of contours to be calculated.

Command Specifications for Action= SYMM

  • Par1 - * OFF, 0, or NO - No symmetry (default).

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

Command Specifications for Action= UMM

Command Specifications for Action= NORM

  • Par1 - Coordinate system number (default = 0, global Cartesian).

  • Par2 - Axis of coordinate system (default = 2, global Cartesian Y-axis).

Command Specifications for Action= EDIR

  • 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

  • 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 red for the direction tangential to the crack front. To clear or delete the plots, issue annot.

Command Specifications for Action= LIST

  • CrackID - Crack ID. Default = ALL.

  • Par2 - No value – Lists the cint commands issued for the crack. Par3 and Par4 are ignored.

    ELEM – Lists 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

  • Par1 - Crack-tip element number or crack-front component name. (Component name must be 32 characters or less.)

Command Specifications for Action= RADIUS

  • Par1 - Radius at which a value is evaluated (used with cint,TYPE,PSMAX or cint,TYPE,STTMAX only).

Command Specifications for Action= RSWEEP

  • Par1 - Number of intervals for the sweep.

  • Par2 - Minimum angle of the sweep.

  • Par3 - Maximum angle of the sweep

Command Specifications for Action= INIT

  • 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

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 and