KCALC, KPLAN, MAT, KCSYM, KLOCPR
Calculates stress intensity factors in fracture mechanics analyses.
KPLANKey to indicate stress state for calculation of stress intensity factors:
0 | — | Plane strain and axisymmetric condition (default). |
1 | — | Plane stress condition. |
MATMaterial number used in the extrapolation (defaults to 1).
KCSYMSymmetry key:
0 or 1 | — | Half-crack model with symmetry boundary conditions [DSYM] in the crack-tip coordinate system. KII = KIII = 0. Three nodes are required on the path. |
2 | — | Like 1 except with antisymmetric boundary conditions (KI = 0). |
3 | — | Full-crack model (both faces). Five nodes are required on the path (one at the tip and two on each face). |
KLOCPRLocal displacements print key:
0 | — | Do not print local crack-tip displacements. |
1 | — | Print local displacements used in the extrapolation technique. |
Calculates the stress intensity factors (KI,
KII, and KIII) associated with
homogeneous isotropic linear elastic fracture mechanics. A displacement extrapolation
method is used in the calculation (see POST1 - Crack Analysis in
the Mechanical APDL Theory Reference). This method assumes that the displacement calculations are
for the plane strain state. If the displacement calculations are performed
using a plane stress formulation, the calculation of the stress intensity
factors can be converted to the plane strain state by using KPLAN =
1. ANSYS Uses minor Poisson's ratio (MP,NUXY) for the stress
intensity factor calculation, therefore the material's Poisson's ratio must
be defined using MP,NUXY command. The PATH and PPATH commands
must be used to define a path with the crack face nodes (NODE1 at
the crack tip, NODE2 and NODE3 on
one face, NODE4 and NODE5 on
the other (optional) face). A crack-tip coordinate system, having x parallel
to the crack face (and perpendicular to the crack front) and y perpendicular
to the crack face, must be the active RSYS and CSYS before KCALC is
issued.