ansys.mapdl.core.Mapdl.czmesh

Mapdl.czmesh(ecomps1='', ecomps2='', kcn='', kdir='', value='', cztol='', **kwargs)

Create and mesh an interface area composed of cohesive zone elements.

Mechanical APDL Command: CZMESH

Parameters:

ecomps1str

Component name or number for the group of plane or solid structural elements adjacent to the interface being meshed.

ecomps2str

Component name or number for the opposing (from ecomps1 ) group of plane or solid structural elements adjacent to the interface being meshed.

kcnstr

Coordinate system number for the separation surface and normal direction. (if ecomps1 and ecomps2 not specified)

kdirstr

Direction (x, y, or z) normal to separation surface in the KCN coordinate system (if ecomps1 and ecomps2 not specified).

valuestr

Coordinate value along the KDIR axis at which to locate the interface (if ecomps1 and ecomps2 not specified).

cztolstr

Optional absolute tolerance about VALUE (if ecomps1 and ecomps2 not specified). Allows nodes occurring slightly above or below the separation to be grouped properly. The following expression represents the default value:

\[equation not available ``max`` - X ``min`` ).\]

Notes

czmesh is used on a mesh with shared nodes at the interface.

If ecomps1 and ecomps2 are specified, the czmesh command creates/meshes interface elements ( INTER202, INTER203, INTER204, INTER205 ) along the boundary between the two components or groups of elements.

The elements in each of the components or groups of elements share nodes with each other and also with the interface elements. This one-element thick boundary of interface elements splits the body between the two components or groups of elements.

Subsequent separation (delamination and failure) of the interface zone results in an increasing displacement between the nodes (within the interface element) along the cohesive zone elements. Unless otherwise specified, the czmesh command analyzes the configuration and geometry of the adjacent structural elements and provides the appropriate interface element.

The czmesh operation copies any nodal temperatures that you have defined on the split surface of the original mesh from the original nodes to the newly created coincident duplicate nodes. Displacements, forces, and other boundary conditions, however, are not copied; therefore, apply boundary conditions and loadings after issuing czmesh.

If using czmesh to generate interface elements ( INTER202 and INTER205 ) in a VCCT- based crack-growth simulation, be aware that those elements do not support degenerate shapes. Examine the resulting mesh, therefore, to verify correct element connectivity around the crack tip.

This command does not support mesh regions with non-solid elements (such as surface-effect and shell elements).

This command is valid for structural analyses only.