CZMESH
CZMESH, ecomps1, ecomps2, KCN, KDIR, VALUE, CZTOL
Create and mesh an interface area composed of cohesive zone elements.
-
ecomps1 Component name or number for the group of plane or solid structural elements adjacent to the interface being meshed.
-
ecomps2 Component name or number for the opposing (from
ecomps1) group of plane or solid structural elements adjacent to the interface being meshed.-
KCN Coordinate system number for the separation surface and normal direction. (if
ecomps1andecomps2not specified)-
KDIR Direction (x, y, or z) normal to separation surface in the
KCNcoordinate system (ifecomps1andecomps2not specified).-
VALUE Coordinate value along the
KDIRaxis at which to locate the interface (ifecomps1andecomps2not specified).-
CZTOL Optional absolute tolerance about
VALUE(ifecomps1andecomps2not specified). Allows nodes occurring slightly above or below the separation to be grouped properly. The following expression represents the default value:Where ΔX, ΔY, and ΔZ are the dimensions of the model based on nodal locations (that is, ΔX = X
max- Xmin).
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.