DEMORPH, ELEM, DIMN, RMSHKY
Move nodes in selected elements to conform to structural displacements.
ELEMNon-structural elements to which mesh movement (morph) applies. If ALL, apply morphing to all selected elements [ESEL]. If ELEM = P, graphical picking is enabled. A component may be substituted for ELEM.
DIMNProblem dimensionality. Use "2" for a 2-D problem and "3" for a 3-D problem (no default).
RMSHKYRemesh flag option:
0 | — | Remesh the selected non-structural regions only if mesh morphing fails. |
1 | — | Remesh the selected non-structural regions and bypass mesh morphing. |
2 | — | Perform mesh morphing only and do not remesh. |
The selected elements should include only non-structural regions adjacent
to structural regions. The exterior nodes of the selected elements will usually
be on the boundary of the region which will have node positions displaced.
For DIMN = 2, elements must lie on a flat plane.
The DEMORPH command requires a single domain grouping of
elements be provided (multiple domains of elements are not permitted). Exterior
nodes will be assumed fixed (no nodes will be morphed) unless they coincide
with structural nodes having nonzero displacements.
Nodes in the structural regions move in accordance with computed displacements. Displacements from a structural analysis must be in the database prior to issuing DEMORPH.
By default (RMSHKY = 0), DEMORPH will
remesh the selected non-structural regions entirely if a satisfactory morphed
mesh cannot be provided.
If boundary conditions and loads are applied directly to nodes and elements, the DEMORPH command requires that these be removed before remeshing can take place.
Exercise care with initial conditions defined by the IC command. Before a structural analysis is performed for a sequentially coupled analysis, the DEMORPH command requires that initial conditions be removed from all null element type nodes in the non-structural regions. Use ICDELE to delete the initial conditions.
Distributed ANSYS Restriction This command is not supported in Distributed ANSYS.