erefine

Mapdl.erefine(ne1='', ne2='', ninc='', level='', depth='', post='', retain='', **kwargs)

Refines the mesh around specified elements.

APDL Command: EREFINE

Parameters
ne1, ne2, ninc

Elements (NE1 to NE2 in increments of NINC) around which the mesh is to be refined. NE2 defaults to NE1, and NINC defaults to 1. If NE1 = ALL, NE2 and NINC are ignored and all selected elements are used for refinement. A component name may also be substituted for NE1 (NE2 and NINC are ignored).

level

Amount of refinement to be done. Specify the value of LEVEL as an integer from 1 to 5, where a value of 1 provides minimal refinement, and a value of 5 provides maximum refinement (defaults to 1).

depth

Depth of mesh refinement in terms of number of elements outward from the indicated elements, NE1 to NE2 (defaults to 0).

post

Type of postprocessing to be done after element splitting, in order to improve element quality:

OFF - No postprocessing will be done.

SMOOTH - Smoothing will be done. Node locations may change.

CLEAN - Smoothing and cleanup will be done. Existing

elements may be deleted, and node locations may change (default).

retain

Flag indicating whether quadrilateral elements must be retained in the refinement of an all-quadrilateral mesh. (The ANSYS program ignores the RETAIN argument when you are refining anything other than a quadrilateral mesh.)

ON - The final mesh will be composed entirely of

quadrilateral elements, regardless of the element quality (default).

OFF - The final mesh may include some triangular elements

in order to maintain element quality and provide transitioning.

Notes

EREFINE performs local mesh refinement around the specified elements. By default, the surrounding elements are split to create new elements with 1/2 the edge length of the original elements (LEVEL = 1).

EREFINE refines all area elements and tetrahedral volume elements that are adjacent to the specified elements. Any volume elements that are adjacent to the specified elements, but are not tetrahedra (for example, hexahedra, wedges, and pyramids), are not refined.

You cannot use mesh refinement on a solid model that contains initial conditions at nodes [IC], coupled nodes [CP family of commands], constraint equations [CE family of commands], or boundary conditions or loads applied directly to any of its nodes or elements. This applies to nodes and elements anywhere in the model, not just in the region where you want to request mesh refinement. If you have detached the mesh from the solid model, you must disable postprocessing cleanup or smoothing (POST = OFF) after the refinement to preserve the element attributes.

For additional restrictions on mesh refinement, see Revising Your Model in the Modeling and Meshing Guide.

This command is also valid for rezoning.

Return type

Optional[str]