nrefine#
- Mapdl.nrefine(nn1='', nn2='', ninc='', level='', depth='', post='', retain='', **kwargs)#
Refines the mesh around specified nodes.
APDL Command: NREFINE
- Parameters:
- nn1, nn2, ninc
Nodes (NN1 to NN2 in increments of NINC) around which the mesh is to be refined. NN2 defaults to NN1, and NINC defaults to 1. If NN1 = ALL, NN2 and NINC are ignored and all selected nodes are used for refinement. If NN1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may also be substituted for NN1 (NN2 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 nodes (defaults to 1).
- 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
NREFINE performs local mesh refinement around the specified nodes. By default, the indicated elements are split to create new elements with 1/2 the edge length of the original elements (LEVEL = 1).
NREFINE refines all area elements and tetrahedral volume elements that are adjacent to the specified nodes. Any volume elements that are adjacent to the specified nodes, 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. For additional restrictions on mesh refinement, see Revising Your Model in the Modeling and Meshing Guide.
This command is also valid for rezoning.