FreeFOAMThe Cross-Platform CFD Toolkit
Hosted by SourceForge:
Get FreeFOAM at SourceForge.net. Fast, secure and Free Open Source software downloads

Name

freefoam-splitMeshRegions — Splits mesh into multiple regions.

Synopsis

freefoam splitMeshRegions [-cellZones] [-help] [-makeCellZones] [-sloppyCellZones] [-blockedFaces <faceSet name>] [-largestOnly] [-srcDoc] [-doc] [-overwrite] [-insidePoint <point>] [-parallel] [-case <dir>] [-detectOnly]

DESCRIPTION

Each region is defined as a domain whose cells can all be reached by cell-face-cell walking without crossing - boundary faces - additional faces from faceset (-blockedFaces faceSet). - any face inbetween differing cellZones (-cellZones)

Output is: - volScalarField with regions as different scalars (-detectOnly) or - mesh with multiple regions or - mesh with cells put into cellZones (-makeCellZones)

OPTIONS

-cellZones
Split different cell zones.
-detectOnly
Do no processing.
-blockedFaces <faceSet name>
Split at give face set.
-sloppyCellZones
Try to match regions to existing cell zones.
-makeCellZones
Create mesh with cells in different cell zones.
-overwrite
Overwrite existing data.
-case <dir>
Case directory.
-parallel
Run in parallel.
-help
Display help message.
-doc
Display Doxygen API documentation page for this application.
-srcDoc
Display Doxygen source documentation page for this application.
-insidePoint <point>
Only keep region containing specified point.
-largestOnly
Only keep largest region.

NOTE

  • cellZonesOnly does not do a walk and uses the cellZones only. Use this if you don’t mind having disconnected domains in a single region. This option requires all cells to be in one (and one only) cellZone.
  • cellZonesFileOnly behaves like -cellZonesOnly but reads the cellZones from the specified file. This allows one to explicitly specify the region distribution and still have multiple cellZones per region.
  • useCellZonesOnly does not do a walk and uses the cellZones only. Use this if you don’t mind having disconnected domains in a single region. This option requires all cells to be in one (and one only) cellZone.
  • Should work in parallel. cellZones can differ on either side of processor boundaries in which case the faces get moved from processor patch to directMapped patch. Not very well tested.
  • If a cell zone gets split into more than one region it can detect the largest matching region (-sloppyCellZones). This will accept any region that covers more than 50% of the zone. It has to be a subset so cannot have any cells in any other zone.

  • writes maps like decomposePar back to original mesh:

    • pointRegionAddressing : for every point in this region the point in the original mesh
    • cellRegionAddressing : ,, cell ,, cell ,,
    • faceRegionAddressing : ,, face ,, face in the original mesh + turning index. For a face in the same orientation this is the original facelabel+1, for a turned face this is -facelabel-1

SEE ALSO

An overview of FreeFOAM is given in freefoam(1).

AUTHOR

OpenCFD Ltd.

FREEFOAM

Part of the freefoam(1) suite.

COPYRIGHT

  • Copyright © 2008-2012 Michael Wild.
  • Copyright © 1991-2010 OpenCFD Ltd.