Difference between revisions of "RefineMesh"
From OpenFOAMWiki
(First version) |
m (→Description) |
||
Line 17: | Line 17: | ||
'''-overwrite''' | '''-overwrite''' | ||
:Overwrite the existing mesh files | :Overwrite the existing mesh files | ||
− | |||
− | |||
− | |||
− | |||
'''-parallel''' | '''-parallel''' | ||
Line 41: | Line 37: | ||
* multiphase/cavitatingFoam/les/throttle3D | * multiphase/cavitatingFoam/les/throttle3D | ||
* multiphase/cavitatingFoam/ras/throttle | * multiphase/cavitatingFoam/ras/throttle | ||
− | * multiphase/interFoam/les/nozzleFlow2D | + | * multiphase/interFoam/les/nozzleFlow2D |
==refineMeshDict description== | ==refineMeshDict description== |
Latest revision as of 19:00, 3 September 2012
1 Name
refineMesh - Utility to refine cells in multiple directions .
2 Synopsis
refineMesh [OPTIONS]
3 Description
Refine the all cells of the mesh by cutting them in 8 for a 3D mesh, respectively 4 for a 2D mesh. If you don't want to refine all the mesh or in all directions, you must write a dictionary system/refineMeshDict.
If the option -dict is specified, the refinement is applied on a cellSet according to the parameters specified in system/refineMeshDict. The example shipped with the source code (in $FOAM_TUTORIALS/combustion/fireFoam/les/oppositeBurningPanels/system/refineMeshDict) is reproduced below.
-dict
- Refine the mesh according the parameters written in system/refineMeshDict
-overwrite
- Overwrite the existing mesh files
-parallel
- Run the utility in parallel
-roots "(DIR1 [...DIRN])"
- Directories through which the data are distributed
-region NAME
- Specify a mesh region by its NAME
-case DIR
- Execute the command on the case directory DIR. If not provided, use the current directory
-noFunctionObjects
- Skip the execution of the functionObjects
-help
- Display the help and exit
This utility is used in the following tutorials:
- combustion/fireFoam/les/oppositeBurningPanels
- multiphase/cavitatingFoam/les/throttle
- multiphase/cavitatingFoam/les/throttle3D
- multiphase/cavitatingFoam/ras/throttle
- multiphase/interFoam/les/nozzleFlow2D
4 refineMeshDict description
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object refineMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Cells to refine; name of 'cellSet' set c0; // Type of coordinate system: // - global : coordinate system same for every cell. Usually aligned with // x,y,z axis. Specify in globalCoeffs section below. // - patchLocal : coordinate system different for every cell. Specify in // patchLocalCoeffs section below. coordinateSystem global; // Specifies 2 directions by a name and a vector. The normal direction is // calculated as tan1^tan2 globalCoeffs { tan1 ( 1 0 0 ); tan2 ( 0 1 0 ); } patchLocalCoeffs { // Normal direction is face normal of zero'th face of patch patch outside; tan1 ( 1 0 0 ); tan2 ( 0 0 1 ); } // Specifies the direction to be refined by the name used above // To refine in the third direction, use the keyword 'normal' directions ( tan1 normal ); // Whether to use hex topology. This will // - if patchLocal: all cells on selected patch should be hex // - split all hexes in 2x2x2 through the middle of edges. useHexTopology yes; // Cut purely geometric (will cut hexes through vertices) or take // topology into account. Incompatible with 'useHexTopology' geometricCut no; // Write meshes from intermediate steps writeMesh no;