|
[Sponsors] |
splitMeshRegions -cellZonesFileOnly <zoneFile> |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Anders
Join Date: Nov 2010
Posts: 10
Rep Power: 16 ![]() |
Dear all,
In splitMeshRegions.C one can read that the flag -cellZonesFileOnly behaves like -cellZonesOnly but reads the cellZones from the specified file, and that this allows you to explicitly specify the region distribution and still have multiple cellZones per region. I.e. just what I need, but it don't explain the syntax in <zoneFile>, and I can't figure it out. Can anyone give me a hint? Cheers, Anders |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
nasir musa yakubu
Join Date: Mar 2014
Location: Birmingham
Posts: 109
Rep Power: 12 ![]() |
Thanks for creating this thread, i am in the same issue, i am wondering if its to be used in the snappyHexMeshDict as follows:
Code:
s5 { // Surface-wise min and max refinement level level (5 5); faceZone s5; faceType baffle; cellZonesFileOnly s5.stl; cellZoneInside inside; |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Senior Member
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13 ![]() |
The zonefile format is the same as yourcase/constant/polyMesh/cellZones
and the default location is yourcase/constant/polyMesh/ e.g. Code:
FoamFile { version 2.0; format ascii; class regIOobject; location "constant/polyMesh"; object cellZones; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 3 ( leftAir { type cellZone; cellLabels List<label> 2128189 ( 28 79 80 81 82 83 84 ... ) } );
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
KaiXu
Join Date: Dec 2023
Posts: 2
Rep Power: 0 ![]() |
to any new foamers who like me also getting confused with the problem "how to actually keep multiple non-empty cellZones in each region via splitRegions -cellZonesFileOnly", especially when converting fluent meshes in opnefoam, this is how I processed:
(a) write under /system a topoSetDict format file (I name it as "topoSetDict_regions" for convenience) which defines the desired regions in the form of different cellzones. (b) run topoSet -dict topoSetDict_regions. Then Copy and rename the generated/modified cellZone file under /constant/polymesh into, e.g. "cellZones_regions". Note that both file "cellZones" and "cellZones_regions" exist; (c) write another topoSetDict format file (similarly, named as topoSet_cellZones) which modifies the "cellZones" file into all the desired cellzones, regardless of the regions they should belong to. In thread merge or combine several cellZone I found useful ways to shifting and temporarily storing the cellzone information from the original mesh file. In this step note that in the final "cellZones" file the zones created via topoSetDict_regions should be removed using the action type "remove", since splitRegions -cellZonesOnly will check that cells only belong to one cellZone in the default "cellZones" file (it doesnt check if multiple belongings across different cellZones syntax files) (d) run topoSet -dict topoSetDict_cellZones. Then run splitRegions -cellZonesFileOnly cellZones_regions -overwrite. |
|
![]() |
![]() |
![]() |
Tags |
cellzonesfileonly, splitmeshregions |
Thread Tools | Search this Thread |
Display Modes | |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[mesh manipulation] why splitMeshRegions creates extra domains? | skuznet | OpenFOAM Meshing & Mesh Conversion | 10 | May 31, 2022 06:54 |
splitMeshRegions doesn't find my regions. | GPesch | OpenFOAM Pre-Processing | 2 | November 14, 2013 06:20 |
splitMeshRegions and boundarys | Tobi | OpenFOAM | 1 | January 25, 2013 14:33 |
splitMeshRegions | VdG | OpenFOAM Bugs | 5 | June 14, 2010 05:31 |
splitMeshRegions | naltang | OpenFOAM | 3 | May 6, 2010 13:22 |