CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

splitMeshRegions -cellZonesFileOnly <zoneFile>

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 28, 2014, 13:05
Default splitMeshRegions -cellZonesFileOnly <zoneFile>
  #1
New Member
 
Anders
Join Date: Nov 2010
Posts: 10
Rep Power: 16
anlj is on a distinguished road
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
anlj is offline   Reply With Quote

Old   November 6, 2015, 15:04
Default
  #2
Senior Member
 
nasir musa yakubu
Join Date: Mar 2014
Location: Birmingham
Posts: 109
Rep Power: 12
esujby is on a distinguished road
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;
thanks
esujby is offline   Reply With Quote

Old   June 16, 2016, 11:22
Default
  #3
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13
derekm is on a distinguished road
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
derekm is offline   Reply With Quote

Old   January 17, 2025, 13:37
Default
  #4
New Member
 
KaiXu
Join Date: Dec 2023
Posts: 2
Rep Power: 0
KXcef is on a distinguished road
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.
KXcef is offline   Reply With Quote

Reply

Tags
cellzonesfileonly, splitmeshregions

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
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


All times are GMT -4. The time now is 11:57.