[aminem]

Hi,

Can I use cfMesh for Multi Region Meshing like snappyHexMesh?

Thanks

[starykov]

You can.
Please find a sample case in attachment, the Allrun-file shows you the way to make the multi-region mesh.

[thegame24]

Originally Posted by starykov

You can.
Please find a sample case in attachment, the Allrun-file shows you the way to make the multi-region mesh.

Hi.

I think the file attached has different patches, as in, different walls are defined. What should I do to define separate regions (volumes) in the mesh.

I am a beginner here, so please correct me if I'm wrong.

[starykov]

Hi,

the multi-regions meshing algorithm is self-explained in Allrun-script, but I can explain it to you.

First you need to create mesh for each region. Since cfmesh has no direct possibility for doing this, you can create two cases and generate mesh for each of them (with custom meshDict-settings):

 
cartesianMesh -case cases/pipewall
cartesianMesh -case cases/pipe

Afterwards you need to copy generated meshes to the constant/polyMesh directory in order to use them as region meshes:

 
cp -r cases/pipe/constant/polyMesh/ constant/pipe
cp -r cases/pipewall/constant/polyMesh/ constant/pipewall

Now you need to correctly adress the field mappings etc. This is done via changeDictionary tool, using the system/changeDictionaryDict for each region. In system/pipe/changeDictionaryDict you have:

 
dictionaryReplacement
{
boundary
   {
   pipe_to_pipewall
     {
      type mappedWall;
      sampleMode nearestPatchFace;
      sampleRegion pipewall;
      samplePatch pipewall_to_pipe;
      }

    }
 
}

That means that in the file constant/polyMesh/pipe/boundary the entry pipe_to_pipewall will be modified with these settings. You define this boundary as mapped on the neighboring region that has name pipewall, and the neighboring patch has name pipewall_to_pipe.
You need to create such mappings for all inter-region boundaries in your system.

Of course you need to properly set the heat transfer conditions at the boundaries, usually via changeDictionaryDict files.

[thegame24]

Thanks. You saved me.

[simrego]

Hi!

I think you should use nearestPatchFaceAMI, since your mesh at the interface is not conform.

[starykov]

Yes, you are right.

[Bastian@MM]

Hi starykov,


I have a question about MultiRegion-Meshing with cfMesh. I have a case with 6 region andbe able to mesh them. But to run chtMultiRegionSimpleFoam I need the cellToRegion file in 0. How did you create it?

[julieng]

Hello,

I try to mesh multiregions, I found this topic and I try the case attached by starykov. When I do the Allrun command it complains with

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*   Windows 32 and 64 bit porting by blueCAPE: http://www.bluecape.com.pt   *\
|  Based on Windows porting (2.0.x v4) by Symscape: http://www.symscape.com   |
\*---------------------------------------------------------------------------*/
Build  : 5.x-963176928289
Exec   : C:/PROGRA~1/BLUECF~1/OpenFOAM-5.x/platforms/mingw_w64GccDPInt32Opt/bin/changeDictionary.exe -region pipe
Date   : Dec 23 2020
Time   : 15:04:35
Host   : "PC_JULIEN"
PID    : 9648
I/O    : uncollated
Case   : C:/PROGRA~1/BLUECF~1/OFUSER~1/run/CFMESH~1/forum/tubeStl
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh pipe for time = 0

Read dictionary changeDictionaryDict with replacements for dictionaries 1(dictionaryReplacement)
Reading polyMesh/boundary file to extract patch names
Loaded dictionary boundary with entries
3
(
minY
maxY
pipe_to_pipewall
)

Replacing entries in dictionary dictionaryReplacement
Loading dictionary dictionaryReplacement


--> FOAM FATAL ERROR:
cannot find file "C:/PROGRA~1/BLUECF~1/OFUSER~1/run/CFMESH~1/forum/tubeStl/0/pipe/dictionaryReplacement"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 522.

FOAM exiting

It is a problem with changeDictionnaryDict file I think but I don't know how to resolve this. I see also that there is no directory constant/polyMesh created. Maybe the problem comes from to this.

I work with bluecorecfd on windows 10.

Best regards

[starykov]

Hello,

for this particular problem you have to remove that dictionaryReplacement with
{} parentheses in the dict file. The file format changed in the meantime.

But there are other changes, you have to adjust your files. Look at the heater-tutorials in the heatTransfer directory and update them accordingly.

Originally Posted by julieng

Hello,

[Adibantwal]

Hi, after running Allrun with your case, it gives this error:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _f3950763fe-20191219 OPENFOAM=1912
Arch   : "LSB;label=32;scalar=64"
Exec   : changeDictionary -region pipewall
Date   : Mar 06 2022
Time   : 18:17:54
Host   : LAPTOP-TT50BSP8
PID    : 21018
I/O    : uncollated
Case   : /mnt/c/Users/Aditya/Desktop/learrn/tubeStl/tubeStl
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh pipewall for time = 0

Read dictionary changeDictionaryDict with replacements for dictionaries 1(dictionaryReplacement)
Reading polyMesh/boundary file to extract patch names
Loaded dictionary boundary with entries 4(minY maxY wall pipewall_to_pipe)
Replacing entries in dictionary dictionaryReplacement
Loading dictionary dictionaryReplacement
--> FOAM Warning :
    From function int main(int, char**)
    in file changeDictionary.C at line 709
    Requested field to change dictionaryReplacement does not exist in "/mnt/c/Users/Aditya/Desktop/learrn/tubeStl/tubeStl/0/pipewall"

End

[itsme_kit]

Originally Posted by starykov

Yes, you are right.

Hi starykov

Though we apply nearestPatchFaceAMI in sampleMode (fields will be mapped in those two different regions in the process of simulation), the generated mesh in Paraview is still not conform, is there a way of creating a conformal mesh in this case in cfmesh?

Looking forward to hearing from you.

Best Regards,

Kit

[chaz]

Hello,
Has anyone been able to get the sample file provided running?
There have been a few issues noted in the thread, and in order to get close to have it running in of2312, there was a missing g file, missing "uniform" designation on boundary, and some other issues.


Now, I get the following errors. changeDictionary is not changing the boundaries. It shows a warning, but if it is not executing, that My modified case is attached.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2312                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _e651d635-20240208 OPENFOAM=2312 patch=240220 version=2312
Arch   : "LSB;label=32;scalar=64"
Exec   : changeDictionary -region pipe
Date   : Sep 03 2024
Time   : 22:01:03
Host   : zalbuntuSpeed
PID    : 83053
I/O    : uncollated
Case   : /home/m/Sync/LNC_Sync/engineering/2024_08_foam_practice/07tubeStl
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh pipe for time = 0

Read dictionary changeDictionaryDict with replacements for dictionaries 1(dictionaryReplacement)
Reading polyMesh/boundary file to extract patch names
Loaded dictionary boundary with entries 3(minY maxY pipe_to_pipewall)
Replacing entries in dictionary dictionaryReplacement
Loading dictionary dictionaryReplacement
--> FOAM Warning : 
    From int main(int, char**)
    in file changeDictionary.C at line 704
    Requested field to change dictionaryReplacement does not exist in "/home/m/Sync/LNC_Sync/engineering/2024_08_foam_practice/07tubeStl/0/pipe"

End

The chtmultiregion has an error, and it appears that this is because changedict is not changing the dictionaries.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2312                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _e651d635-20240208 OPENFOAM=2312 patch=240220 version=2312
Arch   : "LSB;label=32;scalar=64"
Exec   : chtMultiRegionFoam
Date   : Sep 03 2024
Time   : 22:08:23
Host   : zalbuntuSpeed
PID    : 88316
I/O    : uncollated
Case   : /home/m/Sync/LNC_Sync/engineering/2024_08_foam_practice/07tubeStl
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region pipe for time = 0

Create solid mesh for region pipewall for time = 0

*** Reading fluid mesh thermophysical properties for region pipe

    Adding to thermoFluid

Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectFluid;
    specie          specie;
    energy          sensibleEnthalpy;
}



--> FOAM FATAL ERROR: (openfoam-2312 patch=240220)
Incorrect patch type wall for patch pipe_to_pipewall of field T in file "/home/m/Sync/LNC_Sync/engineering/2024_08_foam_practice/07tubeStl/0/pipe/T"
Type should be a mappedPatch

    From static const Foam::mappedPatchBase& Foam::mappedPatchFieldBase<Type>::mapper(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
    in file ./src/finiteVolume/lnInclude/mappedPatchFieldBase.C at line 954.

FOAM exiting

Given this case and the modifications noted in the thread, any idea what this hangup could be?

[Yann]

Hello Chaz,

Your changeDictionaryDict uses a different syntax than the one in OpenFOAM-v2312.

You need to update your changeDictionaryDict to match v2312 syntax.

Errors using cfmesh and muliple regions (chtmultiregionsimplefoam)

Cheers,
Yann

[chaz]

Thank you Yann. Yes, you noted that I asked this question elsewhere, and you answered it already. My memory is failing.


For any future readers, please see the attached case that works in OF V2312 or similar.
-.stl files are converted to meshes using cfmesh
-the meshes at the boundary DO NOT conform, but heat flows across the boundary using mapping
-result looks reasonable....

[CFD_with_Skill-Lync]

Hi Yann,
How are the patches (pipe to pipe wall and pipe wall to pipe) mapped for chtMultiRegionFoam? The free version of cfMesh doesn't allow for multi-region mesh and sorely lacks this one capability. Even when we merge meshes, the mapping doesn't get done properly.
Thanks
Team Skill-Lync

[Yann]

Hello,

The usual workflow when meshing with snappy:

1. Mesh all regions at once in snappy, defining cellZones for each regions. You end up with one single mesh containing all regions.
2. Use splitMeshRegions to split the mesh into separate meshes for each region. This automatically creates interfaces using mappedWall type.

If you use mergeMeshes, you will end up with one single mesh for all regions, but with separate patches at the interface. This is probably why splitMeshRegions will not detect the interfaces and does not create it. After merging the meshes you should use something like stitchMesh to stitch your meshes together and remove the patches at interfaces before running splitMeshRegions.

If you mesh each regions separately, you will probably not have conformal mesh at the interfaces, so I am not sure how stitchMesh will perform (there are several options to deal with conformal or not conformal meshes)

The other way around could be to use createPatch to manually create interfaces between regions based on your existing patches. (possibly using cyclicAMI if your interfaces are non conformal).

One more thought: I don't use cfMesh, but can't you mesh all your regions at once and define cellZones for each regions as it is done in snappy? How does it work when your need to define a cellZone somewhere in your mesh to do something with it later in your simulation? (like in fvOptions, or using MRF or whatever)

Yann