conjugateHeatFoam for 4 different regions

lg88 · July 6, 2012, 22:04

Hello everybody,
I am going to use conjugateHeatFoam to simulate a conduction problem in a multi region case, thus including solid regions and fluid regions. I am using OF 1.6-ext.
There are 4 different regions, corresponding to different materials: A and C are solids, B and D is fluid (laminar). All the mesh is hexa,
Can solver conjugateHeatFoam realize my need?Do I need to modify the solver code?
thank you very much!

regards!

lg88

wyldckat · July 9, 2012, 18:29

Greetings lg88,

In response to the private message you sent me:
I'm not familiar with conjugateHeatFoam. But I think that chtMultiRegionFoam should be able to solve this issue, but again, I'm not very familiar with either one of these solvers.

Best regards,
Bruno

lg88 · July 9, 2012, 22:20

Thank you for your suggestion.But I am familiar with conjugateHeatFoam and my new solver is based on it.I hope use the solver to solve my problem.I found some information about the same problem I meet at [url]http://www.cfd-online.com/Forums/openfoam/89684-conjugateheatfoam-arbitrary-number-region.html.But there is not detailed construction.
Can anyone give me some idea?

Thank you very much!

lg88

su_junwei · July 9, 2012, 22:34

Quote:

Originally Posted by lg88

Hello everybody,
I am going to use conjugateHeatFoam to simulate a conduction problem in a multi region case, thus including solid regions and fluid regions. I am using OF 1.6-ext.
There are 4 different regions, corresponding to different materials: A and C are solids, B and D is fluid (laminar). All the mesh is hexa,
Can solver conjugateHeatFoam realize my need?Do I need to modify the solver code?
thank you very much!

regards!

lg88

conjugateHeatFoam can only deal with two different regions, three or more regions are not allowed. Use chtMultiRegionFoam instead please.

Regards, Junwei

lg88 · July 11, 2012, 01:25

hello
Thank you for your suggestion .I have checked in the forum and found that some people had applied conjugateHeatFoam to multi-regions successfully.And my new foam is developed based on the conjugateHeatFoam.

regards!

lg88

benk · July 13, 2012, 18:43

You need to edit the files attachPatches.H and detachPateches.H. You then have a main region and all other regions are treated as submeshes of the main region.

I've only done this for 3 regions, but 4 or more is definitely possible.

attachPatches.H (for 3 regions):

Code:

{
    const polyPatchList& patches = mesh.boundaryMesh();

    forAll (patches, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    mesh.surfaceInterpolation::movePoints(); 
    
    const polyPatchList& patches1 = separatorMesh.boundaryMesh();

    forAll (patches1, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches1[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches1[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    separatorMesh.surfaceInterpolation::movePoints();
    
    const polyPatchList& patches2 = positiveMesh.boundaryMesh();

    forAll (patches2, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches2[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches2[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    positiveMesh.surfaceInterpolation::movePoints();
}

detachPatches.H (for 3 regions):

Code:

{
    const polyPatchList& patches = mesh.boundaryMesh();

    forAll (patches, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    mesh.surfaceInterpolation::movePoints();

    const polyPatchList& patches1 = separatorMesh.boundaryMesh();

    forAll (patches1, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches1[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches1[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    separatorMesh.surfaceInterpolation::movePoints();
    
    const polyPatchList& patches2 = positiveMesh.boundaryMesh();

    forAll (patches2, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches2[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches2[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    positiveMesh.surfaceInterpolation::movePoints();
}

In the above, my submeshes are called "separatorMesh" and "positiveMesh".

Then in case/constant you have:
polyMesh/... (for the main mesh)
positive/polyMesh/... (for one submesh)
separator/polyMesh/... (for the other submesh)

In case/0 you have:
{fields for main mesh}
positive/{fields for positive mesh}
separator/{fields for separator mesh}

bryant_k · July 14, 2012, 11:53

Thank you for your detailed construction.I am also looking for the multi-region function of conjugateHeatFoam.

Regards!

kob

lg88 · July 14, 2012, 12:01

@benk
Thank you very much.I have modified my code as you said. Now it can work fluently and I am waiting for the results.Hoping it will work.

Regards!

lg88

ramon · August 25, 2012, 16:17

can anyone send me a simple tutorial of conjugateHeatFoam for multiregion (2fluid & 1solid) ?
Can anyone give me some idea?
thanks

mscheng · October 19, 2013, 23:35

Quote:

Originally Posted by lg88

@benk
Thank you very much.I have modified my code as you said. Now it can work fluently and I am waiting for the results.Hoping it will work.

Regards!

lg88

Hi lg88,

In your case, can the boudaryField fully show in the solution file (such as T) using conjugateHeatFoam?

Thanks!
CHENG

nilvxingren · July 30, 2020, 22:35

Hi, benk
I modified my code like these
attachPatches.H (for 4 regions):

Code:

{
    const polyPatchList& patches = mesh.boundaryMesh();

    forAll (patches, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    mesh.surfaceInterpolation::movePoints();

    //solidone
    const polyPatchList& patches1 = solidMesh1.boundaryMesh();

    forAll (patches1, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches1[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches1[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    solidMesh1.surfaceInterpolation::movePoints();


    //solidtwo
    const polyPatchList& patches2 = solidMesh2.boundaryMesh();

    forAll (patches2, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches2[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches2[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    solidMesh2.surfaceInterpolation::movePoints();

    //solidthree
    const polyPatchList& patches3 = solidMesh3.boundaryMesh();

    forAll (patches3, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches3[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches3[patchI]);

            // Attach it here
            rcp.attach();
        }
    }

    // Force recalculation of weights
    solidMesh3.surfaceInterpolation::movePoints();
}

detachPatches.H (for 4 regions):

Code:

{
    const polyPatchList& patches = mesh.boundaryMesh();

    forAll (patches, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    mesh.surfaceInterpolation::movePoints();

    //solidone
    const polyPatchList& patches1 = solidMesh1.boundaryMesh();

    forAll (patches1, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches1[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches1[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    solidMesh1.surfaceInterpolation::movePoints();


    //solidtwo
    const polyPatchList& patches2 = solidtMesh2.boundaryMesh();

    forAll (patches2, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches2[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches2[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    solidMesh2.surfaceInterpolation::movePoints();

    //solidthree
    const polyPatchList& patches3 = solidMesh3.boundaryMesh();

    forAll (patches3, patchI)
    {
        if (isType<regionCouplePolyPatch>(patches3[patchI]))
        {
            const regionCouplePolyPatch& rcp =
                refCast<const regionCouplePolyPatch>(patches3[patchI]);

            // Detach it here
            rcp.detach();
        }
    }

    // Force recalculation of weights
    solidMesh3.surfaceInterpolation::movePoints();
}

but, when I wmake, compile error has occurred:

Code:

In file included from createFields.H(80),
                 from conjugateHeatThreesSimpleFoam.C(51):
attachPatches.H(20): error: identifier "solidMesh1" is undefined
      const polyPatchList& patches1 = solidMesh1.boundaryMesh();
                                      ^

In file included from createFields.H(80),
                 from conjugateHeatThreesSimpleFoam.C(51):
attachPatches.H(39): error: identifier "solidMesh2" is undefined
      const polyPatchList& patches2 = solidMesh2.boundaryMesh();
                                      ^

In file included from createFields.H(80),
                 from conjugateHeatThreesSimpleFoam.C(51):
attachPatches.H(57): error: identifier "solidMesh3" is undefined
      const polyPatchList& patches3 = solidMesh3.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(67):
detachPatches.H(20): error: identifier "solidMesh1" is undefined
      const polyPatchList& patches1 = solidMesh1.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(67):
detachPatches.H(39): error: identifier "solidtMesh2" is undefined
      const polyPatchList& patches2 = solidtMesh2.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(67):
detachPatches.H(54): error: identifier "solidMesh2" is undefined
      solidMesh2.surfaceInterpolation::movePoints();
      ^

In file included from conjugateHeatThreesSimpleFoam.C(67):
detachPatches.H(58): error: identifier "solidMesh3" is undefined
      const polyPatchList& patches3 = solidMesh3.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(87):
attachPatches.H(20): error: identifier "solidMesh1" is undefined
      const polyPatchList& patches1 = solidMesh1.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(87):
attachPatches.H(39): error: identifier "solidMesh2" is undefined
      const polyPatchList& patches2 = solidMesh2.boundaryMesh();
                                      ^

In file included from conjugateHeatThreesSimpleFoam.C(87):
attachPatches.H(57): error: identifier "solidMesh3" is undefined
      const polyPatchList& patches3 = solidMesh3.boundaryMesh();
                                      ^

compilation aborted for conjugateHeatThreesSimpleFoam.C (code 2)

Am I missing something?
Thank you very much

July 9, 2012, 18:29		#2
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Greetings lg88, In response to the private message you sent me: I'm not familiar with conjugateHeatFoam. But I think that chtMultiRegionFoam should be able to solve this issue, but again, I'm not very familiar with either one of these solvers. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

July 9, 2012, 22:20		#3
lg88 Member jack Join Date: Jul 2011 Posts: 52 Rep Power: 15	Thank you for your suggestion.But I am familiar with conjugateHeatFoam and my new solver is based on it.I hope use the solver to solve my problem.I found some information about the same problem I meet at [url]http://www.cfd-online.com/Forums/openfoam/89684-conjugateheatfoam-arbitrary-number-region.html.But there is not detailed construction. Can anyone give me some idea? Thank you very much! lg88 Last edited by lg88; July 9, 2012 at 23:46.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
how the interface between 2 solid regions is treater in chtMultiRegionFoam ?	Cyp	OpenFOAM	2	March 15, 2023 06:35
[CAD formats] beginners how to convert binarySTL to asciiSTL with regions (good for SHM tutorial)	soonic	OpenFOAM Meshing & Mesh Conversion	11	July 28, 2017 16:46
isolated fluid regions were found	alfin	CFX	14	October 8, 2015 02:36
Splitting regions	king_steve	STAR-CCM+	1	September 27, 2010 13:48
conjugateHeatFoam: Problems adding 3rd region	benk	OpenFOAM	5	April 21, 2010 13:46

July 11, 2012, 01:25		#5
lg88 Member jack Join Date: Jul 2011 Posts: 52 Rep Power: 15	hello Thank you for your suggestion .I have checked in the forum and found that some people had applied conjugateHeatFoam to multi-regions successfully.And my new foam is developed based on the conjugateHeatFoam. regards! lg88

July 14, 2012, 11:53		#7
bryant_k New Member kob Join Date: Nov 2011 Posts: 28 Rep Power: 15	Thank you for your detailed construction.I am also looking for the multi-region function of conjugateHeatFoam. Regards! kob

July 14, 2012, 12:01		#8
lg88 Member jack Join Date: Jul 2011 Posts: 52 Rep Power: 15	@benk Thank you very much.I have modified my code as you said. Now it can work fluently and I am waiting for the results.Hoping it will work. Regards! lg88

August 25, 2012, 16:17		#9
ramon New Member reza Join Date: May 2012 Posts: 3 Rep Power: 14	can anyone send me a simple tutorial of conjugateHeatFoam for multiregion (2fluid & 1solid) ? Can anyone give me some idea? thanks