[maddalena]

Hello all,
is there anyone which has a conjugateHeatFoam version modified in such a way that an arbitrary number of solid and fluid regions are allowed? I need something like chtMultiRegionFoam which includes features of conjugateHeatFoam...

Thank you!


mad

[kamkari]

Hi mad
I am currently working with conjugateHeatFoam but with two regions, solid and fluid. You could have two solid parts simply by selecting velocity equal to zero. I have to add that if you want to calculate the gradient of a variable on the interface (coupled boundry) you will face with problem. For more information about this defect have look to the following link:
http://www.cfd-online.com/Forums/ope...6-ext.htmlBest

Best Regards

[maddalena]

Originally Posted by kamkari

conjugateHeatFoam but with two regions, solid and fluid. You could have two solid parts simply by selecting velocity equal to zero.

well... that seems to be not enough for me: I need n solids and 2 fluids at least ! It does not seem to difficult to modify the solver though. Before try by myself, I would like to know if someone else has a piece of code which can be shared...

mad

[benk]

The hardest part when adding more than 2 regions is just editing attachPatches.H. Here's an example for 3 regions:

{
    const polyPatchList& patches = mesh1.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
    mesh1.surfaceInterpolation::movePoints(); 
    
    const polyPatchList& patches1 = mesh2.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
    mesh2.surfaceInterpolation::movePoints();
    
    const polyPatchList& patches2 = mesh3.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
    mesh3.surfaceInterpolation::movePoints();
}

And then you do something similar for detatchPatches.H
After this, all you have to do is make sure you have the right directory structure.

[maddalena]

Hello,
I am still planning how to make conjugateHeatFoam adjustable for an arbitrary number of regions. unfortunately I cannot work on the subject in a continuous way ...
According to what Henrik said on 2009 here:

Originally Posted by henrik

you can solve on three regions, but you need to duplicate the flow physics which is not natural unless the physics is actually different, e.g. turbulent on one side and visco-elastic on the other. [...] Then [...] coupledFvScalarMatrix TEqns(2)

Questions:

1. Is the information given above a little bit outdated or the modification suggested by Benk (Hi!) is not the only one I need to implement?
2. If Henrik's information is correct, then I need to duplicate the physics of the problem for n times, where n are the number of regions with different properties I have. Let us say I implement the solver to handle 20 regions. What if my case has only 5 regions?
3. May be possible to implement a "for loop" for regions working in the same way the "for loop" works for patches on attachPatches and detachPatches? Does this make any sense?

Any opinion / suggestion you can give me may be useful... thank you

mad

[helmut]

Hi Mad,

Have your questions been answered?
I borrowed some ideas from chtMultiRegionFoam and created pointerLists to my regions.
In my master case constant directory I have a regionProperties file listing my fluid and solid region names. See for example $FOAM_TUTORIALS//heatTransfer/chtMultiRegionFoam/multiRegionHeater/constant/regionProperties

My createSolidMeshes.H looks like this:
forAll(rp.solidRegionNames(), i)
{
Info<< "Create solid mesh for region " << rp.solidRegionNames()[i]
<< " for time = " << runTime.timeName() << nl << endl;
solidRegions.set
(
i,
new fvMesh
(
IOobject
(
rp.solidRegionNames()[i],
runTime.timeName(),
runTime,
IOobject::MUST_READ
)
)
);
}
Similarly for the fluid meshes.

In attachPatches.H I have for the solid side:
// solid regions
forAll(solidRegions, i)
{
//Info<< "attaching patches for solid region i =" << i << endl;
const polyPatchList& patches = solidRegions[i].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();
solidRegions[i].surfaceInterpolation::movePoints();
}
Similarly for the fluid side

[nilvxingren]

Originally Posted by helmut

Hi Mad,

Have your questions been answered?
I borrowed some ideas from chtMultiRegionFoam and created pointerLists to my regions.
In my master case constant directory I have a regionProperties file listing my fluid and solid region names. See for example $FOAM_TUTORIALS//heatTransfer/chtMultiRegionFoam/multiRegionHeater/constant/regionProperties

My createSolidMeshes.H looks like this:
forAll(rp.solidRegionNames(), i)
{
Info<< "Create solid mesh for region " << rp.solidRegionNames()[i]
<< " for time = " << runTime.timeName() << nl << endl;
solidRegions.set
(
i,
new fvMesh
(
IOobject
(
rp.solidRegionNames()[i],
runTime.timeName(),
runTime,
IOobject::MUST_READ
)
)
);
}
Similarly for the fluid meshes.

In attachPatches.H I have for the solid side:
// solid regions
forAll(solidRegions, i)
{
//Info<< "attaching patches for solid region i =" << i << endl;
const polyPatchList& patches = solidRegions[i].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();
solidRegions[i].surfaceInterpolation::movePoints();
}
Similarly for the fluid side

Hi, helmut
I modified my code like your method, but the error occurred when I compile it

In file included from conjugateHeatMulSimpleFoam.C(56):
createSolidFields.H(37): error: a reference of type "Foam::Istream &" (not const-qualified) cannot be initialized with a value of type "Foam::fvMesh"
         thermalModel::New(solidRegions[i])
                           ^

In file included from conjugateHeatMulSimpleFoam.C(56):
createSolidFields.H(34): error: no instance of overloaded function "Foam::PtrList<T>::set [with T=Foam::thermalModel]" matches the argument list
In file included from conjugateHeatMulSimpleFoam.C(56):
            argument types are: (Foam::label, Foam::autoPtr<Foam::dictionary>)
In file included from conjugateHeatMulSimpleFoam.C(56):
            object type is: Foam::PtrList<Foam::thermalModel>
In file included from conjugateHeatMulSimpleFoam.C(56):
      solidThermo.set
                  ^

conjugateHeatMulSimpleFoam.C(87): error: class "Foam::PtrList<Foam::thermalModel>" has no member "correct"
          solidThermo.correct();
                      ^

conjugateHeatMulSimpleFoam.C(88): error: identifier "ksolid" is undefined
          ksolid = solidThermo.k();
          ^

conjugateHeatMulSimpleFoam.C(88): error: class "Foam::PtrList<Foam::thermalModel>" has no member "k"
          ksolid = solidThermo.k();
                               ^

conjugateHeatMulSimpleFoam.C(97): error: no instance of overloaded function "Foam::fvc::interpolate" matches the argument list
            argument types are: (<error-type>)
          surfaceScalarField ksolidf = fvc::interpolate(ksolid);
                                       ^

conjugateHeatMulSimpleFoam.C(98): error: class "Foam::PtrList<Foam::thermalModel>" has no member "modifyResistance"
          solidThermo.modifyResistance(ksolidf);
                      ^

In file included from solveEnergy.H(3),
                 from conjugateHeatMulSimpleFoam.C(100):
readSolidControls.H(1): error: identifier "solidMesh" is undefined
      const dictionary& simple = solidMesh.solutionDict().subDict("SIMPLE");
                                 ^

In file included from conjugateHeatMulSimpleFoam.C(100):
solveEnergy.H(29): error: identifier "Tsolid" is undefined
            - fvm::laplacian(ksolidf, Tsolid, "laplacian(k,T)")
                                      ^

In file included from conjugateHeatMulSimpleFoam.C(100):
solveEnergy.H(29): error: no instance of overloaded function "Foam::fvm::laplacian" matches the argument list
In file included from conjugateHeatMulSimpleFoam.C(100):
            argument types are: (Foam::surfaceScalarField, <error-type>, const char [15])
In file included from conjugateHeatMulSimpleFoam.C(100):
            - fvm::laplacian(ksolidf, Tsolid, "laplacian(k,T)")
              ^

In file included from conjugateHeatMulSimpleFoam.C(100):
solveEnergy.H(30): error: class "Foam::PtrList<Foam::thermalModel>" has no member "S"
            + fvm::SuSp(-solidThermo.S()/Tsolid, Tsolid)
                                     ^

In file included from conjugateHeatMulSimpleFoam.C(100):
solveEnergy.H(30): error: no instance of overloaded function "Foam::fvm::SuSp" matches the argument list
In file included from conjugateHeatMulSimpleFoam.C(100):
            argument types are: (<error-type>, <error-type>)
In file included from conjugateHeatMulSimpleFoam.C(100):
            + fvm::SuSp(-solidThermo.S()/Tsolid, Tsolid)
              ^

compilation aborted for conjugateHeatMulSimpleFoam.C (code 2)

I modified the creatSolidField.h like this:

PtrList<thermalModel> solidThermo(solidRegions.size());
PtrList<volScalarField> Ts(solidRegions.size());
PtrList<volScalarField> ks(solidRegions.size());


forAll(solidRegions, i)
{
    Info<< "*** Reading solid mesh thermophysical properties for region "
        << solidRegions[i].name() << nl << endl;

    Info<< "Reading field Tsolid\n" << endl;

    Ts.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "T",
                runTime.timeName(),
                //solidMesh,
                solidRegions[i],
                IOobject::MUST_READ,
                IOobject::AUTO_WRITE
            ),
            //solidMesh
            solidRegions[i]
        )

    );

    Info<< "Reading solid thermal properties" << endl;
    solidThermo.set
    (
       i,
       thermalModel::New(solidRegions[i])
    );

    Info<< "Reading solid diffusivity k\n" << endl;

    ks.set
    (
       i,
       new volScalarField
       (
           IOobject
           (
               "k",
               runTime.timeName(),
               //solidMesh,
               solidRegions[i],
               IOobject::MUST_READ,
               IOobject::AUTO_WRITE
           ),
           //solidMesh
           solidRegions[i]
       )
    );
}

I don't know the solidThermo.set is right, mybe that's reason the error

[nilvxingren]

Originally Posted by maddalena

well... that seems to be not enough for me: I need n solids and 2 fluids at least ! It does not seem to difficult to modify the solver though. Before try by myself, I would like to know if someone else has a piece of code which can be shared...

mad

Hi mad,
Do you modified the solver fot n solids? I've been doing this lately, but I've had some difficulties, can you give some suggstion?