[mm66]

Dear Foamers ,

I am trying to conduct a multi region heat transfer simulation using chtMultiRegionSimpleFoam. I started big and things were going wrong so now I have a very simple geometry of two cubes (i.e. fluids) sharing an interface. The boundary condition on the interface for velocity in both regions is specified as:

    one_to_two
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    two_to_one
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

The same is being used for all other walls. I have also tried noSlip for the interface, still the same problem:

paraFoam - builtin

results in non-zero velocity at the interface, whereas on all other walls the velocity is zero.

I'm using wall functions and checked y+ which is in range 30<y+<300

Some further info for fvSolution:

    "(U|h|e|k|epsilon)"
    {
        solver          PBiCGStab;
        preconditioner  DILU;
        tolerance       1e-6;
        relTol          1e-3;
    }

and fvSchemes:

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss upwind;
    div(phi,h)      bounded Gauss upwind;
    div(phi,e)      bounded Gauss limitedLinear 1;
    div(phi,K)      bounded Gauss upwind;
    div(phi,k)      bounded Gauss upwind;
    div(phi,epsilon) bounded Gauss upwind;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

PS: I'm using OF v1812 and generated the mesh in Salome which cannot create boundary layer for the inner interface (maybe that is the problem?)

[peterhess]

Hello!

I can not see where is the problem and can not give you a direct answer.

Anyway, I have a case, where I have two regions with solid and fluid regions.

I modified the case to have just fluids as in your case and made the necessary changes to let it run.

I tested the case and the velocity at walls (interfaces) are zero!

All I can do is to give you the working case and you could compare your case with mein to see where is the problem/difference.

Just run Allrun.

The mesh is generated using Salome 8.5.

OF7.0 is used!

If the problem still exists please share the case and let me have a closer look to the setups.

Post a feedback please, also if you fixed the problem to share experiences.

Regards

Peter

https://drive.google.com/file/d/1GfD...ew?usp=sharing

[mm66]

Originally Posted by peterhess

Hello!

I can not see where is the problem and can not give you a direct answer.

Anyway, I have a case, where I have two regions with solid and fluid regions.

I modified the case to have just fluids as in your case and made the necessary changes to let it run.

I tested the case and the velocity at walls (interfaces) are zero!

All I can do is to give you the working case and you could compare your case with mein to see where is the problem/difference.

Just run Allrun.

The mesh is generated using Salome 8.5.

OF7.0 is used!

If the problem still exists please share the case and let me have a closer look to the setups.

Post a feedback please, also if you fixed the problem to share experiences.

Regards

Peter

https://drive.google.com/file/d/1GfD...ew?usp=sharing

Hi Peter,

Thank you very much for your reply and sharing the file. I tried to run the case but got some errors. I could resolve two of them but the last one is not going away (probably due to the OF version difference ?)

The error is:

[1] #0  Foam::error::printStack(Foam::Ostream&)[2] #0  Foam::error::printStack(Foam::Ostream&)[0] #0  Foam::error::printStack(Foam::Ostream&)[3] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[1] #1  Foam::sigFpe::sigHandler(int) at ??:?
[2] #1  Foam::sigFpe::sigHandler(int) at ??:?
 at ??:?
[3] #1  Foam::sigFpe::sigHandler(int)[0] #1  Foam::sigFpe::sigHandler(int) at ??:?
[2] #2  ? at ??:?
[1] #2  ? at ??:?
[0] #2  ? at ??:?
[3] #2  ? in /lib/x86_64-linux-gnu/libc.so.6
[1] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in /lib/x86_64-linux-gnu/libc.so.6
[2] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in /lib/x86_64-linux-gnu/libc.so.6
[3] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in /lib/x86_64-linux-gnu/libc.so.6
[0] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
[1] #4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
[2] #4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
[3] #4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
[0] #4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
[1] #5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
[2] #5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
 at ??:?
[3] #5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const[0] #5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
[1] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
[2] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
[3] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
[0] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
[1] #7  Foam::fvMatrix<double>::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
[2] #7  Foam::fvMatrix<double>::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
[3] #7  Foam::fvMatrix<double>::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
[0] #7  Foam::fvMatrix<double>::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
[1] #8  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ??:?
[2] #8  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ??:?
[3] #8  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ??:?
[0] #8  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ??:?
[1] #9   at ??:?
[2] #9  Foam::fvMatrix<double>::solve()Foam::fvMatrix<double>::solve() at ??:?
[3] #9   in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[2] #10   in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[1] #10   at ??:?
[0] #9  Foam::fvMatrix<double>::solve()??Foam::fvMatrix<double>::solve() in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[3] #10   in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[2] #11  __libc_start_main in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[1] #11  __libc_start_main in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[0] #10  ? in /lib/x86_64-linux-gnu/libc.so.6
[2] #12   in /lib/x86_64-linux-gnu/libc.so.6
[1] #12  ??? in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[3] #11  __libc_start_main in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[0] #11  __libc_start_main in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[VM:09945] *** Process received signal ***
[VM:09945] Signal: Floating point exception (8)
[VM:09945] Signal code:  (-6)
[VM:09945] Failing at address: 0x3e8000026d9
[VM:09945] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7f7eb1395f20]
[VM:09945] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xc7)[0x7f7eb1395e97]
[VM:09945] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7f7eb1395f20]
[VM:09945] [ 3] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xae)[0x7f7eb2a0228e]
[VM:09945] [ 4] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4FoamdvERKNS_5UListIdEES3_+0x54)[0x7f7eb2a04674]
[VM:09945] [ 5] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam14diagonalSolver5solveERNS_5FieldIdEERKS2_h+0x4e)[0x7f7eb27be34e]
[VM:09945] [ 6] [VM:09944] *** Process received signal ***
[VM:09944] Signal: Floating point exception (8)
[VM:09944] Signal code:  (-6)
[VM:09944] Failing at address: 0x3e8000026d8
 in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
 in /lib/x86_64-linux-gnu/libc.so.6
[3] #12  /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x187)[0x7f7eb4f8c417]
[VM:09945] [ 7] [VM:09944] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7f7a51c81f20]
[VM:09944] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xc7)[0x7f7a51c81e97]
[VM:09944] [ 2] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE24solveSegregatedOrCoupledERKNS_10dictionaryE+0x3a5)[0x7f7eb4ad8215]
[VM:09945] [ 8] /lib/x86_64-linux-gnu/libc.so.6(/home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam6fvMesh5solveERNS_8fvMatrixIdEERKNS_10dictionaryE+0x23)[0x7f7eb4a7bff3]
[VM:09945] [ 9] +0x3ef20)[0x7f7a51c81f20]
[VM:09944] chtMultiRegionFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xe0)[0x55d8e315e0f0]
[VM:09945] [10] chtMultiRegionFoam(+0x50da0)[0x55d8e312bda0]
[VM:09945] [11] [ 3] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xe7)[0x7f7eb1378b97]
[VM:09945] [12] chtMultiRegionFoam(+0x5588a)[0x55d8e313088a]
[VM:09945] *** End of error message ***
/home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xae)[0x7f7a532ee28e]
[VM:09944] [ 4] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4FoamdvERKNS_5UListIdEES3_+0x54)[0x7f7a532f0674]
[VM:09944] [ 5] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam14diagonalSolver5solveERNS_5FieldIdEERKS2_h+0x4e)[0x7f7a530aa34e]
[VM:09944] [ 6] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x187)[0x7f7a55878417]
[VM:09944] [ 7] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE24solveSegregatedOrCoupledERKNS_10dictionaryE+0x3a5)[0x7f7a553c4215]
[VM:09944] [ 8] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam6fvMesh5solveERNS_8fvMatrixIdEERKNS_10dictionaryE+0x23)[0x7f7a55367ff3]
[VM:09944] [ 9] chtMultiRegionFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xe0)[0x55cbfb7bb0f0]
[VM:09944] [10] chtMultiRegionFoam(+0x50da0)[0x55cbfb788da0]
[VM:09944] [11] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xe7)[0x7f7a51c64b97]
[VM:09944] [12] chtMultiRegionFoam(+0x5588a)[0x55cbfb78d88a]
[VM:09944] *** End of error message ***
 in /lib/x86_64-linux-gnu/libc.so.6
[0] #12  ?? in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[VM:09946] *** Process received signal ***
[VM:09946] Signal: Floating point exception (8)
[VM:09946] Signal code:  (-6)
[VM:09946] Failing at address: 0x3e8000026da
[VM:09946] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7f044a4e1f20]
[VM:09946] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xc7)[0x7f044a4e1e97]
[VM:09946] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7f044a4e1f20]
[VM:09946] [ 3] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xae)[0x7f044bb4e28e]
[VM:09946] [ 4] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4FoamdvERKNS_5UListIdEES3_+0x54)[0x7f044bb50674]
[VM:09946] [ 5] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam14diagonalSolver5solveERNS_5FieldIdEERKS2_h+0x4e)[0x7f044b90a34e]
[VM:09946] [ 6] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x187)[0x7f044e0d8417]
[VM:09946] [ 7] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE24solveSegregatedOrCoupledERKNS_10dictionaryE+0x3a5)[0x7f044dc24215]
[VM:09946] [ 8] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam6fvMesh5solveERNS_8fvMatrixIdEERKNS_10dictionaryE+0x23)[0x7f044dbc7ff3]
[VM:09946] [ 9] chtMultiRegionFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xe0)[0x55ca46a6b0f0]
[VM:09946] [10] chtMultiRegionFoam(+0x50da0)[0x55ca46a38da0]
[VM:09946] [11] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xe7)[0x7f044a4c4b97]
[VM:09946] [12] chtMultiRegionFoam(+0x5588a)[0x55ca46a3d88a]
[VM:09946] *** End of error message ***
 in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam
[VM:09943] *** Process received signal ***
[VM:09943] Signal: Floating point exception (8)
[VM:09943] Signal code:  (-6)
[VM:09943] Failing at address: 0x3e8000026d7
[VM:09943] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7fa38ba79f20]
[VM:09943] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xc7)[0x7fa38ba79e97]
[VM:09943] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x3ef20)[0x7fa38ba79f20]
[VM:09943] [ 3] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xae)[0x7fa38d0e628e]
[VM:09943] [ 4] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4FoamdvERKNS_5UListIdEES3_+0x54)[0x7fa38d0e8674]
[VM:09943] [ 5] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam14diagonalSolver5solveERNS_5FieldIdEERKS2_h+0x4e)[0x7fa38cea234e]
[VM:09943] [ 6] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x187)[0x7fa38f670417]
[VM:09943] [ 7] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE24solveSegregatedOrCoupledERKNS_10dictionaryE+0x3a5)[0x7fa38f1bc215]
[VM:09943] [ 8] /home/administrator/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam6fvMesh5solveERNS_8fvMatrixIdEERKNS_10dictionaryE+0x23)[0x7fa38f15fff3]
[VM:09943] [ 9] chtMultiRegionFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xe0)[0x55e82c06c0f0]
[VM:09943] [10] chtMultiRegionFoam(+0x50da0)[0x55e82c039da0]
[VM:09943] [11] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xe7)[0x7fa38ba5cb97]
[VM:09943] [12] chtMultiRegionFoam(+0x5588a)[0x55e82c03e88a]
[VM:09943] *** End of error message ***

Back to my problem, I checked the velocity over the interface and it returned a value of 0! But the contours are clearly showing non-zero values. Is this a post-processing issue (don't tell me it was a dumb mistake after all! )

[Bloerb]

This is a bug in paraView. ParaView is not able to display the values at the boundary from the boundary condition. This is because it is a mixed boundary condition, which paraView does not display correctly. Hence it extrapolates those values. Nevertheless the profile should be correct. It should only be the value at the face itself which is not zero. You can see that this is the case if you load the face itself.

After opening the case with paraFoam -builtin check the walls under mesh regions and not just the internalMesh. You should see a zero velocity

[mm66]

Originally Posted by Bloerb

This is a bug in paraView. ParaView is not able to display the values at the boundary from the boundary condition. This is because it is a mixed boundary condition, which paraView does not display correctly. Hence it extrapolates those values. Nevertheless the profile should be correct. It should only be the value at the face itself which is not zero. You can see that this is the case if you load the face itself.

After opening the case with paraFoam -builtin check the walls under mesh regions and not just the internalMesh. You should see a zero velocity

Thank you very much for your reply. I thought that the visualization problem would be rectified altogether if the code

paraFoam -builtin

is used (but seems that I was wrong). Yes, I did as you mentioned and observed the velocity over the interface (thanks ). However, I faced another issue which is quite puzzling to me:
I used the following commands to get the heat flux over the shared interface:

chtMultiRegionSimpleFoam -postProcess -func wallHeatFlux -region one -latestTime
chtMultiRegionSimpleFoam -postProcess -func wallHeatFlux -region two -latestTime

However, I obtained different values for different regions. For region one:

wallHeatFlux wallHeatFlux write:
    writing field wallHeatFlux
    min/max/integ(wall) = 0, 0, 0
    min/max/integ(one_to_two) = 971.472, 2360.53, 950.336

While for region two:

wallHeatFlux wallHeatFlux write:
    writing field wallHeatFlux
    min/max/integ(wall) = 0, 0, 0
    min/max/integ(two_to_one) = 122167, 436310, 118863

Is this correct? Shouldn't the heat flux remain constant as there is no heat generation in this simulation?

[Bloerb]

It seems that there is a heat flow between the regions. The numbers for two_to_one one_to_two should be identical (are you using a radiation model?).

That they are not zero and not identical can results from a few things

• Your simulation is not sufficiently converged
• you are using a low relaxation factor for h or e which significantly increases convergence time. 0.99 or 1.0 are preferred if possible.
• Your meshes are not identical at the interface. In other words the two_to_one and one_to_two faces are not identical in paraview. This increases the mapping loss.

even without heat sources your flow can heat up due to density changes, kinetic energy changes etc

Check your temperature field. And evaluate if this is a significant value for your simulation. Maybe 118863W are basically zero for your case.