CFD Online Discussion Forums - Problem with boundary conditions (heatTransfer)

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Problem with boundary conditions (heatTransfer) (https://www.cfd-online.com/Forums/openfoam-solving/144842-problem-boundary-conditions-heattransfer.html)

Problem with boundary conditions (heatTransfer)

Hi there,

i'm new at this forum and also realtively new to OpenFoam.

So here is my Problem:
I want to solve a HeatTransfer problem, i want to examine the cooling of a cylinder in a wind tunnel.

I have a .stl file of the cylinder and my wind tunnel is a hexagon made in the blockMeshdict. I used snappyHexMesh for the .stl file.

Now i have the boundaries of the wind tunnel with the walls and the inlet and outlet as well as the boundaries windtunnel_to_cylinder and cylinder_to_windtunnel.

First of all i only want to look at the cooling, without any turbulence models, so i set the turbulence to off. My Problem now is by using the chtMultiRegionFoam solver, that the temperature of the cylinder isn't changing.

I think, that i don't set the boundary conditions for the temperature right. So here are the initial value files for the temperature of the wind tunnel and the cylinder.

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 

//Cylinder



dimensions      [ 0 0 0 1 0 0 0 ];



internalField   uniform 500;



boundaryField

{

    cylinder_to_windtunnel

    {

        type            fixedValue;

        value           uniform 500;

    }

}





// ************************************************************************* //

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 

//Windtunnel



dimensions      [ 0 0 0 1 0 0 0 ];



internalField   uniform 300;



boundaryField

{

    "(inlet|upperWall|lowerWall|frontWall|backWall)"

    {

        type        fixedValue;

        value        uniform 300;

    }



    windtunnel_to_cylinder

    {

        type            fixedValue;

        value           uniform 300;

    }



    outlet

    {

        type            zeroGradient:

    }

}





// ************************************************************************* //

Thanks for help!

greetings
Wirman

Hi,
you should make a sketch of your setup where you show all boundaries with their names. What means windtunnel_to_cylinder and cylinder_to_windtunnel?

So there is a cylinder inside your wind tunnel, and cool air flows around that cylinder? Do you resolve the solid body (cylinder) with a mesh and solve for heat conduction in the solid?

From what I can guess with the few information: Yes, your boundary conditions seem to be wrong. You have two general possibilities: 1) Fix the temperature at the surface. This means that the simulation can not change the temperature because it is a boundary condition for all time. Even with the highest cooling it will not change. This is what I think what happens here, because your cylinder seems to have a fixed temperature boundary condition. But: The heat flux inside / outside the cylinder can change. This is the temperature gradient at the surface.
2) Fix the gradient of the temperature. If you set the heat flux to zero that means, that your body will heat (or cool) until it gets the temperature of the surrounding fluid.

Hi,

thanks for your response. Sorry for being a bit vague, so here are some explanations. As an attachement i made a little image of my model in 2D, front and back Walls are the 3D-case and the cylinder doesn't touches the front and the back wall (so it is complete in the wind tunnel, without touching any walls)

In the .stl file of the cylinder i have only one region, named cylinder_to_windtunnel (so the points in the .stl file are all boundary points of the cylinder) - i think it could be a problem that there are no inner nodes?!? -

this .stl file will be meshed with snappyHexMesh out of the blockMesh from the wind tunnel. I made the same with the wind tunnel to set up the wind tunnel without the cylinder. So i have the following boundaries in the polyMesh folders of Windtunnel and Cylinder:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// boundary Windtunnel

7

(

    inlet

    {

        type            patch;

        nFaces          100;

        startFace       207208;

    }

    outlet

    {

        type            patch;

        nFaces          100;

        startFace       207308;

    }

    lowerWall

    {

        type            wall;

        inGroups        1(wall);

        nFaces          200;

        startFace       207408;

    }

    upperWall

    {

        type            wall;

        inGroups        1(wall);

        nFaces          200;

        startFace       207608;

    }

    frontWall

    {

        type            wall;

        inGroups        1(wall);

        nFaces          224;

        startFace       207808;

    }

    backWall

    {

        type            wall;

        inGroups        1(wall);

        nFaces          224;

        startFace       208032;

    }

    windtunnel_to_cylinder

    {

        type            wall;

        inGroups        1(wall);

        nFaces          15625;

        startFace       208256;

        sampleMode      nearestPatchFace;

            sampleRegion   cylinder;

            samplePatch     cylinder_to_windtunnel;

    }

)



// ************************************************************************* //

and

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// boundary cylinder

1

(



    cylinder_to_windtunnel

    {

        type            wall;

        inGroups        1(wall);

        nFaces          15856;

        startFace       63660;

        sampleMode      nearestPatchFace;

            sampleRegion    windtunnel;

            samplePatch     windtunnel_to_cylinder;

    }

)



// ************************************************************************* //

After that i set the boundary conditions like in my first post.
I see the point with the fixed Value, so i tried to change the boundary conditions to fixedGradient. So my new 0/cylinder/T file is the following:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



dimensions      [ 0 0 0 1 0 0 0 ];



internalField   uniform 500;



boundaryField

{

    cylinder_to_windtunnel

    {

        type            fixedGradient;

        gradient                        uniform 0;

    }

}





// ************************************************************************* //

But that changes unfortunately nothing.

So here is a snapshot what chtMultiRegionFoam does:

Code:

Solving for fluid region windtunnel

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 0.1691079, Final residual = 7.164976e-08, No Iterations 28

DILUPBiCG:  Solving for Uy, Initial residual = 0.1495004, Final residual = 5.141199e-08, No Iterations 28

DILUPBiCG:  Solving for Uz, Initial residual = 0.1496348, Final residual = 1.371065e-08, No Iterations 30

DILUPBiCG:  Solving for h, Initial residual = 0.1502954, Final residual = 5.238185e-08, No Iterations 29

Min/max T:44.85127 776.2719

GAMG:  Solving for p_rgh, Initial residual = 0.06935177, Final residual = 0.0003099182, No Iterations 5

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 7.980175e-05, global = -2.0367e-05, cumulative = -0.0003824869

GAMG:  Solving for p_rgh, Initial residual = 0.06477691, Final residual = 6.725581e-08, No Iterations 14

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 8.454755e-09, global = 2.64765e-09, cumulative = -0.0003824843



Solving for solid region cylinder

DICPCG:  Solving for h, Initial residual = 0.004598652, Final residual = 7.893509e-07, No Iterations 2

Min/max T:min(T) [0 0 0 1 0 0 0] 500 max(T) [0 0 0 1 0 0 0] 500

ExecutionTime = 58.22 s  ClockTime = 60 s



Region: windtunnel Courant Number mean: 0.3687364 max: 8187.881

Region: cylinder Diffusion Number mean: 9.508806e-05 max: 0.0002090919

Time = 0.83

so you can see, that there is no change in the temperature in the solid region (because of the mesh?!?) and this is the last step before chtMultiRegionFoam terminates with an error, because the minimum temperature in the fluidRegion becomes negative in the next timestep.

i hope you have now enough information. Thanks for your effort.

greetings Wirman

I don't know the details of that solver, but the log output sounds like you have the region "windtunnel" where the fluid flows and the region "cylinder" which is solid inside the cylinder. Is that correct?

PS: Wohoooo, this is my 1000th post.

yes that is correct.

i tried something that i found in the planeWall2D case, which is an example for the chtMultiRegionFoam solver.

i set the boundaries windtunnel_to_cylinder and cylinder_to_windtunnel to mappedWall instead of wall and then i used for the 0 files:

Code:

boundaryField

{

    cylinder_to_windtunnel

    {

        type           compressible::turbulentTemperatureCoupledBaffleMixed;

        Tnbr           T;

        kappa         solidThermo;

        kappaName none;

        value          uniform 500;

    }

}

and

Code:

boundaryField

{

    windtunnel_to_cylinder

    {

        type           compressible::turbulentTemperatureCoupledBaffleMixed;

        Tnbr           T;

        kappa         fluidThermo;

        kappaName none;

        value          uniform 300;

    }

}

that results in a change of the temperature at the solid, which is good. But the incredible decrease in temperature at the fluid is still there. After 0.03 seconds the temperature minimum is -97K. Showing the case in paraview, i can't spot the minimum and the maximum of temperature, so i don't know what's going wrong ...

here is the log of chtMultiRegionFoam

Code:

Solving for fluid region windtunnel

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 0.02460263, Final residual = 3.736507e-08, No Iterations 12

DILUPBiCG:  Solving for Uy, Initial residual = 0.03327333, Final residual = 1.240097e-08, No Iterations 14

DILUPBiCG:  Solving for Uz, Initial residual = 0.3112729, Final residual = 8.590666e-08, No Iterations 15

DILUPBiCG:  Solving for h, Initial residual = 0.003709023, Final residual = 9.252748e-08, No Iterations 12

Min/max T:76.66537 499.9691

GAMG:  Solving for p_rgh, Initial residual = 0.6060488, Final residual = 0.004652162, No Iterations 4

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 1.789022e-05, global = 1.050344e-05, cumulative = -0.0001039832

GAMG:  Solving for p_rgh, Initial residual = 0.1844631, Final residual = 4.072585e-08, No Iterations 14

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 2.188366e-10, global = -1.318627e-10, cumulative = -0.0001039833



Solving for solid region cylinder

DICPCG:  Solving for h, Initial residual = 0.3283636, Final residual = 1.500188e-08, No Iterations 4

Min/max T:min(T) [0 0 0 1 0 0 0] 499.6061 max(T) [0 0 0 1 0 0 0] 499.9998

ExecutionTime = 2.91 s  ClockTime = 4 s



Region: windtunnel Courant Number mean: 0.2657095 max: 21.11159

Region: cylinder Diffusion Number mean: 9.508806e-05 max: 0.0002090919

Time = 0.03

PS: Congrats to your 1000th post!

Ok, again: I never used that solver, but you need a coupled boundary condition for this fluid / solid intersection. This sounds familiar and makes sense. Glad it works now.

The other problem sounds like a numerical failure. Some questions:
1) Is this a transient solver?
2) Can you post more than one time step log output?
3) Can you post fvSchemes and fvSolution?

sure i can ;-)

1.) chtMultiRegionFoam is a transient solver, the steady-state version is the chtMultiRegionSimpleFoam.

2. )
Here is the complete log of the solver. Unfortunately it terminates after 3 time steps:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create fluid mesh for region windtunnel for time = 0



Create solid mesh for region cylinder for time = 0



*** Reading fluid mesh thermophysical properties for region windtunnel



    Adding to thermoFluid



Selecting thermodynamics package 

{

    type            heRhoThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState perfectGas;

    specie          specie;

    energy          sensibleEnthalpy;

}



    Adding to rhoFluid



    Adding to UFluid



    Adding to phiFluid



    Adding to gFluid



    Adding turbulence 



Selecting turbulence model type laminar

    Adding to ghFluid



    Adding to ghfFluid



Selecting radiationModel none

    Adding to KFluid



    Adding to dpdtFluid



    Adding fvOptions



No finite volume options present



*** Reading solid mesh thermophysical properties for region cylinder



    Adding to thermos



Selecting thermodynamics package 

{

    type            heSolidThermo;

    mixture         pureMixture;

    transport       constIso;

    thermo          hConst;

    equationOfState rhoConst;

    specie          specie;

    energy          sensibleEnthalpy;

}



    Adding to radiations



Selecting radiationModel none

    Adding fvOptions



No finite volume options present



Region: windtunnel Courant Number mean: 0.1320233 max: 6.178983

Region: cylinder Diffusion Number mean: 4.754403e-05 max: 0.0001045459

Region: windtunnel Courant Number mean: 0.1320233 max: 6.178983

Region: cylinder Diffusion Number mean: 4.754403e-05 max: 0.0001045459

Time = 0.005





Solving for fluid region windtunnel

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 1.70178e-08, No Iterations 10

DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 4.406888e-08, No Iterations 8

DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 7.053572e-08, No Iterations 8

DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 4.709673e-08, No Iterations 13

Min/max T:300 499.9901

GAMG:  Solving for p_rgh, Initial residual = 0.9248417, Final residual = 0.002323891, No Iterations 2

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 4.026599e-05, global = -2.333879e-05, cumulative = -2.333879e-05

GAMG:  Solving for p_rgh, Initial residual = 0.5507993, Final residual = 5.446465e-08, No Iterations 13

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 8.541335e-11, global = 4.909502e-11, cumulative = -2.333874e-05



Solving for solid region cylinder

DICPCG:  Solving for h, Initial residual = 1, Final residual = 1.22016e-07, No Iterations 3

Min/max T:min(T) [0 0 0 1 0 0 0] 499.8234 max(T) [0 0 0 1 0 0 0] 500

ExecutionTime = 1.78 s  ClockTime = 2 s



Region: windtunnel Courant Number mean: 0.1322938 max: 11.29372

Region: cylinder Diffusion Number mean: 4.754403e-05 max: 0.0001045459

Time = 0.01





Solving for fluid region windtunnel

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 0.1074785, Final residual = 1.815122e-08, No Iterations 11

DILUPBiCG:  Solving for Uy, Initial residual = 0.022709, Final residual = 8.128951e-08, No Iterations 8

DILUPBiCG:  Solving for Uz, Initial residual = 0.2808652, Final residual = 1.207978e-08, No Iterations 11

DILUPBiCG:  Solving for h, Initial residual = 0.002674789, Final residual = 1.18252e-08, No Iterations 9

Min/max T:86.33847 499.9713

GAMG:  Solving for p_rgh, Initial residual = 0.2937693, Final residual = 0.001758145, No Iterations 4

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 2.432616e-06, global = 7.712725e-07, cumulative = -2.256746e-05

GAMG:  Solving for p_rgh, Initial residual = 0.1388996, Final residual = 6.941843e-08, No Iterations 13

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (windtunnel): sum local = 8.460298e-11, global = -4.874945e-11, cumulative = -2.256751e-05



Solving for solid region cylinder

DICPCG:  Solving for h, Initial residual = 0.307672, Final residual = 3.77194e-08, No Iterations 3

Min/max T:min(T) [0 0 0 1 0 0 0] 499.6128 max(T) [0 0 0 1 0 0 0] 500.0002

ExecutionTime = 2.76 s  ClockTime = 3 s



Region: windtunnel Courant Number mean: 0.1322697 max: 8.331021

Region: cylinder Diffusion Number mean: 4.754403e-05 max: 0.0001045459

Time = 0.015





Solving for fluid region windtunnel

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 0.02061106, Final residual = 9.475351e-08, No Iterations 12

DILUPBiCG:  Solving for Uy, Initial residual = 0.02154275, Final residual = 5.186294e-08, No Iterations 10

DILUPBiCG:  Solving for Uz, Initial residual = 0.1588295, Final residual = 3.479565e-08, No Iterations 13

DILUPBiCG:  Solving for h, Initial residual = 0.002320682, Final residual = 7.601028e-08, No Iterations 10

Min/max T:-64.83592 499.9816

#0  Foam::error::printStack(Foam::Ostream&) in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#1  Foam::sigFpe::sigHandler(int) in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#2   in "/lib/x86_64-linux-gnu/libc.so.6"

#3  Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"

#7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"

#8  

 in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"

#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"

#10  

 in "/soft/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"

Floating exception

3.) i copied these two from the snappyMultiRegionHeater tutorial

fvSchemes windtunnel

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



ddtSchemes

{

    default Euler;

}



gradSchemes

{

    default         Gauss linear;

}



divSchemes

{

    default         none;



    div(phi,U)      Gauss upwind;

    div(phi,K)      Gauss linear;

    div(phi,h)      Gauss upwind;

    div(phi,k)      Gauss upwind;

    div(phi,epsilon) Gauss upwind;

    div(phi,R)      Gauss upwind;

    div(R)          Gauss linear;

    div((muEff*dev2(T(grad(U))))) Gauss linear;

}



laplacianSchemes

{

    default         Gauss linear corrected;

}



interpolationSchemes

{

    default         linear;

}



snGradSchemes

{

    default         corrected;

}



fluxRequired

{

    default         no;

    p_rgh;

}



// ************************************************************************* //

fvSolution windtunnel:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



solvers

{

    "(rho|rhoFinal)"

    {

        solver          PCG

        preconditioner  DIC;

        tolerance       1e-7;

        relTol          0;

    }



    p_rgh

    {

        solver           GAMG;

        tolerance        1e-7;

        relTol           0.01;



        smoother         GaussSeidel;



        cacheAgglomeration true;

        nCellsInCoarsestLevel 10;

        agglomerator     faceAreaPair;

        mergeLevels      1;

    }



    p_rghFinal

    {

        $p_rgh;

        tolerance        1e-7;

        relTol           0;

    }



    "(U|h|k|epsilon|R)"

    {

        solver           PBiCG;

        preconditioner   DILU;

        tolerance        1e-7;

        relTol           0.1;

    }



    "(U|h|k|epsilon|R)Final"

    {

        $U;

        tolerance        1e-07;

        relTol           0;

    }

}



PIMPLE

{

    momentumPredictor   on;

    nCorrectors         2;

    nNonOrthogonalCorrectors 0;

}



relaxationFactors

{

    fields

    {

    }

    equations

    {

        "h.*"           1;

        "U.*"           1;

    }

}



// ************************************************************************* //

fvSchemes cylinder:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



ddtSchemes

{

    default         Euler;

}



gradSchemes

{

    default         Gauss linear;

}



divSchemes

{

    default         none;

}



laplacianSchemes

{

    default             none;

    laplacian(alpha,h)  Gauss linear corrected;

}



interpolationSchemes

{

    default         linear;

}



snGradSchemes

{

    default         corrected;

}



fluxRequired

{

    default         no;

}



// ************************************************************************* //

fvSolution cylinder:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



solvers

{

    h

    {

        solver           PCG;

        preconditioner   DIC;

        tolerance        1e-06;

        relTol           0.1;

    }



    hFinal

    {

        $h;

        tolerance        1e-06;

        relTol           0;

    }

}



PIMPLE

{

    nNonOrthogonalCorrectors 0;

}



// ************************************************************************* //

Ok, tell me if you don't get me. The fluid solver part is something like PIMPLE. Currently you run PIMPLE in PISO mode, because you did not set nOuterCorrectors to anything higher than "1" (actually, you didn't set it at all, thus I see from your log it is set to "1").
Now, your max. Courant number is much too high for the PISO solver. Normally, this leads to numerical instabilities. I recommend to make the time step 20 times smaller, so the max. Co becomes about "0.5". See what happens.

i think i can follow you, but i haven't dealt with the theory behind the solvers. Are there any manuals of the theory behind e.g. the chtMultiRegionFoam?

To your suggestion:
There is another fvSolution file in the system ordner and there the nOuterCorrectors is set to 1. 1 or lower is PISO Mode, what are other numbers?

When i make the time steps about 100 times smaller the Courant number looks good (<0.5, beetween something about 0.04 at the beginning and 0.3 at the end where it terminates) but it terminates nevertheless at a t about 0.0004.

Moreover the change in temperature in the solid is very small, but that is maybe because of the short time. But the heavily decrease of the temperature in the fluid is still there...

Your "min" value in the fluid should not become less than 300, is that what you say?

Try setting laplacian scheme to "uncorrected". Sometimes this can lead to negative wiggles.

yep, thats what im saying ... there is a fixed temperature of 300 at the inlet and the cylinder has a temperature of 500, so why should the minimum temperature be under 300? Correct me if i overlook something ...

Setting the laplacian schemes to uncorrected doesn't help :(

What does "checkMesh" show you?

checkMesh gives me an FOAM FATAL ERROR:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create polyMesh for time = 0







--> FOAM FATAL ERROR: 

Cannot find file "points" in directory "polyMesh" in times 0 down to constant



    From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&)

    in file db/Time/findInstance.C at line 203.



FOAM exiting

But that makes sense, because i have no polyMesh folder in the constant folder. the polyMesh folder are in the subfolders of windtunnel and cylinder

Code:

-- constant

   -- windtunnel

       -- polyMesh

   -- cylinder

       -- polyMesh

I don't know how to use checkMesh for these kind of meshes, sorry.

any other ideas? i thought it is actually a primitive case, so it can't be that difficult to make the solver run correctly :confused: i really dislike openFoam :mad: maybe im too stupid to use it ...

Don't give up that fast...
You need to spot the points where the temperature goes down in paraview. The numerics seem to be ok, so maybe it's some boundary condition error. Whatever, finding it will probably help.
Edit: And you need to get checkMesh running...

Quote:

Originally Posted by RodriguezFatz (Post 520851)

I don't know how to use checkMesh for these kind of meshes, sorry.

hey, for these multi-region cases, you have to run "checkMesh -region "region_name".

the other thing worth looking into is how you set your thermophysicalProperties for your fluid/solid regions.

okay, so new try:

first of all i got checkMesh running with the region option (thanks to zhengzh5)

it says that the mesh is ok, but i don't know exactly what it does, so here are the log files:

checkMesh cylinder:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create polyMesh cylinder for time = 0



Time = 0



Mesh stats

    points:           33596

    faces:            79516

    internal faces:   63660

    cells:            23292

    faces per cell:   6.147003

    boundary patches: 1

    point zones:      0

    face zones:       0

    cell zones:       0



Overall number of cells of each type:

    hexahedra:     21416

    prisms:        424

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    polyhedra:     1452

    Breakdown of polyhedra by number of faces:

        faces   number of cells

            4   40

            5   344

            6   372

            9   268

           12   212

           15   132

           18   84



Checking topology...

    Boundary definition OK.

    Cell to face addressing OK.

    Point usage OK.

    Upper triangular ordering OK.

    Face vertices OK.

    Number of regions: 1 (OK).



Checking patch topology for multiply connected surfaces...

                   Patch    Faces   Points                  Surface topology

    cylinder_to_windtunnel    15856    16354      ok (closed singly connected)



Checking geometry...

    Overall domain bounding box (-0.124999 0 -0.124315) (0.124999 0.01 0.124315)

    Mesh (non-empty, non-wedge) directions (1 1 1)

    Mesh (non-empty) directions (1 1 1)

    Boundary openness (-2.007952e-18 9.761436e-16 -1.672787e-18) OK.

    Max cell openness = 2.747404e-16 OK.

    Max aspect ratio = 4.733498 OK.

    Minimum face area = 9.65406e-07. Maximum face area = 1.294591e-05.  Face area magnitudes OK.

    Min volume = 8.679143e-10. Max volume = 4.122625e-08.  Total volume = 0.0004866705.  Cell volumes OK.:

    Mesh non-orthogonality Max: 37.56666 average: 7.999011

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 1.115269 OK.

    Coupled point location match (average 0) OK.



Mesh OK.



End

and here the checkMesh for the windtunnel:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create polyMesh windtunnel for time = 0



Time = 0



Mesh stats

    points:           90587

    faces:            223881

    internal faces:   207208

    cells:            66936

    faces per cell:   6.440316

    boundary patches: 7

    point zones:      0

    face zones:       0

    cell zones:       0



Overall number of cells of each type:

    hexahedra:     54757

    prisms:        724

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    polyhedra:     11455

    Breakdown of polyhedra by number of faces:

        faces   number of cells

            5   376

            6   3004

            9   6523

           12   1000

           15   540

           18   12



Checking topology...

    Boundary definition OK.

    Cell to face addressing OK.

    Point usage OK.

    Upper triangular ordering OK.

    Face vertices OK.

    Number of regions: 1 (OK).



Checking patch topology for multiply connected surfaces...

                   Patch    Faces   Points                  Surface topology

                   inlet      100      121  ok (non-closed singly connected)

                  outlet      100      121  ok (non-closed singly connected)

               lowerWall      200      231  ok (non-closed singly connected)

               upperWall      200      231  ok (non-closed singly connected)

               frontWall      224      261  ok (non-closed singly connected)

                backWall      224      261  ok (non-closed singly connected)

    windtunnel_to_cylinder    15625    16119      ok (closed singly connected)



Checking geometry...

    Overall domain bounding box (-0.5 -0.25 -0.25) (0.5 0.25 0.25)

    Mesh (non-empty, non-wedge) directions (1 1 1)

    Mesh (non-empty) directions (1 1 1)

    Boundary openness (3.994897e-17 3.968973e-17 1.058756e-16) OK.

    Max cell openness = 2.883646e-16 OK.

    Max aspect ratio = 3.224365 OK.

    Minimum face area = 1.049937e-06. Maximum face area = 0.002505055.  Face area magnitudes OK.

    Min volume = 1.671137e-09. Max volume = 0.000125249.  Total volume = 0.2495132.  Cell volumes OK.

    Mesh non-orthogonality Max: 41.73929 average: 11.41158

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 1.23016 OK.

    Coupled point location match (average 0) OK.



Mesh OK.



End

and here are the thermophysicalProperties: The properties for air are from the internet, the Properties for the cylinder are properties of a metal, i think steel.

thermophysicalProperties windtunnel (air)

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



thermoType

{

    type            heRhoThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState perfectGas;

    specie          specie;

    energy          sensibleEnthalpy;

}



mixture

{

    specie

    {

        nMoles      1;

        molWeight   28.96;

    }



    transport

    {

                mu                         1.8e-05;

                Pr                        0.7;

    }



    thermodynamics

    {

        Hf      2.544e+06;

        Cp      1004.5;

    }

}



// ************************************************************************* //

thermophysicalProperties cylinder (steel)

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



thermoType

{

    type            heSolidThermo;

    mixture         pureMixture;

    transport       constIso;

    thermo          hConst;

    equationOfState rhoConst;

    specie          specie;

    energy          sensibleEnthalpy;

}



mixture

{

    specie

    {

        nMoles      1;

        molWeight   12;

    }



    transport

    {

        kappa   80;

    }



    thermodynamics

    {

        Hf      0;

        Cp      450;

    }



    equationOfState

    {

        rho     8000;

    }

}



// ************************************************************************* //