[SeMar]

Hey guys,

I've been using chtMultiRegionSimpleFoam for conjugate heat transfer problems in heat exchangers for a while now. Lately I checked the energybalance of of the system and noticed, that fluid1 does not heat up in the same manner, that fluid2 cools down.

Q_1=phi1*cp1*(T_1out-T_1in)
Q_2=phi2*cp2*(T_2out-T_2in)

Q_1=-Q_2

At first I thought, that maybe the BC was not set properly and set up a simple test case (image1).
testcase-setup.png
The case contains 2 Regions (1*solid, 1*fluid). The volumefraction (solid/fluid) is 1/99. There is no gravity and velocity in the fluid phase is set 0. Initial temperature of region solid and fluid is 400K and 300K. Boundary temperature is set zeroGradient. Further Details can be found in the Zipfile. At the end of the simulation there should be a homogenious temperature in the system. testcase-chtMultiRegionSimpleFoam.zip

The first result was, that the adiabate mixing temperature of the system was nowere near my expected value. I played with the parameters of thermophysicalProperties in fluid and solid region and found out that density does not have an influence on the results (even thoung it should have) but suprisingly changing the viscousity does. Also changing the number of cells did not result in a different temperature, so boundary effects can be excluded.

I did search in the source files but could noch find out, where Cp or other thermophysical values are used for calculations e.g. enthalpy.

Maybe someone here can help me, or give me a hint?

[skuznet]

Hello!

I'm trying to solve a steady-state conjugate heat transfer in a simple heat exchanger, using chtMultiRegionSimpleFoam.
And I think I have some problems with my thermodynamical model. When I run my case with air - it looks ok, but when I try to replace air with water - the results do no look correct. There is no temperature change inside water domain, there are some problems with definition of water properties or setting the case to run with properties.

I wonder in you were able to solve your problem? Can you please help me to set up thermodynamical properties of water instead of air?

Thank you!

Sergey

[SeMar]

Hello Sergey,

so far I found out, that my testcase is not appropriate for a STEADYstate solver, because it is actually the opposite of a steady state. Second thing is, that heat transfer varyies with viscousity, because thermal conductivity is calculated from Pr-Number and viscosity. For the PISO solver I found out, that there is a "bug" in the algorithm. The wall-temperature is updated for each domain in the timeloop, resulting in a loss in heat. but I guess these things have nothing to do with your problem.
Can you be more specific on your thermophysicalProperties file? Which entries did you change from the original "air-file" of the "multiRegionHeater"-case? In my opinion you should change the following:

-> equationOfState rhoConst;
-> Cp 3569;
-> mu 8.91e-4;
-> Pr 7.3;
-> EquationOfState
    {
            rho 1027;
    }

Since your temperature doesn't change at all, maybe you should also check your BCs for the mappedWalls. Let me know when you make progress.

Best regards

Sebastian

[skuznet]

Hi Sebastian!

Thanks for your reply.

I used thermophysicalProperties from example for transient solver chtMultiRegionFoam
/tutorial/heatTransfer/chtMultiRegionFoam/mutiRegionLiquidHeater/constant/bottomWater/thermophysicalProperties:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

mixture
{
    specie
    {
        nMoles          1;
        molWeight       18;
    }
    equationOfState
    {
        rho             1000;
    }
    thermodynamics
    {
        Cp              4181;
        Hf              0;
    }
    transport
    {
        mu              959e-6;
        Pr              6.62;
    }
}

I also changed

myCase/system/fluidDomain/fvSolution

SIMPLE
{
    momentumPredictor on;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       100000;
    rhoMin          rhoMin [1 -3 0 0 0] 0.2;
    rhoMax          rhoMax [1 -3 0 0 0] 2;
}

to

SIMPLE
{
    momentumPredictor on;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       100000;
    rhoMin          rhoMin [1 -3 0 0 0] 999;
    rhoMax          rhoMax [1 -3 0 0 0] 1001;
}

But it doesn't work properly with chtMultiRegionSimpleFoam.
There is no heat conduction inside fluid region when I use water properties as show above. The temperature in fluid domain remains constant.
I think it might be due to inconsistency: i'm using constant density thermophysical model with compressible solver.


I don't think it is due to boundary conditions, because when i use air instead of water I get solution which looks at least qualitatively correct.


Sergey

[skuznet]

Sebastian,

Do you have a working example chtMultiRegionSimpleFoam with water or any other fluid, not gas?
I really stack with this case.

Sergey

[SeMar]

Hello Sergey,

from what your config files look like, there is nothing wrong with your thermophysicalProperties or fvSolution. If you just change these properties in the tutorial case of "multiRegionHeater" it should work. In my opinion there is something wrong with your boundary condition. Are you shure the all heat transfering (domain1_to_domain2) walls are mappedWall and you set up the temperature boundary condition right?

The boundary configuration in case/constant/region/polyMesh/boundary should look similar to that:

domain1_to_domain2
{
      type       mappedWall;
      nFaces    500;
      startFace 123456;
      sampleMode  nearestPatchFace;
      sampleRegion domain2;
      samplePatch  domain2_to_domain1;
      offsetMode    uniform;
      offset           (0 0 0);
}

The respecting T file in case/0/region/T should contain the entry:

domain1_to_domain2
{
    type       compressible::turbulentTemperatureCoupledBaffleMixed;
    neighbourFieldName   T;
    kappa     fluidThermo;
    kappaName     none;
    value      uniform 350;
}

[skuznet]

Sebastian,

I do have these entries:

/fin/constant/solidDomain/polyMesh/boundary:
solidDomain_to_fluidDomain
{
type mappedWall;
nFaces 1760;
startFace 25648;
sampleMode nearestPatchFace;
sampleRegion fluidDomain;
samplePatch fluidDomain_to_solidDomain;
offsetMode uniform;
offset (0 0 0);
}

/fin/constant/fluidDomain/polyMesh/boundary:
fluidDomain_to_solidDomain
{
type mappedWall;
nFaces 1760;
startFace 22592;
sampleMode nearestPatchFace;
sampleRegion solidDomain;
samplePatch solidDomain_to_fluidDomain;
offsetMode uniform;
offset (0 0 0);
}

/fin/0/fluidDomain/T:
fluidDomain_to_solidDomain
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 300;
neighbourFieldName T;
kappa fluidThermo;
kappaName none;
}

/fin/0/solidDomain/T:
solidDomain_to_fluidDomain
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 300;
neighbourFieldName T;
kappa solidThermo;
kappaName none;
}


Moreover, the case seems to run OK if I use water properties.