[Phil910]

Dear all,

i'm facing a weird problem simulating a channel flow with chtMultiRegionFoam in openFoam 8. Some information about my Setup:

Purpose of my Simulation:

I want to simulate a multi region channel flow and compare the wall temperature values to experimental values. In my case i have an upper wall and a lower wall which are heated with a constant heat flux from the outside. Between the two walls is a turbulent air flow with a velocity of approx. 15 m/s, i want to do a LES for the fluid part. The dimensions of my channel are 0.3 x 0.03 x 0.07 m and the Reynolds number is somewhere around 10000.
After the wall temperature is in a relatively steady state i want to compare the wall temperature values with experimental values.
As the wall temperature will converge very slowly if i am doing a cht simulation with a small timestep, but the solid region could possibly be simulated with a much higher time step my plan is to do the following:
Solve only the energy equation in fluid and solid region with the option frozenFlow = true in PIMPLE settings in fvSolution and use a large timestep (1E-02) for around 300 s. After that a normal conjugate heat transfer simulation with flowing fluid for around 0.1 s (approx. 5 through flow times) with a very small timestep (1E-05) to achieve a CFL number of around 0.3 (max). Repeat these two steps until wall temperature "converges".

My Setup:

For my simulationg i am using the chtMultiRegionFoam solver with a Mesh consisting of three regions: Upper Wall, Lower Wall and Fluid. For upper and lower wall the initial temperature is 300 K and on the outer surface i am using externalWallHeatFluxTemperature BC. The Temperature Boundary and Initial Conditions for both walls are defined as follows:

dimensions      [ 0 0 0 1 0 0 0 ];

internalField   uniform 300;

boundaryField
{
    lowerHeater
    {
        type            externalWallHeatFluxTemperature;
        value           uniform 600;
        mode            flux;
        q               uniform 20000;
    }
    lowerWallSides
    {
        type            zeroGradient;
        value           $internalField;
    }
    lowerWall_to_fluid
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
    }
}

Lower heater is the patch in the outside of the domain which is not directly on the fluid region. The BC for the upper wall is analogous with a heater on the upper side.
The fluid BC for temperature is the following:

dimensions      [ 0 0 0 1 0 0 0 ];

internalField   uniform 300;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 300;
    }
    outlet
    {
        type            inletOutlet;
        value           300;
        inletValue      300;
    }
    front
    {
        type            zeroGradient;
        value           uniform 300;
    }
    back
    {
        type            zeroGradient;
        value           uniform 300;
    }
    fluid_to_lowerWall
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
    }
    fluid_to_upperWall
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
    }
}

I am using Smagorinsky model for subgrid stress modeling.The fvSchemes for the fluid region looks the following:

ddtSchemes
{
    default         CrankNicolson 0.9;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linear;
    div(phi,e)      Gauss limitedLinear 1;
    div(phi,K)      Gauss linear;
    div(phiv,p)     Gauss linear;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,B)      Gauss limitedLinear 1;
    div(phi,muTilda) Gauss limitedLinear 1;
    div(B)          Gauss linear;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

My Problem:

As soon as i start the simulation with frozen fluid there is one region in the internal field where the fluid temperature rises quickly to >1000 K after a few ms.
This hot region of fluid can be seen in the attached image.
The first layer of cells at the outlet is at >1000 K while the rest of the fluid remains at around 300 K. When i set the fluid outlet to inletOutlet the outlet temperature is also at the same level, when is use fixedValue with 300 K as an outlet BC the outlet remains at 300 K while the first cell layer at the outlet raises to the same level again. So the boundary condition seems to not influence this weird behaviour. Changing the div(phi, e) scheme to Gauss linear makes the temperature rise even faster which results in an "out of temperature range" warning and eventually make the solver crash. Using Gauss limitedLinear 1; for div(phi, e) results in the image i uploaded here.
Another weird aspect about this is that when i switch the internal velocity field from "uniform (15 0 0)" to "uniform (-15 0 0)" the region of high temperature arises at the inlet, even though the frozenFlow option is active and the fluid in fact is at rest in my simulation.
The temperature is the only variable showing this strange behaviour, pressure and velocity are the way they should be. The temperature in the walls is also not showing any strange behaviour.

Has anyone ever experienced something similar when using chtMultiRegionFoam or has an idea how to deal with this problem? I would be super thankful for any help or recommendation as i am trying to solve this particular problem for more than a week now.

Best regards,
Philipp

[Phil910]

Trying to find the source of the error i modified my case in a way that i am left with only a fluid region (so i basically removed the solid walls to check if something in these regions is causing my problem). I am now still solving the fluid region with the frozenFlow = true option and the chtMultiRegionFoam solver. For only the fluid region the problem still persists. Switching the internal velocity field to uniform (0 0 0) will give me the temperature rise at the inlet instead of the outlet and it will spread into the fluid domain as it can be seen in the attached image (t=3 s).

What i also tried:
- Experimenting with different temperature boundary conditions at inlet and outlet
- Switching the flow to laminar instead of LES (even though it is still frozen and this shouldn't make a difference)
- Experimenting with the numerical schemes in fvSchemes

None of the above seemed to make any difference...
I also can not find any heat source in my setup that could possibly cause such a temperature rise (at this point there is no heat source left in my setup at all).

Does anyone have any idea what could cause this behaviour?

[lonewanderer]

hi i don't know completely about your case
I think the possible things you can check are

1. did you try the frozen flow option = false. ?
2. Please perform steady state simulation first. Once the model is working you can perform transient
3. Please also check for thermal conductivity in material properties.
4. Instead of taking 'externalWallHeatFluxTemperature;' for solid's temperature while defining flux in 0 folder did you use this in fvOptions in constant folder solids file
{
energySource
{
type scalarSemiImplicitSource;

timeStart 0;
duration 10e6;
selectionMode all;
volumeMode specific;

injectionRateSuSp
{
h (2.230555e+10 0); // W/m^3 == kg/m/s^3
}
}
}
Note: if you are defining flux in fvOptions, please make changes in Temperature file lowerHeater 'externalWallHeatFluxTemperature;' to 'zeroGradient' bc

Hope these help you

[Bloerb]

frozenFlow requires a well solved initial velocity/pressure field and alphat should be initialized as well for turbulent flow...you are adding a heat flux of 20000 which to me seems pretty high...so high temperatures shouldn't be surprising. Keep in mind this is flux so... 20kW/m²


You solved only the fluid domain and get a temperature increase that's crazy? Where is the heat entering the fluid domain...externalWallHeatFlux directly on the fluid wall? Or have you removed all heat sources and still get weird temperatures?


"Another weird aspect about this is that when i switch the internal velocity field from "uniform (15 0 0)" to "uniform (-15 0 0)" the region of high temperature arises at the inlet, even though the frozenFlow option is active and the fluid in fact is at rest in my simulation."


That is not weird....you are solving with that velocity field...so 15 m/s or -15m/s in x. This is loaded for every cell and is unchanged.


The first thing I'd do is reduce the schemes to upwind and do a test run...


what is your Diffusion and Co number when solving with the frozenFlow time step? You can get away with crazy Co numbers but you should atleast keep an eye on the Diffusion number. You should however use backward time stepping. What are the residuals? Is the enthalpy residual dropping?


Please post your U boundary conditions!