[Shibi]

Hello to all,


I would like to have an opinion on a case I am assembling with chtMultiRegionSimpleFoam.
I want to simulate the temperature distribution of a container [box] having a sphere inside it which produces a constant heat flux of 120 w/m². The container and sphere are surrounded by air without any initial imposed velocity.


The mesh was generated with snappyHexMesh to define the air, box and sphere regions. Afterwards, I separate the region with slitMeshRegions, and get the patches for the interface regions [sphere_to_air and air_to_sphere].



I would like to know how to set a constant heat flux on the sphere.


Right now I that the following in T field for the sphere

internalField   uniform 300;

boundaryField
{
    sphere_to_air
    {
        type            fixedGradient;
        gradient    uniform 120;
    }
}

And the same for the T field on the Air folder

    walls
    {
        type            zeroGradient;
    }
    air_to_box
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           $internalField;
        Tnbr            T;
        kappaMethod     fluidThermo;
    }
    air_to_sphere
    {
        type            fixedGradient;
        gradient    uniform 120;
    }

Is this a correct way for setting a uniform heat flux out of the sphere?

[crubio.abujas]

Originally Posted by Shibi

Hello to all,
I would like to have an opinion on a case I am assembling with chtMultiRegionSimpleFoam.
I want to simulate the temperature distribution of a container [box] having a sphere inside it which produces a constant heat flux of 120 w/m². The container and sphere are surrounded by air without any initial imposed velocity.

Using fixedGradient what you're applying a value to dT/dx, which have units of [K/m], so is not a heatFlux. Check if in your OF version is available a type externalWallHeatFluxTemperature. The usage for your specifications shall be as follows:

internalField   uniform 300;

boundaryField
{
    sphere_to_air
    {
        type            externalWallHeatFluxTemperature;
        mode          flux;
       q                  uniform 120;     // Heat Flux [W/m2]
       value           $internalField;

     }
}

Notice that it would only apply to the shell of the sphere. If you have a volumetric heat inside and you want to model it you may want to check a fvOption to add a source.

Hope it helps!

[Shibi]

Hello,

Thank you very much for the clarification regarding the boundary!


I think it can be modeled like that (heat flow on the shell of the sphere) since I have no interest in the temperature distribution inside the sphere.

However, I would like to have clarified if the definition of the same boundary on the interface patches is Ok.

So, for me to define to constant heat flux, the same boundary must be applied to both interface patches, like:

boundaryField
{
    sphere_to_air
    {
        type            externalWallHeatFluxTemperature;
         mode          flux;
        q                  uniform 120;     // Heat Flux [W/m2]
       kappaMethod    solidThermo;

        value           $internalField;

     }
}

and

boundaryField
{
   air_to_ sphere
    {
        type            externalWallHeatFluxTemperature;
        mode          flux;
        q                  uniform 120;     // Heat Flux [W/m2] 

      kappaMethod    fluidThermo;

        value           $internalField;

     }
}

Thanks for the help!

[crubio.abujas]

Hi again Shibi,

I don't think that the simulation would crash if you use the boundary as stated in your previous post, the thing is that the sphere region and the air region will be totally independent simulations, so why to model the sphere in the first place? You can just drop the sphere from the simulation and model the air with an externalWallHeatFluxTemperature condition in the sphere interface.

If you want to include the sphere region inside the model shall be because the temperature distribution on the sphere region is important and you want to solve its interaction with the rest of regions. Otherwise the best approach is to drop this geometry. It saves computation power, saves space and saves time.

I do not know the nature of the problem you want to solve, but I can assume it has to be related on two possible option: rather there is an spherical shell surrounding some kind of heat source, in which case the shell is a thermal resistance; or the spherical body is the heat source itself.

For the first case, if you're not interested in the temperature of the shell itself you can still use the externalWallHeatFluxTemperature model of boundary and add a thickness property to model the thermal resistance. If you are interested in the distribution though, the interface between regions shall be of the type compressible::turbulentTemperatureCoupledBaffleMix ed, and it is in internal boundary of the spherical shell where you can apply the externalWallHeatFluxTemperature.

For the second case, you just model all the interfaces using compressible::turbulentTemperatureCoupledBaffleMix ed and apply a volumetric source of heat using an fvOption. Check the tutorial heatDuct to see how to apply this source.

I hope it helps to clarify the different approaches you have.

[Shibi]

Originally Posted by crubio.abujas

Hi again Shibi,

I don't think that the simulation would crash if you use the boundary as stated in your previous post, the thing is that the sphere region and the air region will be totally independent simulations, so why to model the sphere in the first place? You can just drop the sphere from the simulation and model the air with an externalWallHeatFluxTemperature condition in the sphere interface.

If you want to include the sphere region inside the model shall be because the temperature distribution on the sphere region is important and you want to solve its interaction with the rest of regions. Otherwise the best approach is to drop this geometry. It saves computation power, saves space and saves time.

I do not know the nature of the problem you want to solve, but I can assume it has to be related on two possible option: rather there is an spherical shell surrounding some kind of heat source, in which case the shell is a thermal resistance; or the spherical body is the heat source itself.

For the first case, if you're not interested in the temperature of the shell itself you can still use the externalWallHeatFluxTemperature model of boundary and add a thickness property to model the thermal resistance. If you are interested in the distribution though, the interface between regions shall be of the type compressible::turbulentTemperatureCoupledBaffleMix ed, and it is in internal boundary of the spherical shell where you can apply the externalWallHeatFluxTemperature.

For the second case, you just model all the interfaces using compressible::turbulentTemperatureCoupledBaffleMix ed and apply a volumetric source of heat using an fvOption. Check the tutorial heatDuct to see how to apply this source.

I hope it helps to clarify the different approaches you have.

In OpenFOAM v1912 I do not have that tutorial. Can you supply it?


Thanks!

[crubio.abujas]

Originally Posted by Shibi

In OpenFOAM v1912 I do not have that tutorial. Can you supply it?

Thanks!

Sure! Try this link:
https://drive.google.com/file/d/1VFh...ew?usp=sharing

However, for sure that in OF v1912 there are other tutorials in chrMultiRegionFoam using the same boundaries.

Good luck and happy foaming!