[Owais Shabbir]

Dear all,



I want to apply a boundary condition on a wall so it duplicate the following behaviour from ANSYS:


>Thermal resistance:
The wall of solid.stl is covered by a plastic foil with a thickness
of 0.13 mm and a thermal conductivity (k) of 0.19 W/(m K). So it can a thermal conductivity (k) of 0.19 W/(m K). This gives a thermal resistance between wall and air of 0.00068 m 2 K/W in a simulation



Is there a way to introduce this?

I have checked the externalHeatFluxWallTemperature but that seems to be applicable in MultiRegion simulations.
Thanks

[Bloerb]

    
{
        type            externalWallHeatFluxTemperature;

        // option 1
        mode             coefficient;     // ambient temp. and htc
        Ta               constant 300.0;
        h                uniform 10.0;

        // option 2
        mode             power; 
        Q                10;              // [10W]

        // option 3
        mode             flux;
        q                   uniform 10.0; // [10W/m²]

        thicknessLayers (0.1 0.2 0.3 0.4);
        kappaLayers     (1 2 3 4);

        value           $internalField;
    }

Gives you 4 layers of thickness 0.1 0.2 0.3 and 0.4m with a thermal conductivity of 1 2 3 and 4 W/mK. This boundary condition is applicable to your solver. Or use the cht solver with Bousinesq thermal model as that is equivalent to your solver. The cht solver can solve only 1 region. The Bousinesq approximation was however only introduced in recent versions to the cht solver. I think OF 5 or 6 / 1712 onwards maybe.

[Owais Shabbir]

Dear Bloerb,

Thanks a lot for this BC. I'm using OFv5.



I have already developed a chtMultiRegionSimpleFoam model as well. But as you know the heat source is only possible to add through fvOptions. I wanted to use this BC but the boundary patch for my solid.stl is overridden by solid_to_fluid patches. Therefore, I couldn't use this BC for my solid in cht and had to move to buoyantBousinessqSimpleFoam.


Secondly, you mention cht solver with boussinessq model? could you throw some more lights on it. Do I have to change the solver settings and introduce new equations? Because my knowledge with that is null. In my case I have two solids (one of them is generating heat) in the fluid region. Expectedly, I know the delta T_air is less than 20K.



and what do you mean by "The cht solver can solve only 1 region".

[Bloerb]

thermoType
{
    type                ...;
    mixture             ...;
    transport           ...;
    thermo              ...;
    equationOfState     Boussinesq;
    specie              ...;
    energy              ...;
}

In your thermophysicalProperties file you can select the Bousinesq approximation for equationOfState. Again, not sure if this was introduced in OF5 or later.

The CHT solver is basically BuoyantBousinesqSimpleFoam / BuoyantSimpleFoam. The only difference is that you have to move all the settings you'd make in that solver into subfolders. You then have to specify all the regions in regionProperties. Do not add a solid region if you do not need it and it should behave (nearly) identical.

regions
(
    fluid       (fluidRegionA)
    solid       ()
);

Regions are only coupled via the coupling boundary condition "turbulentTemperatureCoupledBaffleMixed" (or in rare cases an fvOption). If you do not use this boundary condition you can solve 5 different or identical cases at once, since there is zero connection between them. You could even simple copy the same mesh inside another region folder and run the case with a different flow rate boundary condition. The only thing coupling those regions is the boundary condition.

solid_to_fluid patches are created automatically if the mesh is split into different regions using splitMeshRegions. Inside the polyMesh/boundary files you'll find that those patches are of type mappedWall. Replace that by wall and they are uncoupled. You obviously can't use the coupling BC turbulentTemperatureCoupledBaffleMixed on them anymore, but you could use externalWallHeatFluxTemperature. Or simply use the mesh from your BuoyantBousinesqSimpleFoam case

[Owais Shabbir]

Hi Bloerb,


I have searched and this link states that there is the option of boussinesq model for of5.


https://cfd.direct/openfoam/user-gui...35-2640007.1.5


I want to try this model on my old CHT where I have 2 solid regions in a fluid domain before I can implement single region.


Now with this said, I just need to change the entry in thermophysicalProperties of air and introduce 'transportProperties' in addition in my CHT case setup. Or do I need to make any other changes?



Thanks

[Bloerb]

Yes, excactly. You don't need to create a transportProperties file, but OpenFOAM will ask you define the missing parameter inside thermophysicalProperties.

[Owais Shabbir]

Hi Bloerb,



I am slightly confused regarding the validity of this model in my case setup.

I read at different places that this B. approx is valid if delta_T is 15K but this is even valid if my inlet_air is at 348K and the expected heat increases is 20K at maximum?



T_inlet=348K T_outlet=368K (max limit)
pressure drop is 30Pa but i have to run same setup with 200Pa and 300Pa as well.


Secondly, in transportProperties, do I have to chose Tref = 348K or 296K ? or it doesn't matter?.

Thanks