[Adam_K]

I've been having an issue with multiPhase heat transfer in solid (see this thread) and now I'm wondering if it's an issue with the version of OpenFOAM.


In the v5 user guide it says:

chtMultiRegionFoam

Transient solver for buoyant, turbulent fluid flow and solid heat conduction with conjugate heat transfer between solid and fluid regions.

While in the v6 user guide it says :

chtMultiRegionFoam

Solver for steady or transient fluid flow and solid heat conduction, with conjugate heat transfer between regions, buoyancy effects, turbulence, reactions and radiation modelling.

Based on the wording, I'm left to wonder if they mean that v5 can only handle heat transfer between solid AND fluid regions, but not between two solid regions.

Does this mean that I need to be using OpenFOAM v6 in order to look at heat transfer across solid-solid interfaces (with and without thermal resistances)?

[Robin.Kamenicky]

Hi Adam,

I have had a quick look at the solvers. I think that both of them are capable to deal with solid-solid interface. multiRegionHeater tutorial in of-5 calculates solid-solid interface.

I have checked a bit the codes. I have not noticed any crucial difference for solid-solid interface.

In my opinion, the type of the interface is only dealt by BC. Which do you use? I have not had a look at your case setup.

Kind regards,
Robin

[Adam_K]

Originally Posted by Robin.Kamenicky

Hi Adam,

I have had a quick look at the solvers. I think that both of them are capable to deal with solid-solid interface. multiRegionHeater tutorial in of-5 calculates solid-solid interface.

I have checked a bit the codes. I have not noticed any crucial difference for solid-solid interface.

In my opinion, the type of the interface is only dealt by BC. Which do you use? I have not had a look at your case setup.

Kind regards,
Robin

Thanks for taking a look at the solvers. I was looking at them as well, but am not sure that I'd be able to really identify the differences.

I have been following the multiRegionHeater tutorial to see how to set up my case. I have defined in 0/matrix/T

boundaryField
{
    matrix_to_fibres
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
        kappaMethod     solidThermo;
    }
...
}

0/fibres/T includes

boundaryField
{
    fibres_to_matrix
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
        kappaMethod     solidThermo;
    }
...
}

The code runs, it just seems as if there's barely any exchange between the two phases. For example inclusions of the same thermal diffusivity leads to an overall temperature response (as measured by the increase in temperature at the center of the slab) much slower than expected, 5% of a material with K = 30 mixed into a matrix of K = 300 should not respond as if the K were somewhere around 3.

If I add the following lines, I get an exchange between the two phases. However, they do not tend towards a reasonable limiting case, I describe a few of my results in this thread.

        thicknessLayers	(1e-2);
        kappaLayers	    (1);

[Robin.Kamenicky]

Hi Adam,

I have answered you in the other thread.

It is good to notice that the BC just evaluates the temperature for given region.
If you define layer thickness then it uses:

contactRes = thicknessLayers/kappaLayers
contactRes = 1.0/contactRes
nbrKDelta = contactRes

if you do not use it

nbrKDelta = kappa_nbrField*distance_cells_on_both_sides

Then the code is common for both cases. It calculates

valueFracion = nbrKDelta/(nbrKDelta+myKDelta)

Then it just estimate temperature based on the valueFraction.

I have a few ideas, what could be the problem but I need the log file or possibly try to run it myself. Hope this helps somehow.

Kind regards,
Robin