[nullicle]

Hi all,

I am currently modelling heat transfer in a house with buoyantPimpleFoam and I am wanting to take variable humidity into account. I cannot seem to find any tutorials or information about other solvers that do this.

Thus, does anyone know of whether a solver like this is available?

Thanks in advance,

Chris

[dlahaye]

Allow radiative heat transfer with absorption coefficient that depends on H2O mass fraction? If yes, see reserveBurner tutorial of bouyantSimpleFoam. Possibly (?) is suffices to with reactions and combustion off.

[nullicle]

Originally Posted by dlahaye

Allow radiative heat transfer with absorption coefficient that depends on H2O mass fraction? If yes, see reserveBurner tutorial of bouyantSimpleFoam. Possibly (?) is suffices to with reactions and combustion off.

Thanks, I found it in the chtMultiRegionFoam and had a glance through the source code (could not find any written explanation as to what this case actually is...)

So it seems I should not find a different solver, rather add the appropriate functionality that replicates the chemical process, namely the interaction with air/water? Is there anywhere that actually explains this tutorial with words, so I can match it to the code? Or interaction with air/water for humidity elsewhere?

Thanks,

Chris

[dlahaye]

No clue on water/air interactions.

Chemical reactions can be added as shown in the reverseBurner tutorial and in the tutorials on the combustion solver (reactingFoam and related).

Apologies for being vague.

[nullicle]

Originally Posted by dlahaye

No clue on water/air interactions.

Chemical reactions can be added as shown in the reverseBurner tutorial and in the tutorials on the combustion solver (reactingFoam and related).

Apologies for being vague.

Thanks this is helpful. I think for now the way forward is to study these tutorials to find the right way to add the reaction in. If I have issues I will reply again to this thread.

Thanks!

[nullicle]

Hi again,

I have successfully updated my thermophysicalProperties file to include a mixture of air and water. The important part is:

thermoType
{
type heRhoThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy;
}

inertSpecie air;

chemistryReader foamChemistryReader;

foamChemistryFile "<constant>/foam.inp";

foamChemistryThermoFile "<constant>/foam.dat";

where the species are set in foam.inp:

H2O
{
specie
{
molWeight 18.0153;
}
thermodynamics
{
Tlow 200;
Thigh 3500;
Tcommon 1000;
highCpCoeffs ( 3.03399 0.00217692 -1.64073e-07 -9.7042e-11 1.68201e-14 -30004.3 4.96677 );
lowCpCoeffs ( 4.19864 -0.00203643 6.5204e-06 -5.48797e-09 1.77198e-12 -30293.7 -0.849032 );
}
transport
{
As 1.67212e-06;
Ts 170.672;
}
}

air
{
specie
{
molWeight 28.9596;
}
thermodynamics
{
Tlow 200;
Thigh 3500;
Tcommon 1000;
highCpCoeffs ( 3.57304 -7.24383e-04 1.67022e-06 -1.26501e-10 -4.20580e-13 -1047.41 3.12431 );
lowCpCoeffs ( 3.09589 1.22835e-03 -4.14267e-07 6.56910e-11 -3.87021e-15 -983.191 5.34161 );
}
transport
{
As 1.67212e-06;
Ts 170.672;
}
}

I have combustion, radiation and reactions off and added appropriate air and H2O files in the 0 directory. This runs no problem.

The problem is now I need to compute individual properties of the gases using the ideal gas law in order to calculate the relative humidity. Is there a relevant tutorial somewhere that computes properties of the individual gases?

I also noticed that unlike the reverseBurner tutorial for example, the air and H2O files in subsequent times are not updated. I assume this is because their mass fractions remain equal? I am not pumping anything in or taking anything out.

Thanks in advance.

[jherb]

As far as I know, buoyantPimpleFoam cannot be used to simulate different species. It just ignores the air and H2O files and calculates if as there is just one species. Look at the other solvers like reactingFoam. There you see in the output, that at least one equation for the species concentration is solved.

[nullicle]

Originally Posted by jherb

As far as I know, buoyantPimpleFoam cannot be used to simulate different species. It just ignores the air and H2O files and calculates if as there is just one species. Look at the other solvers like reactingFoam. There you see in the output, that at least one equation for the species concentration is solved.

That matches what I see, in that the later files for H2O etc are exactly the same as the initial one (i.e. not filled with values).

So reactingFoam should do everything that buoyantPimpleFoam does, but with the added functionality of evolving the mixtures? I've noticed for example the reverseBurner tutorial in chtMultiRegionFoam evolves the mixtures.

Thanks.

[nullicle]

Update:

I have the thing running with rhoReactingBuoyantFoam, however the results are not as expected.

I am modelling a room at a fixed temperature with an inlet blowing in hot air, and I am trying to incorporate water vapour.

What I find when using buoyantPimpleFoam is that the heat is not transferred through the air very fast, and it is quite localised. However when using rhoReactingBuoyantFoam (or just rhoPimpleFoam) with just air, the heat gets transferred to the entire room very quickly and it heats up uniformly, looking very unrealistic. I am guessing this has something to do with the thermophysicalProperties, although I use the same for both solvers above.

Is there anyone out there who has an idea about this?

I attach two pictures below of temperature on a vertical slice of the room after some time, one solved with buoyantPimpleFoam, the other with rhoReactingBuoyantFoam. One can see how the room is heated much quicker with the rhoReactingBuoyantFoam solver, and this has me worried. Sorry about the quality, but the point I'm trying to make is obvious nonetheless.

Thanks in advance.

[nullicle]

Two pictures.

[nullicle]

Update #2:

I think the reason why the temperature increases everywhere is because the pressure increases rapidly everywhere after not so many iterations. This could be because I have no outlet, but I have the BC of the inlet for the air file as

Heatpump_Inlet
{
type fixedValue;
value uniform 0;
}

So I am not "pumping in air", but rather blowing it around. I will run a test case with an outlet and see if that makes a difference.

[khafagy]

Hi nullicle,

I am currently doing a very similar case (blowing hot humid air into a room and observing the temperature and the relative humidity). So I were wondering did you finish your case? If so, can you help me figuring out which solver did you use in addition to the updated thermophysical properties!

Thank you in advance.

[g0v1n]

Hi, is there any template available for using rhoReactingBuoyantFoam ?

[shubhamkv1]

Hi @khafagy
I am working on the same problem. Will you please help me in sorting this out?

Thanks

[tian]

Hi,

You can give a try with: buoyantHumiditySimpleFoam or buoyantHumidityPimpleFoam.

Bye
Thomas

[zog]

Originally Posted by tian

Hi,

You can give a try with: buoyantHumiditySimpleFoam or buoyantHumidityPimpleFoam.

Bye
Thomas

Have you tried it yourself ?
I tried to run the tutorial for RAS with moisture, but it seems it is not up to date with v2212 despite the comments.

Namley : I had to change the inletBottom relHum BC to fixedHumidity as FixedValue is not vaid, and I could not run it wiht Kepsilon as I could not find. a alphat BC that weas valid. compressible::alphatwallfunction is not found, and alphatJayatillekeWallFunction is not compatible with buoyantsimplefoam...

I would appreciate if you could give some help (just running the tutorials for starters, with v2212 or later) !

[tian]

Hi,

Yes I am using it often without any trouble under 2312, too. Did you download the solver from my GIT or are you using my windows version?

Bye
Thomad

[zog]

https://github.com/shor-ty/humidityRhoThermo

I found this git on a linux rhel8, is it what you are refering to ? I couldn't find any other git though...

As for my issues I described them here buoyantHumiditysimplefoam

edit: seems like it is indeed the git you are referering to. Well then, I would be very grateful if you could help me with the first steps, as I have issues as soon as trying to run the tutorials : the fixedValue for the relHum BC inletBottom and (probably related to the same compilation issue ?) the alphat BC wall function.

Edit : i added 23 -lthermoTools \ in the make/options, now the BC are recognized. However I had to change in fvSchemes and fvSolution the thermo:specificHumidity for specificHumidity, and add it in the fvSolution. Also, while going trhough this, what is "R" in the fvSolution ?

 41 
 42     "(U|h|e|k|epsilon|R|specificHumidity)"
 43     {
 44         solver          PBiCGStab;
 45         preconditioner  DILU;
 46         tolerance       1e-6;
 47         relTol          0.1;
 48     }

Now it "runs" but crashes as soon as it starts. I also tried the "withoutHumidity" one but despite putting a relHum BC in 0, it does not find it and :

--> FOAM Warning : 
    From bool Foam::IOobject::typeHeaderOk(bool, bool, bool) [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /clust/softs/OpenFOAM/OpenFOAM-v2212/src/OpenFOAM/lnInclude/IOobjectTemplates.C at line 72
    Unexpected class name "dictionary" expected "volScalarField" when reading "/clust/opti/Projets/PROJET_JUNE/TestsSolvers/BenchOpenFoam/OF_HT/humidityRhoThermo/tutorials/RAS/withoutHumidity/0/relHum"
--> FOAM Warning : 
    From bool Foam::IOobject::typeHeaderOk(bool, bool, bool) [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /clust/softs/OpenFOAM/OpenFOAM-v2212/src/OpenFOAM/lnInclude/IOobjectTemplates.C at line 72
    Unexpected class name "dictionary" expected "volScalarField" when reading "/clust/opti/Projets/PROJET_JUNE/TestsSolvers/BenchOpenFoam/OF_HT/humidityRhoThermo/tutorials/RAS/withoutHumidity/0/relHum"


--> FOAM FATAL ERROR: (openfoam-2212)
Neither the specificHumidity or the relHum field was provided in the time-folder

    From virtual void Foam::humidityRhoThermo::readOrInitSpecificHumidity()
    in file humidityRhoThermo/humidityRhoThermo.C at line 698.

FOAM exiting

My understanding from the code was that it would use relHum if no specifichumidity was provided but I probably did something wrong again.
If i add specifichumidity definition in 0 it "runs" and crashes as the other one. Welp that's it for tonight, we'll see about that tomorrow !

I also am at a loss at what the /src/thermodynamic/basic/humidityRhoThermo/humidityRhoThermos.C does...

[tian]

Hi,

Maybe try this one here:

https://github.com/TBE-ThomasTian/HVAC-for-OpenFOAM

Otherwise you can contact me per email and I can check your case.

Bye
Thomas

[zog]

Originally Posted by tian

Hi,

Maybe try this one here:

https://github.com/TBE-ThomasTian/HVAC-for-OpenFOAM

Otherwise you can contact me per email and I can check your case.

Bye
Thomas

Thanks I will try with this one, i see the laminar tutorials got cleaned up too, thanks a relief !

By the way one quick question : the scalar transport equation for specific humidity is in the herhothermo.c file : is there a good reason for that, instead of in the actual solver file ?