CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   ChtMultiRegionFoam and P1 radiation model (http://www.cfd-online.com/Forums/openfoam-solving/57927-chtmultiregionfoam-p1-radiation-model.html)

mabinty January 16, 2009 10:40

dear all!! i would like to
 
dear all!!

i would like to implement the P1 radiation model (used in the buoyantSimplRadiationFoam solver) into the chtMultiRegionFoam solver. i m using the 1.5 version and started first by implementing the P1-model into the transient buoyantFoam solver which i think works well as a parameter study with respect to the absorption/emission coefficients showed plausible results. Now i m about to realize the implementation into the chtMultiRegionFoam solver, but the same parameter study indicates that the energy balance is decoupled from the radiative transfer equation (plausible behavior of the radiative flux but no changes in temperature distribution). my implementation looks like this:

1.) create a radiationModel "rad" in creatFluidFields.H with the temperature field thermof[i].T().

2.) the object "rad" is given to the function solveEnthalpyEquation, done at the top of hEqn.H and solveEnthalpyEquation.C.

3.) add the radiation source term to the enthalpy equation in solveEnthalpyEquation.C in the form rad.Sh(thermo).

i ll keep working on it and report, and would greatly appreciate any comments!! thx in advance!!

aram

mabinty January 19, 2009 12:45

hi!! now i face another fun
 
hi!!

now i face another fundamental problem with this new solver: i simulated a 10x5x10 m3 room with a small solid heater (2x05x2 m3) in the middle of the room. when holding the heater temperature constant over the simulation time, results seem to be ok; but at the moment i prescribe the conjugated heat transfer BC (solidWallHeatFluxTemperatureCoupled/solidWallTemperatureCoupled) at the solid/fluid interface i get surface temperatures higher than the initial heater temperature. as a result i had a closer look at the solidWallHeatFluxTemperatureCoupled/solidWallTemperatureCoupled BC and have two remarks:

1) why is the flux not divided by the patch surface for the calculation of the gradient, as the flux, calculated in solidWallTemperatureCoupledFvPatchScalarField.C is determined in the units of Watt?

_solidWallHeatFluxTemperatureCoupledFvPatchScalarF ield.C:

gradient() = refCast<const>(neighbourField).flux()/K;

_solidWallTemperatureCoupledFvPatchScalarField.C:

Foam::tmp<foam::scalarfield>
Foam::solidWallTemperatureCoupledFvPatchScalarFiel d::flux() const
{
const fvPatchScalarField& Kw =
patch().lookupPatchField<volscalarfield,>(KName_);

const fvPatchScalarField& Tw = *this;

return Tw.snGrad()*patch().magSf()*Kw;
}

2) how and what kind of information about the T-field is given from solidWallHeatFluxTemperatureCoupled to solidWallTemperatureCoupled?

thx for any comments!!
aram

mattijs January 19, 2009 15:36

1) You are better off starting
 
1) You are better off starting from 1.5.x. It fixes the flux issue and introduces a mixed boundary conditions which makes setup much easier. See the tutorial case.

2) from memory: K and neighbour internal field.

mabinty January 20, 2009 13:19

1) oh yeah, actually i m using
 
1) oh yeah, actually i m using 1.5.x (updated with git from 1.5). sorry for the confusion!

2)ok, but when i m looking into solidWallTemperatureCoupledFvPatchScalarField.C i can basically find the member functions flux() and updateCoeffs() including the operation

operator==(neighbourField);

but what is this operator doing or where is K and neighbour internal field given over? i searched the codes from which this BC type is derived and was not able to figure out what operator==() means.

3) additionally i checked out again the chtMultiRegionFoam and simulated a simplified case of the tutorial case (heater without "wings", no left/right solid and no inlet in the upper domain). First i used convertToMeters = 1 like the tutorial, and then convertToMeters = 10 (with additional changes in makeCellSets.setSet). when i compare the temperature plots, i see plausible results for convertToMeters = 1, but the problem of a higher heater surface temperature than the initial one (508 K vs 500 K) for convertToMeters = 10.

i m about to investigate further in how the data flow at the fluid-solid interface is solved and greatly appreciate comments on that!!

thx a lot!
aram

mabinty January 28, 2009 05:43

hi! ad 3) i refined the mes
 
hi!

ad 3) i refined the mesh (twice) for the simplified and scaled chtMultiRegionFoam tutorial case, but still have the problem of a higher heater surface temperature than the initial one (now 502 K vs 500 K). i really have no idea what i m doing wrong here.

thx in advance for any help!
aram

jano February 19, 2009 15:18

Hi Aram, I would like to mo
 
Hi Aram,

I would like to model the heating of a solid in air. I think that I need to do what you are doing. I found on a forum the tutorial "multiRegionHeater" but I find it very complicated for a start.
Would you mind sending me the simplified case that you made?
Maybe would could work together from this point? I will need to add surface radiation and other terms in the solid in the future.

Thanks,
Jean

PS: I have no idea if this can help, but did you check the stability if an explicit scheme is used? (value of the Courant number)

mabinty February 20, 2009 03:47

hi jean! give me your mail
 
hi jean!

give me your mail address so i can send you the set-up. concerning the courant number, the time-step is adjusted to keep Co=0.3.

aram

jano February 20, 2009 14:28

Hi Aram, That would be very
 
Hi Aram,

That would be very nice. My E-mail address is:

jean.lachaud@gmail.com

Thanks,

Jean

autumn1012 November 12, 2009 01:15

Hi Aram,

Nice meeting you here again. Actually I am doing the same job as you with OpenFOAM-1.6, adding radiation model to the solver chtMultiRegionFoam. The implementation is almost the same,
1.) ...
2.) ...
3.) ...
4.) rad.correct() after h equation is solved.

I used a case to calculate with this new solver which I called chtMultiRegionRadiationFoam but can't get reasonable results. Here are some problems I want to ask you,
1.) Can chtMultiRegionFoam be used to calculate turbulent flow? I found that the multiRegionHeater case is using laminar model, so I have such a wonder.
2.) If I want to calculate radiation in non-participating media, what kind of radiation model should I choose? P1 or fvDOM?
3.) If one of the solid region is semitransparent, what should I do to deal with this situation? Is there any relationship with the radiation model? It seems that fvDOM is more flexible than P1.

I am looking forward to your answer. Thanks.

Xinyuan

samulu November 20, 2009 14:37

add Raditon model to buoyantBoussinesqPisoFoam
 
Quote:

Originally Posted by mabinty (Post 184467)
dear all!!

i would like to implement the P1 radiation model (used in the buoyantSimplRadiationFoam solver) into the chtMultiRegionFoam solver. i m using the 1.5 version and started first by implementing the P1-model into the transient buoyantFoam solver which i think works well as a parameter study with respect to the absorption/emission coefficients showed plausible results. Now i m about to realize the implementation into the chtMultiRegionFoam solver, but the same parameter study indicates that the energy balance is decoupled from the radiative transfer equation (plausible behavior of the radiative flux but no changes in temperature distribution). my implementation looks like this:

1.) create a radiationModel "rad" in creatFluidFields.H with the temperature field thermof[i].T().

2.) the object "rad" is given to the function solveEnthalpyEquation, done at the top of hEqn.H and solveEnthalpyEquation.C.

3.) add the radiation source term to the enthalpy equation in solveEnthalpyEquation.C in the form rad.Sh(thermo).

i ll keep working on it and report, and would greatly appreciate any comments!! thx in advance!!

aram


Hi Aram,

I am simulating a HVAC application in OF v1.6 with buoyantBoussinesqPisoFoam. I intend to run this again, but this time around integrating the P1 radiation model into the buoyantBoussinesqPisoFoam solver. It seems that you implemented a similar process as mentioned in your previous post "implementing the P1-model into the transient buoyantFoam solver ".

I am fairly new to OpenFOAM use, could you please educate me on how to implement the P1 radiation model in buoyantBoussinesqPisoFoam?

Thank you very much for your assistance.

mabinty February 17, 2010 15:18

Hi!!

Sorry for the late response but it seems that I haven t got a message about your posts.

@Xinyuan

1.) yes; check constant/<fluidRegion>/RASProperties and constant/<fluidRegion>/turbulenceProperties
2.) I optained results with both models, but those with fvDOM were more accurate
3.) I would try to use a fluidRegion and eliminate convection (g=(0 0 0))

@samulu

I have no experience with buoyantBoussinesqPisoFoam but I would say the approach is the same. Study how the radiation model is implemented in buoyantSimpleRadiationFoam (creat a radiation model in creatFields.H; add the radiation source term Sh() to the energy equation hEqn.H).

All the best,
Aram

mabinty May 21, 2010 04:30

1 Attachment(s)
Dear all,

I added the radiation model to chtMultiRegionFoam and modified the solidWallMixedTemperatureCoupled BC (couples solid-fluid regions) to take the radiative wall heat flux into account (for now only with the fvDOM radiation model). I attached the solver (chtMultiRegionRadFoam.tar.gz) maybe its useful for you; appreciate your comments on it. Thanks in advance!

Regards,
Aram

mirko July 30, 2010 04:28

Hi Aram,

would you mind reposting your solver. The tar.gz file is invalid.

Thank you,

Mirko

kumar July 30, 2010 04:59

Hi Aram,
I am trying to set up a simple case and check the solver chtMultiregionFoam. I looked into the tutorial case and got some idea about setting up the cell sets and the region. Actually I have been working on a different topic using interFoam. But now i need to set up a simple case in chtMultiregionFOam, for demonstrating the capabilitites of chtMultiregionFoam.

I need a simple case like the one you have specified in your post to understand the basic set up first.

So could you please send me the set up files of the case with a heater in the middle of the room.
My email I.D is kumar.kannan@uni.lu.

thankyou
regards
K.Suresh kumar

mabinty August 10, 2010 07:55

1 Attachment(s)
please check the following .gz file

marval September 8, 2010 05:02

chtMultiRegionRadFoam
 
Hello,

I'm using OF-1.6.x and would like to try our new solver. A newbie-question:
How do I implement it?

Regards
Marco

mabinty September 8, 2010 09:18

hi!

extract the files and copy the chtMultiRegionRadFoam folder to the <user>-1.6.x/applications directory. go to <user>-1.6.x/applications/chtMultiRegionRadFoam and execute wmake.

regards,
aram

tH3f0rC3 March 28, 2011 12:34

Hi,

is it just the same procedure to implement radiation in chtMultiRegionSimpleFoam?

Best Regards,
tH3f0rC3

tH3f0rC3 April 8, 2011 04:41

Hi,

I want to use the solver chtMultiRegionRadFoam.
Does someone have a tutorial case for me so that I can study the boundary conditions and the fvshemes,...

That would be very nice, because there is no tutorial of this solver.
So if someone has a little case solved by his own, I would me glad to see how he changed the data (fvShemes, fvSolution, ...).

Best Regards,
tH3f0rC3


All times are GMT -4. The time now is 04:05.