[msarkar]

Hi All,

I am almost new in OpenFOAM but not in CFD, using OF 1.6. I need to include radiation model to the solver chtMultiRegionFoam. Could anyone help me how to approach it?

Any help would be very much appreciated.

Regards
msarkar

[mabinty]

Hi msarkar, hi all,

I implemented radiation into chtMultiRegionFoam (OF 1.6.x); in general you just have to add the contribution of radiation to the energy equation (hEqn). First I studied the steady solver buoyantSimpleRadiationFoam and than added radiation to the transient solver buoyantPisoFoam (what seemed to work); introducing radiation to chtMultiRegionFoam was similar. Download the attached file (chtMultiRegionRadFoam.tar.gz), extract it to your USER/application directory and wmake for compilation.

A simple 3D Geometry, a hot block cools down in a cold ambient showed plausible results with the fvDOM model. But now, when considering a 2D geometry, air between two parallel plates of const. Temp. (T_left < T_right) the solver crashes after the first time the radiative transfer equation (RTE) is solved:

DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 2.358645e-16, No Iterations 1

--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded

    From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
    in file /home/aa/OpenFOAM/OpenFOAM-1.6.x/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 68.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#3  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#4  main in "/home/aa/OpenFOAM/aa-1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionRadFoam"
#5  __libc_start_main in "/lib/libc.so.6"
#6  _start at /build/buildd/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116

The h-field determined including the results of the RTE seem not to allow the calculation of reasonable temperatures. I m not sure if its the BC at solit_fluid interface or the empty patch causing the problem. I ll keep on digging.

Appreciate your comments,
Aram

[msarkar]

Hi Aram,

Thanks a lot for sharing the solver you developed. My present simulation is similar to the 2D problem you described. First, I want to simulate a square cavity with top and bottom walls are adiabatic and left wall is cold set temperature is same as the inside air tempterature. Right side is a solid heater with certain thickness and has constant temperature. However, let me compile the solver and check it for this 2D problem. I will let you know my comments.

Regards
msarkar

[msarkar]

Hi Aram,

I compiled it but I could not run any tutorials/examples as I am not sure about boundary/initial conditions needed for DOM radiation model . I would very much appreciate if you let me know the boundary/initial conditions for fvDOM radiation model. Actually I never used DOM. I noticed that in this solver you used DOM instead P1 model. If you can send me the tutorial files you ran that will be very helpful to me.

Thanks and Regards
msarkar

[mabinty]

Hi,

look at the settings for radiation in the tutorial cases

tutorials/heatTransfer/buoyantSimpleRadiationFoam/hotRadiationRoom

and

tutorials$ cd heatTransfer/buoyantSimpleRadiationFoam/hotRadiationRoomFvDOM

using P1 and fvDOM model respectively. These have to be adjusted in the respective fluidRegions (constant/<fluidRegion>/radiationPrpperties). I attached a simple 3D case (radBlock.tar.gz).

Cheers,
Aram

[mabinty]

Sorry, what I forgot: BC and IC of G/IDefault (P1/fvDOM model) are set in changeDictionary of the respective <fluidRegion> located in system/<fluidRegion>

Aram

[msarkar]

Hi Aram,

I very much appreciate your help. I will run my 2D case and let you know the status.

[msarkar]

Hi Aram,

I am able to run this solver for a simple 2D case. I simulated a 2D cavity flow with horizontal walls as adiabatic, left wall is isothermal, temperature of 293 K and right side is a solid heater maintained at constant temperature of 333K. I simulated this problem based on a published work. However, the results are not good. It's not comparable to the published result. My results are attached below. ((from left to right) First Fg. shows mesh and temperature boundary conditions, second Fig. shows temperature variation at the center of the fluid domain (current simulation) and 3rd Fig. shows temperature variation at the center of the fluid region (published result)).
There may be a problem with chtMutiRegionFoam solver as I found different results for different mesh pattern using chtMultiRegionFoam. If you are interested I can share my chtMltiRegionFoam results also.. Actually I am not able to validate chtMultiRegionFoam solver as well. I am not sure, what is the problem. If you find anything, please let me know.

Is there any chance that you already validated the chtMultiRegionFoam solver or your new solver (chtMultiRegionRadFoam)?

[mabinty]

hi MSarkar!

I validated chtMultiRegionFoam with the cases "forced convection of a heated plate" and "natural convection of a heated plate" where semi-empirical results are available. Concerning your case, could you send me a reference of the published work you re trying to reproduce so I can imagine the case set-up and give some input. Furthermore I would also be interested to include it to my current validation of the chtMultiRegionRadFoam. When I finished the validation I can send you the results.

Cheers,
Aram

[msarkar]

Hi Aram,

I am trying to reproduce the following reference papers..

1. Xama, J., Alvarez, G., Hinojosa, J. & Flores, J., “Conjugate turbulent heat transfer in s square cavity with solar control coating deposited to a vertical semitransparent wall”, Int. Journal of Heat and Fluid Flow, Vol. 30, pp. 237-248, 2009.

2. Velusamy, K., Sundararajan, T. and Seetharamu, K. N., “Interaction effects between surface radiation and turbulent natural convection in square and rectangular enclosures”, Journal of Heat Transfer – Transactions of the ASME, Vol. 123, pp. 1062-1070, 2001.

The files are too big to attach here. If you can not find the papers, give me your email address, I will send you. When you have time, please look at my other post regarding chtMultiRegionFoam where I posted two different cases and results. I did not find any good explanations for the result differences between two cases with same boundary conditions. If you find any explanations, please let me know.
Thanks!

[mange]

Hi,

I am just curious of your settings of the DOM ? how many discrete angles are you using?

/M

[mabinty]

Hi MSarkar,

Thx for the references. As far as I understood your re trying to solve a heat transfer problem without radiation. Hence you refer to the chtMultiRegionFoam solver. It would be helpful if you could post some details of your set up (geometry, BCs, etc.).

Concerning the solver I up-loaded in a previous post I m now studying how to consider radiation at the fluid-solid interface. For that I look at the temperature-BC "solidWallMixedTemperatureCoupled" coupling the solid and fluid region. It fixes the temperature of the considered patch if the flux is outgoing, otherwise it prescribes the gradient where the radiative part hast to come into. I ll keep on posting my progress and appreciate any comments!!

All the best,
Aram

[msarkar]

Hi Aram,

The results I posted in my previous reply, it is from your solver chtMultiRegionRadFoam. If I understood correctly, I think it (your solver) can solve conjugate heat transfer with radiation effects on the boundary of the domain.

I already posted the geometry and temperature boundary condition in my previous post (mesh file, 1st Fig.). I tried to simulate conjugate heat transfer with natural convection inside a square cavity and surface radiation effects. I used all walls have radiation emissivity of 0.9 (except solid-air interface), all walls have no slip condition (i.e. velocity zero).

When you get a chance, please look at this set up and let me know your comments.

[msarkar]

Hi Aram,

I got another question, in your solver chtMultiRegionRadFoam, I noticed that apart from radiation inclusion you also included SortableList.H and buildGlobalBoundaryList.H. These two were not included with chtMultiRegionFoam solver. Do these two need for Radiation or you tried to modify the chtMultiregionFoam solver itself?

[mabinty]

Hi MSarkar,

the code I uploaded is based on chtMultiRegionFoam where I added the coupling of convection and radiation by introducing the radiationModel in the fluid region. But the code isn t compete yet as I still have to adapt the boundary conditions (see my last post). I ll keep you up-dated about my progress.
Concerning SortableList.H and buildGlobalBoundaryList.H, I added these lines to calculate the mass flux at the boundaries (here for see http://openfoamwiki.net/index.php/Sn...ting_mass_flow).

Cheers,
Aram

[mirko]

Originally Posted by mabinty

Hi,

look at the settings for radiation in the tutorial cases

tutorials/heatTransfer/buoyantSimpleRadiationFoam/hotRadiationRoom

and

tutorials$ cd heatTransfer/buoyantSimpleRadiationFoam/hotRadiationRoomFvDOM

using P1 and fvDOM model respectively. These have to be adjusted in the respective fluidRegions (constant/<fluidRegion>/radiationPrpperties). I attached a simple 3D case (radBlock.tar.gz).

Cheers,
Aram

Aram,

I ran this case using the version of the solver that you posted last summer. The result that I got was that the block temperature increases in time from 500 to about 530K.

I was expecting the block to cool. Am I missing something?

Thanks,

Mirko

[mabinty]

hey mirko!

i don t exactly know which solver your are referring to but the most recent one i used is found here http://www.cfd-online.com/Forums/ope...ion-model.html (#15) for download. for now it only works with the fvDOM radiation model. please keep me informed about your progress!

cheers,
aram

[mirko]

Originally Posted by mabinty

hey mirko!

i don t exactly know which solver your are referring to but the most recent one i used is found here http://www.cfd-online.com/Forums/ope...ion-model.html (#15) for download. for now it only works with the fvDOM radiation model. please keep me informed about your progress!

cheers,
aram

Hi Aram,

I used exactly that solver for the problem that you posted here (A hot block at 500K in a room at 300K). My result was that the block temperature increased to 529.5 instead of decreasing. Maybe I am missing something.

Thanks :-)

Mirko

[mabinty]

Hi!

Which version of OF are you using? Please send me the set-up you are using and i ll have a look on it!

Regards,
Aram

[mirko]

Originally Posted by mabinty

Hi!

Which version of OF are you using? Please send me the set-up you are using and i ll have a look on it!

Regards,
Aram

Aram

(I was unable to upload the files - for some reason the tar.gz was too large)

Both your solver and example problem are linked to in my prior message: http://www.cfd-online.com/Forums/ope...tml#post290954

I am running them on OF1.7.1

Mirko