
[Sponsors] 
February 16, 2010, 04:37 
chtMultiRegionFoam and Radiation

#1 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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 

February 17, 2010, 14:54 

#2 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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: Code:
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 2.358645e16, 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/OpenFOAM1.6.x/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 68. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/aa/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/home/aa/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/home/aa/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #3 Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/home/aa/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #4 main in "/home/aa/OpenFOAM/aa1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionRadFoam" #5 __libc_start_main in "/lib/libc.so.6" #6 _start at /build/buildd/glibc2.9/csu/../sysdeps/x86_64/elf/start.S:116 Appreciate your comments, Aram 

February 17, 2010, 23:54 

#3 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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 

February 18, 2010, 01:28 

#4 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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 

February 18, 2010, 07:06 

#5 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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 

February 18, 2010, 07:09 

#6 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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 

February 18, 2010, 08:23 

#7 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
Hi Aram,
I very much appreciate your help. I will run my 2D case and let you know the status. 

February 24, 2010, 02:30 

#8 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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)? 

February 24, 2010, 04:55 

#9 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
hi MSarkar!
I validated chtMultiRegionFoam with the cases "forced convection of a heated plate" and "natural convection of a heated plate" where semiempirical 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 setup 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 

February 24, 2010, 05:30 

#10 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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. 237248, 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. 10621070, 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! 

February 24, 2010, 06:29 

#11 
New Member
magnus
Join Date: Apr 2009
Posts: 7
Rep Power: 10 
Hi,
I am just curious of your settings of the DOM ? how many discrete angles are you using? /M Last edited by mange; February 24, 2010 at 06:54. 

February 25, 2010, 04:54 

#12 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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 uploaded in a previous post I m now studying how to consider radiation at the fluidsolid interface. For that I look at the temperatureBC "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 

February 26, 2010, 01:28 

#13 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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 solidair 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. Last edited by msarkar; February 26, 2010 at 03:58. 

February 26, 2010, 05:50 

#14 
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 9 
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? 

February 27, 2010, 13:22 

#15 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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 updated 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 

January 14, 2011, 10:56 

#16  
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 10 
Quote:
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 

January 17, 2011, 13:59 

#17 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
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.cfdonline.com/Forums/ope...ionmodel.html (#15) for download. for now it only works with the fvDOM radiation model. please keep me informed about your progress! cheers, aram 

January 18, 2011, 11:23 

#18  
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 10 
Quote:
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 

January 21, 2011, 04:31 

#19 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 10 
Hi!
Which version of OF are you using? Please send me the setup you are using and i ll have a look on it! Regards, Aram 

January 21, 2011, 18:36 

#20  
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 10 
Quote:
(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.cfdonline.com/Forums/ope...tml#post290954 I am running them on OF1.7.1 Mirko 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ChtMultiRegionFoam and P1 radiation model  mabinty  OpenFOAM Running, Solving & CFD  18  April 8, 2011 04:41 