
[Sponsors] 
January 16, 2009, 10:40 
dear all!!
i would like to

#1 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 P1model 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 

January 19, 2009, 12:45 
hi!!
now i face another fun

#2 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 Tfield is given from solidWallHeatFluxTemperatureCoupled to solidWallTemperatureCoupled? thx for any comments!! aram 

January 19, 2009, 15:36 
1) You are better off starting

#3 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16 
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. 

January 20, 2009, 13:19 
1) oh yeah, actually i m using

#4 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 fluidsolid interface is solved and greatly appreciate comments on that!! thx a lot! aram 

January 28, 2009, 05:43 
hi!
ad 3) i refined the mes

#5 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 

February 19, 2009, 15:18 
Hi Aram,
I would like to mo

#6 
New Member
Jean Lachaud
Join Date: Mar 2009
Location: Moffett Field, Ca
Posts: 5
Rep Power: 8 
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) 

February 20, 2009, 03:47 
hi jean!
give me your mail

#7 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
hi jean!
give me your mail address so i can send you the setup. concerning the courant number, the timestep is adjusted to keep Co=0.3. aram 

February 20, 2009, 14:28 
Hi Aram,
That would be very

#8 
New Member
Jean Lachaud
Join Date: Mar 2009
Location: Moffett Field, Ca
Posts: 5
Rep Power: 8 

November 12, 2009, 01:15 

#9 
New Member
Xinyuan FAN
Join Date: Sep 2009
Location: Beijing
Posts: 13
Rep Power: 8 
Hi Aram,
Nice meeting you here again. Actually I am doing the same job as you with OpenFOAM1.6, 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 nonparticipating 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 

November 20, 2009, 14:37 
add Raditon model to buoyantBoussinesqPisoFoam

#10  
New Member
Sam Ulu
Join Date: Nov 2009
Posts: 4
Rep Power: 7 
Quote:
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 P1model 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. 

February 17, 2010, 15:18 

#11 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 

May 21, 2010, 04:30 

#12 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
Dear all,
I added the radiation model to chtMultiRegionFoam and modified the solidWallMixedTemperatureCoupled BC (couples solidfluid 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 

July 30, 2010, 04:28 

#13 
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8 
Hi Aram,
would you mind reposting your solver. The tar.gz file is invalid. Thank you, Mirko 

July 30, 2010, 04:59 

#14 
Senior Member
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 8 
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 

August 10, 2010, 07:55 

#15 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
please check the following .gz file


September 8, 2010, 05:02 
chtMultiRegionRadFoam

#16 
Member
Join Date: Dec 2009
Posts: 39
Rep Power: 7 
Hello,
I'm using OF1.6.x and would like to try our new solver. A newbiequestion: How do I implement it? Regards Marco 

September 8, 2010, 09:18 

#17 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8 
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 

March 28, 2011, 12:34 

#18 
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 6 
Hi,
is it just the same procedure to implement radiation in chtMultiRegionSimpleFoam? Best Regards, tH3f0rC3 

April 8, 2011, 04:41 

#19 
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 6 
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ChtMultiRegionFoam  haewon  OpenFOAM Running, Solving & CFD  6  August 27, 2009 10:02 
Please help develop new BC for chtMultiRegionFoam  hsieh  OpenFOAM Running, Solving & CFD  0  January 21, 2009 10:48 
ChtMultiRegionFoam kOmegaSST solidDisplacementFoam  marico  OpenFOAM Running, Solving & CFD  4  January 16, 2009 03:51 
Radiation P1 Model with Spectral Model: Multigray  A. Thellmann  CFX  0  October 25, 2008 12:44 
Radiation Model  Spectral Model  Ray  CFX  3  April 10, 2006 09:33 