CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

ChtMultiRegionFoam and P1 radiation model

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 16, 2009, 10:40
Default dear all!! i would like to
  #1
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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 is offline   Reply With Quote

Old   January 19, 2009, 12:45
Default hi!! now i face another fun
  #2
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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
mabinty is offline   Reply With Quote

Old   January 19, 2009, 15:36
Default 1) You are better off starting
  #3
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
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.
mattijs is offline   Reply With Quote

Old   January 20, 2009, 13:19
Default 1) oh yeah, actually i m using
  #4
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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 is offline   Reply With Quote

Old   January 28, 2009, 05:43
Default hi! ad 3) i refined the mes
  #5
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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
mabinty is offline   Reply With Quote

Old   February 19, 2009, 15:18
Default 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
jano is on a distinguished road
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)
jano is offline   Reply With Quote

Old   February 20, 2009, 03:47
Default hi jean! give me your mail
  #7
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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
mabinty is offline   Reply With Quote

Old   February 20, 2009, 14:28
Default Hi Aram, That would be very
  #8
New Member
 
Jean Lachaud
Join Date: Mar 2009
Location: Moffett Field, Ca
Posts: 5
Rep Power: 8
jano is on a distinguished road
Hi Aram,

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

jean.lachaud@gmail.com

Thanks,

Jean
jano is offline   Reply With Quote

Old   November 12, 2009, 01:15
Default
  #9
New Member
 
Xinyuan FAN
Join Date: Sep 2009
Location: Beijing
Posts: 13
Rep Power: 7
autumn1012 is on a distinguished road
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
autumn1012 is offline   Reply With Quote

Old   November 20, 2009, 14:37
Default add Raditon model to buoyantBoussinesqPisoFoam
  #10
New Member
 
Sam Ulu
Join Date: Nov 2009
Posts: 4
Rep Power: 7
samulu is on a distinguished road
Quote:
Originally Posted by mabinty View Post
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.
samulu is offline   Reply With Quote

Old   February 17, 2010, 15:18
Default
  #11
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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 is offline   Reply With Quote

Old   May 21, 2010, 04:30
Default
  #12
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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
Attached Files
File Type: gz chtMultiRegionRadFoam.tar.gz (85 Bytes, 92 views)
mabinty is offline   Reply With Quote

Old   July 30, 2010, 04:28
Default
  #13
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
mirko is on a distinguished road
Hi Aram,

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

Thank you,

Mirko
mirko is offline   Reply With Quote

Old   July 30, 2010, 04:59
Default
  #14
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 8
kumar is on a distinguished road
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
kumar is offline   Reply With Quote

Old   August 10, 2010, 07:55
Default
  #15
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
please check the following .gz file
Attached Files
File Type: gz chtMultiRegionRadFoam.gz (11.8 KB, 107 views)
mabinty is offline   Reply With Quote

Old   September 8, 2010, 05:02
Default chtMultiRegionRadFoam
  #16
Member
 
Join Date: Dec 2009
Posts: 39
Rep Power: 7
marval is on a distinguished road
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
marval is offline   Reply With Quote

Old   September 8, 2010, 09:18
Default
  #17
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 184
Rep Power: 8
mabinty is on a distinguished road
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
mabinty is offline   Reply With Quote

Old   March 28, 2011, 12:34
Default
  #18
Senior Member
 
Join Date: Mar 2011
Posts: 155
Rep Power: 6
tH3f0rC3 is on a distinguished road
Hi,

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

Best Regards,
tH3f0rC3
tH3f0rC3 is offline   Reply With Quote

Old   April 8, 2011, 04:41
Default
  #19
Senior Member
 
Join Date: Mar 2011
Posts: 155
Rep Power: 6
tH3f0rC3 is on a distinguished road
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
tH3f0rC3 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 13:59.