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

Stability issue while running buoyantFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 1, 2007, 05:01
Default I'm experiencing some trouble
  #1
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
I'm experiencing some trouble running the buoyantFoam solver. During computation, while the Courant Numbers are still below 1, the following message, even if I employed a smaller timestep, appeared resulting in an interrupt of the computation:

--> 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/dm2/henry/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/specie/lnInclude/ specieThermoI.H at line 83.

FOAM aborting

To me it seems like the scheme for the temperature did not converge anymore. How can I influence the stability of it? The timestep alone doesn't seem to be enough.

My fvSchemes file is identical to the one used in the HotRoom Example Case, using also the same solver parameters for the turbulence model.

Any help is greatly appreciated
fandall is offline   Reply With Quote

Old   June 1, 2007, 12:12
Default Try upwind on h convection. In
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Try upwind on h convection. In fact put upwind on everything except div(phi,U) for which you can use linearUpwind cellLimited Gauss linear 1;

linearUpwind with a limiter is from my experience the most stable second order scheme around.

Also, if your mesh has any significant non-orthogonality (check with checkMesh) you should change all the laplacianSchemes entries to "Gauss linear limited 0.333;" and snGradSchemes to "limited 0.333"

At least these are the settings I use and I do quite a bit of buoyant flow calculations on meshes of questionable pedigree.
eugene is offline   Reply With Quote

Old   June 4, 2007, 03:20
Default Wow thanks! Altough I learne
  #3
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
Wow thanks!
Altough I learned about the stability of upwind schemes in my lectures, it didn't occur to me to use them (*D'oh*). I somehow thought this didn't apply to turbulent flow :-) Will surely give it a try.
My mesh is strictly orthogonal, so the laplacianSchemes (all set to Gauss linear) should do fine.

The Problem that I now have is, if I attempt to apply an upwind scheme to the div((mueEff*dev2(grad(U).T()))) term, the following error is put out before the calculation is even started:

--> FOAM FATAL IO ERROR : attempt to read beyond EOF

file: /opt/OpenFOAM/root1.2/run/shaftVentilation//shaftVentilation/system/fvSchemes::d iv((muEff*dev2(grad(U).T()))) at line 46.

From function ITstream::read(token& t)
in file db/IOstreams/Tstreams/ITread.C at line 70.

FOAM exiting

If I leave this term at 'linear', the whole thing is still diverging after a couple hundreds of time steps, seemingly independent of the time step size. And it is still the temperature solution that explodes. :-(
fandall is offline   Reply With Quote

Old   June 4, 2007, 03:41
Default I can't figure out why it show
  #4
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
I can't figure out why it shows this error message. "Attempt to read beyond EOF" means, that it attempts to read beyond the end of the file if I'm not mistaken, but I haven't forgotten a semicolon or anything like that. All I did was exchanging 'linear' with 'upwind' which even has the same number of letters. ?:-S

Please enlighten me
fandall is offline   Reply With Quote

Old   June 4, 2007, 06:17
Default Keep checking, there is either
  #5
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Keep checking, there is either an keyword entry missing or a punctuation error. Nothing else would cause that error.
eugene is offline   Reply With Quote

Old   June 4, 2007, 07:40
Default I still can't find any errors
  #6
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
I still can't find any errors :-(
I deposited my fvschemes file here:
http://n.ethz.ch/student/rohnerth/download/fvSchemes
All the other files in the system folder haven't been altered (except for the 'deltaT' and the 'writeInterval' values in controlDict) and are still the same as found in the hotRoom Example.
My suspicion is, that the scheme definition on line 46 needs additional input if any other interpolation scheme than linear is used, but I have no idea what kind that could be.
fandall is offline   Reply With Quote

Old   June 4, 2007, 07:53
Default What version of Foam are you r
  #7
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
What version of Foam are you running? linearUpwind with a cellLimited limiter is only supported from 1.4.
eugene is offline   Reply With Quote

Old   June 4, 2007, 08:01
Default I'm running Version 1.2 on thi
  #8
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
I'm running Version 1.2 on this machine.
If I try it without the limiter, I still get the same error message...
fandall is offline   Reply With Quote

Old   June 4, 2007, 08:06
Default linearUpwind didnt work very w
  #9
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
linearUpwind didnt work very well in 1.2, so I would switch to GammaV for div(phi,U).
eugene is offline   Reply With Quote

Old   June 4, 2007, 08:25
Default Perhaps I found the missing ar
  #10
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
Perhaps I found the missing argument:
If I want to use an upwind scheme on the term on line 46, it seems that I have to specify to which reference the upwind direction is identified. So I guess this missing reference should be the flux phi e.g.: "div((muEff*dev2(grad(U).T()))) Gauss upwind phi" should specify the correct flow direction. What do you think?
fandall is offline   Reply With Quote

Old   June 4, 2007, 08:56
Default So, setting up every divergenc
  #11
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
So, setting up every divergence scheme with upwind, the last one described as above, I end up with the same explosion of the temperature solution with which I started: The computation runs smoothly for a couple of hundred time steps and then diverges. :-(((
I guess I have to read some more literature about the stability of turbulent flow simulation or this one will never converge...
fandall is offline   Reply With Quote

Old   June 4, 2007, 10:17
Default Given that you are now using t
  #12
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Given that you are now using the most stable schemes available and are still experiencing divergence, I would hazard a guess that either your initial or boundary conditions are in error. (with boundary conditions being the more likely of the two.)
eugene is offline   Reply With Quote

Old   June 4, 2007, 10:29
Default Thanks for thinking aloud. Out
  #13
New Member
 
Thomas Rohner
Join Date: Mar 2009
Location: Switzerland
Posts: 12
Rep Power: 8
fandall is on a distinguished road
Thanks for thinking aloud. Out of these two, I would also go for the boundary conditions as the computation runs great for a rather big number of time steps. I'll reconsider my choice of b.c.'s carefully and will update you on any success stories.
fandall is offline   Reply With Quote

Old   May 9, 2011, 11:36
Default FOAM FATAL ERROR: Maximum number of iterations exceeded
  #14
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
Hii,

I am getting a similar error too, and don't seem to find an appropriate solution. Can someone please tell if he has managed to solve the issue?

Thanks,
Tarak
Tarak 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
TotalPressure and buoyantFoam ariorus OpenFOAM Running, Solving & CFD 1 January 22, 2008 09:41
BuoyantFoam braennstroem OpenFOAM Running, Solving & CFD 22 September 19, 2007 16:55
BuoyantFoam in parallel sylvester OpenFOAM Running, Solving & CFD 0 July 19, 2007 05:38
BuoyantFoam in channel ogloth OpenFOAM Running, Solving & CFD 0 April 20, 2007 11:28
Reference for buoyantFoam maka OpenFOAM Running, Solving & CFD 0 October 23, 2006 08:21


All times are GMT -4. The time now is 07:18.