|
[Sponsors] |
July 17, 2007, 18:53 |
Hi all,
I'm trying to code
|
#1 |
Member
Doug Hunsaker
Join Date: Mar 2009
Location: Logan, UT
Posts: 63
Rep Power: 17 |
Hi all,
I'm trying to code in a k-omega model. The model compiles, but during runtime I get the following error: Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0529457, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0290519, No Iterations 1 DICPCG: Solving for p, Initial residual = 1, Final residual = 0.0083708, No Iterations 171 time step continuity errors : sum local = 0.146471, global = -0.000598041, cumulative = -0.000598041 DILUPBiCG: Solving for omega, Initial residual = 0.183509, Final residual = 0.0054477, No Iterations 1 --> FOAM FATAL ERROR : incompatible fields for operation [k] == [omega]#0 Foam::error::printStack(Foam:stream&) #1 Foam::error::abort() #2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) #3 Foam::turbulenceModels::myKOmega::correct() #4 main #5 __libc_start_main #6 __gxx_personality_v0 at /usr/src/packages/BUILD/glibc-2.3/csu/../sysdeps/i386/elf/start.S:122 From function checkMethod(const fvMatrix<type>&, const fvMatrix<type>&) in file /home/doug/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude/fvMatrix.C at line 1005. FOAM aborting From the error message it is apparent that the error happens in the myKOmega::correct() function. I've tried adding print statements to see exactly where the error occurs, but haven't figured out how to get things to print to the screen. I tried Info<<"here"<<endl; statements, but they didn't work. Any ideas on how I might track down this runtime error? Here is the portion of the code I think it is breaking at in case anyone can spot the error from the code. However, I'm not sure if it's breaking here because I can't figure out at what line the program aborts. // Turbulent kinetic energy equation tmp<fvscalarmatrix> kEqn ( fvm::ddt(k_) + fvm::div(phi_, k_) - fvm::Sp(fvc::div(phi_), k_) - fvm::laplacian(DkEff(), k_) == G - fvm::Sp(Cmu*k_, omega_) ); Thanks in advance. Doug |
|
July 17, 2007, 18:57 |
Easy: you are building a matri
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
Easy: you are building a matrix for k_ and the last term is implicit in omega_ - you cannot add it to this matrix.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
July 17, 2007, 19:13 |
Thanks for the quick reply. So
|
#3 |
Member
Doug Hunsaker
Join Date: Mar 2009
Location: Logan, UT
Posts: 63
Rep Power: 17 |
Thanks for the quick reply. So how would you write Cmu*k_*omega_ ?
I tried fvc::Sp(Cmu*k_, omega_) and it didn't work either. It must be obvious from that line of code what I'm trying to do (?). -Doug |
|
July 17, 2007, 19:27 |
How about Cmu*omega_, k)?
H
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
How about Cmu*omega_, k)?
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
July 17, 2007, 19:35 |
You mean fvm::Sp(Cmu*omega_,k_
|
#5 |
Member
Doug Hunsaker
Join Date: Mar 2009
Location: Logan, UT
Posts: 63
Rep Power: 17 |
You mean fvm::Sp(Cmu*omega_,k_) right? I tried that too and it gives the same error. This is very similar to the code that kOmegaSST.C uses in its correct() function. So, I'm not sure what is causing the error. Any other ideas? Is there a way to print statements to the screen so I can track down which line it is aborting on?
Thanks again. |
|
July 18, 2007, 04:02 |
Hi Doug,
that correction is w
|
#6 |
Member
|
Hi Doug,
that correction is what you need to avoid the error you are referring. I mean: fvm::Sp(Cmu*omega_,k_). And you are right, this is a way you can add printouts: Info << "Solving for k_" << endl; Are you sure you manage to correctly compile the update version of your turbulence model? Don't know what else could be. Good luck, Cosimo
__________________
Cosimo Bianchini Ergon Research s.r.l. Via Panciatichi, 92 50127 Florence - ITALY Tel: +39 055 0763716 Mob: +39 320 9460153 e-mail: cosimo.bianchini@ergonresearch.it URL: www.ergonresearch.it |
|
July 18, 2007, 04:09 |
Well Doug, you've got a proble
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
Well Doug, you've got a problem - I am not guessing what's wrong: I actually know for a fact (been writing this code since 1993). The solution is fvm::Sp(Cmu*omega_,k_). Check the file, check the compilation, check that you are running what you think you are running etc.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
KOmega Turbulence model from wwwopenFOAMWikinet | philippose | OpenFOAM Running, Solving & CFD | 30 | August 4, 2010 11:26 |
Has anyone tried a delta form of pressure equation pressurecorrection equation with OpenFOAM | sek | OpenFOAM Running, Solving & CFD | 2 | July 24, 2007 08:53 |
Komega turbulence model | jasonb | OpenFOAM Running, Solving & CFD | 6 | August 29, 2006 09:46 |
KEpsilon and KOmega | larry | OpenFOAM Running, Solving & CFD | 3 | June 29, 2006 02:38 |
Komega turbulent viscosity model | guggi | OpenFOAM Running, Solving & CFD | 3 | May 18, 2006 21:07 |