
[Sponsors] 
August 30, 2007, 06:04 
Hi,
I'm not really sure it i

#1 
Member

Hi,
I'm not really sure it is a bug (I'm still working with version 1.3 and so I didn't try it) but it seems to me that the new (1.4.1 release) compressible kOmegaSSTomega has wrong production terms for both omega and k equations (also dimensionally): /* this is the relevant part of the code volScalarField GbyMu = 2*mut_*(tgradU() && dev(symm(tgradU()))); volScalarField G = mut_*GbyMu; tmp<fvscalarmatrix> omegaEqn ( fvm::ddt(rho_, omega_) + fvm::div(phi_, omega_)  fvm::laplacian(DomegaEff(F1), omega_) == rhoGammaF1*GbyMu  fvm::SuSp((2.0/3.0)*rhoGammaF1*divU, omega_)  fvm::Sp(rho_*beta(F1)*omega_, omega_)  fvm::SuSp ( rho_*(F1  scalar(1))*CDkOmega/omega_, omega_ ) tmp<fvscalarmatrix> kEqn ( fvm::ddt(rho_, k_) + fvm::div(phi_, k_)  fvm::laplacian(DkEff(F1), k_) == min(G, c1*betaStar*k_*omega_)  fvm::SuSp(2.0/3.0*rho_*divU, k_)  fvm::Sp(rho_*betaStar*omega_, k_) ); I guess that it should instead be something like: volScalarField G_DividedbyMu = 2*(tgradU() && dev(symm(tgradU()))); volScalarField G = mut_*G_DividedbyMu; tmp<fvscalarmatrix> omegaEqn ( fvm::ddt(rho_, omega_) + fvm::div(phi_, omega_)  fvm::laplacian(DomegaEff(F1), omega_) == rhoGammaF1*G_DividedbyMu  fvm::SuSp((2.0/3.0)*rhoGammaF1*divU, omega_)  fvm::Sp(rho_*beta(F1)*omega_, omega_)  fvm::SuSp ( rho_*(F1  scalar(1))*CDkOmega/omega_, omega_ ) tmp<fvscalarmatrix> kEqn ( fvm::ddt(rho_, k_) + fvm::div(phi_, k_)  fvm::laplacian(DkEff(F1), k_) == min(G, c1*betaStar*k_*omega_)  fvm::SuSp(2.0/3.0*rho_*divU, k_)  fvm::Sp(rho_*betaStar*omega_, k_) ); Can you please tell me if someone agrees with me? Regards Cosimo
__________________
Cosimo Bianchini Energy Engineering Department "S. Stecco" University of Florence Via di S.Marta, 3 50139 Florence  ITALY Tel: +39 055 4796575 Fax: +39 055 4796342 Mob: +39 320 9460153 email: cosimo.bianchini@htc.de.unifi.it URL: www.htc.de.unifi.it 

August 30, 2007, 06:17 
Yes your are correct, I implem

#2 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Yes your are correct, I implemented the model just before release and didn't have time to test it. I will check it through again, test it and post a corrected version next week sometime.


August 31, 2007, 10:18 
Here is a corrected version of

#3 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Here is a corrected version of kOmegaSST.C
kOmegaSST.C to replace the file in OpenFOAM1.4.1/src/turbulenceModels/compressible/kOmegaSST I have tested the model runs and give sensible results but I have not performed a rigorous validation. 

September 24, 2007, 06:39 
Hi Henry,
just another small

#4 
Member

Hi Henry,
just another small doubt about the limiter for mut. I could not download the paper you suggest as reference for this model but the reference paper I used for implementing the kOmegaSST (Heat Transfer Predictions using Advanced TwoEquation Turbulence Models; Wolfgang Vieser, Thomas Esch and Florian Menter; CFX Technical Memorandum: CFXVAL10/0602, 2002) have a different limiter for mut: mut = rho* a1*k/max(a1*omega,sqrt(2)*mag(symm(gradU)*F2)); The standard release instead is using: mut = rho* a1*k/max(a1*omega,mag(symm(gradU)*F2)); Is it a bug or it is just a correction to make it suitable for heat transfer applications? Please tell me what is your paper saying about that. Thanks a lot Cosimo
__________________
Cosimo Bianchini Energy Engineering Department "S. Stecco" University of Florence Via di S.Marta, 3 50139 Florence  ITALY Tel: +39 055 4796575 Fax: +39 055 4796342 Mob: +39 320 9460153 email: cosimo.bianchini@htc.de.unifi.it URL: www.htc.de.unifi.it 

September 24, 2007, 06:51 
All the kOmega papers I have

#5 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
All the kOmega papers I have give this term without the sqrt(2) but then it could easily be contained in a1. What value is proposed for a1 in CFXVAL10/0602 and does it differ from the value proposed in the papers on the model?


September 24, 2007, 07:50 
I defintely agree with you.

#6 
Member

I defintely agree with you.
My value for a1 is 0.31 so if the two equations are consistent your should be 0.31/sqrt(2) = 0.2192. Thanks for confirming that. Cosimo
__________________
Cosimo Bianchini Energy Engineering Department "S. Stecco" University of Florence Via di S.Marta, 3 50139 Florence  ITALY Tel: +39 055 4796575 Fax: +39 055 4796342 Mob: +39 320 9460153 email: cosimo.bianchini@htc.de.unifi.it URL: www.htc.de.unifi.it 

September 24, 2007, 07:52 
Hi,
I am testing the kOmega

#7 
New Member
Claus H. Ibsen
Join Date: Mar 2009
Location: Denmark
Posts: 6
Rep Power: 8 
Hi,
I am testing the kOmegaSST model using the above kOmegaSST.C file. I am getting this error messages: > FOAM FATAL ERROR : incompatible dimensions for operation [omega[1 3 2 0 0 0 0] ]  [((rho*((tanh(pow4(min(min(max((((1betaStar)*sqrt( k))(omega*y)),((500*(murho) )(sqr(y)*omega))),(((4*alphaOmega2)*k)(max((((2* alphaOmega2)*(grad(k)&grad(ome ga)))omega),1.0e10)*sqr(y)))),10)))*(gamma1gamma2))+gamma2))*((2*mut)*(grad(U )&&dev(symm(grad(U))))))[2 4 3 0 0 0 0] ]#0 Foam::error::printStack(Foam:stream&) in "/home/ci/OpenFOAM/OpenFOAM1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/home/ci/OpenFOAM/OpenFOAM1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::GeometricField<double,> const&, char const*) in "/home/ci/OpenFOAM/OpenFOAM1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFoam" #3 Foam::tmp<foam::fvmatrix<double> > Foam::operator<double>(Foam::tmp<foam::geometricfield<double,> > const&, Foam::tmp<foam::fvmatrix<double> > const&) in "/home/ci/OpenFOAM/OpenFOAM1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceMod els.so" #4 Foam::compressible::turbulenceModels::kOmegaSST::c orrect() in "/home/ci/OpenFOAM/OpenFOAM1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceMod els.so" #5 main in "/home/ci/OpenFOAM/OpenFOAM1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFoam" #6 __libc_start_main in "/lib/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/ci/OpenFOAM/OpenFOAM1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFoam" From function checkMethod(const fvMatrix<type>&, const GeometricField<type,>&) in file /home/dm2/henry/OpenFOAM/OpenFOAM1.4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1232. FOAM aborting Is that an error in my setup of the case, or is the error in the kOmegaSST.C file? Thanks, Claus. 

September 24, 2007, 08:56 
The value of a1 in the papers

#8 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
The value of a1 in the papers I have is also 0.31. I don't know at what point Menter added the sqrt(2) prefactor I haven't seen it in any of the published papers on the kOmega model I have but I don't have a full set.


September 24, 2007, 11:16 
Hi Claus!
I would guess tha

#9 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40 
Hi Claus!
I would guess that the problem is with the setup. One common problem is that people take a kepscase, rename the epsilonfile to omega but don't change the dimensions (although that would not explain the difference in dimensions in your case). Check the dimensions Bernhard
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

September 24, 2007, 11:54 
Hi Weller,
I also have got a

#10 
Member

Hi Weller,
I also have got an article without the sqrt(2): Menter, Two Equation EddyViscosity Turbulence Models for Engineering Applications, AIAA Journal Vol.32 , N 8, 1994. In that case however: mut = rho* a1*k/max(a1*omega,mag(OMEGA)*F2)); with OMEGA = absolute value of vorticity = mag(curl(U)) != strain rate magnitude = 0.5*(grad(U) + grad(U).T). Could this be the mistake? Am I misunderstanding anything? Regards Cosimo
__________________
Cosimo Bianchini Energy Engineering Department "S. Stecco" University of Florence Via di S.Marta, 3 50139 Florence  ITALY Tel: +39 055 4796575 Fax: +39 055 4796342 Mob: +39 320 9460153 email: cosimo.bianchini@htc.de.unifi.it URL: www.htc.de.unifi.it 

September 24, 2007, 12:03 
It is not a mistake, the model

#11 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
It is not a mistake, the model has evolved over the years particularly in this term. I assure your that what I have implemented is what is in the paper I refer to in the header. I cannot say if the form you are referring to is preferable to the form I have implemented as I do not have all the relevant literature on the subject.


September 24, 2007, 12:44 
You are right: there are sever

#12 
Member

You are right: there are several different versions of such model. I do not have all the papers as well but, as far as I can see, your version is actually the same model implemented in CFX 10.
Thanks for this clarification, Cosimo
__________________
Cosimo Bianchini Energy Engineering Department "S. Stecco" University of Florence Via di S.Marta, 3 50139 Florence  ITALY Tel: +39 055 4796575 Fax: +39 055 4796342 Mob: +39 320 9460153 email: cosimo.bianchini@htc.de.unifi.it URL: www.htc.de.unifi.it 

September 25, 2007, 05:48 
I forgot to wmake... everythin

#13 
New Member
Claus H. Ibsen
Join Date: Mar 2009
Location: Denmark
Posts: 6
Rep Power: 8 
I forgot to wmake... everything is working nice now.
Sorry for the inconvenience. Claus. 

January 21, 2009, 10:55 
Could somebody please supply m

#14 
New Member
Andrew Parker
Join Date: Mar 2009
Posts: 1
Rep Power: 0 
Could somebody please supply me with an electronic copy of: Heat Transfer Predictions using Advanced TwoEquation Turbulence Models; Wolfgang Vieser, Thomas Esch and Florian Menter; CFX Technical Memorandum: CFXVAL10/0602, 2002
I understand this explains the automatic wall function treatment for the SST model, I would appreciate any papers which discuss this, not just the above. The only reference I can find is in Menter's Ten years of industrial experiance with the SST model, ref [8], but I can't seem to find the paper anywhere?? Any help would be appreciated. Cheers, Andy 

November 14, 2009, 00:59 

#15 
New Member
Mahwish
Join Date: Oct 2009
Posts: 7
Rep Power: 8 
I have the same problem .I want to know how SSt handels low Re number flows


November 14, 2009, 06:19 

#16 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
The komegaSST model I implemented is the highRe form to be used with the standard, continuous/adaptive or rough wallfunctions supplied. However it would be quite easy to implement the lowRe form of the model as this simply requires the application of damping functions on a few terms.
H 

November 14, 2009, 14:23 

#17 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10 
As I understood it, the current implemented SST model is suitable for lowre flows as well. Though one needs different wall treatment (especially for omega). And maybe the use of some damping functions is better. Do you have any experience in it?
Fabian 

November 14, 2009, 15:25 

#18 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
The komegaSST model we currently release is based on a blend of the highRe kepsilon and komega models, not the low Re komega model. With an adaptive/continuous wallfunction you can use this model to resolve the nearwall lowRe flow with some degree of accuracy but if you want to resolve these details accurately you will need to include the lowRe dampingfunctions into the komega part of the model and use a mesh with adequate resolution in the nearwall region.
H 

November 14, 2009, 15:44 

#19 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10 
Thanks for the explanation!
Fabian 

November 15, 2009, 18:12 

#20 
New Member
Mahwish
Join Date: Oct 2009
Posts: 7
Rep Power: 8 
Thanks a lot .
But by solving right to the wall will be espensive right that's why we avoid that .Rather than using wall functions will be a cheap alternative. I don't know what CFX using as a standard SST model . 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Nearwall treatment for the kOmegaSST turbulence model  johnb  OpenFOAM Running, Solving & CFD  3  January 22, 2009 03:52 
ChtMultiRegionFoam kOmegaSST solidDisplacementFoam  marico  OpenFOAM Running, Solving & CFD  4  January 16, 2009 03:51 
How can run MRFSimpleFoam with KOmegaSST turbulence model  waynezw0618  OpenFOAM Running, Solving & CFD  0  April 21, 2008 04:40 
Question on new implemented komegaSST model in OF 14  peterh  OpenFOAM Running, Solving & CFD  7  February 7, 2008 03:09 
compressible  John  Main CFD Forum  1  April 6, 2003 12:35 