CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Bugs (http://www.cfd-online.com/Forums/openfoam-bugs/)
-   -   Compressible kOmegaSST (http://www.cfd-online.com/Forums/openfoam-bugs/62339-compressible-komegasst.html)

cosimobianchini August 30, 2007 06:04

Hi, I'm not really sure it i
 
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

henry August 30, 2007 06:17

Yes your are correct, I implem
 
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.

henry August 31, 2007 10:18

Here is a corrected version of
 
Here is a corrected version of kOmegaSST.C
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif kOmegaSST.C
to replace the file in OpenFOAM-1.4.1/src/turbulenceModels/compressible/kOmegaSST

I have tested the model runs and give sensible results but I have not performed a rigorous validation.

cosimobianchini September 24, 2007 06:39

Hi Henry, just another small
 
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 Two-Equation Turbulence Models; Wolfgang Vieser, Thomas Esch and Florian Menter; CFX Technical Memorandum: CFX-VAL10/0602, 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

henry September 24, 2007 06:51

All the k-Omega papers I have
 
All the k-Omega 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 CFX-VAL10/0602 and does it differ from the value proposed in the papers on the model?

cosimobianchini September 24, 2007 07:50

I defintely agree with you.
 
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

chibsen September 24, 2007 07:52

Hi, I am testing the kOmega
 
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((((1|betaStar)*sqrt( k))|(omega*y)),((500*(mu|rho) )|(sqr(y)*omega))),(((4*alphaOmega2)*k)|(max((((2* alphaOmega2)*(grad(k)&grad(ome ga)))|omega),1.0e-10)*sqr(y)))),10)))*(gamma1-gamma2))+gamma2))*((2*mut)*(grad(U )&&dev(symm(grad(U))))))[2 -4 -3 0 0 0 0] ]#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::GeometricField<double,> const&, char const*) in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/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/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceMod els.so"
#4 Foam::compressible::turbulenceModels::kOmegaSST::c orrect() in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceMod els.so"
#5 main in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFoam"
#6 __libc_start_main in "/lib/libc.so.6"
#7 Foam::regIOobject::readIfModified() in "/home/ci/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoSimpleFoam"


From function checkMethod(const fvMatrix<type>&, const GeometricField<type,>&)
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.4.1/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.

henry September 24, 2007 08:56

The value of a1 in the papers
 
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 k-Omega model I have but I don't have a full set.

gschaider September 24, 2007 11:16

Hi Claus! I would guess tha
 
Hi Claus!

I would guess that the problem is with the setup. One common problem is that people take a k-eps-case, rename the epsilon-file to omega but don't change the dimensions (although that would not explain the difference in dimensions in your case). Check the dimensions

Bernhard

cosimobianchini September 24, 2007 11:54

Hi Weller, I also have got a
 
Hi Weller,
I also have got an article without the sqrt(2):
Menter, Two Equation Eddy-Viscosity 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

henry September 24, 2007 12:03

It is not a mistake, the model
 
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.

cosimobianchini September 24, 2007 12:44

You are right: there are sever
 
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

chibsen September 25, 2007 05:48

I forgot to wmake... everythin
 
I forgot to wmake... everything is working nice now.
Sorry for the inconvenience.

Claus.

andy_parker January 21, 2009 10:55

Could somebody please supply m
 
Could somebody please supply me with an electronic copy of: Heat Transfer Predictions using Advanced Two-Equation Turbulence Models; Wolfgang Vieser, Thomas Esch and Florian Menter; CFX Technical Memorandum: CFX-VAL10/0602, 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

msohail November 14, 2009 00:59

I have the same problem .I want to know how SSt handels low Re number flows

henry November 14, 2009 06:19

The k-omega-SST model I implemented is the high-Re form to be used with the standard, continuous/adaptive or rough wall-functions supplied. However it would be quite easy to implement the low-Re form of the model as this simply requires the application of damping functions on a few terms.

H

braennstroem November 14, 2009 14:23

As I understood it, the current implemented SST model is suitable for low-re 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

henry November 14, 2009 15:25

The k-omega-SST model we currently release is based on a blend of the high-Re k-epsilon and k-omega models, not the low Re k-omega model. With an adaptive/continuous wall-function you can use this model to resolve the near-wall low-Re flow with some degree of accuracy but if you want to resolve these details accurately you will need to include the low-Re damping-functions into the k-omega part of the model and use a mesh with adequate resolution in the near-wall region.

H

braennstroem November 14, 2009 15:44

Thanks for the explanation!

Fabian

msohail November 15, 2009 18:12

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 .


All times are GMT -4. The time now is 08:13.