[zordiack]

Hi, I recently implemented the kOmegaSST-SAS model to RAS turbulence model side, so one can use wall functions if desired. It's based on the paper

"Development and Application of SST-SAS Turbulence Model in the DESIDER
Project"
(C) Springer-Verlag Heidelberg 2008
Y. Egorov and F. Menter

and the existing kOmegaSST turbulence model. I didn't know exactly where to put it so I created a new directory called OpenFOAM-2.3.x/src/turbulenceModels/incompressible/RAS/mykOmegaSSTSAS and added mykOmegaSSTSAS/mykOmegaSSTSAS.C to OpenFOAM-2.3.x/src/turbulenceModels/incompressible/RAS/Make/files.

Feel free to test it if you like

[fsaltara]

Very good idea, but what about the .dep file?

[fsaltara]

Sorry, the .dep file was not necessary. Compiled it and it is runing.

I wrote the delta option in the RASProperties file:

delta cubeRootVol;

cubeRootVolCoeffs
{
deltaCoeff 1;
}

Am I doing the right thing?

thanks

Fabio

[zordiack]

As this is a RAS implementation, you don't need the delta option in RASproperties, it's only needed for the LES model. The cubic root of cell volumes is calculated in the code.

    // Set the internal field values. 
    hInternal = pow(mesh_.V(), 1.0 / 3.0);

[ayoros]

Hi pekka,

Great job with this kOmegaSSTSAS !

Unfortunately, I have a problem when I come to run in parallel.

The same case is running fine in serial (1 processor) but crashes in parallel at the very first turbulence iteration.

Do you have any idea about this ?

Best regards,
Fabien

Edit : After looking at it, it seems that the volScalarField h is not filled correctly. It takes the correct value for the first processor I think, but stays at a value of 0 for the others, generating a floating point exception.

[zordiack]

Ok, that is weird. I tried it with the first case that I had about (centrifugal fan with AMI) and it doesn't crash. I'm using 4 processors at the moment and it's been running for 20 iterations now.

If it has problems with zero fields, then maybe adding ROOTVSMALL into strategic places could fix it? I'm also wondering how could h field be zero, since it's the cubic root of cell volumes? It would mean that you have zero volume cells in your mesh.

[ayoros]

Ok, looks like my problem comes from the cellLimited I apply to grad(U) in my fvSchemes.

When I set grad(U) to cellLimited Gauss linear 1, the case crashes.

When I set grad(U) to Gauss linear, it runs fine (at least for a few time steps).

This looks strange to me, but that's how it goes with my case.

[FrankFlow]

Originally Posted by zordiack

Feel free to test it if you like

Hi Pekka,

great contribution, I highly appreciate that. Would it it possible for you to also attach a little working case to make testing and usage of your code easier?

Thanks a lot and kind regards,
Frank

[zordiack]

It should work with any existing kOmegaSST case by just replacing kOmegaSST with mykOmegaSSTSAS in the file constant/RASproperties. The instructions for compiling are in the first post.

The real benefits of the SAS formulation are in the time dependent computations (URANS), as can be seen from the papers.

[zordiack]

There seems to be an "official" implementation of this in the upcoming OpenFOAM-dev repository, so maybe we should all switch to using that one once it becomes available. Just a heads up for people if someone comes across this thread

[zordiack]

I'm going to post a little update to this old thread, because the kOmegaSSTSAS version which is implemented in OpenFOAM-dev and OpenFOAM-3.0.x is still using to old formulation from 2008. I made a new version of the model and it can be downloaded from here:

https://github.com/zordiack/foam-dev

It compiles a user lib so it doesn't mess up original source code. This implementation is based on the paper:

Egorov, Y., & Menter F.R. (2009). Formulation of of the Scale-Adaptive Simulation (SAS) Model during the DESIDER Project. DESider – A European Effort on Hybrid RANS-LES Modelling, Notes on Num. Fluid Mech. And Multidisciplinary Design, Volume 103, 19-67.

which is reference by the 2010 SAS papers by Menter & Egorov. The L_vk field calculation and model coefficients are different compared to the 2008 model.

PS. If someone could provide a simple tutorial for making an own turbulence model for this new (-dev 3.0.x) system, that would be really great. I'm certain the way I did it is not practical, but it works. But using the custom model produces these kind of nasty error messages:

Create time

Duplicate entry laminar in runtime selection table TurbulenceModel
#0 /home/pppekkapa/OpenFOAM/OpenFOAM-dev/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+ 0x27) [0x7f8030a82337]
..

and the same for LES and RAS. I just don't know how to not make duplicate entries in my custom libraries.

[student666]

Hi, can you please share the two papers you're talking about?I mean the one from your last post and the one in your cirst thread, thank you

[jherb]

Y. Egorov, F. Menter
Development and Application of SST-SAS Turbulence Model in the DESIDER Project
http://link.springer.com/chapter/10....540-77815-8_27
http://cfd.mace.manchester.ac.uk/des...3-1-Egorov.pdf

[zordiack]

There is now an updated version available which no longer complains about duplicate entries. For details see here:

https://github.com/zordiack/foam-dev...abaaaa6f86c197

Links to the relevant papers:

The original SAS paper from 2008 (already in the previous post):

http://link.springer.com/chapter/10....540-77815-8_27

The updated version from 2009 (referenced by the 2010 paper):

http://link.springer.com/chapter/10....-540-92773-0_2

The more comprehensive papers describing the SAS model in more detail from 2010:

http://link.springer.com/article/10....494-010-9264-5
http://link.springer.com/article/10....494-010-9265-4

[kingjewel1]

Hi

Thanks for writing this, it looks like it will be very useful.

I tried to compile the turbulence model in 3.0.0 and it is coming up with this error, any ideas why that might be, i have to say it isn't one I've come up against before and I'm not sure how to go about finding the source to fix it.

derivedFvPatchFields/wallFunctions/omegaWallFunctions/omegaKnoppWallFunction/omegaKnoppWallFunctionFvPatchScalarField.C:50:9: error: ‘FatalErrorInFunction’ was not declared in this scope

Thanks

EDIT: This has been fixed by altering the Error check as follows:

// * * * * * * * * * * * * Protected Member Functions * * * * * * * * * * * //

void omegaKnoppWallFunctionFvPatchScalarField::checkTyp e()
{
if (!isA<wallFvPatch>(patch()))
{
FatalErrorIn
(
"omegaKnoppWallFunctionFvPatchScalarField::checkTy pe()"
) << "Invalid wall function specification" << nl
<< " Patch type for patch " << patch().name()
<< " must be wall" << nl
<< " Current patch type is " << patch().type() << nl << endl
<< abort(FatalError);
}
}



This compiles and runs fine in serial but not in parallel...

[zordiack]

Knopp wall function compilation in -dev is fixed in commit https://github.com/zordiack/foam-dev...a633c983e327e1

[zordiack]

Originally Posted by kingjewel1

Hi

Thanks for writing this, it looks like it will be very useful.

I tried to compile the turbulence model in 3.0.0 and it is coming up with this error, any ideas why that might be, i have to say it isn't one I've come up against before and I'm not sure how to go about finding the source to fix it.

derivedFvPatchFields/wallFunctions/omegaWallFunctions/omegaKnoppWallFunction/omegaKnoppWallFunctionFvPatchScalarField.C:50:9: error: ‘FatalErrorInFunction’ was not declared in this scope

Thanks

EDIT: This has been fixed by altering the Error check as follows:

// * * * * * * * * * * * * Protected Member Functions * * * * * * * * * * * //

void omegaKnoppWallFunctionFvPatchScalarField::checkTyp e()
{
if (!isA<wallFvPatch>(patch()))
{
FatalErrorIn
(
"omegaKnoppWallFunctionFvPatchScalarField::checkTy pe()"
) << "Invalid wall function specification" << nl
<< " Patch type for patch " << patch().name()
<< " must be wall" << nl
<< " Current patch type is " << patch().type() << nl << endl
<< abort(FatalError);
}
}



This compiles and runs fine in serial but not in parallel...

This is propably caused by differences between 3.0.0 and -dev branches, I'm not experienced enough to figure out the serial/parallel problem, sorry

[kingjewel1]

Hello Pekka,

Many thanks for your hard work. Could you clarify what the fundamental difference between your formulation and that by Erogov and Menter? Or between yours and the inbuilt OF version?

cheers

[zordiack]

This is the formulation by Egorov and Menter, and more specifically the later formulation described in the 2010 papers. Official OpenFOAM version is also using the Egorov and Menter formulation, but from year 2008. The main difference is in the calculation of Lvk term and also some constants have different values. There is no dramatic difference between the models in calculations (I think), I just wanted to use the model formulation from the more recent papers.

[be_inspired]

Should it work ok with extended version?
What about wall function and y+ requirements?
Did you validate the model against a cylinder test case?