CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   V2f turbulence model (http://www.cfd-online.com/Forums/openfoam-solving/58440-v2f-turbulence-model.html)

qtian December 26, 2007 15:50

Hello, all, Do we have v2-f
 
Hello, all,

Do we have v2-f turbulence model implemented in OpenFoam? I checked turbulence models in src/turbulencemodel folder and there is no such model. However, I searched message board and some folks discussed the implementation of v2f model in 2005. Am I missing anything? My version is 1.4.

Thanks.

Quinn

msha December 27, 2007 07:08

Not really Foam doesn't hav
 
Not really

Foam doesn't have this model

michele January 7, 2008 06:01

Quinn, here you will find an
 
Quinn,
here you will find an implementation of v2f (Lien/Kalitzin a.k.a. code-friendly version) I made a couple of years ago.
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif DurbinV2F.tar.gz
It is not fully tested, so use at your own risk...
As a tutorial test (BC and configuration example), herebelow you find a configuration for the asymmetric diffuser, in which the v2f model is known to predict quite well separation/reattachment. No grid is included.
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif diffuser_V2F_noMesh.tar.gz
Herebelow a plot of velocity/streamlines
http://www.cfd-online.com/OpenFOAM_D...ges/1/6321.gif
A comparison with experimental friction coefficient is given below
http://www.cfd-online.com/OpenFOAM_D...ges/1/6322.gif
From the Cf plot you can see the separation/reattachment points on the bottom wall...
Separation occurs at x/H=5 for v2f and at about 7 experimentally.
Reattachement occurs at x/H=29 for v2f and at about 29 experimentally.

Regards,
Michele.

qtian January 7, 2008 11:17

hi, Rattin, It is great. Th
 
hi, Rattin,

It is great. Thanks for sharing this model with me. I am doing three dimensional separated flow simulation now and want to try all different kind of turbulence models to see how good is the prediction.

qtian January 23, 2008 17:40

Dear Rattin, I am reading
 
Dear Rattin,

I am reading the v2f model you sent me. would you mind to answer a few questions for me about this v2f model?

Is this v2f model from Davidson's v2f model? Can you please give me a reference? What is the coefficient yStarLim for? I did not see this parameter in the durbin's version?

Thanks

QT

michele January 29, 2008 05:43

Quinn, sorry for the late r
 
Quinn,
sorry for the late reply, I was abroad last week.
Here attached you will find a small reference for the model implemented:
http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif v2f_description.pdf
The models includes the Davidson modifications and a limiter switch for time (T) and length (L) scales (Kolmogorov scales).
In this way the limiter is always active if you set yStarLim to a large number (say 10e+10), is never active if you set yStarLim to zero and is active partially if you set to, say, 30. The last case is consistent with the validity of the theoretical Kolmogorov microscales in the near-wall region.
Hope this helps.
P.S. v2f requires to mesh the near-wall region up to y<sup>+</sup><1, like any low-Re turbulence model.

Regards,
Michele.

qtian January 29, 2008 10:22

Michele, Thanks you so much
 
Michele,

Thanks you so much for your help and suggestions. I have completed my simulation. The results from v2f are awesome. This is the best results after I tried a number of turbulence models.

michele January 30, 2008 06:22

Quinn, I'm glad that the info
 
Quinn,
I'm glad that the info were useful, and I hope you will make available to the forum the experience/results once completed the study.

Michele

sek February 20, 2008 14:21

Hi Michele, Can you please
 
Hi Michele,

Can you please tell me how you computed and plotted in OpenFOAM or any package the skin-friction coefficient along the wall for your diffuser case?

sek February 20, 2008 14:53

Hi Michele, Can you please
 
Hi Michele,

Can you please tell me how you computed and plotted in OpenFOAM or any package the skin-friction coefficient along the wall for your diffuser case?

braennstroem April 14, 2008 09:27

Hi Rattin, as you wrote, yo
 
Hi Rattin,

as you wrote, you implemented the Davidson modifications. I assume you mean Lars Davidson and you 'just' implemnted the first modification. Do you have an idea, how to implenent the second modification, i.e. using different turbulent viscosities for different compononts?

Greetings!
Fabian

anger April 30, 2008 07:17

Hi Michele, in the turbulen
 
Hi Michele,

in the turbulenceProperties file of your V2F- example, there is also an entry for the constants of a k- Omega model. Can the implementation of this model be found somewhere in the forum or on sourceforge?

Best regards,
-Thomas

michele April 30, 2008 08:14

Thomas, the k-w model availab
 
Thomas,
the k-w model available in the OpenFOAM release is the SST version.
You may also want to try the SAS modification (and several other models), available at
http://openfoamwiki.net/index.php/Turbulence_Modeling
for download.

The k-w properties you found inside the dictionary refer to an implementation I made a couple of years ago (at the time the k-w model was not yet implemented in the OpenFOAM distribution).
If you are interested, I may pack the k-w models I implemented (little testing has been made).
The particularities of the models are:
- Wilcox k-w with and without the transitional modification
- consistent treatment of the wall region ("Model-consistent universal wall-function" - Knopp)
- rough surfaces (whose equivalent sand-roughness may be specified on a patch-by-patch basis)

Regards,
Michele.

anger April 30, 2008 09:53

Michele, thanks for the hin
 
Michele,

thanks for the hint to the wiki.
Do you have any references for the transitional modification of the k-w model you mentioned?

Best regards,
-Thomas

michele April 30, 2008 10:52

Thomas, the transitional modi
 
Thomas,
the transitional modification is needed when you want to analyse laminar-to-turbulent boundary layer transition (turbulence models tipically predict transition at Reynolds numbers at least one order of magnitude too low...).
The transitional modifications are discussed in the Wilcox's book "Turbulence modeling for CFD".

Regards
Michele.

anger May 21, 2008 03:24

Hello Michele, I downloaded
 
Hello Michele,

I downloaded the k-w models and compiled them (after changing volTensorField to volSymmTensorField for R) but trying to run the k-w model gave an error:

Selecting incompressible transport model Newtonian
Selecting turbulence model kOmega


--> FOAM FATAL ERROR : LHS and RHS of + have different dimensions
dimensions : [0 0 -1 0 0 0 0] + [0 2 -3 0 0 0 0]
#0 Foam::error::printStack(Foam:: Ostream&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::operator+(Foam::dimensionSet const&, Foam::dimensionSet const&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 Foam::tmp<foam::geometricfield<double,> > Foam::operator+<foam::fvpatchfield,>(Foam::Geometr icField<double,> const&, Foam::dimensioned<double> const&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libincompressibleTu rbulenceModels.so"
#4 Foam::turbulenceModels::kOmega::kOmega(Foam::Geome tricField<foam::vector<double> , Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::transportModel&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libincompressibleTu rbulenceModels.so"
#5 Foam::turbulenceModel::adddictionaryConstructorToT able<foam::turbulencemodels::k omega>::New(Foam::GeometricField<foam::vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::transportModel&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libincompressibleTu rbulenceModels.so"
#6 Foam::turbulenceModel::New(Foam::GeometricField<fo am::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::transportModel&) in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/lib/linux64GccDPOpt/libincompressibleTu rbulenceModels.so"
#7 main in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/applications/bin/linux64GccDPOpt/simple Foam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 Foam::regIOobject::readIfModified() in "/home/anger/OpenFOAM/OpenFOAM-1.4.1-dev/applications/bin/linux64GccDPOpt/simple Foam"


From function operator+(const dimensionSet& ds1, const dimensionSet& ds2)
in file dimensionSet/dimensionSet.C at line 385.

FOAM aborting (FOAM_ABORT set)

It seems that there gets something messed up with w and epsilon, but I have no idea where this could come from. Did you experience similar behaviour in one of your implementations and could you solve it?

Best regards,
-Thomas

michele May 21, 2008 05:34

Thomas, no problems on my imp
 
Thomas,
no problems on my implementations.

I suspect there may be an error in the source code.
Enstropy has frequency units.
I never tried this SAS implementation.
In the laminarOmega.H code seems to lie the error:

dimensionedScalar
(
"omega", sqr(U_.dimensions())/dimTime, 0.0
)

At a first glance you may change the above with:
dimensionedScalar
(
"omega", dimless/dimTime, 0.0
)

Now I have no possibility to try it... so may you try this for me and let me know.

Regards,
Michele.

anger June 10, 2008 01:32

Hello Michele, your above m
 
Hello Michele,

your above mentioned fix did not do the trick. I assume that you did the turbulence models implementation for an older version than 1.4.1-dev. I decided to take the SST- model provided with OF and modify it using your implementation as template to program the standard k-w model which seemed to work.
I was now trying to implement the k-w model with transitional behaviour but ran into problems with some of the terms. You mentioned that you have implemeted this. Would you be so kind to share this implementation so that I can again use it as template?

Best regards,
-Thomas

braennstroem August 10, 2008 06:09

Hi Michele, I am just tryin
 
Hi Michele,

I am just trying to implement the zeta-f model, which is based on v2f by zeta=v2/k. For this I read in the thesis of Popovac http://repository.tudelft.nl/file/354721/370010, that the boundary condition for f should be similar implemented as for epsilon. I wonder, if there is a reason, tha you did not use it!? Was it more unstable?


Regards!
Fabian

braennstroem August 10, 2008 06:28

... one more question: for wh
 
... one more question:
for what, does one need pos(yStarLim-yStar_) for the calculation of T and L?

Fabian


All times are GMT -4. The time now is 06:32.