
[Sponsors] 
May 10, 2008, 09:08 
or maybe...
Did you copy yo

#21 
Member
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8 
or maybe...
Did you copy your p, U, and phi files from a simpleFoam (incompressible) case? In which case your phi and pressure fields won't have the correct dimensions (they are divided by rho in the incompressible solvers). Try and copy those files from the rhoTurbFoam tutorial. 

May 12, 2008, 11:44 
Hi Niels and Patrick!
Thank y

#22 
New Member
Daniele Bonetti
Join Date: Mar 2009
Posts: 3
Rep Power: 8 
Hi Niels and Patrick!
Thank you for the quick answer. So far I've tried the simplest way so, as Patrick suggested, I used an initial condition derived from rhoTurbFoam and the solver seems to work indeed (at least it runs). I didn't modify the solver, I hope it wasn't necessary. Again, thanks a lot Daniele 

October 3, 2008, 13:08 
Good afternoon,
I'm using t

#23 
Senior Member
PierreOlivier Dallaire
Join Date: Mar 2009
Location: Montreal, Quebec, Canada
Posts: 185
Rep Power: 8 
Good afternoon,
I'm using the SpalartAllmaras model with simpleFoam and I need to clarify one thing regarding the inlet BC. I'm using the "standard" approximation ( (3/2)^0.5 U Iturb len ) for inlet/freestream and I want to be sure that I'm not confused netween nut and nuTilda : For inlet :  nuTilda = (3/2)^0.5 U Iturb len  nut = nuTilda / 5 Can somebody confirm that this is correct and not other way around (nut= (3/2)^0.5 U Iturb len and nuTilda = nut / 5) ? Best regards, PO 

October 3, 2008, 16:14 
Hi PO,
nuTilda is simply a

#24 
Member
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8 
Hi PO,
nuTilda is simply a 'scaled' nut, so that it is a linear function of the distance from the wall in the fully resolved inner layer (including the viscous sublayer). Away from the wall, nuTilda matches therefore nut. For a freestream BC in external aerodynamics, I would then specify the same values for nut and nuTilda. As far as I am concerned, I specify 1 <= nut/nu <=10 at the freestream boundary for a fully turbulent external flow (e.g., nut = nuTilda = 5 nu). Cheers, Patrick 

October 3, 2008, 16:33 
Thanks for the clarification P

#25 
Senior Member
PierreOlivier Dallaire
Join Date: Mar 2009
Location: Montreal, Quebec, Canada
Posts: 185
Rep Power: 8 
Thanks for the clarification Patrick, for some reason I was confused with nut and nu.
Have a good weekend PO 

January 2, 2009, 04:04 
HI EVERYONE
MY SELF NAVEE

#26 
Senior Member
NAVEEN.K.M
Join Date: Mar 2009
Location: Bangalore, Karnataka, india
Posts: 114
Rep Power: 8 
HI EVERYONE
MY SELF NAVEEN i am new to openfoam cfd software i am not able to solve the naca0012 airfoil case in openfoam ..can u please help me regarding this and if u r having any tutorial based on openfoam please send me... 

January 2, 2009, 08:36 
Hi Naveen
this is just the

#27 
Member
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8 
Hi Naveen
this is just the system directory where i have setted the properties of my solver in a very conservative way.  /** C++ **\  =========    \ / F ield  OpenFOAM: The Open Source CFD Toolbox   \ / O peration  Version: 1.5   \ / A nd  Web: http://www.OpenFOAM.org   \/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application simpleFoam; startFrom startTime; startTime 4000; stopAt endTime; endTime 8000; deltaT 1; writeControl timeStep; writeInterval 100; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; graphFormat raw; runTimeModifiable yes; // ************************************************** *********************** //  /** C++ **\  =========    \ / F ield  OpenFOAM: The Open Source CFD Toolbox   \ / O peration  Version: 1.5   \ / A nd  Web: http://www.OpenFOAM.org   \/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear limited 0.7; laplacian(nu,U) Gauss linear limited 0.7; laplacian((1A(U)),p) Gauss linear limited 1; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } // ************************************************** *********************** //  /** C++ **\  =========    \ / F ield  OpenFOAM: The Open Source CFD Toolbox   \ / O peration  Version: 1.5   \ / A nd  Web: http://www.OpenFOAM.org   \/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p PCG { preconditioner DIC; tolerance 1e08; relTol 0; }; U PBiCG { preconditioner DILU; tolerance 1e08; relTol 0; }; k PBiCG { preconditioner DILU; tolerance 1e08; relTol 0.1; }; epsilon PBiCG { preconditioner DILU; tolerance 1e08; relTol 0.1; }; R PBiCG { preconditioner DILU; tolerance 1e08; relTol 0.1; }; nuTilda PBiCG { preconditioner DILU; tolerance 1e08; relTol 0.1; }; } /* k BICCG 1e06 0; epsilon BICCG 1e06 0; R BICCG 1e06 0; nuTilda BICCG 1e06 0; */ SIMPLE { nNonOrthogonalCorrectors 2; } PISO { nCorrectors 1; nNonOrthogonalCorrectors 1; /* pRefCell 0; pRefValue 0;*/ } relaxationFactors { p 0.3; U 0.7; k 0.5; epsilon 0.5; /* R 0.7;*/ nuTilda 0.7; } // ************************************************** *********************** // actually the spalartallmaras model uses two different files, nut and nuTilda. To have a very low freestream turbulence i have setted nut=1e12 and nuTilda=0.077e5. The BC of nut and nuTilda are zero gradient everywhere but the inlet (where you put your freestream value) I hope this will help 

January 3, 2009, 09:28 
Hello Hi Hello Hi!
Happy ne

#28  
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
Hello Hi Hello Hi!
Happy new year! A question concerning DES. Quote:
And what about nut? Another question, has DDES been implemented? Thanks Daniel
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

January 4, 2009, 08:26 
if you look at the SpalartAll

#29 
Member
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8 
if you look at the SpalartAllmaras model you will see directly the definition of nut and nuTilda. If you want a very low freestream turbulence you can derive the simple relation
nuTilda=nu*4.349*(nut/nu)^0.25 where nu is you kinematic viscosity and the ratio nut/nuTilda is the ratio between the turbulent viscosity and the real viscosity 

January 10, 2009, 11:23 
wow, sorry for that. Daniel

#30 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
wow, sorry for that. Daniel
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

January 12, 2009, 01:44 
Hi Daniel,
is there a chanc

#31 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10 
Hi Daniel,
is there a chance to put the model to the wiki page: http://openfoamwiki.net/index.php/Sig_Turbulence_/_Collection_of_additional_turb ulence_models Would be a nice start :) Fabian 

January 12, 2009, 03:56 
Actually, I did nothing but co

#32 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
Actually, I did nothing but copy SpalartAllmaras to SpalartAllmaras2, and defined a function fd(), and redifine the dTilda_ as Spalart said, Please pardon me for I really feel ashamed to put a crude code like that to the wiki.
Could anybody give me some hints on the error I met? Then the SpalartAllmaras2 will looks more stylishly. If not, the alternative for me now is to simplly copy SpalartAllmaras to SpalartAllmaras2 and do just as what I have mentioned above. Using this SpalartAllmaras2, I calculate a flat plat with at high incidence, Re is 20000, the following are my findings: 1. I got better results using pure 2DRANS, SpalartAllmaras than the original reference paper. See the grid I used, 2. I tried to mapFields to 3DDES case, using oodles, and it took a long time to get a good Cd and Cl number, I think the 3D flow field is already setup. So then I continue to calculate it in both methods, namely DES and DDES, and began to use fieldAverage utility. The simulation is still going now, and they are so far so good. 3. See the picture below, This is why I think a max(deltaX, deltaY, deltaZ), should be written besides cubicRootVol for the following two reasons: a) the bad nuSgs field as the places where mesh are refined (using cubicRootVol). b) At least some DES test cases will use Z direction mesh lenth as a simple control of "RANS region". Any ideas? Daniel
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

January 23, 2009, 14:33 
Daniel,
It's very interesti

#33 
Member
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8 
Daniel,
It's very interesting that you share your DDES implementation. I'm working on that too and I encountered some problems. Even if the modification to the SpalartAllmaras DES model looks quite minor, it is a significant change to use the solution (mag(gradU)) in the definition of dTilda. I would be interested to see your whole spalartAllmaras2.c file because I can't compile the formulation you posted before. Maybe I missed something obvious. How exactly did you manage to run your DDES case while you have an error message? 

February 6, 2009, 09:30 
Going back to nut and nuTilda

#34 
Senior Member
David Boger
Join Date: Mar 2009
Location: Penn State Applied Research Laboratory
Posts: 146
Rep Power: 8 
Going back to nut and nuTilda for a moment... It's not clear to me why both quantities should be specified in the 0/ directory. For SpalartAllmaras, nuTilda is the unknown variable, and nut is derived from nuTilda, right? Why are both specified as if they are independent at the boundaries?
Thanks, David
__________________
David A. Boger 

February 6, 2009, 10:56 
Actually they give different i

#35 
Member
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8 
Actually they give different informations. They are related but not the same. nut is the effective turbulent viscodity while nuTilda is the solved variable that is proportional to nut with a coefficient fv1 that is variable, depending on the strength of the turbulence compared with viscous effects (csi). You can see this directly in this site where you can see some details of the model
http://www.cfdonline.com/Wiki/SpalartAllmaras_model 

February 6, 2009, 12:51 
Good morning,
Still, nut=nu

#36 
Member
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8 
Good morning,
Still, nut=nuTilda*fv1 and fv1 is a function of nuTilda only (with nu and Cv1 being constants), so I agree with David that is seems redundant to specify both quantities at the boundaries, isn't? Philippe 

February 6, 2009, 14:23 
I guess you specify them both

#37 
Member
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8 
I guess you specify them both to have a "universal" hookup of the turbulence models. nut is needed first because momentum equations are solved first, then turbulence quantity/ies is/are solved for after the pressure equation: if it's the SA model, you solve for nuTilda which allows you to update the nut field. You need to store both fields, nut will be needed for the next momentum predictor and nuTilda will be needed to initialize the next iterative solution of nuTilda. If you build a solver relying exclusively on the SA model, you could get away by storing only one field. However OpenFOAM standard solvers assume various turbulent models can be hooked up. The nut and nuTilda files are here for the sake of generality of the solver.


February 6, 2009, 15:31 
Thanks guys. I think what I'm

#38 
Senior Member
David Boger
Join Date: Mar 2009
Location: Penn State Applied Research Laboratory
Posts: 146
Rep Power: 8 
Thanks guys. I think what I'm hearing (here and offline) is that it's a "simple matter of programming," as Patrick is pointing out. As to Patrick's point, I'd argue that a better "universal" way would be to never specify nut but instead to always and only specify the solution variables (k and epsilon or k and omega or nuTilda, etc.). The solvers would then need to calculate nut first from these specifications to provide for the momentum predictor.
I guess I'll need to dig into the code to see whether there's a compelling reason to do it this way. It was just bugging me to "specify" boundary conditions on a derived quantity like this.
__________________
David A. Boger 

March 12, 2009, 22:54 
Hi, Philippe! Morning!
I di

#39 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
Hi, Philippe! Morning!
I did not get converged with my flat plate case. It's annoying to specify the B.C., Could you share how you set the B.C.? I think I have finished my channelOodles with DES and DDES, and they looks fine and interpretable, so I will stop here and move to next case and IDDES (seems not very complicated).
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

March 13, 2009, 06:15 
Hi..friends,
I am testing tur

#40 
Member
Join Date: Mar 2009
Posts: 39
Rep Power: 8 
Hi..friends,
I am testing turbulent subsonic(0.3Ma) viscous compressible(air) flow over an airfoil naca0012 with grid type otopology.I am using SpalartAllmaras model for modeling turbulence. I am confuse about the declaration of BC values for 0/nuTilda and 0/mut as well as BCtype at airfoil for the same. Thanks for suggestion!! 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SimpleFoam case with SpalartAllmaras turbulence model implemented  nedved  OpenFOAM Running, Solving & CFD  2  November 30, 2014 23:43 
Bug in SpalartAllmaras  seb62  OpenFOAM Bugs  39  May 30, 2012 14:25 
SpalartAllmaras DES question  ivan_cozza  OpenFOAM Running, Solving & CFD  0  December 15, 2008 07:34 
YPlus for SpalartAllmaras  ddigrask  OpenFOAM Running, Solving & CFD  1  December 12, 2008 15:29 
Pow in lib64tlslibmso6 SigFpe when running coodles with SpalartAllmaras  lillberg  OpenFOAM Bugs  4  December 7, 2007 09:17 