
[Sponsors] 
February 21, 2011, 08:18 
fvSchemes

#1 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6 
Hi all!
I have been using OpenFOAM for 2 months, so I am quite new with this software. I am using it to do a study in 2D of the flow over a NACA0015, at Re=2x10^6 at steady state. Using simpleFoam and the komega SST turbulence model. I have been doing a sensitivity study of the numerical schemes. Thus, I have been changing the divSchemes. I have tried changing all the entries in there to QUICK/QUICKV, linear, linearUpwind and upwind. I couldn´t change the entry "div((nuEff*dev(grad(U).T())))" to any of those (I have to keep at as linear, otherwise the programme does not recognize it), why? I have upload the file fvSchemes used so you can have a look at it. I have also uplodaded a figure showing the results obtained compared with a reference. They do not look as expected since the closest solution obtained for the lift coefficient calculations is for the upwind numerical scheme, while this one should give the worst results, shouldn´t it? Thank you for your attention. I will really appreciate your help. Regards, José 

February 21, 2011, 08:23 

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,768
Rep Power: 21 
It does not recognise it because this is a straightforward div(thing) term and not convection div(phi, thing).
Therefore you cannot do upwinding, since there's no flux to decide the direction from. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

February 21, 2011, 08:30 

#3 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6 
Thank you very much. It makes sense
Any suggestion for the results presented? Using such a fvSchemes file? 

February 21, 2011, 08:33 

#4 
Senior Member

1. To change the scheme for "div((nuEff*dev(grad(U).T())))" you should define the flux variable by hand (see the User Guide p. 112 for interpolation schemes)
2. There are issues regarding wrong calculation for the viscous term for komega SST in OF on this forum. Its is different from other model for the value of sqrt(2). Perhaps that is the case for your comparison witrh reference solution. 3. "Gauss linear limited 1;" in your laplacian section is the same as "Gauss linear corrected;"
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

February 21, 2011, 08:41 

#5 
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 9 
Hello, José,
these are pretty neat results you have there. It is interesting to see how different divergence schemes affect the results. However, did you perfom a grid sensitivity analysis when you compare your results? It would be a bit more meaningful if you'd analyze how the discretization error of each scheme is reduced when grid spacing is e.g. halfed. The good reproduction of experimental data of lift coefficient when using upwinding really is surprising, but I wouldn't say upwinding is more accurate in this case. Especially at high lift coefficients separation occurs and this is where the choice of turbulence modeling becomes much more important than in attached cases. My guess is that kOmegaSST is not able to reproduce the separation at high angle of attacks of this airfoil, but the increased diffusivity caused by using a first order scheme like upwinding sort of "accidently" corrects this shortcoming. A comparison using different turbulence models (SpalartAllmaras or LowReKEpsilon) would make sense, but it of course also means many more simulations. Greetings, Felix. 

February 21, 2011, 08:56 

#6 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6 
Thank you for your answers. Comments to Alex´s reply:
1) I will have a look at it. 2) I already corrected this issue. 3) Ok. Comments to Felix´s reply: I had already thought on that but I don´t know if I will have time enough to see this (I am doing a master thesis...). Good to know that this can be coincidence. I will have a look at it! I was advised to use komega SST since it was predicting better the stall region. I also did some computations previously using Spalart Allmaras but the results obtained were very similar. Anyway...I may check other turbulence models. Thank you for your help. More suggestions are very welcome. Regards, José 

February 23, 2011, 02:17 

#7  
New Member
Alexandre Rubel
Join Date: Dec 2010
Location: Launceston, Tasmania AUSTRALIA
Posts: 28
Rep Power: 6 
Hi all,
I'm using simpleFoam with kOmegaSST and I get accuracy issues with my Drag coefficient. Can you tell me more about what you said Alex : Quote:


February 23, 2011, 03:57 

#8 
Member
Alex
Join Date: Apr 2010
Posts: 32
Rep Power: 7 
There was a bug in the kOmegaSST model regarding the computation of nut (missing sqrt(2)). This was fixed on 12 November 2010 in the git repository of OpenFOAM1.7.x.
So you have to check your version. If you have 1.6.x or 1.7.1, then you have to fix the bug yourself. You can check the files and fix here: https://github.com/OpenCFD/OpenFOAM...f7a0b26d64265d Good luck, Alex (another one) 

February 23, 2011, 04:02 

#9 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6 
there you are Alex I:
Wrong calculation of nut in the kOmegaSST turbulence model 

February 23, 2011, 05:57 

#10 
New Member
Alexandre Rubel
Join Date: Dec 2010
Location: Launceston, Tasmania AUSTRALIA
Posts: 28
Rep Power: 6 
Thanks that's good to know, I got the 1.6.8 version I think.
I hope this will lead to improvement in my case. Anyway, here is the link of my topic maybe you can help me : Submarine with SimpleFoam Alex 

May 24, 2011, 15:19 
anything about div(thing)

#11  
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 553
Rep Power: 18 
Quote:
I just had a simple question about the div((nuEff*dev(grad(U).T()))) term in fvSchemes for a simpleFoam simulation. I know that one cannot just use Gauss upwind since there is no flux and the direction of flux is not known. One can simply provide a phi as div((nuEff*dev(grad(U).T()))) Gauss upwind phi 1; Is this correct and usable? I ask because the default is linear and I thought that the cell Peclet number would have an effect (lead to unbounded results for this term) for central differencing...hence why upwinding with a prescribed phi=1 would be better. What is a good 1st order scheme and a good second order scheme...or should Gauss linear always be sufficient for div(thing) terms? Thanks for your help. Dan 

May 24, 2011, 23:16 

#12 
New Member
Oky Andytya
Join Date: Nov 2010
Posts: 26
Rep Power: 7 
Hi everyone,
I need help, how to get the value of convection coefficient [h] from Fluent directly? Thank you. Regrads, Oky 

May 24, 2011, 23:25 

#13  
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 553
Rep Power: 18 
Quote:
http://www.cfdonline.com/Forums/ansys/ 

May 25, 2011, 02:52 

#14 
Senior Member

Dan,
you can use predefined flux to use the upwind scheme for your diffusion term. I didn't find any advantages applying this approach and usually your convection term produces unboundedness not the diffusion one.
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

May 25, 2011, 10:42 

#15  
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 553
Rep Power: 18 
Quote:
Dan 

August 30, 2013, 04:01 
Gauss linear corrected

#16 
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 5 
Hi Dr. Alexander
i need formulation of Gauss linear corrected. but i dont found it! please can you help me? 

August 30, 2013, 04:04 

#17 
Senior Member

Pardon, what do you need and for which term (diffusive, convective)?
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

August 30, 2013, 04:19 

#18  
Member
xuheopenfoam
Join Date: Aug 2013
Location: DaLian，china
Posts: 82
Rep Power: 4 
Quote:
{ default none; div(phi,U) Gauss QUICKV cellLimited Gauss linear 1; div(phi,k) Gauss QUICK cellLimited Gauss linear 1; div(phi,omega) Gauss QUICK cellLimited Gauss linear 1; div((nuEff*dev(grad(U).T()))) Gauss linear cellLimited Gauss linear 1; } The above is your divschemes. Does the number "1" in every schemes indicate the nonorthogonal correction? thank you! 

August 30, 2013, 04:26 

#19 
Senior Member

From User Guide: Some TVD/NVD schemes require a coefficient ψ, 0 ≤ ψ ≤ 1 , where ψ = 1 corresponds to TVD conformance, usually giving best convergence and ψ = 0 corresponds to best accuracy. Running with ψ = 1 is generally recommended
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

August 30, 2013, 07:02 

#20 
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 5 
thanks
yes i need it for diffusive : laplacian(muEff,U) Gauss linear corrected i need the formulation of corrected snGradient.i see Hrvoj.jasak thesis but I could not find it... please help me 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
fvschemes and fvsolutions in MRFSimpleFoam  renyun0511  OpenFOAM Running, Solving & CFD  23  August 3, 2011 04:07 
OpenFOAM fvSchemes: laplacianScheme,  thomek  Main CFD Forum  1  October 18, 2010 05:17 
Implementation issues of fvSchemes / laplacianScheme, in particular gaussLaplacianSch  thomek  OpenFOAM Programming & Development  0  October 18, 2010 05:10 
General help for fvSchemes and fvSolution settings  harly  OpenFOAM Running, Solving & CFD  4  September 7, 2009 10:31 
Doubt in term representation in the fvSchemes dictionary  titio  OpenFOAM Running, Solving & CFD  0  July 17, 2009 13:21 