
[Sponsors] 
October 18, 2007, 09:57 
Hello,
Looking at the UserG

#1 
Member
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 10 
Hello,
Looking at the UserGuide, it's something I should be able to do. I want to use the linear Upwind scheme for div(phi,U). Using simpleFoam in Openfoam 1.4.1 on linux 64bit. div(phi,U) Gauss linear; div(phi,U) Gauss linear corrected; div(phi,U) Gauss QUICK; works fine. But div(phi,U) Gauss linearUpwind; does not. I get: > FOAM FATAL IO ERROR : Grad scheme not specified Valid grad schemes are : 8 ( cellMDLimited extendedLeastSquares faceMDLimited leastSquares fourth faceLimited cellLimited Gauss ) file: /home/nr/OpenFOAM/nrousselon1.4.1/run/ccm2foam4/system/fvSchemes::div(phi,U) at line 40. From function gradScheme<type>::New(Istream& schemeData) in file /home/nr/OpenFOAM/OpenFOAM1.4.1/src/finiteVolume/lnInclude/gradScheme.C at line 65. FOAM exiting /**\  =========    \ / F ield  OpenFOAM: The Open Source CFD Toolbox   \ / O peration  Version: 1.4   \ / A nd  Web: http://www.openfoam.org   \/ M anipulation   \**/ FoamFile { version 2.0; format ascii; root ""; case ""; instance ""; local ""; 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 linear corrected; 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 corrected; laplacian((1A(U)),p) Gauss linear corrected; 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; } // ************************************************** *********************** // 

October 18, 2007, 10:13 
You need to specify the grads

#2 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
You need to specify the gradscheme used by linearUpwind, e.g.
div(phi,U) Gauss linearUpwind Gauss linear; or div(phi,U) Gauss linearUpwind leastSquares; or if you want to limit the gradient used by the linearUpwind scheme which is often beneficial div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1; etc. 

October 24, 2007, 07:18 
Thanks,
just what I needed.

#3 
Member
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 10 
Thanks,
just what I needed. Nicolas 

January 18, 2010, 10:45 

#4  
Member
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 9 
I have the same problem and tried to adapte it on my case with the bouyantBoussinesqSimpleFoam, but it didn't work.
This is what I get: Quote:
Quote:


January 19, 2010, 05:11 

#5 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,803
Rep Power: 24 
You messed up the order: cellLimited is a modifier for a gradient scheme, so it comes first. Think about which class should contain which.
div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1; Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 22, 2010, 04:26 

#6 
Member
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 9 
Hi Hrvoje,
thank you. Stupid mistake. Now it's running! :) Regards, Erik 

September 26, 2010, 15:55 

#7 
Senior Member
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 11 
Hello!
I got a question. Does div(phi,U) Gauss linearUpwind fourth mean that with order fourt the velocity field is approximated? Cheers 

September 27, 2010, 03:07 

#8 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
No, it means you use a fourthorder scheme to compute the gradients, but clearly the order of the linearUpwind stays unchanged.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 27, 2010, 03:31 

#9 
Senior Member
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 11 
I think I have to learn something. Could you send me a reference which contains the derivation of this kind of scheme?


February 21, 2011, 08:21 

#10 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 8 
Could you please have a look at this thread I just created?
http://www.cfdonline.com/Forums/ope...fvschemes.html thanks! 

November 12, 2011, 11:53 
fvSchemes in OF20

#11 
New Member
Jozsef Rideg
Join Date: Feb 2011
Location: Budapest, Hungary
Posts: 21
Rep Power: 8 
"
div(phi,U) Gauss linearUpwind Gauss linear; or div(phi,U) Gauss linearUpwind leastSquares; or if you want to limit the gradient used by the linearUpwind scheme which is often beneficial div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1; etc.[/QUOTE]" Does anyone know, how should the same fvSchemes be set in the 2.0 version of OpenFOAM? 

November 12, 2011, 16:16 

#12 
Senior Member

Hi!
Code:
gradSchemes { default cellLimited leastSquares 1; } divSchemes { default none; div(phi,epsilon) Gauss linearUpwind grad(epsilon); // OF20x syntax div(phi,k) Gauss linearUpwind grad(k); // OF20x syntax div(phi,U) Gauss linearUpwind grad(U); // OF20x syntax div((nuEff*dev(T(grad(U))))) Gauss linear; // OF20x syntax }
__________________
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 

November 14, 2011, 13:16 

#13 
New Member
Felipe
Join Date: Apr 2010
Posts: 13
Rep Power: 9 
Could you help me with this:
Implementing: laplacian(nuEff,U) Gauss linear Gauss fourth; gives: [0] > FOAM FATAL IO ERROR: [0] Unknown discretisation scheme fourth Valid schemes are : 3 ( corrected limited uncorrected ) but it should be able to work with fourth... Thanks 

November 14, 2011, 13:21 

#14  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
Gauss <scheme> <correction option>; so Gauss linear corrected; For fourthorder it is: Gauss cubic corrected; Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 14, 2011, 14:02 

#15 
New Member
Felipe
Join Date: Apr 2010
Posts: 13
Rep Power: 9 
Thanks Alberto for your reply
Now it is running, so I hope my solution will improve. Thanks Felipe 

November 14, 2011, 17:39 
Thanks

#16 
New Member
Jozsef Rideg
Join Date: Feb 2011
Location: Budapest, Hungary
Posts: 21
Rep Power: 8 

November 14, 2011, 18:00 

#17 
New Member
Felipe
Join Date: Apr 2010
Posts: 13
Rep Power: 9 
Hi again Alberto
Well my simulation ran, but I guess I have not achieved what I wanted. In the attached graph I have made the simulations from 0 to 20 degrees with a step of 2 degrees with OpenFOAM and another CFD code. I want to use the QUICK scheme, but I am over predicting my solution with OF in comparison to the other CFD code and both over predict lift in comparison to the measurements (Abbot and Doenhoff). I have my convection terms with QUICK and the diffusion terms with second order scheme (Gauss linear corrected). Thus I change my diffusion terms to a fourth interpolation scheme in order to improve my solution (QUICK2), and I can see that the curve is lower, but still it can not capture the separation pretty well. In this case my diffusion terms are Gauss cubic corrected. Do you have any suggestions for improving my results? Regards Felipe ps: I was going to upload the case but due to the size, it did not let allow me to do it. But I could send you a tar file with it (2.7 MB). 

November 15, 2011, 10:25 

#18 
Senior Member

Which OF version do you use?
__________________
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 

November 16, 2011, 02:10 

#19 
New Member
Felipe
Join Date: Apr 2010
Posts: 13
Rep Power: 9 
I use 1.7.1


November 16, 2011, 03:28 

#20 
Senior Member

Ok, because in 20x I noticed strange behavior: viscous terms are underestimated in my case with equal settings I was simulating in v16 and 17x. I will study it in details and also report here on forum.
__________________
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
DivSchemes Gauss limitedLinearV and interfaceCompression  nicasch  OpenFOAM Running, Solving & CFD  1  July 12, 2010 10:26 
FvSchemes  sega  OpenFOAM Running, Solving & CFD  2  February 15, 2010 12:07 
DivSchemes limitedLinearV and interfaceCompression  nicasch  OpenFOAM  0  February 28, 2008 11:33 
Divschemes limitedLinearV 1 and interfaceCompression  nicasch  OpenFOAM  0  February 27, 2008 13:24 
FvSchemes from 12 to 11  fedegavo  OpenFOAM Running, Solving & CFD  1  January 20, 2006 14:49 