
[Sponsors] 
January 29, 2006, 20:26 
I am simulating a turbulent fl

#1 
Guest
Posts: n/a

I am simulating a turbulent flow in a square duct (0.2*0.2*6) in foam and fluent. I am concern about the velocity distribution difference between the two programs.
Reynolds number around 11 000. in fluent i obtain a max velocity around 1.24 while in Foam the max velocity is 1.14. Does anybody know why and how i can correct this? in both programs i introduced the same inlet (velocity, V=1m/s), the same initial k and epsilon, and outlet condition. turb_flow_v2.tar.gz ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default Gauss <>; 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 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; } The boudary condition are: ( wall { type wall; physicalType wall; startFace 97040; nFaces 6720; } outlet { type patch; physicalType pressureOutlet; startFace 103760; nFaces 400; } inlet { type patch; physicalType inlet; startFace 104160; nFaces 400; } ) 

January 30, 2006, 08:25 
What does the experimental dat

#2 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
What does the experimental data say?
From what information you provided I would guess the source of inconsistency is either the turbulence model or the wall function. Please post which turbulence models and wall options you used for Fluent and Foam. Also, what is your y+ value. 

February 2, 2006, 11:51 
hello
thanks for your reply

#3 
Guest
Posts: n/a

hello
thanks for your reply 1  in both programs Foam and Fluent I used the basic kepsilon equations 2 the standard wall functions based on launder and spalding is used in both cases (the same Constants E =9.0 and kappa=0.4187) 3 The same keps coeff have been used cmu=0.009, c1=1.44, c2=1.92. I do not know why in Foam we do not have Tke=1 and TDR=1.3 but a coeff alphaEps = 0.7692. What is this coeff? 4 The y+ is 24 5 For the moment i do not have experimental data to compare with. It is strange i obtain so different results. 

February 2, 2006, 12:08 
If you are using log the law o

#4 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
If you are using log the law of the wall it is not valid at y+ = 24. My best guess is that fluent does something clever to improve at these intermediate values.
For Foam y+ needs to be around 100 with the standard kepsilon model. 

February 2, 2006, 14:28 
FLUENT has different requireme

#5 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27 
FLUENT has different requirements for its wall functions, according to its manual (30 < y+ < 60).
Also, in the OpenFOAM case files there is an error: in the 0\k dictionary the condition at the wall should be wall { type zeroGradient; } instead of wall { type fixedValue; value uniform 0; } However it's strange that OpenFOAM 1.2 starts the calculation because it should quit and tell you the error. Best regards, Alberto
__________________
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. 

February 3, 2006, 06:01 
Unfortunately/fortunately that

#6 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
Unfortunately/fortunately that is one of the features of OpenFOAM. It allows you complete freedom in choosing individual boundary conditions, but at the same time, it wont tell you if you make an unwise choice.


February 3, 2006, 11:04 
Sorry, I wasn't clear. I disco

#7 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27 
Sorry, I wasn't clear. I discovered the error because trying to run the case with a grid I did, OpenFOAM 1.2 told me the problem in the BC ;)
Regards, Alberto
__________________
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. 

February 13, 2007, 15:42 
Well... So the problem was jus

#8 
New Member
Cesar Belaunde Zarate
Join Date: Mar 2009
Location: Quillota, V region, Chile
Posts: 8
Rep Power: 9 
Well... So the problem was just de grid ? it's the same mesh for both programs?
Another questions... What is the BC ? And what represent de y+ value ? thanks. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Turbulent Flow in a Square Duct using LES  Hock Ming  FLUENT  0  February 7, 2009 21:25 
Turbulence flow in a rectangular duct  Watchapon  Main CFD Forum  0  April 7, 2007 07:34 
Turbulence Model for Rectangular Duct Flow  ken  FLUENT  4  May 26, 2005 20:39 
3D rectangular duct flow UDF  urgnet  Yogesh  FLUENT  0  March 27, 2005 01:36 
laminar viscous flow in a rectangular duct  Bastian  FLUENT  0  July 2, 2004 08:51 