# Turbulent flow in a rectangular duct foam vs fluent

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 29, 2006, 20:26 I am simulating a turbulent fl #1 atzaru 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(1|A(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: 12 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 atzaru Guest   Posts: n/a hello thanks for your reply 1 - in both programs Foam and Fluent I used the basic k-epsilon 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 k-eps 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: 12 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 k-epsilon 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: 1,894 Rep Power: 26 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 live DVD/USB, hard drive image and virtual image. OpenQBMM - An open-source implementation of quadrature-based moment methods

 February 3, 2006, 06:01 Unfortunately/fortunately that #6 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 12 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: 1,894 Rep Power: 26 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 live DVD/USB, hard drive image and virtual image. OpenQBMM - An open-source implementation of quadrature-based moment methods

 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: 8 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 Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Hock Ming FLUENT 0 February 7, 2009 21:25 Watchapon Main CFD Forum 0 April 7, 2007 07:34 ken FLUENT 4 May 26, 2005 20:39 Yogesh FLUENT 0 March 27, 2005 01:36 Bastian FLUENT 0 July 2, 2004 08:51

All times are GMT -4. The time now is 15:54.