# Wing Aerodynamics Fluent OF 15 comparison

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

 February 16, 2009, 10:57 Hi FOAMers! In order to fin #41 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 14 Hi FOAMers! In order to find a proper case set up, I am considering a wing with an AoA = 8°, that it is easier to simulate and has not problem with flow detachment. After trying different schemes combinations, I applied: - gradSchemes: faceMDLimited Gauss linear 0.5 - divSchemes: Gauss upwind everywhere, except for div(phi,U) Gauss limitedLinearV 1 - laplacianSchemes: Gauss linear corrected. A comparison between OF and Fluent is presented in the following pictures: As you can see, two problems are still opened: 1)There is a big gap between OF and Fluent converged cd value: the latter is higher of about 50% in respect to OF. Comparing pressure contours, I have the same general behaviour, but different max and min values. Might it be connected with wallFunctions? I have patch 0 named surf y+: min: 1.27842 max: 52.8088 average: 10.0848 in OF and Yplus max 168.2676 in Fluent... Remember that I am using realizableKE on both. 2)OF cl and cd shows wiggles in their histories, while Fluent values becomes smooth after about 300 iterations. It seems like OF values stop converging after a while. I tried to decrease tolerances for U and p, but no improvement was obtained. Is this problem connected with numerical schemes, relaxation factors and so on or is this more a wrong physical condition? Suggestions are welcome!! Maddalena.

 February 16, 2009, 16:09 Hi, I have similar problem #42 New Member   Mathias Kvick Join Date: Mar 2009 Location: Stockholm / Istanbul, Sweden / Turkey Posts: 11 Rep Power: 9 Hi, I have similar problems, here are plots of the pressure coefficient at a cross section of the upper and lower surface of my wing. As you can see, the results does not look good at the upper surface, on the lower surface it looks better, but still not good. As I understood it Fluent uses the same wallfunctions as I have in my case.. Let me know if you find out something..

 February 16, 2009, 16:34 In Genral different solvers gi #43 Senior Member   BastiL Join Date: Mar 2009 Posts: 488 Rep Power: 12 In Genral different solvers give different results. However, 50% difference on drag seems massively to big for me. However I currently have no real explanation for it. It might be possible that the turbulence models behave different in the transition area. I get very simular results on meshes with prism layers (= fewer transition). I never tried it without. Regards BastiL

 February 18, 2009, 13:33 Hi FOAMers, In order to under #44 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 14 Hi FOAMers, In order to understand why OF and Fluent converge to such different coefficient values, I analyzed the single forces contribution. Here the results: Fluent pressure force: (-0,4409 0,7928 10,5498) viscous force: (0,4121 -0,0003 0,0159) cl: 0,63170 (converged) cd: 0,08700 (converged) yPlus : min 14,79 max 129,71 OF pressure force: (-0,7441 0,720801 10,7649) viscous force: (0,07900 -0,0011 0,0045) cl: 0,6538 (not converged) cd: 0,0504 (not converged) yPlus: min 1,28 max 52,81 In particular, the contribution along x axis is the main cause of such a difference in the resulting aerodynamic coefficients, and since I have an AoA = 8°, this is more pronounced in cd. In addition, besides I am using the same Hi-Re turbulence model in the two solvers (realizableKE), the same standard wall function including wall roughness and the same mesh, the yPlus values are different. Note that Fluent values are close to experimental ones. In order to have an insight on this points, I run a inviscid case (viscosity → inviscid in Fluent and slip bc at wall in OF) with a A0A = 0°. Here the results: Fluent pressure force: (0,3334 -0,4700 0,5896) viscous force: (0 0 0) (Ok!) cl: 0.035580496 cd: 0.020121824 OF pressure force: (0,1937 -0,5229 0,5089) viscous force: (3,011e-5 -8,3081e-6 -2,4340e-5) (ok!) cl: 0,0307 cd: 0,01169 As you can see, x-component of pressure force is very different in the two solvers, it is the main reason of the 50% difference in cd here, and so it is to the viscous original case. I have been searching in the message board and surfing the web for quite a while now, in order to find an explanation, but with no luck. I have still some open questions: 1)Why there is such a difference between the two solvers in pressure calculation? As reported by Mathias above, the pressure distribution in chord-wise direction is different as well. 2)Why there is such a difference in y+, besides the same mesh, the same wall function and the same grid? 3)Is there something that I am missing (The entire case set up is explained in detail in the previous posts)? 4)Is there any hidden tricks in Fluent that let Fluent simulation converge? Schemes? Boundary conditions? 5)Besides using a prism-layer mesh, is there any other suggestions? Note that I do not use a prism-layer mesh since: - It is difficult to obtain a good mesh with my model - I do not want to end up with millions of cells to have a first estimation of values, - Doing a geometry sensitivities study with a prism-layer mesh will take me more time in creating mesh than running the case itself. Any help will be appreciated!!! Regards, Maddalena

 February 19, 2009, 04:38 Hello Maddalena, #45 Member   Maruthamuthu Venkatraman Join Date: Mar 2009 Location: Norway Posts: 80 Rep Power: 9 Hello Maddalena, Good work in regards with inviscid computation for comparing pressure forces. 1. I realized you are using Gaussian Node based gradients in Fluent which is recommended for unstructured mesh. In Openfoam are you using something similar type ? Still i am a new to OpenFoam , may be how much this may influence i dont know. 2. To be sure you have to set the kinematic viscosity [m^2/s] in OpenFoam, which is Default.i did this mistake once so just reminding you. 3.The physical distance from the wall to the next cell grid may be different if it is cell centred schemes or its counter part. Make sure that its taking the same physical distance for Y+... 4. There are lots of variables and modeling assumptions involved here, quite difficult to find the exact one for turbulent flows. But looking at your results for potential flow, its seems there may be some better Numerical settings can be used for OpenFoam. Have Fun. Your contribution will end up in some better understanding of OpenFoam.

 February 24, 2009, 08:14 Hi Maddalena, Any success #46 New Member   Mathias Kvick Join Date: Mar 2009 Location: Stockholm / Istanbul, Sweden / Turkey Posts: 11 Rep Power: 9 Hi Maddalena, Any success in reducing the difference between the two calculations? //Mathias

 February 24, 2009, 11:52 Hi Mathias, in the last days #47 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 14 Hi Mathias, in the last days I have been busy with other stuff and I haven't tested anything new. I will try some more settings, included what Maruthamuthu suggested, as soon as I will have some free time. In the meanwhile, please let me know of every updates/news/improvement you have! Cheers, Maddalena

 February 27, 2009, 07:39 Hi Maddalena, from your pro #48 New Member   Mitja Morgut Join Date: Mar 2009 Location: Trieste, TS, Italy Posts: 1 Rep Power: 0 Hi Maddalena, from your profile I have noticed that you are working in Trieste. I am also from Trieste. Recently I have compared CFX-11 and OF-1.5 for prediction of the flow around NACA0012. If you are interested to contact me, (to arrange a meeting in TS) you can find my e-mail address in the profile. Have a nice day Mitja

 March 2, 2009, 04:14 hi Maruthamuthu Venkatraman #49 Senior Member   NAVEEN.K.M Join Date: Mar 2009 Location: Bangalore, Karnataka, india Posts: 114 Rep Power: 9 hi Maruthamuthu Venkatraman i am from india,In order to find a proper convergent solution, I am considering a naca 0012 airfoil case with an AoA = 4°, can u please send me how wil u know that whether the solution is converged or not like fluent v wil get at some point v wil get that the solution is converged,but i dont know how v wil get in openfoam 1.4.1.....

 March 2, 2009, 04:14 hi Maruthamuthu Venkatraman si #50 Senior Member   NAVEEN.K.M Join Date: Mar 2009 Location: Bangalore, Karnataka, india Posts: 114 Rep Power: 9 hi Maruthamuthu Venkatraman sir i am from india,In order to find a proper convergent solution, I am considering a naca 0012 airfoil case with an AoA = 4°, can u please send me how wil u know that whether the solution is converged or not like fluent v wil get at some point v wil get that the solution is converged,but i dont know how v wil get in openfoam 1.4.1.....

 March 2, 2009, 04:29 Hello Naveen, #51 Member   Maruthamuthu Venkatraman Join Date: Mar 2009 Location: Norway Posts: 80 Rep Power: 9 Hello Naveen, Iam glad to see your progress in using OpenFoam.For your calculation i would recommend you to check the convergence of the drag and lift coeffcient. You need not to address people here in the forum with Sir. Just put your question clearly and if people dont have time to reply you then better try it out... I would recommend you to read Fluid mechanics book by Munsion, Youung and Okashi under the Section "Flow over the immersed bodies". Also Fluid Mechanics by Frank M white. Most of the external aerodynamic theories and expoerimental results are there. You shall make some test case and check your answers... Good luck

 March 2, 2009, 23:12 Hi Fomers, i am also facin #52 Member   Vishal Jambhekar Join Date: Mar 2009 Location: University Stuttgart, Stuttgart Germany Posts: 90 Blog Entries: 1 Rep Power: 9 Hi Fomers, i am also facing some issues using sonicTurboFoam for Supersonic Flow. i am mainly interested to capture shock boundary layer interaction. Please have a look at this post. Use this link to go directly to the discussion: http://www.cfd-online.com/cgi-bin/Op...ow.cgi?1/11454 __________________ Cheers, Vishal Jambhekar... "Simulate the way ahead......!!!"

 March 3, 2009, 08:34 Hi Foamers, when I tried to #53 Senior Member   Wolfgang Heydlauff Join Date: Mar 2009 Location: Germany Posts: 136 Rep Power: 10 Hi Foamers, when I tried to simulate an airfoil I realized that to further the boundary borders were, the better the solution got (compared to some windtunnel results). best results I got with a distance of the boundary borders of approx. 160 time the chordlenght (!!). (komegaSST-Model). Since OF has no farfield-correction like "Fluent" or "Flower" I think this is at least necessary. Improving the results a lot I also change the top and bottom boundary type from symmetryPlane to inlet. If far away you get better undisturbed stream flow at the airfoil itself. If symmetryPlane is used, the airflow is changing angle to apply the symmetryPlane conditions. In bad case, the AoA decreases.

 April 15, 2009, 04:40 Conclusion #54 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 14 Hello FOAMers, in order to obtain better convergence and results closer to Fluent for my external aerodynamic simulation, I changed one more time my fvSchemes, following some suggestions I had from HRV. Now it looks like this: gradSchemes: faceMDLimited Gauss linear 0.5; divSchemes: Gauss GammaV 1 on div(phi,U); Gauss upwind everywhere else. laplacianSchemes: Gauss linear limited 0.33 on laplacian(DepsilonEff,epsilon), Gauss linear limited 0.5 everywhere else. interpolationSchemes: linear; snGradSchemes: limited 0.5; Moreover, I increased tolerance and relTol for every variable: { ... tolerance 1e-09; relTol 0.01; } This helped me to obtain better numerical convergence. However, a certain difference between OF and Fluent still remain (alpha = 8°): Fluent:CL: 0.6317 CD: 0.0870 pmax:137 pmin:-199 OF:CL: 0.6596 CD: 0.0522 pmax: 115 pmin: -179 I could not find a numerical set-up or domain discretisation that allows me to obtain a smaller gap between the two solvers, so I can say that this is the best I could have with the standard OF distribution for a case similar to mine. Since Fluent results are closer to experimental values, I can conclude that OF 1.5 underestimates aerodynamic coefficients as a consequence of a numerically different pressure field around the wing. Please, feel free to add anything in addition to this. Regards, Maddalena s.m likes this.

 April 15, 2009, 11:32 #55 Senior Member   Join Date: Mar 2009 Posts: 138 Rep Power: 9 HI Maddalena! HI Foamers! Just by a fluke I found this thread. I am also simulating a flow around an airfoil and I am enthused of the possibility of writing cl cd to file. But I am struggling with some difficulties. Is there anywhere more information about this function?? Best Regards Camoesas Last edited by camoesas; April 16, 2009 at 03:12.

 April 20, 2009, 08:20 #56 Senior Member   Join Date: Mar 2009 Posts: 138 Rep Power: 9 HI Everybody! I still have not found more information about the forceCoeffs function. Altough it is working fine. But in the end I get this error message: *** glibc detected *** simpleFoam: corrupted double-linked list: 0x0000000000cc1ae0 *** Inconsistency detected by ld.so: dl-open.c: 260: dl_open_worker: Assertion `_dl_debug_initialize (0, args->nsid)->r_state == RT_CONSISTENT' failed! Do I have to worry? I have already searched this board but without results. Any ideas? Anyone gets this message too? Best Regards Camoesas

 June 10, 2009, 02:55 solving multielement airfoil case in openfoam #58 Senior Member   NAVEEN.K.M Join Date: Mar 2009 Location: Bangalore, Karnataka, india Posts: 114 Rep Power: 9 does any one know how to solve multielement airfoil case in openfoam which is imported from gambit...and suggest me how to set boundary conditions for mach no 0.15..

 June 11, 2009, 02:03 Multielement airfoil analysis #59 Senior Member   NAVEEN.K.M Join Date: Mar 2009 Location: Bangalore, Karnataka, india Posts: 114 Rep Power: 9 HI EVERYBODY Does any one know how to solve mutielement airfoil in openfoam 1.4.1 or 1.5...if any one knows suggest me how to set boundary conditions which is imported from gambit..

 June 11, 2009, 02:18 #60 Senior Member   NAVEEN.K.M Join Date: Mar 2009 Location: Bangalore, Karnataka, india Posts: 114 Rep Power: 9 hi maruthamuthu_venkatraman my self NAVEEN from INDIA...i hav completed my naca 0012 airfoil analysis case in openfoa 1.4.1 and 1.5....i got good results in both the versions...thanks for your suggestions....now i am doing MTech project on multielement airfoil analysis with double slotted flaps and i hav completed my grid in gambit(c-grid) and now i need to solve in openfoam...i am getting some errors like this during solving in openfoam 1.4.1 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::PCG::solve(Foam::Field&, Foam::Field const&, unsigned char) const in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::fvMatrix::solve(Foam::Istream&) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so" #5 main in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam" can u give me some suggestions whare i am going wrong and also suggest how to set boundary conditions.....

 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 Solarfinder Main CFD Forum 5 November 12, 2014 14:23 Mick FLUENT 0 October 3, 2005 08:13 Jihwan Main CFD Forum 13 October 12, 2004 12:02 rou CFX 3 April 26, 2003 01:10 rou FLUENT 1 April 1, 2003 19:18

All times are GMT -4. The time now is 03:17.