# Comparison the airfoil 0012 experimental result and simulation result

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

 November 12, 2009, 02:49 try LES #21 Member   Ivan Join Date: May 2009 Posts: 85 Rep Power: 16 you guys may want to try LES. I did some airfoil flow simulation. though Cl and Cd are not important in my cases, I did simple comparison and they match experimental data pretty well. I guess the reason is that LES deals with the transition from leminar to turbulence pretty well. But surely the computation cost is much much higher. parallel computation is needed for LES.

 November 12, 2009, 05:28 #22 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 16 @ Makaero: roughness constant 0.5 is fine for flat plate, would expect to be ok for airfoil. However, it only takes effect when your roughness height is sufficiently large. So just converge your solution for smooth foil (ie rougness height = 0) and then try, say, roughness height of 0.0001 m. Roughness height is the diameter of the roughness grains on your surface. @ harrislcy: Maybe the following will work? First converge your solution with 1st upwind laminar model. Then (do not initialize) for 1st upwind k-e. Finally (again do not initialize) for 2nd upwind k-e.

 November 12, 2009, 12:46 #23 Member   ANIL Join Date: Apr 2009 Posts: 35 Rep Power: 16 @ jack1980 Thnx...

 November 16, 2009, 01:25 What is this? #24 New Member   Yang Join Date: Oct 2009 Posts: 15 Rep Power: 16 "turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 2 cells " What make this happen? Is it the meshing problem? How to solve it?

 November 16, 2009, 08:33 #25 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 16 Sorry, should have told, that happens oftenly. Before running k-e calcs, do the following: Solve -> Initialize -> Initialize ... Do not press Init! Scroll to the box containing Turbulent Kinetic Energy and write down the value. Press Close. Solve -> Initialize -> Patch ... Variable = Turbulent Kinetic Energy Value = value you've written down Zones to patch = fluid Press patch This should help, good luck! blgypeng likes this.

 November 18, 2009, 06:09 error... #26 New Member   Yang Join Date: Oct 2009 Posts: 15 Rep Power: 16 Error: divergence detected in AMG solver: temperature Again, another error opup again when in the K-ep silmulation. This happen after 200 iterations. How to avoid this?Thanks

 November 19, 2009, 12:37 Inflow Boundary #27 Member   Andy Robertson Join Date: Mar 2009 Location: Long Island NY Posts: 46 Rep Power: 16 Check your inflow condition. Make sure that the inflow is a close to laminar conditions as possible. Core flow of wind tunnels is generally turbulent, but at a very small intensity and length scale. This depends on the tunnel of course. Look at what the viscosity ratio is just downstream from the inlet. Except at tunnel walls (if you modeled them). It should be less than 1. A good quiet tunnel might have a turbulent viscosity ration of less than .1 Learned this the hard way myself - Andy

 December 9, 2010, 11:50 #28 New Member   Join Date: Jun 2009 Posts: 6 Rep Power: 16 Hello people! I want to test the profile NACA 0012 for differents alfa and compare the results with experimental and XFoil graphics. It should be simple, but my results are not satisfactory: ro= 1,225 Kg/m^3 Mu_air=1,75*10^5 Kg/(m*s) D=1 with these Data, i obtain the differents velocities (in m/s): Re=200K -> vs= 2,8 Re=500k -> vs= 7,102 Re=3M -> vs=42,612 Re=6M -> vs=85,224 For alpha= 0°and different viscosity theories: RE=6M Spall. Alm. /// K-E Stndrd /// K-w SST Trans.flow /// X-Foil(=Exper.) cd 3.31*10^(-2) /// 6.2*10^(-2) /// 3.32*10^(-2) /// 5.08*10^(-3) RE=1M K-E RNG /// K-E Stand (Ehn. W.T.) /// K-w SST Trs.fl /// X-Foil(=Exper.) cd 2.1*10^(-3) /// 3.24*10^(-3) /// 1.73*10^(-3) /// 5.4*10^(-3) RE=200k Spall. Alm. /// K-E RNG /// K-w SST/// Trs.flow /// X-Foil(=Exper.) cd 6.4*10^(-5) /// 1.5*10^(-4)/// 3.14*10^(-4) /// 1.02*10^(-2) For Low-Re I thought that K-omega sst could be better than K-Epsylon, but I don't see a good result...anywhere (the mesh is good, from the profes.) Thank you for your help! Ferran blgypeng likes this.

 December 9, 2010, 12:46 #29 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 16 Hi, you might be having trouble with the transition point. I think there are two approaches: - Move from xfoil to experimental data with a ' trip wire '. This should fix the transition point near the leading edge. Now you can really use a turbulence model in you entire domain. - If you want to stick with the xfoil data: try running viscous as well. If the exp. data is somewhere between your viscous and turbulent (for examp. rke) results, you might want to look into fixing the transition point manually. This can be done by splitting your grid in a viscous and a turbulent part. Good luck!

 June 24, 2011, 04:06 #30 Senior Member   Join Date: Mar 2011 Location: Germany Posts: 552 Rep Power: 19 hey all of you try k-w turbulence model. This works best for airfoils

 August 29, 2013, 11:27 #31 New Member   Alexandre Felipe Medina Correa Join Date: Aug 2013 Posts: 4 Rep Power: 12 Hey guys, I am having the same problem with Fluent here. I am an aeronautical engineering bachelor's student and as part of a research project I am first simulating the flow around a NACA0012 with 0 AoA. My Reynolds is about 1.0 e4, and my Cd should be around 0.037. First I tried to use a K-Omega SST, but after reaching 1.0e-7 residuals, my cd is still 0.13. I tried also S-A, and the cd drops to 0.05, but my continuity can't converge to less than 1.0e-4. Since it is a symmetric airfoil, the Cl should be zero, but now is around 1.0e-5 for S-A and 1.0e-3 for k-W SST. I used all the standart settings. Also, my Y+ is in the range 1.0 to 1.4.

 Tags airfoil, experimental data, fluent, naca 0012, naca 4415