I'm working on a 3D wing with aspect ratio equal to 10 and chord=1m. Re=3000000. I'm working with a computational grid with 221656 tetrahedral cells. Lately I'm using a sphere with a radius of 50m to impose to impose the inlet velocity (as my boundary condition)specifying its magnitude and direction. For the turbulence I'm applying the k-e model with a null BC. Fluid is incompressible air (so energy equation isn't considered). I'm using a second order solver + simplec. Eventually I obtain good results for lift coefficient(1% error), but the drag coefficient is badly approximated (70-80%). what can I do to obtain a better estimate for my drag coefficient?

Check your Y+ values. If you are using ke model with standard wall functions your Y+ value should be 30<Y+<60. Try changing your wall function model to the realizable model.

Or you might want to change your turbulence model to the reynolds stress model but this uses much more computational resources.

Hope this helps

Hi Xwang,

I have a few questions.

For your analysis, what are your alpha ranges? Does it also include near stall or post stall? When you say you have Cl only 1% off, I am really interested to know if these excellent Cl values are from high alpha cases too.

If I read your post correctly, you have a 50m radius sphere as your overal computational domain and a wing buried at the middle, right? Based on the size of your computational model, how long is it to get a converged solution? How many iterations has it gone through? What are the residuals before you confirmed the solution is converged (1e-3 or 1e-4 or etc.)? Also what is the Mach number, is this analysis incompressible, subonic, or transonic?

I am just kinda interested in the procedures of the analysis.

Looking forward to hearing from you.

Hi CFD Rookie, my analysys doesn't include near or post stall.I've tried with alpha=0 and =7 degree.For both cases I've obtained an error of 1% regards Cl. Residuals are 1e-3 and forces are costant for hundreds iterations before I confirmed the solution is converged. I've considered an incompressible flow so mach number is not defined. Perhaps I've to use much more elements but I can't because of lack of RAM (I've "only" 512MB). Can you help me? P.S.:excuse me for my english but I don't know it very well.

Hi Xwang,

I have not done any wing analysis. But I have carried out the NASA LS(1)-0417 airfoil analysis of various alpha, including at stall. Similar to what you have, my Cl is very close. In fact, my Cp vs x/c is indeed very close (a few percents). However, my Cd is 300% - 400% off. I tried adjusting the mesh so that my y+ is within (35-350), as suggested by the code I am using (CFdesign). Still the smaller my y+ (from 300 - 200), my Cl dcviates more from the experimental data. (By the way, the Re I have is between 1.5e6 to 4e6). So if you would like to know how to improve drag, I am afraid I can't be any help to you. If your lift is right, and if you check your Cp vs x/c at different span locations, and they are all very close, then your wave drag is right. My guess is the reason your drag is off is due to friction drag. Like Mark pointed out, adjust the y+ might help. Also try different turbulence model. The SA turbulence model works well with adverse pressure gradient, like what we have on airfoil. You might want to try that. I will definitely not use K-e or any Ke derivative models when the alpha is high.

The problem is that I've alredy tried every turbolence model except RNS.

Which turbulence model gave you the best results? Ke?

How is your Cp vs x/c matching? Especially at leading and trailing edges. You might want to furhter refine the mesh at leading and trailing edge location.

How is your mesh dependency test tell you. Is your current best result already comes from the finest mesh?

My thought is if you have already gone through different turbulence model, then based on your current mesh (due to hardware limitation), this is indeed your "best computational result".

Drag is always difficult to match. I have a post on CFX section: "Re: how to make sure the simulation result is corr (39) - Ken" I mentioned about the drag is always tough to match. Some agree and some don't. I really hate to say this since I myself is a CFD guy, but that's the way it is.

ke gives me the best results but there wasn't a great difference with other turbolence model. Cp seems correct (at the trailing edges it doesn't go to 1 but I think it must be so because of the presence of the wake).I have tried to refine the grid but results are the same. I've tried also with an airfoil 2d. In this case I've used a boundary layer, made of 24 layers, which starts with a size 0.0001 and grows with factor 2. I've obtained the same results regards accuracy. I don't know what to do! Anybody knows a cheap 3d program based on panel method with integral boundary layer equation?