Hi all, I was performing some test with a NACA 0012 in 3DDP mode. Basically I extruded the airfoil 0.2 meters (the cord is 1 meter) and put two symmetrical boundaries at the both ends of the airfoil. I meshed four cases: 0, 3, 6 and 9 degrees of angle of attack with a very good mesh quality. I just wanted to draw the Cl slope and the polar curve. The shape of those were very good (the Cl vs Alpha had a linear behaivor, just like the real thing) The problem is that the Cl´s and Cd´s that Fluent gave me were high comparing the real data of the NACA 0012. Here´re the numbers that I got: AOA Cl Cd 0 0.00334 0.2406 3 1.4715 0.2857 6 2.9052 0.3670 9 4.2353 0.5245

I used velocity inlet at 5 m/s (Reynolds about 360000) and used k-w SST.

Any idea how can I get the real numbers??

Thanks for your time!

Did you fix your reference values? (Report->Reference Values)

Jason

hmm perhaps I didn´t catch a part of the theory, but I think that is only neccesary to select the surfrace in the Force monitors panel? I mean, I select the airfoil surfrace to show the Cl and Cd. Is it not sufficient to calculate them?

Thanks.

Hi, You can carry out following things & check is there any variation in your present work and the suggested one's.

1.i think you should carry out a study of Grid Independence.

2. Increase the domain area. ( dist. from inlet to blade and blade to exit)

I hope this things will bring you good results.

bye san

No, it's not enough to select the surfaces. You must define reference values if you're going to report coefficients (Cf = F/(1/2*rho_ref*V_ref^2*A_ref)). Fluent doesn't make any assumption of what you're using for reference values, becuase it's not a discipline specific code and many different disciplines use many different things. Airplanes tend to use wing planar area, but guided missile designers tend to use "stowed frontal area" (which typically doesn't count any deployable surfaces like wings or tail fins, even though they typically have wings). How is Fluent supposed to know which you inted for your reference values? Or about reference fluid properties... do you want to use average inlet (and if you have multiple inlets, which inlet), maximum values in the flow field, average within the flow field? Or some people don't care about the coefficient and just want the actual forces, so they set the reference values so that F=Cf... I could keep going, but what it boils down to is that if Fluent starts making assumptions for one group of people then it will cause problems for another. It's just easier/safer to leave reference values as user defineable.

The default values I believe are 1m, 1m^2 (for geometry values) and air properties at 1atm (for fluid values), but you should double check this.

Hope this helps, and good luck, Jason

Very clear Jason!! Thanks a lot guys!! now it seems to be working.

Thanks again.

Hi,

what was the final adjustments you carried out to get correct result.

bye san