2d Airfoil simulation
 

hi,
I'm simulating a NACA0021 with 2ddp FLUENT. I've got some problems and would be happy if anyone could help. the info is as below:
Chord based Re = 120,000
v=25 m/s
AOA = 8 deg.
Turbulence method = k-w SST , transitional flow
till now used both SIMPLE and SIMPLEC for coupling
Pressure - PRESTO!
the rest - 2nd order upwind

so one problem is the refiner my mesh becomes, the amount of Cl and Cd become more different from the experimental data. WHY?!!!
second problem is, my Cl and Cd are 10 times smaller than the experimental data. WHY?!!!
and I would like to know which coupling is better to use. also for pressure and other equations which scheme is better to use.
oh and can anyone tell me the amount of elements in the mesh that are around enough for mesh independency?
thanks.

I think you should focus on why your drag and lift coefficients are off. Have your checked your reference values?

SIMPLE & SIMPLEC should be ok. SIMPLEC allows higher urf for faster convergence than SIMPLE. The fullly COUPLED algorithm is not a bad choice if you are unsure. PISO is generally for transient calculations where it really outshines the SIMPLE algorithms.

I tend to prefer second order scheme for pressure, but PRESTO is probably better for airfoils.

For advected quantities, 2nd order is ok.

Thank you for the reply LuckyTran,
I set the reference values to compute from inlet. I really don't understand why the lift and drag coef. end up like that. I also check lift and drag convergence through the iteration.
Also I used COUPLED today and it ended way faster than the other two.

i prefer to you use Spalart-Allmaras_model
make sure about references parameter

Thank you AHF for the reply.
I set the reference values to be computed from the inlet.

Setting the reference values from the inlet is fine, but you manually have to input values for reference length, Area and depth. depth should be equal to 1 as you are doing your calculation in 2d, are and length then depend on the dimensions of your aerofoil.

Setting the reference values from the inlet is fine, but you manually have to input values for reference length, Area and depth. depth should be equal to 1 as you are doing your calculation in 2d, are and length then depend on the dimensions of your aerofoil.

Thanks dynamic,
I did what you suggested but it ended up in another wrong series of solutions. actually they became totally off.

You need to compute somewhere else what the reference area and length is and then specify those reference values in Fluent. The reference area and length are in the definition of the drag and lift coefficients. Depending on the field of study, the reference area and length may be different, so it's very important to the same definition that you are comparing your results to. Usually the reference length is the chord length and reference area is the planform area. Usually...

Well I found out that since my simulation is 2D, the reference area and depth should be 1. The reference length is the chord C. I changed it in " report --> reference values " from 1 to 0.07 (my chord is 0.07m or 70mm) but nothing changed.

CL and CD uses the reference density, reference velocity and reference area (0.5 * density * area * velocity^2).

So changing length (not directly) and area will affect them. (reference area = depth of wing * chord length)

Just coming to main point, change your area to 1 * 0.07 = 0.07 m^2 will do the trick...

Thanks Far for the reply,
I'll try it and let you know the results. actually I'm busy with something else right now.

Thank you Far,
the problem of the amount of Cd and Cl is solved. but still the other problem remains that the more the mesh elements become, the results have more difference from the experimental results. and I haven't reached mesh independency yet. can you help me there too?!

What was the issue?

mesh Independence does not imply the accuracy of your results. It is to reduce discretization errors. There are are also more source of errors. Like physical model e.g. turbulence modeling and Y+ is important aspect of this study.

Do you see the error in Cd only or both in Cd and Cl. If both then you need to worry ... :eek:

sorry for replying this late and thank you for your help.
both of them (Cd and Cl) show the same problem. the first mesh G1 with 26600 elements is the most accurate and G4 with 117600 elements has the least accuracy and is way off course. Also G5 with 236000 elements diverges with 2-3 iterations.
i read in a paper that K-omega SST turb. model is the best for these cases, although in that paper the model was 3d but I'm trying to solve a 2d first. about Y+ actually I don't have much info and haven't found anything similar to my problem.