NACA Airfoil simulation giving different lift coefficients in 2D vs 3D
 

Hello everyone,

I am relatively new to CFD and ANSYS Fluent and have been trying to simulate flow of water at low Re (~50000 to 300000) around a 0.3 m chord NACA 0010 airfoil with an attack angle of 5 degrees to confirm the correct lift and drag coefficients.

When I run a 2D simulation using the Spalart-Allmaras turbulence model I get values that correspond to the Xfoil Polars at http://airfoiltools.com/airfoil/deta...il=naca0008-il
(Cd of 0.025 and Cl of 0.6)

However, when I run a 3D simulation of the same airfoil extruded to a span of 0.5 m, the lift coefficient I get is much lower (Cl of about 0.2). The drag coefficient seems to stay accurate.

I am pretty sure that the reference values I am using are correct:
Area - 0.15 m^2 (0.3 m chord length x 0.5 m span)
Velocity - 1 m/s (the same as the inlet boundary velocity)
Density - 998 kg/m^3

I have tried refining the mesh and changing the size of the inflation layers next to the airfoil (I read somewhere that y+ can significantly affect accuracy), but so far I am having the same issue.

If anybody could help, that would be much appreciated!

Hi mrlam
I've done a similar simulation on NACA 4412 at a low Re (3e+4) and various angles of attack. I used k-kl-omega model which leads to pretty accurate results in low Re due to its transition prediction capability. I recommend to use this turbulence model.
By the way, what is the grid y+ and what boundary conditions do you use?
Could you attach a picture of your mesh?

Thank you for your reply! I will definitely try that model since I'm dealing with a similar Re range. I will post pictures of my y+ distribution and meshes tomorrow, I don't have access to them currently.

When you say Low Reynolds number, how low are they? Can you please specify the exact range of values?

Thank you

I am working in the range of Re = 50000 to 300000, I've edited my original post to reflect this

That's very interesting. I myself I'm running at the moment 2D airfoil simulations in the range of 60,000 to 300,000 to validate some meshes and Fluent setups to compute polars. I'm validating my data against experimental wind tunnel meassurements in order to do so.

The turbulence model, as well as some of the key setup parameters are the following:
-Airfoil length = 1m
-Upstream domain size = 20 times the chords length
-Downstream domain size = 40 times the chords length
-Sides domain size = 15 times the chords length
-Y+ value is <1. The number of cells from the airfoil wall to the end of the domain is 250, with an expansion ratio from the first cell of 1.05. It's an structured, streamwised mesh.
-Number of cells: 240K
The reported mesh quality in ICEM is very high as well.

The Fluent setup is as follows:
-Turbulence model: Transition SST
-Inlet = velocity inlet with a defined speed corresponding to the desired Re number with respect to the airfoils chord
-Outlet = pressure outlet
-Coupled , Least Squares Cell Based ,Second order upwind, with reduced explicit relaxation factors to favour convergence
-Convergence criteria = 10^-6
-Hybrid Initialization


Would you mind sharing your setup and simulation parameters to see how they differ and if they would be a better fit for my simulation?
How accurate are the lift and drag values you're obtaining?

At the moment, for cases from 100,000 this setup works fine, with an average error of 5% for the lift coefficient and 15% for the drag coefficient, although I'm not fully satisfied with it. On the other hand, the results for the 60,000 are quite inconsistent and erroneous.

Thanks in advance

I'm not sure if there is an specific range in which the Re is considered low or high, but the lower Re gets the worse results you get from common turbulence modles like K-omega. It's beacuase these turbulence models consider that entire boundary layer is fully turbulent, while boundary layer flow is laminar at first, then goes through a transition phase and finaly turns to turbulent flow. Therefore, a lower Re number means a wider length of laminar boundary layer.
In the previous post I said that I've done the simulation in Re=3e+4 by mistake, it was 3e+5 similar to yours.

Is the wing extruded through the whole domain (i.e. modelling an infinitely long span)? If it has a finite span, then getting lower C_L is normal - it will vary depending on your aspect ratio.

here is a good example:

https://history.nasa.gov/SP-367/f56.htm

Hi tbwake,

I had no idea about this, in my case the aspect ratio is finite so that could definitely explain it. Thanks for your response.