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

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 12, 2019, 13:04 
NACA Airfoil simulation giving different lift coefficients in 2D vs 3D

#1 
New Member
Matthew Lam
Join Date: May 2019
Posts: 4
Rep Power: 3 
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 SpalartAllmaras turbulence model I get values that correspond to the Xfoil Polars at http://airfoiltools.com/airfoil/deta...il=naca0008il (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! Last edited by mrlam; May 14, 2019 at 09:20. 

May 13, 2019, 13:09 

#2 
New Member
kia abdollahi makuyi
Join Date: Nov 2018
Posts: 7
Rep Power: 3 
Hi mrlam
I've done a similar simulation on NACA 4412 at a low Re (3e+4) and various angles of attack. I used kklomega 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? 

May 13, 2019, 19:06 

#3  
New Member
Matthew Lam
Join Date: May 2019
Posts: 4
Rep Power: 3 
Quote:


May 14, 2019, 06:00 

#4  
New Member
Daniel Barreiro Clemente
Join Date: Feb 2019
Location: Munich
Posts: 15
Rep Power: 3 
Quote:
When you say Low Reynolds number, how low are they? Can you please specify the exact range of values? Thank you 

May 14, 2019, 09:19 

#5 
New Member
Matthew Lam
Join Date: May 2019
Posts: 4
Rep Power: 3 

May 14, 2019, 09:37 

#6  
New Member
Daniel Barreiro Clemente
Join Date: Feb 2019
Location: Munich
Posts: 15
Rep Power: 3 
Quote:
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 

May 15, 2019, 09:33 

#7  
New Member
kia abdollahi makuyi
Join Date: Nov 2018
Posts: 7
Rep Power: 3 
Quote:
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. 

May 16, 2019, 02:16 

#8 
New Member
New South Wales
Join Date: Feb 2016
Posts: 5
Rep Power: 6 
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/SP367/f56.htm 

May 16, 2019, 18:17 

#9  
New Member
Matthew Lam
Join Date: May 2019
Posts: 4
Rep Power: 3 
Quote:
I had no idea about this, in my case the aspect ratio is finite so that could definitely explain it. Thanks for your response. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Need help for the 2D airfoil simulation using OpenFoam  losiola  OpenFOAM Running, Solving & CFD  0  October 10, 2018 10:22 
How to not overwrite drag and lift coefficients after a simulation  Giovanni Trovato  FLUENT  1  August 1, 2018 00:31 
problem numerical results of lift and drag in airfoil simulation using fluent solver  Mohammad1994  FLUENT  0  June 7, 2018 02:59 
Lift and drag coefficient with strange values for NACA airfoil  antonio_ing  OpenFOAM Running, Solving & CFD  16  September 13, 2012 12:21 
Airfoil Simulation for Validation Purposes  Angela Bong  Main CFD Forum  7  September 13, 2006 13:04 