
[Sponsors] 
May 4, 2010, 12:40 
Polar airfoil of the Naca 0015

#1 
New Member
Maxime
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Hi,
I need some help. I try to correlate the polar airfoil of the NACA 0015 (for a Reynolds Number equal to 700 000) on Fluent. I used SpalartAllmaras and kw sst model referring to User's guide, but i get a huge gap between theoretical values and fluent. To be precise, i use a Cgrid meshing with a y+=30 (about 0.8mm*0.8mm for the smallest mesh). About the solver, i have worked on a pressure based solver, with a coupling between pressure and velocity. I have choosen PRESTO! for the pressure interpolation and Quick for the momentum interpolation because i found in the User's guide that will be the best way for this kind of simulation. The thing is, i don't know really the different parameters i have to set up on Fluent (for exemple the Explicit relaxation factors, the underrelaxation factors...). I don't know where i may a mistake. Thanks for your time, Titasse. 

May 4, 2010, 15:18 

#2 
Senior Member
Join Date: Nov 2009
Posts: 411
Rep Power: 10 
By "huge gap you mean" a big difference between the experimental Cd and the calculated Cd or you have the same discrepancies for the CL ?
For such a low Re=7*10^5 a large part of your airfoil is actually in a laminar flow, so if you have used a turbulence model on the entire calculation domain you will have a poor Cd, however your CL should be close to the experimental CL at least for the linear part. You need to take transition into account for this simulation if you want to obtain a better estimation for Cd. Do 

May 4, 2010, 16:08 

#3 
New Member
Maxime
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Hi,
Thank you for your help. Indeed, when i say a "huge gap" i mean that i got a important difference between experimental and simulation values. The thing is, generally, in function of the angle of attack (between 016 degres), the both of Cl and Cd are wrong, not only the Cd. 

May 4, 2010, 16:46 

#4 
Senior Member
Join Date: Nov 2009
Posts: 411
Rep Power: 10 
Even with a fully turbulent simulation your CL should be close to the experimental result if you have the same Mach and Reynolds in your simulation as in the exp. data.
Do 

May 6, 2010, 12:16 

#5 
New Member
Maxime
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
I ran new simulation with finest mesh, you were right, i found a Cl close the experimental values.
How can i choose to calculate the transitional flow on SpalartAllmaras model? Cheers, Titasse 

May 6, 2010, 14:46 

#6 
Senior Member
Join Date: Nov 2009
Posts: 411
Rep Power: 10 
In Fluent 12 you have 2 turbulence models that also take into account the transition, none of them uses SA. This is the easiest and probably the best approach with Fluent.
With SA you can split your domain in two zones: a turbulent region and a laminar one, this can be done by manually splitting your mesh in Gambit, see this article for a similar approach: PaulDan Silisteanu; Ruxandra M. Botez  TransitionFlowOccurrence Estimation: A New Method, Journal of aricraft 2010 vol. 47 no. 2 If you have access to Fluent 12 better use the first suggestion. Do 

June 9, 2010, 02:57 

#7 
Member
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8 
Hello DoHander and Titasse,
I'm doing simulation on NACA 0012. My purpose is checking the lift coefficient as long as the drag coefficient then compare with experimental data from text book (Theory of Wing Sections). I use StarCCM+, but I think the model and the setting parameters almost the same. That's why I want to discuss with you here. In my simulation, the physical model is set as follows:  Fluid: air  Segregated flow  Constant density (incompressible)  Steady  Turbulent (Re 2000000)  RANS  Ke  Realizable Ke Two layer  Twolayer all y+ wall treatment The Bcs:  Velocity inlet: v=29.215 m/s  Foil: noslip wall  Pressure outlet Actually, I did this simulation almost 1 year ago, but now I've not successed yet! Cl is lower than exp data after 8deg, and Cd is very larger than exp data. Also the stall angle is smaller about 3deg. Could you tell me your experiences in very detail for this simulation as long as the foil problems. Thanks you a lot!  Trieu email: trieuckgt@gmail.com MSN: trieu.dut@live.com YM: trieu_tme@yahoo.com 

June 10, 2010, 09:08 

#8 
Senior Member
Join Date: Nov 2009
Posts: 411
Rep Power: 10 
Hello,
1. You will never get quite the experimental data from an usual CFD simulation. 2. You should be able to get the correct Cl on the linear region (say 4 deg to about 8 degree). Also I don't think you can catch the "true" stall angle. 3. For a Re=2*10^6 as in your simulation a large part of the flow around your airfoil is actually laminar, but your simulation consider the entire flow as a turbulent region, this is why you get a larger Cd. If you want to obtain good results you need to respect the physics of your problem by using a software that has a transition model (Xfoil, Fluent 12 ... not sure if OpenFoam can model the transition). Do 

June 16, 2010, 13:54 

#9 
Member
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8 
Thanks you so much, DoHander
As I known from another simulation studies, the simulation data compared well with experimental data, so in my opinion, we also can use CFD to get a good results. At least, the differences between CFD results and experimental data are not significant. Base on the Re value, 2million, I'll try to use laminar flow and check again. For the using another CFD commercial codes (e.g. Xfoilm Fluent 12...), I afraid that for me it's impossible because the limit of time. I'm going to finish my research on several next moths. That's why I just want to continue with StarCCM+, but thanks you anyway about this point. I've been studying the foil simulation. Thanks you! Trieu. 

June 16, 2010, 18:45 

#10 
Senior Member
Join Date: Nov 2009
Posts: 411
Rep Power: 10 
Xfoil is free (open source) and the learning path is 1 hour maybe less.
I didn't say CFD can't be used to get an agreement between experiment and calculated data. I've said an "usual CFD" calculation, usual means one in which your flow is considered entirely laminar or turbulent. Let me give you an example: take your NACA 0015 at Mach=0.2 and Reynolds 2 millions and an incidence of 4 degrees, you will have laminar flow on about 40% from the upper side and 60% from the lower side of your airfoil. If your simulation does not take into account the transition from laminar to turbulence you will have a bad estimation for your Cd (you can have more then 40% error between experimental and calculation). I've mentioned Fluent 12 because your posting is at the Fluent users here on cfdonline, and because Fluent 12 contains a turbulence model that takes into account the transition. From a practical point of view Xfoil is free, will get you a polar in 23 minutes and can be used after a few hours of practice. If you need help I can send you a tutorial that will show exactly how to calculate a polar for a given airfoil. Do 

June 27, 2010, 09:39 

#11 
Member
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8 
Hello DoHander,
Thanks you so much! I'm sorry for my misunderstood. You are right, I got the Cd results within 30% errors. Therefore, my simulation has to take into account the transition. As I known, the komega SST can do it well. However, this turbulence model is very sensitive with the inlet condition (e.g Turbulent Intensity, Turbulent viscosity ratio, ...). Thereby, I have to set the right values for these parameters. But I don't know what values I should use! As you said, Fluent includes the turbulence model for the transition problem. It is komega SST, isn't it? if not, could you tell me in detail about how to set the parameters for that turbulence model? Thanks you so much! Best regards,  Trieu. Email: trieuckgt@gmail.com 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Symmetric NACA Airfoil Lift and Drag Data  jrider22  Main CFD Forum  3  April 15, 2010 04:59 
Laminar flow past oscillating Naca 0012 airfoil  kafkaf  Main CFD Forum  1  April 7, 2009 02:49 
Drag prediction for Naca 23012 airfoil  Ravel Bogatec  CFX  17  February 15, 2008 01:21 
NACA 0015 2D problem  arnold  FLUENT  1  May 3, 2007 02:17 
center of mass for naca airfoil  frederic Felten  Main CFD Forum  3  February 20, 2002 12:55 