Polar airfoil of the Naca 0015
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 Spalart-Allmaras and k-w sst model referring to User's guide, but i get a huge gap between theoretical values and fluent.
To be precise, i use a C-grid 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 under-relaxation factors...).
I don't know where i may a mistake.
Thanks for your time,
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.
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 0-16 degres), the both of Cl and Cd are wrong, not only the Cd.
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.
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 Spalart-Allmaras model?
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:
Paul-Dan Silisteanu; Ruxandra M. Botez - Transition-Flow-Occurrence Estimation: A New Method, Journal of aricraft 2010 vol. 47 no. 2
If you have access to Fluent 12 better use the first suggestion.
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 Star-CCM+, 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)
- Turbulent (Re 2000000)
- Realizable K-e Two layer
- Two-layer all y+ wall treatment
- Velocity inlet: v=29.215 m/s
- Foil: no-slip 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!
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).
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 Star-CCM+, but thanks you anyway about this point.
I've been studying the foil simulation.
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 cfd-online, 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 2-3 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.
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 k-omega 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 k-omega 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!
|All times are GMT -4. The time now is 08:32.|