[Naruto]

Dear FOAMers,
Greetings everyone. Currently I am simulating low Re. no. flow over NACA0012 airfoil. You can call me a novice in the world of CFD. For the last couple of weeks I have been trying to match the experimental data of the following link:
http://mac6.ma.psu.edu/VAWT/Sand80-2114.pdf
with my simulation. But I absolutely got no luck. Right now I am very frustrated. I tried everything I could. But nothing seems to work. Let me share my result of Re. no. of 40000. It is the attachment named comparison.xlsx. Though the trends seem similar, the simulated values of Cd, Cl do not make any sense. I do not know what is wrong.

Let me share some of my thoughts:
1. I think the whole problem is occuring due to the meshing. I did my meshing using pointwise. I drew my computational domain using Mechanical AutoCAD 2013. Then I transferred the geometry to pointwise. I used "Connectors on the Database entity" option of pointwise to create connectors on airfoil. I saw that pointwise was not able to map the geometry correctly. Could this be a problem.

2. The points were on the connectors. Some of the pointers did not seem to sit on the curve of airfoil exported from Mechanical AutoCAD 2013.

3. In the controlDict file I changed the forceCoeff file a little bit after changing angle of attack. My change is like : Drag Dir.: (-sinA cosA 0), Lift Dir (cosA sinA 0) where A is the angle of attack. The simulation is taking place on X-Y plane. Is this assumption correct?

4. I chose the chord length 1. I chose velocity as 1m/s. On that way I could control the Re. no. parameter very easily. Because the only thing that I need to change is the viscosity in transfer properties. Could this lead to any problem.

I am attaching my case file of NACA0012. https://dl.dropbox.com/u/108216538/naca0012_.rar
You can download a rar file named naca0012_.rar from the folder for your convenience.
Thanks in advance.

[haakon]

I'm sorry, but I can't manage to download the case file you link to. Can you check the link and make sure the file is readable by the public?

But as you say, the trend is similar between the graphs. Have you checked that you have used the right parameters for when calculating the drag and lift coefficients? That is checking that U and Aref is correct in the forceCoeffs section in controlDict.

[Naruto]

I am really sorry for my late reply. I was sick. Here is the link of my case files. Please take a look at it.
https://dl.dropbox.com/u/108216538/naca0012_.rar

[haakon]

First of all I think that the assumption stated in my previous post is correct. Your airfoil has a chord length of one meter, and the mesh is 1 meter in the spanwise direction. This gives a reference area of 1 meter squared. In the forceCoeffs file you have used Aref = 0.1, witch gives (exactly) 10 times as large lift and drag coefficients as you should have with Aref=1.0.

Looking at your spreadsheet, dividing all your coefficients by 10 seems to give results at least within 5-10% of your reference values.

Regarding your thought #3, I would at least use the definition of lift as being perpendicular to the mean, undisturbed incoming flow, i.e. that the direction of lift does not change with changing angle of attack. But I guess there are several definitions here.

[Naruto]

Thanks for your kind and informative reply. I have a question in my mind. I am taking Drag Dir.: (-sinA cosA 0), Lift Dir (cosA sinA 0) where A is the angle of attack. You told me to keep the Lift dir. as it is in the system folder. But is the drag dir. ok? I found this thing in the forum. But it seems a little bit awkward to me. Is this assumption correct?

[haakon]

Originally Posted by Naruto

Thanks for your kind and informative reply. I have a question in my mind. I am taking Drag Dir.: (-sinA cosA 0), Lift Dir (cosA sinA 0) where A is the angle of attack. You told me to keep the Lift dir. as it is in the system folder.

Did I tell you that? I just told that the definition of lift that I'm used to is to define lift as the force component normal to the undisturbed incoming flow, regardless of the geometry in question. If the problem is such that the lift force is to oppose the gravity I would choose to define positive lift in the opposite direction of the gravitational force, but that is a personal preference.

Originally Posted by Naruto

But is the drag dir. ok? I found this thing in the forum. But it seems a little bit awkward to me. Is this assumption correct?

I think that you should keep the lift and drag directions normal to each other in all situations. This applies both if you choose to change them with the angle of attack or not. If you define the lift direction to be perpendicular to the incoming flow, keep the drag parallel and in alignment with the flow.

In the end I guess that you just have to be careful about any references and what definitions they are using. I would guess you find multiple definitions out there. Good luck with your work.