NACA 0012 lift and drag coefficient.
 

I am running ANSYS fluent simulation flow over naca 0012 airfoil.
So far the lift coefficient is similar with the published papers.
The problem is drag coefficient is different so much in term of value compared to published papers.
I have check my mesh quality and boundary condition, it shows no problem.
Any idea why drag coefficient is different ???

you may check the tubulrence model. which turbulence model did you appplied? generally, S-A 1equation model predict the drag coefficient less than compare with published paper. I recommand to you T-SST 4equation turbulence model.

if you solving 2 dimensional problem using about 300 surface nodes on the airfoil, that the drag coefficient is predicted less than 5% error.

Reynolds number = 360,000
Is it laminar or turbulence flow??

The flow is fully turbulent flow when Re>2,300 in pipe flow for air. So I recommand to you that you need to apply the turbulence model especially transition-SST 4equation model. In addition, not only you have to making surface nodes more than 270 but also consider wall y plus.
(you can find the wall y plus information NASA hompage.)

At this reynolds number the flow is transitional. E.g. at zero angle of attack transition to turbulent at this Re and this airfoil happens at about 80-90% of the wing chord. At angle attack 5deg it happens at about 25% of wing chord.

Using turbulence models in CFD-software without special user input will likely give very wrong results for drag at such reynolds number.

Truffaldino

Truffaldino ,

Sorry for my poor knowledge, how to determine which reynolds number is laminar or turbulent? I google it and cant find the knowledge i want. Any source for me to study?

I face problems in drag coefficient where it is different from the published papers.

Hello Tom,

Your question where the flow is turbulent and where is laminar is not an easy question: this is one of the difficult problems of fluid dynamics and the answer depends not only on reynolds number, but also on problem geometry, boundary condition and amount of free-stream turbulence. In your case flow is neither turbulent nor laminar, there will be a transition from the laminar to turbulent flow somewhere.

In the above examples I have used XFOIL program to find the transition location: For instance, at zero angle of attack and Re=3.6E5 the flow is laminar at both sides of airfoil up to approximately 80% of the airfoil chord and it becomes turbulent after.
For angle of attack 5 deg the flow is fully laminar at lower side of airfoil. At upper side it is laminar up to 25% of the chord and turbulent after.

X-foil is so far the best software for analysing flows past conventional airfoils at low reynolds numbers: it is more accurate in predicting drag than RANS modelling. This program is free and easy to use.

So, before using CFD software with RANS I reccomend you to run XFOIL analysys to have an idea what to expect, where to expect flow separation and reattachment, transition etc.

Truffaldino