Hi, I'm modeling a low reynolds number eppler 205 airfoil for Re=304300 because the experimental data aviable. I've used invicid formulation, S-A turbulence model and many types of bondary conditions but I've not had success.

If some budy has experience, please let me know all the step for modeling low reynolds number airfoils.

bye.

Low Re (Re < 400000 to 500000) are typically laminar (instead of inviscid or using a turbulence model). Assuming its in the incompressible regime, you can use a Velocity Inlet or a Pressure Inlet. Your outlet should be a pressure outlet. All of your BCs should be far enough from the airfoil not to be affected by the flow (10 chords or so in every direction).

If you've tried this, then be more specific about what problems you've had.

Hope this helps, and good luck, Jason

Thanks Jason.

At Low Re, you have both a laminar part and a turbulent part, I dont't know if fluent is capable to predict the laminar to turbulent transition though . I would like to calculate the lineal part of the cl v/s alpha, so I'm goin to use invicid flow . BUT IT DOEST'N WORKS! I want just to validate the model to modelate an entire airplane.

experimental data: alpha=0 CL=0.48

fluent : alpha=0 CL=0.028

Did you check your reference values? (Report->Reference Values).

Jason

Yes I'did.

thanks*10e20 Jason.

Sorry Pablo, that won't work. At low Mach number (incompressible in this case?) the solver will not enforce a Kutta condition (i.e. flow leaving the wing at the trailing edge) in inviscid flow, and thus it won't model the lift generation. You can't really model transition (and hence things like separation bubbles) with a conventional turbulence model, but a viscous solution will at least give you your Kutta condition and lift. The turbulence models don't necessarily do badly, where the real world flow is laminar it will give a thin but turbulent boundary layer, and where the real flow is turbulent it will give you a good approximation to reality. But at low Reynolds number the transition separation bubble can have a big effect on drag in particular, and this will be extremely difficult to get right. I've had some luck with the Langtry-Menter transition model implimented in CFX, but the bubble remains a difficult thing to model.

You're absolutely right Charles. Do you know if it's possible to incorporate some transition model(for instance the e-n method) into fluent like a UDF?. I'm goin to try with CFX, but I can't use it officially because my university doesn't have CFX's license, I only can use fluent.

I'm sure it can be done, but I suspect that it will be pretty difficult!

Ok, I'll try it , it could be a good project's subject, "Incorporation of a transition model into Fluent code " I've not seen if somebody has done it. It could be fun.

thanks a lot Charles. Pablo.

Well, even just a normal turbulence model should be producing reasonable lift values, without fiddling with transition. What I have seen done is to emulate transition at a known chordwise position by introducing turbulence there.

It works. I used S-A turbulence model and new bondary condition. Now, how I can get the y+ values?

thanksssssss

I have bring a transition model into Fluent with UDF, and it's very good! But, I don't think it can solve your problem! I think you maybe give some error boundary condition example pressure in experiment 54000Pa( at 5KM) but you in Fluent 101325. You should check it!

can you give me some tips to do it? How you done it?

I don't think transition can solve your problem! You can search some article about transtio!

I know about transition. I don't know how incorporate some transition model into fluent.

pablo.