CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Thin foil analsis (sail) - Lift Coeff Problem (

Kelvin December 20, 2008 13:19

Thin foil analsis (sail) - Lift Coeff Problem
Hi All,

I am analysing the lift coefficients of a thin cambered foil much like a sail. I have created geometry (in 2D) whereby two bodies are together each with a curved face that represents either side of the sail surface (so effectively there is 0 thickness). This is in a domain made up by another two rectangular bodies. I have used domain interface between all 4 bodies and the two surfaces that represent either side of the sail are walls with no slip.

The domain is one unit deep, ie 1m in this case. The chord of the sail is 2.2m and it has a camber ratio of 0.1. I have obtained theoretical lift coefs for such a section from Marchaj's Aerohydrodynamics of sailing (P319.

I have been using the SST turbulence model, an inlet speed of 2.2m/s to give a Reynolds no of 3.14x10^5 (air 25degreesC) as used by Marchaj. I've used symmetry and openings for the sides and top/bottom of the domain respectfully and the outlet pressure is 0. I have been changing the angle of attack by changing the inlets angle.

My mesh is ok, about 1.6 million elements. I have played with this and found the answers don't change alot.

I am successfully getting convergence. I then take force values of both sides of the sail (both surfaces) which I add together then calculate the lift coeff using the combined force.

However I have two problems.

For an attack angle of 0 degrees, the theoretical lift coef should be 0.9, I am getting answers around 1.18 which is well over estimated and seems very high for what is only a cambered flat plate at 0 degrees attack?

At angle of attack 3 degrees, I get a closer answer, 1.23 compared to a theoretical value of about 1.2. OK there. At 5deg it appears to again be over estimated at 1.39 compared to 1.3 theoretically. Not a huge error however.

Why is the 0 degrees so over estimated?

Secondly, as I begin to increase the angle of attack stall begins and the coef is greatly under-estimated. The theoretical data suggests an angle of attack of 13deg will produce the highest lift coef for the sail of about 1.7. From my understanding stall should not be occurring until beyond this point but my CFX analysis is showing that stall has occurred (quite alot) and I therefore calculate a lift coef of only 1.44. At 10deg, stall is occurring and hence under-estimates the lift coef (1.48 instead of 1.62ish). At 8 deg stall is just begging to occur but has little effect as the lift coef as it is very close at about 1.5.

Does anyone have any suggestions as to why the flow stalls at such low angles of attack? This is a problem I've also been having when analysing a simple symmetrical foil at different AoA!!

I hope I have explained the problem ok, some help will be very much appriciated!


Glenn Horrocks December 21, 2008 21:07

Re: Thin foil analsis (sail) - Lift Coeff Problem

At the Re number you mention it is possible that a significant fraction of the sail has laminar flow. This will change things around a bit, especially near separations. Try using the turbulence transition model.

Getting accurate simulations near stall points is very challenging. Are you sure you have the upstream turbulence correct, surface roughness correct, effect of features like the mast, rigging or sail stitching etc. These all affect the exact point where separation occurs.

Glenn Horrocks

Kelvin December 22, 2008 10:08

Re: Thin foil analsis (sail) - Lift Coeff Problem
Thank you very much Glenn, I will certainly be looking into the things you mention.

The turbulence transition model is a new area to me and I will have to do some reading into it. Would you have any quick pointers that may apply to this particular problem, just to get me started or is it a fairly easy area?

Regards Kelvin

Glenn Horrocks December 22, 2008 17:22

Re: Thin foil analsis (sail) - Lift Coeff Problem

Turbulence transition modelling adds another layer of complexity to the simulation. Read the CFX documentation, go to some training, read the literature and do your own experiments to understand how it works and validate against experimental results. After you have done that you will be fine.

Key points are the mesh has to be good quality in the transition region (and over the airfoil in general). y+ at most 1 and graded out by no more than about 1.05, lower if possible. If a mesh with y+ of about 1 is not possible then forget the transition model.

Also upstream turbulence levels can be critical. Make sure you know what the ambient turbulence level is, or at least do a sensitivity analysis of it.

Glenn Horrocks

All times are GMT -4. The time now is 06:19.