[galcom]

Hi guys,

I am currently working on investigating what effect on Lift coefficient various types of flaps have on an NACA2412 aerofoil. A Reynolds’ number of 100,000 is initially considered. I’ve done some experimental tests in a wind tunnel for these types of profiles:

• Plain Flap
• Split Flap
• Slotted Flap
• Fowler Flap
• Handley-Page LE Slat

After comparing the experimental analysis with those obtained from FLUENT, it resulted in lift coefficients for CFD being much larger than those obtained from experiments (Experimental data for 0 degrees AoA came out to be around 0.22 – 0.4 while those obtained in CFD are all > 1.18). I did a grid independence check and verified convergence by assessing the graph of lift coefficient vs Number of Iterations. I used a density-based solver with a Laminar model due to the low Reynold’s number. I also tried out the Spalart Allmaras, k-w SST, Realizable k-e and Transitional k-kl-w turbulent models. I also tried to lower the explicit-Under Relaxation factors where necessary but all seem to hinder the same results.

Is there anyone who might have encountered the same problem or is this behaviour normal due to poor drag calculation on the model?

Cheers

[truffaldino]

Originally Posted by galcom

Hi guys,

I am currently working on investigating what effect on Lift coefficient various types of flaps have on an NACA2412 aerofoil.

Is there anyone who might have encountered the same problem or is this behaviour normal due to poor drag calculation on the model?

Cheers

This kind of problem is encountered quite often due to inability of turbulence modelling to predict separation and transition at low reynolds numbers and due to big measurement errors and fluctuation in wind tunnel for such reynolds numbers.

But one order of magnitude seems to be too much. It might happen that you set wrong rederence lengt or velocity in fluent or/and wrong direction of force evaluation.

Try to do the following: take your airfoil and run inviscid in x-foil with unit chord (this takes 5 minutes to learn and fraction of second to run), then do inviscid in FLUENT with your former fluent settings. If the difference in Cl will be big then the problem is in your fluent settings. If not, the problem is in the turbulence modelling or/and measurements.

Trufaldino

[FMDenaro]

Originally Posted by truffaldino

This kind of problem is encountered quite often due to inability of turbulence modelling to predict separation and transition at low reynolds numbers and due to big measurement errors and fluctuation in wind tunnel for such reynolds numbers.

But one order of magnitude seems to be too much. It might happen that you set wrong rederence lengt or velocity in fluent or/and wrong direction of force evaluation.

Try to do the following: take your airfoil and run inviscid in x-foil (with unit chord and re=10^5, this takes 5 minutes), then do inviscid in FLUENT. If the difference will be big then the problem is in your settings. If not, the problem is in the turbulence modelling or/and measurements.

Trufaldino

well, but the Re number should ensure a laminar flow along the profile, isn't it? maybe the grid resolution is not adequate and the used scheme is too dissipative ...

[truffaldino]

Originally Posted by FMDenaro

well, but the Re number should ensure a laminar flow along the profile, isn't it? maybe the grid resolution is not adequate and the used scheme is too dissipative ...

Sorry I just did correction about reynolds number in my previous post. For inviscid you do not need to set reynolds number (this was the silly thing).

I think the numeric dissipation will not lead to error of one order of magitude for the lift coefficient. This is just to chek that there is no big error in the Fluent settings.

[galcom]

Appreciate for your reply guys.

I did arrange the reference value of Area appropriately Trufaldino. I also run the calculation for a unit length just like you said while setting the reference values to match that geometry. I got the same results using an inviscid model since it’s a laminar flow.

FMDenaro, mesh-wise, I made use of a tet-mesh in a C profile using inflation layers around the aerofoil, making sure that the y+ is around 1 (it varied between 0.7 and 2), so that shouldn’t be a problem either. Clearly the problem started when modelling the aerofoil with flaps since when I ran an NACA2412 profile, CFD results matched perfectly experimental data. I guess it’s the turbulence model then; but I’m still sceptical on how it can lead to a large difference between experiments and CFD.

Knowing that turbulence models give unreliable data for transitional flows, can the problem be a transition region somewhere close to the flap, which is leading FLUENT to give wrong data?

[Totalsim]

I would say its like to be a mismatch in the setup/geometry between CFD and experiment.

Have you matched blockage ratio?
Have you replicated the physical 3D nature of the experiment?
Are you measuring the AoA in the same way?
Have you non dimensionalised the same way as they did?

I would double check those first.

[Aeronautics El. K.]

I would also add: Are you sure you've used the correct boundary conditions? Irrespectively of the grid convergence study, are you sure that your boundaries don't affect the solution elsewhere in the domain? And, why are you using a density-based solver?