Overpredicting Lift coefficent, NACA 4412
 

Hi all,

I am studying an airfoil similar to the NACA 4412 profile, and I am getting too high lift coefficient when comparing to experiment. I can't discuss the profile in question, but I notice the same behavior for NACA 4412.

My CL vs Angle of attack can be seen lying way too high compared to experimental data, see:
http://i.imgur.com/fIfFtzY.png

When i plot Cp vs chord (10 degrees) I can see that I have too low pressure on top, and too high pressure on the bottom. I have the same problem (especially on the suction side) for the NACA4412 profile
http://i.imgur.com/L78VcmY.png

- I am using the SST model in CFX. Y+ have been investigated and no longer affects the solution. I am below 1.

- Re is about 400 000

- I have tried using transition model, but am getting worse values.

- Tried matching turbulence intensity to match the experiments. 5% is set on the inlet and the length scale is adjusted so that the level is kept in the regions of interest. Ok method?

- A ran with k-epsilon showed closer similarities for this AOA, which is kind of unexpected for this type of flow?

- Using surface roughness gave me closer results, but the value used is way higher than in reality, so I think it might be coincidental. But it might give a clue of what the issue can be?

Can anyone give me some ideas of what can be incorrect in my simulation? Sorry I cant share too detailed images, but ask away if you have questions.

http://i.imgur.com/rKIXOVc.png

just an idea of the mesh resoultion close to the blade

Is your Cp chart showing turbulence transition on the top at about 0.8? Also, what is the wobbles in your CFD results on the Cp chart around 0.8?

I presume you have checked that you are converging tight enough. You mesh looks high quality.

Have you checked the mesh resolution along the chord? You say you have checked the y+, but it looks like this has resulted in very high aspect ratio elements adjacent the blade. You might need a finer mesh along the chord to improve mesh quality.

Also have you considered surface roughness?

Hi Glenn, Thanks for your reply and interest in this.

In the plots i have not used any transition model, if thats what you are referring to by turbulence transition. I would say that the flow seperation occurs at about 0.8. Bear in mind that this is not the 4412, but a more "bent" airfoil (more camber?).

Lift and Drag are stabile and all residuals go to the floor. I have tried running with 4 times more nodes along the chord and unfortunately have found no change for the better.

Now about surface roughness. The infrmation I have from the experimental guys is that surface roughness is measured to below 1 mu. Before i knew this I did a run with Ra = 15 mu. This turned out to be a great match at the top surface (see orange in figure below), but I'm having a hard time explaining it. What is the actual effect that the surface roughness model have on, in this case, the pressure?

The sand grain roughness was in this case calculated as:
"hs = 5.863Ra was assumed according to “A Simple Algorithm to Relate Measured Surface Roughness to Equivalent Sand-grain Roughness”, Thomas Adams, Christopher Grant, Heather Watson, 2012. "

http://i.imgur.com/M197cU3.png

As the CFX theory manual states: "Surface roughness increases wall shear stress and breaks up the viscous sublayer".

It looks like you need to investigate exactly what surface roughness the experimental device had. While you are at it I recommend measuring the form of the body as well. Small deviations from the modelled form will also explain differences.

I would also check your sensitivity to upstream turbulence. Don't forget that you need to define two values for most RANS turbulence models - so check a range of turbulence intensities and length scales would be a good pair of parameters.

What I can see from the experimental model is that the surface looks a bit "wavy". Not as in roughness, but rather long low amplitude wave patterns along the chord.

The turbulence intensity check i have performed consisted of setting the intesnity to fixed 3% and then do a parametric study of length scale. A length of 100mm, approximately the chord length, assured that i still had about 3 % in the freestream at the LE x coordinate. Not sur if this is the way to do it?

The wave pattern might explain your difference. Do you have some tools to measure the true surface?

No, what I was suggesting with the turbulence study was how sensitive your result is to the free stream turbulence. If you change the turbulence to 4% or 6%, does that make a significant change to the result? If no then your 5% value is OK. If yes then you better do a really accurate measure of turbulence intensity as the simulation is very sensitive to it. And do likewise with the turbulence length scale.

Along the lines of turbulence, why are you using such a high number? The experiment is wind tunnel data correct?

Did they measure the turbulence level in the tunnel and you are matching that? Wind tunnels often are below 1%.

singer1812,

A grid is placed in the tunnel and the measured turbulence intensity is around 3%