Problem with Cp results.
 

Hi am trying to compare my CFD data with Exp data for a 2-D airfoil case but although the CL values are very close it seems that the CFD over predicts the Cp over the leading edge of the airfoil. Does anyone know why this happens?? I am using the K-w SST model at Re approximately 1x106.

I would be grateful for any comments.

Could be separation or wind tunnel walls. What is your angle of attack and which airfoil?

I don’t think is separation since it happens at low angles of attack 4 and 8 deg. The airfoil is a NACA 4415. Could it have anything to do with the turbulence model? How do I correct for the wind tunnel walls?
I thought that the effect of the wind tunnel walls is opposite (increases the suction peck) since the air between them and the model accelerates is that not the case?

It could be the turbulence model, but, if you do not expect a separation bubble, I'm skeptical. At the leading edge, the boundary layer is thin. In general, and for separated flow, I expect the difference in cp to show up and the trailing edge where the boundary layer thickens.

The NACA 4415 is thick and your Reynolds number is high. So I'm skeptical about separation at the L.E. also.

What is your Mach number? I'm assuming it is less than 0.3. If it is greater, you may also be seeing compressibility affects.

In regards to wind tunnels, there are wind tunnels with porous walls, slotted walls, and solid walls. The porous and slotted wall ones can be challenging to compare to. But they are required for high subsonic flow.

In regards to solid walls, for zero angle of attack, what you say is true. The Cp peak will be higher. As the angle of attack is increased, I'm not sure what will happen since there is a trade off going on, the location of the stagnation point and the area constriction. So, yes the area constricts causing the flow to increase in speed, but the stagnation point also moves up (I believe) causing the flow to slow down.

To model the WT, just create a rectangular box and insert the airfoil in it. Assuming your WT is solid walls. Keep it simple to get the trend. The WT walls can be slip (i.e. no boundary layer).

I don’t expect a separation bubble at the leading edge. My Mach number is well below 0.3 and I am currently using a similar domain as the one you suggested with moving walls.
I know that the k-w sst model sometimes over predicts the turbulent kinetic energy does this have an impact on the Cp?

In general, and this is from my own limited (as far as I'm concerned!) experience, the impact will depend on thickness, chamber, and Re and is usually seen more at the trailing edge than the leading edge, in regards to cp. The thicker, and I believe(?) more chamber you have, the more difference you'll see. Also the lower the Re. I wish I could point out results, but a reference has not come to mind. However, for something like a NACA 0012, the SA and SST, I believe, give similar results for angles lower than stall and higher Re numbers (i.e. 1e6).

How did your results modeling WT walls turn out?

My results are similar as before. I did not see any major difference in the results with the only exception at high angles of attack where I had convergence problems. I believe that it might be due to blockade effect.


I used both models SA and SST. Both models predict similar Cl within 5% of each other for the same Re (1e6 - 2e6) and mesh. The SST predicted stall a bit better than the SA.


I also used Xfoil which yields results close to the CFD study which makes me wonder that the problem might be with the experimental results.

Thanks for your update.

Can you provide a reference for the WT results and which flow solver are you using?

I ran my CFD code, AT CFD (structured RANS with SA turb model), on the 4415. http://www.hegedusaero.com/software.html

The outer boundary is 150x the chord, the 4415 includes the base, there are 151 points on the top surface, 151 points on the bottom surface, and the points are clustered at the leading and trailing edge such that the cell length is 1/10 the average cell length. The first offwall spacing is 1.0e-5. There are 151 points in the z direction. It is a C grid.

The first two plots are cl vs. alpha for AT CFD vs. various published reports. The first plot is for Re 1.0e6 only, the second plot is for various Res. The Ohio State data was digitized from http://wind.nrel.gov/OSU_data/reports/3x5/n4415.pdf The NACA data was digitized from reports retrieved from ntrs.nasa.gov. The Abbott and von Doenhoff data was digitized from "Theory of Wing Sections"

The last two plots are cp comparisons to the Ohio State data for alpha 0.0 and 6.2. Not sure the reason for the discrepancy between AT CFD and data. The data was taken in the 3'x5' WT (3' wide, 5' high). The chord for the airfoil was 1.5'. The airfoil span ran along the width. Thus the aspect ratio is only 2. And the height/chord ratio is 3.33. Unfortunately, in my opinion, this means that the airfoil is too big for the tunnel. Any cp errors could be due to this. However, I could not find better cp data. Also, I definitely do not trust the stall data. But, I don't necessarily trust the NACA data either. The NACA TN 1945 data for Re 1e6 looks odd and the NACA TR 832 data was for a low to high subsonic Mach number run. Therefore the TR 832 WT may have been slotted. The Abbott and von Doenhoff data at 3e6 seems to be qualitatively inline with the CFD results. That's good.

My angles of attack of 10 to 17 degrees were slightly unsteady on the trailing edge. Thus the wiggles in the cl curve. I did not time average the CFD results. I just took what I had at the point I stopped the code. The unsteadiness could be because of physics, the trailing edge grid clustering, and/or the method (DADI) used to converge the results. Most likely the RANS/SA physics was on the verge of being unstable and the DADI method, in conjunction with the grid, pushed it over the edge.

Hi Dear

I have a question about best turbulence model and mesh generation for contraction nozzle in a subsonic wind tunnel, entrance velocity is about 2.5 m/s and exit velocity is 20 m/s , cross section of nozzle in entrance is square and in exit is rectangular

do you think K-e- RNG is good?

Thanks

Best Regard