[sasanghomi]

Dear friends,

I am simulating fluid flow around the airfoil NACA 2414 at RE=10e6 and alfa =5 Degrees. The turbulence model is KW SST.
Unfortunately, the results are not that promising. Drag coefficient is 2 times as much reported in XFOIL software program.

Yplus is around 4-5 and the domain in large enough (40chord)

Which surface area is used for drag coefficient definition? (chord*domain thickness) ??
Any idea?

[ehsanspp63]

at first, you should check the reference area used by your experimental reference( or validated numerical data), in this case, you can use the reference area based on this link https://web.calpoly.edu/~rcumming/Airfoils_Wings.pdf). secondly, for k-w SST turbulence model, you should use yplus=1 or less. turbulence intensity at inlet boundary condition is also important. Finally, mesh quality is really important and you must use adequate convergence criteria in your simulation.

[sasanghomi]

Thank you so much. How much should be the turbulent intensity at inlet?
what is the meaning of Ncr=9 ?
I used the default setup in CFX (5% turbulent intensity at inlet)

[ghorrocks]

Have you read the FAQ on accuracy? https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Also, I would not regard XFOIL as a good benchmark result to assess accuracy.

[sasanghomi]

Thank you. 1 more question;

Do you think Mach number is important as well? I did not care about Mach number and just justified Reynolds number and compared CD & CL with the reference values.

[ghorrocks]

The rule of thumb is that under Mach 0.3 compressibility effects are small and can be ignored. But this is just a rule of thumb. If you want to be sure you should run with and without compressibility and see if it is important in your case.

[cfd seeker]

If you have already considered Re. No. then it is enough. To calculate the drag coefficient the reference area normally taken in Span*Chord. For 2D airfoil Span is taken as 1. So reference area becomes 1*Chord. But some people use different refernces to calculate reference area. So check how the reference area is taken in Xfoil.

When i was doing aerodynamic simulations in Fluent, the drag coefficient was v sensitive to Turbulent intensity/Turbulent length scale. What i was doing back then, was using the following formula to calculate the turbulent length scale l=0.4*Boundary Layer Thickness. As it is very difficult to estimate the B.L thickness for airfoil, so i was using the B.L thickness formula for Flat plate and then was reducing it by an order of magnitude. This estimate for turbulent length scale worked very well for aerodynamic simulations in Fluent. But when i tried the same simulations in CFX the default values of turbulence parameters were working fine.
I hope this would help you.

PHP Code:

http://jullio.pe.kr/fluent6.1/help/html/ug/node178.htm 


This is a reference to read about the turbulence parameters.

[sasanghomi]

That is interesting that when I simulate the flow at Re=10e4, everything is fine.
There is a perfect agreement between the results of CFX and XFOIL when the fluid flow is laminar.
So, it seems the problem comes from turbulence models even though I have decreased Yplus to 1. (I checked K-W SST and K-epsilon and Spalart Almaras)

Best Regards

[cfd seeker]

Originally Posted by sasanghomi

That is interesting that when I simulate the flow at Re=10e4, everything is fine.
There is a perfect agreement between the results of CFX and XFOIL when the fluid flow is laminar.
So, it seems the problem comes from turbulence models even though I have decreased Yplus to 1. (I checked K-W SST and K-epsilon and Spalart Almaras)

Best Regards

from this i got another clue. Try with the Transition turbulence model, it is quite possible that at 10^6 Re. No. the flow is still laminar on some part of airfoil and then it becomes turbulent. This also happened to me for some simulations, despite of very fine and good mesh i was not able to get good results for Cd. But then the transition model solved this problem Try this but take care that aprat of y+ 1, you also need fine mesh in chord direction like 30 to 40 points to properly capture the transition. I hope this gonna work for you.

[ghorrocks]

cfd seeker's comment is correct, you should look at the turbulence transition model.

But I also repeat that you should not regard XFOIL as an accurate benchmark, especially for more complex flows with turbulence, separations and transition.

[sasanghomi]

Thank you all.

1) Dear Horrocks, you are right. It seems that Xfoil results are not completely accurate. I made a comparison between the results of NACA 23015 Drag coefficient versus angle of attack mentioned in FOX Fluid Mechanics book and xfoil results. (Re=9*10e6 AOA 8 degrees). There is a discrepancy of 24%. (It could give us a rough data at least)

2) You guys are completely right. Transitional Turbulence option solved the problem. The results are getting close to xfoil results (it is still running). It should be mentioned that Yplus is around 1 and high resolution is used for discretization. So, I think that we can come to this conclusion that at least, two-equation models are not capable of simulating such simulation expect for SST which is equipped with transitional turbulence.

That was an interesting experience that I added to my basket.

Best Regards