|
[Sponsors] |
November 21, 2018, 04:58 |
Airfoil - Turbulence Model
|
#1 |
Senior Member
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 292
Rep Power: 14 |
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? |
|
November 25, 2018, 03:18 |
|
#2 |
New Member
ehsan
Join Date: Nov 2018
Posts: 4
Rep Power: 7 |
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.
|
|
November 25, 2018, 13:22 |
|
#3 |
Senior Member
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 292
Rep Power: 14 |
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) |
|
November 25, 2018, 16:24 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
November 26, 2018, 02:46 |
|
#5 |
Senior Member
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 292
Rep Power: 14 |
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. |
|
November 26, 2018, 04:40 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
November 26, 2018, 05:36 |
|
#7 |
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20 |
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:
This is a reference to read about the turbulence parameters. |
|
November 27, 2018, 00:31 |
|
#8 |
Senior Member
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 292
Rep Power: 14 |
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 |
|
November 27, 2018, 02:30 |
|
#9 | |
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20 |
Quote:
|
||
November 27, 2018, 17:17 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
November 28, 2018, 06:54 |
|
#11 |
Senior Member
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 292
Rep Power: 14 |
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
NEW turbulence TRANSITIONAL model | giammy92 | OpenFOAM | 3 | June 30, 2016 09:47 |
Airfoil lift and drag using k-kl-omega turbulence model | hylleman | OpenFOAM Running, Solving & CFD | 6 | June 17, 2016 15:10 |
Overflow Error in Multiphase Modelling with Two Continuous Fluids | ashtonJ | CFX | 6 | August 11, 2014 14:32 |
What model of turbulence choose to study an external aerodynamics case | raffale | OpenFOAM | 0 | August 23, 2012 05:45 |
Centrifugal Pump and Turbulence Model | Michiel | CFX | 12 | January 25, 2010 03:20 |