CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

CFD on Aerofoil Flaps

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 19, 2014, 06:57
Default CFD on Aerofoil Flaps
  #1
New Member
 
Ryan Paul Galea
Join Date: Mar 2014
Posts: 2
Rep Power: 0
galcom is on a distinguished road
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
galcom is offline   Reply With Quote

Old   March 19, 2014, 17:39
Default
  #2
Senior Member
 
truffaldino's Avatar
 
Join Date: Jan 2011
Posts: 234
Blog Entries: 5
Rep Power: 8
truffaldino is on a distinguished road
Quote:
Originally Posted by galcom View Post
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
truffaldino is offline   Reply With Quote

Old   March 19, 2014, 17:45
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,568
Rep Power: 20
FMDenaro will become famous soon enough
Quote:
Originally Posted by truffaldino View Post
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 ...
FMDenaro is online now   Reply With Quote

Old   March 19, 2014, 17:55
Default
  #4
Senior Member
 
truffaldino's Avatar
 
Join Date: Jan 2011
Posts: 234
Blog Entries: 5
Rep Power: 8
truffaldino is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
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.
truffaldino is offline   Reply With Quote

Old   March 20, 2014, 10:28
Default
  #5
New Member
 
Ryan Paul Galea
Join Date: Mar 2014
Posts: 2
Rep Power: 0
galcom is on a distinguished road
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?
galcom is offline   Reply With Quote

Old   March 20, 2014, 16:43
Default
  #6
Member
 
Totalsim's Avatar
 
Jon
Join Date: Mar 2013
Posts: 40
Rep Power: 4
Totalsim is on a distinguished road
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.
__________________
TotalSim CFD Engineer
www.totalsimulation.co.uk
Totalsim is offline   Reply With Quote

Old   March 23, 2014, 09:17
Default
  #7
Senior Member
 
Lefteris
Join Date: Oct 2011
Location: UK, Greece
Posts: 187
Rep Power: 5
Aeronautics El. K. is on a distinguished road
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?
__________________
Lefteris

Aeronautics El. K. is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
STAR-Works : Mainstream CAD with CFD CD adapco Group Marketing CD-adapco 0 February 13, 2002 13:23
Where do we go from here? CFD in 2001 John C. Chien Main CFD Forum 36 January 24, 2001 22:10
ASME CFD Symposium, Atlanta, July 2001 Chris R. Kleijn Main CFD Forum 0 September 13, 2000 04:48
ASME CFD Symposium, Atlanta, July 2001 Chris R. Kleijn Main CFD Forum 0 August 21, 2000 04:49
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 18:09.