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

result on airfoil wortmann fx63-137 simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 29, 2011, 05:29
Default result on airfoil wortmann fx63-137 simulation
  #1
New Member
 
jason fortune
Join Date: Jan 2011
Posts: 4
Rep Power: 6
jdfortune is on a distinguished road
Hi,
I am doing a simulation on this airfoil to obtain the similar aerodynamic curve as from the literature
http://www.worldofkrauss.com/foils/243

the maximum Cl is obtained at correct angle which is at 11 degree. However, the value is slightly off. The value obtained from simulation is
Cl=1.7 while real Cl=2.013 from the website
Cd=0.18 which is much higher than real Cd=0.05

Im using spalart allmaras and Re=1 million
any advice is appreciated thanks

attached is the Y+ plot on airfoil wall.
And here is the url to download my mesh file
http://www.sendspace.com/file/tld05b
Attached Images
File Type: jpg Capture.jpg (24.3 KB, 20 views)
jdfortune is offline   Reply With Quote

Old   January 29, 2011, 10:35
Default
  #2
Senior Member
 
Join Date: Nov 2009
Posts: 411
Rep Power: 10
DoHander is on a distinguished road
You won't be able to obtain the correct Cd with Spalart Allmaras, this is because the model, as implemented in Fluent, assumes the entire flow domain is turbulent which is not true.

For a short explanation check this article:

http://larcase.etsmtl.ca/PDF/Note-Paul-f.pdf

Do
DoHander is offline   Reply With Quote

Old   January 29, 2011, 10:36
Default
  #3
Senior Member
 
Join Date: Nov 2009
Posts: 411
Rep Power: 10
DoHander is on a distinguished road
In Fluent 12 and 13 you can use a transition model, this will give you a better Cd.
DoHander is offline   Reply With Quote

Old   January 30, 2011, 11:47
Default
  #4
New Member
 
jason fortune
Join Date: Jan 2011
Posts: 4
Rep Power: 6
jdfortune is on a distinguished road
thank you for the input DoHander, very much appreciated.
I've read the paper you gave and it seems that fully turbulent model on the entire domain is the reason for overprediction of Cd. So the overprediction is due to the skin friction alone or both pressure and friction drag?

I'm using Fluent 6.3, so does fluent 6.3 has transition model?
Or do i have to shift to version 12/13?

How about the error in Cl (around 15%)? is it due to the meshing not being fine enough?

thanks.
jdfortune is offline   Reply With Quote

Old   January 31, 2011, 17:17
Default
  #5
Member
 
David Stanbridge
Join Date: Apr 2010
Location: Norwich, UK
Posts: 58
Rep Power: 7
swiftaircraft is on a distinguished road
Also your y+ values are very high. For accurate predictions you need to resolve the boundary layer. You will not be doing that with the mesh you currently have.
swiftaircraft is offline   Reply With Quote

Old   January 31, 2011, 20:26
Default
  #6
Senior Member
 
Join Date: Nov 2009
Posts: 411
Rep Power: 10
DoHander is on a distinguished road
@jdfortune Fluent 6.3 doesn't have any transition model, you will need to switch to Fluent 12 or 13 if you want to use a transition model.

Also your mesh is bad, as swiftaircraft has noticed. If you want good results for Cd y+ must be less than 1 OR from 30 to 100. You can't use a mesh with y+ from 1 to 30 !!!

My advice is to try to keep your y+ from 30 to 100, this will allow you to use a reasonable mesh (from a memory usage perspective).
DoHander 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
NO STAGNATION POINT FOR AIRFOIL SIMULATION Rif Main CFD Forum 6 February 4, 2008 08:33
Airfoil Simulation for Validation Purposes Angela Bong Main CFD Forum 7 September 13, 2006 13:04
how to make sure the simulation result is correct? sham81 CFX 3 March 22, 2004 17:41
TASCflow simulation result problem? Mason CFX 0 February 22, 2004 08:54
Looking for :Multi-element airfoil simulation Larry Main CFD Forum 0 February 8, 2001 11:14


All times are GMT -4. The time now is 04:49.