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

Airfoil negative drag coefficent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 21, 2004, 19:48
Default Airfoil negative drag coefficent
  #1
James Forrest
Guest
 
Posts: n/a
Hi, I am modelling a 2D airfoil in Fluent (using segregated 2nd order solver) and as I increase the angle of attack the drag (due to pressure) is decreasing. At angles greated than 10 degrees this drag force becomes negative - i.e. producing thrust!!!!! If a turbulence model is added the pressure drag still outweighs the viscous drag so overall drag is still negative. This is obviously not correct - can anybody shed any light on this? It's quite urgent as I have to write a report on this by next week. It seems that only the upper airfoil surface is producing negative drag which is also strange. I am quite confident that the quality of the mesh is good - I'm baffled! Thanks for any help anyone can offer.

James.
  Reply With Quote

Old   February 22, 2004, 00:41
Default Re: Airfoil negative drag coefficent
  #2
Praveen
Guest
 
Posts: n/a
First question that comes to my mind is whether your equation for drag is correct. This equation will involve the surface normal; if the direction of normal is wrong then you will get the wrong sign. If the magnitude of the drag seems correct except for the sign then this is most likely the problem. Then just reverse the direction of the normal.
  Reply With Quote

Old   February 22, 2004, 07:16
Default Re: Airfoil negative drag coefficent
  #3
James Forrest
Guest
 
Posts: n/a
Thanks for your reply. I don't think this is the problem as at zero angle of attack the drag is in the correct direction. It is only once I begin to increase the angle that drag decreases, then passes through zero and becomes negative. The drag vector is set to act in the positive x direction. The thing I find strange is that, for example, at 10 degrees AoA the drag on the bottom surface is positive, but the drag on the upper surface is a larger negative value. The net sum of these two forces leads to the negative drag coefficient.
  Reply With Quote

Old   February 22, 2004, 13:33
Default Re: Airfoil negative drag coefficent
  #4
James Date
Guest
 
Posts: n/a
James

I'm sure you have got your vectors wrong somewhere! Obviously the force will be in the correct direction at zero incidence when alpha = 0 even if you have the sin's and cos's wrong!

Send me the files if you still have a problem. I assume you're either doing aeronautics or ship science at soton!

Regards James
  Reply With Quote

Old   February 23, 2004, 02:03
Default Re: Airfoil negative drag coefficent
  #5
Charles Crosby
Guest
 
Posts: n/a
James,

You did convert axial force and normal force to lift and drag via

L=Fy cos(alpha) - Fx sin(alpha) D=Fx cos(alpha) + Fy sin(alpha)

didn't you? (refer to aerodynamics 101 ....)
  Reply With Quote

Old   February 23, 2004, 03:10
Default Re: Airfoil negative drag coefficent
  #6
James Forrest
Guest
 
Posts: n/a
Well, I solved the problem last night by simply rotating the grid by the required number of degrees. However, when using the above formula on data I had obtained previously, that also works! I think the problem was that I assumed Fluent already did that calculation when displaying lift and drag forces - I overlooked the fact that forces acting in the x and y directions were not necessarily acting parallel and normal to the oncoming flow.

Thanks to all that helped out!

James.
  Reply With Quote

Old   April 2, 2010, 16:44
Default the problem could turn out to be as simple as
  #7
lfc
New Member
 
Join Date: Feb 2010
Posts: 3
Rep Power: 7
lfc is on a distinguished road
Hi there

i have spent some time now getting used to fluent it is fairly simple for the most part but the devil is in the detail, i have been under-taking a comparison between 2d and 3d aerofoil cfd results in fluent, for the 3d models i change the coordinate system pre-meshing to allow for changes in AOA but for the 2D models i just changed the flow direction accordingly in boundary conditions>>velocity,direction and magnitude. this brought about some very strange results from the forces monitors for Cl and Cd. To cut to the chase, lift is taken to be as perpendicular to the free-stream flow and drag is taken to be parallel to the flow. so for my 3d models the flow was always coming into the flow domain horizontally so i had no problems like receiving negative drag ( the chance would be a fine thing), this only occurred when i changed the flow direction in the 2d models.

simply change the force vectors in the force monitors to:
for lift
x=-sin(alpha)
y=cos(alpha)

drag
x=cos(alpha)
y=sin(alpha)


i hope this helps,
lfc is offline   Reply With Quote

Old   April 9, 2011, 07:06
Default
  #8
Member
 
Aamer Shahzad
Join Date: Mar 2010
Posts: 58
Rep Power: 7
aamer is on a distinguished road
HI lfc....

it is true that lift and drag components will be, the way you wrote, for an incomg flow.... but what will be done , if there is a case in which motion is in still air...

.....For instance.... If i am rotating (azimuth motion) my wing in a still air from o to pi radians, through udf (i.e no inflow velocity). Assume that the wing is given constant angle of attack of 20 degree by tilting the whole grid. Now how will the components of lift and drag be given to fluent ????
aamer 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
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06
BlockMesh FOAM warning gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11
negative airfoil drag?? Robin FLUENT 4 January 7, 2010 17:29
airfoil optimizer chain with drag problem Arnolm OpenFOAM Running, Solving & CFD 2 October 18, 2009 13:43
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00


All times are GMT -4. The time now is 22:27.