# Airfoil negative drag coefficent

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

 February 21, 2004, 19:48 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.

 February 22, 2004, 00:41 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.

 February 22, 2004, 07:16 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.

 February 22, 2004, 13:33 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

 February 23, 2004, 02:03 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 ....)

 February 23, 2004, 03:10 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.

 April 2, 2010, 16:44 the problem could turn out to be as simple as #7 New Member   Join Date: Feb 2010 Posts: 3 Rep Power: 8 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,

 April 9, 2011, 07:06 #8 Member   Aamer Shahzad Join Date: Mar 2010 Posts: 58 Rep Power: 8 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 ????

 March 8, 2016, 10:31 #9 New Member   Limam Join Date: Feb 2016 Posts: 1 Rep Power: 0 Hi, I'm simulating drag and lift coefficient of flow around a cylinder but my drag coefficient keep fluctuating between negative and positive value and some time it is even negative, is this possible and if yes what is the cause behind this, thank you in advance please help.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06 gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11 Robin FLUENT 4 January 7, 2010 17:29 Arnolm OpenFOAM Running, Solving & CFD 2 October 18, 2009 13:43 Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00

All times are GMT -4. The time now is 00:57.