# negative airfoil drag??

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

January 7, 2010, 12:58
negative airfoil drag??
#1
New Member

Robin East
Join Date: Oct 2009
Posts: 5
Rep Power: 9
im modelling a low speed (50m/s) airfoil (NACA 4415) in fluent and at zero angle of attack i have a higher than expected drag coefficient at about 0.02. when the angle of attack is increased to 5 degrees the value for the drag coefficient then becomes negative for some reason?? the lift coefficient in first case is 10% out and 45% out in the latter.

to mesh the airfoil i followed the tutorial http://courses.cit.cornell.edu/fluent/airfoil/step1.htm as suggested in many other posts. i also tried using the tranisent SST solver technique as opposed to SKE as the fluent user manual suggests that that is a better solver for negative pressure gradients. also i read that it was more suitable for low Y+ values that occur with finer meshes although i have no idea why?

for the solution methods i used SIMPLEC green gauss cell based for the gradient standard for the pressure and second order upwind for all the others as recomended in many other topics.

the problem is set the the standard solution controls (under relaxations etc) and converges after 162 iterations and comes up with no messages saying turbulent viscosity ratio limited etc.

ive attached a residuals plot, force report and summary report if that helps.

could anyone suggest what is wrong / how i could get more accurate answers?
Attached Files
 Drag Report 2.txt (2.2 KB, 23 views) Summary 2.txt (11.9 KB, 10 views)

January 7, 2010, 13:04
#2
New Member

Robin East
Join Date: Oct 2009
Posts: 5
Rep Power: 9
ooops forgot to add the scaled residuals
Attached Images
 Scaled residuals 2.jpg (97.5 KB, 31 views)

 January 7, 2010, 14:39 #3 Senior Member   Join Date: Nov 2009 Posts: 411 Rep Power: 12 "m modelling a low speed (50m/s) airfoil (NACA 4415) in fluent and at zero angle of attack i have a higher than expected drag coefficient at about 0.02. when the angle of attack is increased to 5 degrees the value for the drag coefficient then becomes negative for some reason?? the lift coefficient in first case is 10% out and 45% out in the latter." Do you use the laminar or the turbulent model ??? If you use a turbulence model you should note that at such a low speed you will have a large portion of your airfoil in the laminar region and only a part of the airfoil in a completely turbulent zone. You have a NEGATIVE drag because you didn't changed the directions for Lift and Drag according to the new angle (0,1) for Lift is OK only for zero degree, same for Drag (1,0). For 5 degree you must change these values. Do

 January 7, 2010, 16:06 #4 New Member   Robin East Join Date: Oct 2009 Posts: 5 Rep Power: 9 I am using a turbulent model, (transient SST). is there a method of setting the flow to enter the domain as laminar flow and transition to turbulent flow? i tried running the simulation with a laminar model and the answers seemed to be less accurate in gereral (even with changing the direction of the force reports as required.) Is that likly to be because my model is wrong?? if i were to increase the velocity of the flow would that help yeild more accurate Cl and Cd values if i used a turbulent model?

 January 7, 2010, 17:29 #5 Senior Member   Join Date: Nov 2009 Posts: 411 Rep Power: 12 I think Fluent 12 has a turbulence model that include the transition from laminar to turbulence (at least they claim so - I've used only Fluent 5 - 6.3 so I'm not an expert in Fluent 12). It is a new model developed by Menter, check your Help files for turbulence models. This should partially solve the large discrepancy between the calculated Cd and the experimental value. A different solution will be to use for example Xfoil in order to have an estimation of the transition point and then you can split your mesh roughly in 2 regions - a turbulent region and a laminar region. This must be done in geometrically. Then in Fluent you set the respective region as "laminar region" and use a turbulence model. It should give you less then 20% error for Cd. If you need more details about the second solution send me a private message and I will give you my email address. Do

 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 James Forrest Main CFD Forum 8 March 8, 2016 10:31 gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11 mahzironrazak FLUENT 0 October 19, 2009 18:41 Arnolm OpenFOAM Running, Solving & CFD 2 October 18, 2009 13:43 Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00