
[Sponsors] 
August 12, 2012, 11:59 

#21 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
Sponsored Links


Sponsored Links 
August 12, 2012, 12:17 

#22  
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Quote:
What is the difference between solid (fluid) and interiorsolid zones? Should it be deforming? When I change interiorsolid to deforming, the wing starts to move but the error appears again. The wing tips remain in the domain during the movement of the wing. 

August 12, 2012, 22:58 

#23 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
You don't need deforming. You don't have a deforming boundary. You could use it if your wing stretch.


August 12, 2012, 23:38 

#24 
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 10 
Hi guys,
when handling with dynamic mesh, you don't need to change any boundary type. 1After Creating geometry and mesh generation in Gambit, just Define your boundary types: one Farfield b.c. for for your domain and one symmetry at your wing root. Do not bother yourself by defining wall b.c.s 2Import the mesh file into Fluent as you have generated in Gambit and do not change any boundary type. 3Write your UDF file, probabely by Define_cg_motion and compile it. 4Hook your UDF in dynamic mesh panel.Remember to active Remeshing option. 5Your time step must be below 0.00001, your case is 3d and computationally costly. 6Attention!!drag is defined in opposite direction of motion and lift is always perpendicular to drag. you should know drag and lift normal vectors at each time step to obtain correct values of lift and drag. THESE values may be obtained negative if you don't define corresponding vectors properly. You may write an additional line in your UDF code to get AOA at each time step. Good luck 

August 13, 2012, 20:32 

#25  
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Quote:
The 3D model still does not work even when I use very small time step. I still don't understand why I get the error when the wing tips are not going outside of the domain and all settings are correct. For the 3D model, I increased the thickness of the domain on each side for 5 cm, is that enough or it should be the same as the wing length (55 cm) on each side? Can it be the cause of error? I have attached a screenshot of lift curve that I simulated today but every time I start the simulation, the curve is different! The highest amount of Cl is around 3.0 which seems to be wrong. As a substantial amount of lift is generated during the flapping motion, can it be meaningful? Which of the reference values should be selected to allow Fluent to calculate cl? Should I change the area and length? 

August 13, 2012, 21:16 

#26  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 10 
Quote:
By the way, in implementing dynamic mesh you should consider the domain large enough to minimize the grid changes affecting boundary faces. Reference Area for calculating Aerodynamic coefficients of the wing is usually considered: MAC*SPAN which is referring to mean aerodynamic chord multiplied by span. 

August 13, 2012, 22:33 

#27 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
I took my aerodynamics course since a long time ago. As Syavash said, your domain must be enough big to apply the symmetry condition which means that there is no no mass transfer on that surfaces.
For the vortex on the tip it depends of the flow field (http://en.wikipedia.org/wiki/Wingtip_vortices). You have to chose your reference area which is generally a planform (projected) area. Most of the time in fluid mechanics, the reference area is given by the projection on the vertical plane, but in aerodynamics the reference area is the projection of the wing on the horizontal plane. You can check the area defined as planformed at http://en.wikipedia.org/wiki/Lift_coefficient. Theoretically you could use the MAC chord, but personally, I had never seen aerodynamics coefficients defined like that in graphs. Don't break your head with the MAC chord (http://en.wikipedia.org/wiki/Chord_(aircraft)). The reference area is simply the product of the chord and the span. For the length of reference, it is the chord in aerodynamics. In fluid mechanics, for example the reference length is the diameter of a tube but someone could use the length of the pipe. You have to change theses values in "Reference values". Don't forget to click on "Compute from" and select the farfield or inlet 

August 14, 2012, 19:40 
none

#28 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
Maybe you could have something like that.


August 15, 2012, 02:20 

#29  
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Quote:


August 15, 2012, 17:50 

#30  
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Quote:
First simulation, lift force: 0.4 N when the thickness of domain is equal to the wing length but in other directions the boundary is 20 chord lengths away from the airfoil Second simulation, lift force: 0.8 N when the thickness of the domain is three times wing length According to the Fluent manual, the boundary for an airfoil should be placed far enough from the airfoil. Is that true along the wing length? 

August 15, 2012, 19:04 

#31  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 10 
Quote:
Good point, I bring an example: my friend has experimentally tested a 3d wing in a wind tunnel. The tunnel test section is such that it can only enclose whole the wing in spanwise direction (root to tip). As it can be seen this condition does not let to capture tip vortex effects. In a comparative manner and in order to validate the test results with numerical ones, he decided to simulate the wing in Fluent. But he didn't extend computational domain further than tip location in spanwise direction.Why? because he would only intended to compare experimental results with numerical,thus computational domain size must be the same as experimental condition in spanwise direction(only in spanwise). Conclusion: you must look at your experimental condition in which data are obtained and set your domain width depending on it. By the way if you want to consider tip vortex effects, you should extend domain at least 8 times of semi span (8*0.5*span). Goodluck. 

August 15, 2012, 19:06 

#32 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
Yes. It's true along the wing. It should be the same distance as your radius for the far field. In aerodynamics, it could be hundred times the dimension of the plane. You need a cluster for such computation. A pretty good dimension for a computer would be 5 times the dimension of the span. The length could be 5 times the span in front and 10 times the span at the back to catch the wake behind the airfoil.


August 17, 2012, 12:25 

#33 
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Finally, I could do the simulation without the negative cell error. However, the lift curve does not seem to be correct and is not smooth.
Also, every time I do the simulation the Yaxis values (lift coefficient) change although I use the same values in the "Reference Values"and boundary conditions. Do you know why this happens? Please see the attachment. 

August 17, 2012, 14:58 

#34 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
According to your drawing, your lift is on zaxis and your drag is on xaxis. I don't know the name on the force coefficient on the third direction that you have drawn. When you select Lift (coefficient) in Monitors, you should change your "Force Vector" to (0, 0, 1). The name lift of drag in Monitors does not mean that the "Force Vector" is in the good direction. You must verify the "Force Vector" according to the position of your drawing.
If you want the drag coefficient, your "Force Vector" is (1, 0, 0). 

August 17, 2012, 19:02 

#35  
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Quote:
I corrected the direction of lift and drag forces as you said but I still get wrong lift and drag graphs. Could you look at those, please? 

August 24, 2012, 08:16 
Explaining lift & Drag curves

#36 
Member
Join Date: Aug 2012
Posts: 36
Rep Power: 7 
Finally, I managed to plot lift & drag coefficient curves for a pitching/rolling 3D wing. However, I have difficultly in understanding them.
According to my results, more lift is generated during downstroke while the generated lift during upstroke is low. (Please see the screenshot) I need to calculate an average lift coefficient that the wing can produce but this number is too low. Although cl goes up to 4.2, the mean cl is 0.79. Is it because the values of cl go to negative direction? My questions is: it is said that a flapping/pitching wing can produce more lift than a static wing with the same AOA and velocity. In my case, the simulation of the wing in the steadystate at AOA of 10 and 4 m/s produces cl 1.1 while for the transient one, the mean cl is 0.79. Why is the average lift lower than the static? 

August 24, 2012, 19:37 

#37 
Member
Guiliguili
Join Date: Aug 2010
Location: Montréal
Posts: 94
Rep Power: 9 
I had never heard about that theory but I guess that they didn't have a negative value of AOA because your negative lift will decrease your total lift.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
lift and drag coefficients around a ground vehicle  Pedro  CFX  3  September 5, 2012 18:31 
Design of a flapping wing aircraft  yahya_azizi  FLUENT  0  July 11, 2012 11:26 
Great lift coefficients but negative drag coefficient?!  nez  FLUENT  0  November 28, 2011 14:57 
Lift and Drag on airplane wing  Arj  CFX  4  October 6, 2006 04:05 
Lift and Drag Coefficients Reliability  Luis  FLUENT  2  December 27, 2005 15:45 
Sponsored Links 