
[Sponsors] 
June 1, 2014, 10:46 
Drag in inviscid flow

#1 
New Member
Hakjin lee
Join Date: Jun 2014
Posts: 4
Rep Power: 4 
Dear all
 Euler simulation  Test model :NACA0012 airfoil (symmetric airfoil)  Mach number : 0.1 (incompressible flow)  Angle of attack : 0 deg. As above condition, there is no lift and drag As you known, D'Alembert proved that for incompressible flow and inviscid potential flow  the drag force is zero on a body moving with constant velocity relative to the fluid  Euler simulation  Test model :NACA0012 airfoil (symmetric airfoil)  Mach number : 0.1 (incompressible flow)  Angle of attack : 2 deg. However, in case of angle of attack of 2 deg. the drag force occur ! I don't know where the draq come from ? please explain the drag force in inviscid flow (Euler simulation) Thanks in advance Jinny 

June 1, 2014, 11:02 

#2 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,700
Rep Power: 33 
this is a classical issue in an aerodynamic course, generally the topic is illustrated by the flow problem of the lift generated by a 2D cylinder.
The key is in the circuitation generated by the position of the rear stagnation point (Kutta condition says it at trailing edge). Any textbook of basic fluid/aerodynamic can help you... just start see in...wikepedia http://en.wikipedia.org/wiki/Lift_%28force%29 

June 1, 2014, 12:42 

#3 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 476
Rep Power: 11 
Artificial/numerical dissipation and numerical error. A high order code with very little numerical dissipation should produce zero drag.


June 1, 2014, 13:01 

#4 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,700
Rep Power: 33 
As you said, the answer is that the code "implicitly" fix the Kutta condition ...it is as a check to compute the integral of the tangential velocity along the airfoil


June 1, 2014, 23:18 

#5 
New Member
Hakjin lee
Join Date: Jun 2014
Posts: 4
Rep Power: 4 
Dear Martin Hegedus
Thnak you for your reply ! You means that the drag force generated in Euler simulation is numerical error ? If I used highoder scheme, such as DGM, the drag force does not occur ? Um....Could you explain why the drag force does not occur in inviscid flow (Not potential flow) Thanks in advance jinny 

June 1, 2014, 23:21 

#6 
New Member
Hakjin lee
Join Date: Jun 2014
Posts: 4
Rep Power: 4 
Dear FMDenaro
Thanks, FMDerao As you said, I have to check the surface integral routine which calculate a normal force to the aifoil surface Thank you, have a nice day Jinny 

June 1, 2014, 23:59 

#7 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 476
Rep Power: 11 
Jinny,
Inviscid, incompressible, steady state flow is irrotational (due to vorticity transport equation), therefore inviscid incompressible steady state Euler is potential flow. Once the bound vortex reaches steady state, vorticity is not shed into the flow field, and then drag goes to zero. However, numerical error causes the bound vortex to decay and therefore vorticity needs to be constantly shed into the field to maintain it (and the implicit kutta condition). If there is no error, then the bound vortex does not decay and eventually all the vorticity in the field is transported away. On this page is a grid refinement study of the NACA 0012 airfoil at M=0.5 and alpha=1.25. http://www.hegedusaero.com/examples/.../Vassberg.html. You can see that drag drops as the grid is refined. For the case of FLO82HCUSP, drag basically approaches zero. AO_CFD has a more challenging time probably because of higher artificial dissipation. I assume the same is true for OVERFLOW. 

Tags 
d'alembert paradox, drag force, euler simulation, inviscid flow, naca0012 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Drag coefficient too high at flow around a cyclinder  Gunni  OpenFOAM Running, Solving & CFD  16  October 19, 2015 19:21 
Inviscid Turbulent flow  Vino  Main CFD Forum  10  August 29, 2013 15:07 
Nozzle flow simulation in inviscid and viscous  Cath  FLUENT  0  January 28, 2007 03:16 
Inviscid flow solver  luca_g  OpenFOAM Running, Solving & CFD  0  December 21, 2006 13:55 
Can 'shock waves' occur in viscous fluid flows?  diaw  Main CFD Forum  104  February 16, 2006 06:44 