# Drag in inviscid flow

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

 June 1, 2014, 10:46 Drag in inviscid flow #1 New Member   Hakjin lee Join Date: Jun 2014 Posts: 4 Rep Power: 5 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: 3,503 Rep Power: 40 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: 480 Rep Power: 12 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: 3,503
Rep Power: 40
Quote:
 Originally Posted by Martin Hegedus Artificial/numerical dissipation and numerical error. A high order code with very little numerical dissipation should produce zero drag.
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: 5 Dear Martin Hegedus Thnak you for your reply ! You means that the drag force generated in Euler simulation is numerical error ? If I used high-oder 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: 5 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: 480 Rep Power: 12 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 FLO82-HCUSP, 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 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 Gunni OpenFOAM Running, Solving & CFD 16 October 19, 2015 19:21 Vino Main CFD Forum 10 August 29, 2013 15:07 Cath FLUENT 0 January 28, 2007 03:16 luca_g OpenFOAM Running, Solving & CFD 0 December 21, 2006 13:55 diaw Main CFD Forum 104 February 16, 2006 06:44

All times are GMT -4. The time now is 13:25.