
[Sponsors] 
March 27, 2014, 18:16 
Is there a problem in the Euler solver?

#1 
Member
Join Date: Sep 2013
Posts: 39
Rep Power: 5 
I am doing some validation cases in Euler and NavierStokes with the naca0012 airfoil.
The NavierStokes solver seems to give good results compared to the ones provided by NASA (http://turbmodels.larc.nasa.gov/naca0012_val_sa.html) In my opinion, at low Mach number, the Euler solver should give zero drag (in 2D). Unfortunately, it is not what I get with the naca0012 airfoil. For example, at zero angle of attack, I get Cd = 0.0004 (even if it is not huge, it is not negligible). When I zoom on the flow around the airfoil, there is a loss of speed near the airfoil, and so a loss of total pressure, which could explain the drag I get. My question is: is it a problem of numerical scheme, or a problem of mesh (it is the same mesh as the one used for NavierStokes, so with very thin cells near the boundary), or a problem in the Euler solver? I put the some files in attachment to illustrate what I said. Thank you for your answers Laurent 

March 27, 2014, 21:17 

#2 
Senior Member
Heather Kline
Join Date: Jun 2013
Posts: 259
Rep Power: 6 
Yes, for a 2D body in inviscid flow there should be zero drag (d'Alembert's paradox).
The small finite drag is likely due to numerical dissipation, which is the same mechanism that enforces the Kutta condition here. Most if not all CFD codes have this effect to some extent. Mesh refinement can reduce the magnitude, as would reduced numerical error within the scheme. 

March 28, 2014, 05:31 

#3 
Member
Join Date: Sep 2013
Posts: 39
Rep Power: 5 
Thank you for your answer, but what seems strange to me is that with the same mesh and the same scheme but in NavierStokes, results are much better (I get exactly the drag given by NASA on http://turbmodels.larc.nasa.gov/naca0012_val_sa.html so a numerical error on Cd below 0.0001)
And the loss of velocity near the wall should not happen: it looks like a boundary layer with a very low friction coefficient... That is why I am wondering if the Euler solver does not have a problem... Laurent 

March 28, 2014, 14:49 

#4  
Super Moderator
Francisco Palacios
Join Date: Jan 2013
Location: Long Beach, CA
Posts: 342
Rep Power: 7 
Quote:
My answer is related with Heather's reply. The key is the artificial dissipation introduced by the numerical scheme. NavierStokes grids have been created to simulate problems with boundary layers, in other words they have an apriori grid adaptation that has beneficial effect when you run a NavierStokes problems. But these grids are a very bad choice when you try to run an Euler problem (completely different behavior on the wall: hyperbolic vs. elliptic). So… with highstretching grids, the convective scheme is not adding the optimal dissipation (in the normal direction the wall) and you detect that strange effect. Obviously, if you solve a NS problem, the viscous effects are dominant close to the wall and the solution is correct. Conclusion, the apriori adaptation should be done based on the equation that you are solving. Otherwise it will deteriorate the convergence and the solution quality because you are adapting some features that are not present in your continuous model. Thanks for using SU2, Best, Francisco 

March 28, 2014, 16:48 

#5 
Member
Join Date: Sep 2013
Posts: 39
Rep Power: 5 
Thank you very much for this answer that solves my problem. So I am going to try better meshes for Euler cases.
Thank you for your great work! Best regards, Laurent 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Abaqus/cfd steadystate solver problem  skuznet  Main CFD Forum  2  June 11, 2016 15:46 
Problem with compiling new solver  palazi88  OpenFOAM Programming & Development  2  December 24, 2013 20:52 
Problem with implicit unsteady solver  CCMuser  STARCCM+  2  March 3, 2010 12:20 
Problem Interface Solid Fluid with wall velocity Solver v12  hills1  CFX  2  October 12, 2009 05:36 
compressible two phase flow in CFX4.4  youngan  CFX  0  July 1, 2003 23:32 