CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

Is there a problem in the Euler solver?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 27, 2014, 18:16
Default Is there a problem in the Euler solver?
  #1
Member
 
Join Date: Sep 2013
Posts: 38
Rep Power: 3
Combas is on a distinguished road
I am doing some validation cases in Euler and Navier-Stokes with the naca0012 airfoil.

The Navier-Stokes 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 Navier-Stokes, 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
Attached Images
File Type: jpg NACA0012_Euler_Mach_015_Cdrag.jpg (23.6 KB, 17 views)
File Type: jpg NACA0012_Euler_Mach_015_Cp.jpg (14.0 KB, 14 views)
File Type: jpg NACA0012_Euler_Mach_015_Mach.jpg (15.9 KB, 15 views)
File Type: jpg NACA0012_Euler_Mach_015_Ptot.jpg (17.8 KB, 17 views)
Attached Files
File Type: gz inv_NACA0012_Roe_d.cfg.gz (3.0 KB, 4 views)
Combas is offline   Reply With Quote

Old   March 27, 2014, 21:17
Default
  #2
hlk
Senior Member
 
Heather Kline
Join Date: Jun 2013
Posts: 158
Rep Power: 4
hlk is on a distinguished road
Yes, for a 2-D 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.
hlk is offline   Reply With Quote

Old   March 28, 2014, 05:31
Default
  #3
Member
 
Join Date: Sep 2013
Posts: 38
Rep Power: 3
Combas is on a distinguished road
Thank you for your answer, but what seems strange to me is that with the same mesh and the same scheme but in Navier-Stokes, 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
Combas is offline   Reply With Quote

Old   March 28, 2014, 14:49
Default
  #4
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Quote:
Originally Posted by Combas View Post
Thank you for your answer, but what seems strange to me is that with the same mesh and the same scheme but in Navier-Stokes, 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
Hi,

My answer is related with Heather's reply. The key is the artificial dissipation introduced by the numerical scheme.

Navier-Stokes grids have been created to simulate problems with boundary layers, in other words they have an a-priori grid adaptation that has beneficial effect when you run a Navier-Stokes 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 high-stretching 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 a-priori 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
fpalacios is offline   Reply With Quote

Old   March 28, 2014, 16:48
Default
  #5
Member
 
Join Date: Sep 2013
Posts: 38
Rep Power: 3
Combas is on a distinguished road
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
Combas is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with compiling new solver palazi88 OpenFOAM Programming & Development 2 December 24, 2013 20:52
Abaqus/cfd steady-state solver problem skuznet Main CFD Forum 0 November 24, 2013 22:13
Problem with implicit unsteady solver CCMuser STAR-CCM+ 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


All times are GMT -4. The time now is 15:13.