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

asymmetry

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 3, 2005, 13:07
Default asymmetry
  #1
Anmol
Guest
 
Posts: n/a
Hi,

I am solving flow around an airfoil with triagular mesh at a Reynold's # ~1,000,000. The pressure distribution is not exactly symmetrical. I tried grid refinement and reducing residuals but it helps little. If anyone can suggest a reason, I would be really thankful.

Regards, Anmol
  Reply With Quote

Old   July 3, 2005, 15:32
Default Re: asymmetry
  #2
Jason
Guest
 
Posts: n/a
Tet meshes run into problems like this. Grid refinement will help, but you have to refine the entire flow field, not just local to the model. Even a quad mesh may run into this if the mesh is different above and below the model. The best recommendation I have is to use a structured mesh (quad mesh). This way you can control the mesh above and below the airfoil and create a symmetrical mesh above and below the airfoil. Unfortunately due to numerical averaging, you may still get a small amount of lift on the airfoil. Run the model at a couple of angles of attack to calculate a Cnalpha... then use this to calculate the rotational error in your 0deg model. Odds are it's VERY small.

I've been told a couple of other tricks that are supposed to help (unfortunately I was told these after that project was over, so I did not get a chance to test it and see if it works). These tricks are for the segregated solver, not sure how well they'd carry over to the coupled solver (be careful of your Mach number... Coupled solver does do some pre-conditioning to allow for low speed flow analysis, but the segregated solver is typically a better choice for low speed flow). When you initialize the solution, initialize it closer to stagnation than to freestream... i.e. initialize the solution with a velocity about 25 to 50% of the freestream velocity and calculate at a static pressure at this speed that results in the same total pressure as the freestream. Also, the PISO scheme for Pressure-Velocity Coupling is supposed to help. Like I said, I never got to try these, so I'm not sure if they're going to work.

One other thing... you mention "reducing residuals"... I'm guessing that you're talking about reducing the convergence criteria for the residuals... Are you monitoring the forces on the airfoil to make sure they really are converged? Judging convergence only by the residuals is dangerous because of all of the normalizing and what-not that they go through before they are presented. Your residuals can be very low, or leveled off, but the forces are still leveling off to a converged value... It's very important that you monitor whatever it is you're trying to get out of the model to make sure it's converged!

Hope this helps, and good luck, Jason
  Reply With Quote

Old   July 4, 2005, 03:29
Default Re: asymmetry
  #3
Luca
Guest
 
Posts: n/a
I run into the same problem( well, it's not such a dangerous problem...) I had a simmetric profile on a wing, with a simmetric hexaedral mesh. At 0 deg the lift is not perfectly null but nearly. No problem! Luca
  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
Asymmetry induced by the mesh Ale FLUENT 1 December 14, 2007 02:35
Asymmetry in SIMPLE-R algorithm Naresh Main CFD Forum 0 May 31, 2006 22:32
Asymmetry from symmetrical boundary conditions Bearcat Main CFD Forum 8 January 25, 2006 03:57
ENO scheme asymmetry Vinod Venugopalan Main CFD Forum 5 July 22, 2004 13:06
asymmetry factor (C1/3) Scattering phase function Ahmed Main CFD Forum 1 September 24, 2003 04:31


All times are GMT -4. The time now is 20:50.