# pressure oscillation near pressure outlet boundary

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

 April 9, 2011, 08:15 pressure oscillation near pressure outlet boundary #1 New Member   Liu Yang Join Date: Apr 2011 Posts: 5 Rep Power: 8 Sponsored Links Hello: I'm working on my own pressure-based code, using fractional-step method, referring to OpenFlower. Now this code can deal with lid-driven cavity, but when simulating flow around a cylinder(Re=100), pressure oscillation can be seen near the pressure outlet boundary, so unphysical result appears. For the pressure outlet boundary, in the moment equation, the normal gradient of velocity is set to zero; in the pressure equation, the pressure is set to zero. What may cause this oscillation? I checked my code carefully but found nothing. Thank you for your instructions!

 April 11, 2011, 04:04 #2 Senior Member   Rami Ben-Zvi Join Date: Mar 2009 Posts: 148 Rep Power: 10 Vortex shedding?

 April 11, 2011, 10:32 #3 New Member   Liu Yang Join Date: Apr 2011 Posts: 5 Rep Power: 8 Thank you very much for your reply, but I think the outflow boundary is far enough from the cylinder. I used to enlarge the computational domain but the problem remains.

 April 12, 2011, 04:25 #4 Senior Member   Rami Ben-Zvi Join Date: Mar 2009 Posts: 148 Rep Power: 10 Hi Kino, Let me try again. The problem you are experiencing might be an expression of the vortex shedding phenomenon, AKA Von Kármán vortex street (see, for example, http://en.wikipedia.org/wiki/Vortex_shedding and references therein). If my guess is correct, then you cannot solve this inherently unsteady (and also asymmetric) problem with a steady-state solver, no matter how far your outlet is, and if you try - you'll probably notice oscillations or divergence in the iterative process. If this is the case, either try a transient solution, with no symmetry assumptions, far enough outlet and/or appropriate non-reflecting BC, or (easier way) reduce the Re No. far below the instability limit, so that a steady, symmetric solution exists. I hope this helps, Rami

 April 12, 2011, 19:07 #5 Senior Member   Julien de Charentenay Join Date: Jun 2009 Location: Australia Posts: 230 Rep Power: 11 I think that the problem may be in the setting of your outflow boundary conditions. You are using a pressure based solver and setting constraints on both pressure (fixed condition) and velocity (zero gradient). I did some work long ago on a finite difference solver and I seem to recall that I used a gradient calculation for the velocity at the outflow (using a backward scheme), not zero gradient. If you are using finite volume, you could achieve similar results by changing how you compute the gradients at the near boundary cell. Let me know if it helps. Sincerely, Julien __________________ --- Julien de Charentenay

 April 13, 2011, 11:03 #6 New Member   Liu Yang Join Date: Apr 2011 Posts: 5 Rep Power: 8 Thank you for your kindly help. Hello Rami, actually I'm using an unsteady solver, and the pressure oscillation can be seen from beginning, so I think it's not caused by vortex shedding. Hello julien. decharentenay, I checked my code carefully today and found that when dealing with the convection term, the transporting velocity at cell face can't be treated by interpolation, but have to be updated using the pressure correction equation. Primiry results shows that the pressure oscillation can be removed. Thank you all the same for your instruction.

 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 HMR CFX 5 October 10, 2016 05:57 Saturn CFX 45 February 8, 2016 05:42 engahmed FLUENT 0 June 13, 2010 15:33 jubs FLUENT 0 February 8, 2007 01:27 Richard Pemberton CFX 2 April 12, 2001 06:35