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

pressure oscillation near pressure outlet boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 9, 2011, 08:15
Default pressure oscillation near pressure outlet boundary
  #1
New Member
 
Liu Yang
Join Date: Apr 2011
Posts: 5
Rep Power: 5
kino is on a distinguished road
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!
kino is offline   Reply With Quote

Old   April 11, 2011, 04:04
Default
  #2
Senior Member
 
Rami Ben-Zvi
Join Date: Mar 2009
Posts: 140
Rep Power: 7
Rami is on a distinguished road
Vortex shedding?
Rami is offline   Reply With Quote

Old   April 11, 2011, 10:32
Default
  #3
New Member
 
Liu Yang
Join Date: Apr 2011
Posts: 5
Rep Power: 5
kino is on a distinguished road
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.
kino is offline   Reply With Quote

Old   April 12, 2011, 04:25
Default
  #4
Senior Member
 
Rami Ben-Zvi
Join Date: Mar 2009
Posts: 140
Rep Power: 7
Rami is on a distinguished road
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
Rami is offline   Reply With Quote

Old   April 12, 2011, 19:07
Default
  #5
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 228
Rep Power: 8
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
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
julien.decharentenay is offline   Reply With Quote

Old   April 13, 2011, 11:03
Default
  #6
New Member
 
Liu Yang
Join Date: Apr 2011
Posts: 5
Rep Power: 5
kino is on a distinguished road
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.
kino 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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
Domain Imbalance HMR CFX 3 March 6, 2011 20:10
Help ASAP! pressure inlet & outlet engahmed FLUENT 0 June 13, 2010 15:33
Pressure outlet boundary condition jubs FLUENT 0 February 8, 2007 00:27
Setting Pressure on an Outlet Boundary Richard Pemberton CFX 2 April 12, 2001 06:35


All times are GMT -4. The time now is 16:08.