CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Velocity spikes at interfase (interFoam)

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

Like Tree1Likes
  • 1 Post By santiagomarquezd

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2009, 15:27
Default Velocity spikes at interfase (interFoam)
  #1
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 16
santiagomarquezd will become famous soon enough
Hello all, I'm running interFoam under a OpenFoam-1.5 distro. Actually I'm facing problems described by Henry in #27 (About interFoam solver)

Quote:
Look carfully at where the velocity is causing the maximum Courant number and why. I guess there is some level of numerical instability causing spikes in the velocity field which need to be delt with. Are these spikes at boundaries? near the interface? near corners? Are they reduced or removed by using upwind? Also how good is the mesh? Try running checkMesh on it if you are unsure about the quality
namely velocity spikes, they are near the boundaries and persists even using upwind schemes for U and gamma, by the way mesh quality is excellent. Ratio between Co_max and Co_mean is 250, in a quasi uniform mesh, it implies near a ratio of 250 in velocities too.
This spikes causes spurious deformations in the free surface that ought to be sinusoidal (is a mass pendulum, sloshing problem).

Any clues in solving?, I've been working in this for several weeks, without success...

Thanks in advance.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   October 27, 2009, 20:34
Default
  #2
Senior Member
 
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 9
chiven is on a distinguished road
Hi, dear Santiago, you can try to use setFields/funkySetFields to set different initialized fields to calculate your case. Hope it works.
Best regards,
Chiven
chiven is offline   Reply With Quote

Old   October 27, 2009, 21:36
Default
  #3
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 16
santiagomarquezd will become famous soon enough
Chiven, thanks for your reply. If I understand your answer I think actually my problem is not the initialization. I initialize the problem by hand, setting a sinusoidal wave as the free surface. The idea is that this form remains in time but attenuating, oscillating as a mass pendulum. Problems arises few steps after the beginning, velocity spikes starts to show up at the intefase zone, then the sinusoidal is completely smeared out (see another post from me: Setting up interFoam for sloshing). I know the problem is the indicator function advection or the compressive scheme, but I can't figure what parameter must I change.

Thanks in advance.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   October 28, 2009, 05:01
Default
  #4
Member
 
Jean-Peer Lorenz
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 33
Rep Power: 9
jploz is on a distinguished road
Hi,

what value of cGamma are you using? I prefer values between 0.5 and 1.0, not higher. The cGamma coefficient determines the strength of the 'artificial compressive velocity' in the interface region. Too high values can distort the free surface.

HTH,
Jean-Peer

Last edited by jploz; October 28, 2009 at 05:47.
jploz is offline   Reply With Quote

Old   June 19, 2013, 09:05
Default
  #5
Member
 
Join Date: Apr 2013
Posts: 32
Rep Power: 5
simt is on a distinguished road
Anything new on this topic?

I also get very low courant no. sometimes when using interFoam (OF 2.1.x) for free surface ship flow, similar to the wigley hull case. Oddly, no extreme velocities are observed in the postprocessing though.

The low courant-"spikes" happens independent of :
  • numerical scheme (I've tried using upwind for all convection terms)
  • for cAlpha = 0 (no compession)
  • nNonOrthogonalCorrectors
  • even for low time step equivalent to maxAlphaCo = 0.5 & maxCo= 0.5 with nAlphaSubCycles = 5
So my questions are,
  1. Anyone know how to deal with this?
  2. Is there any alternative which is more robust (navalFoam to 1.6-ext, shipFoam, using MULES::Implicit instead of explicit as in interFoam etc) ?
Best regards, simt.
simt is offline   Reply With Quote

Old   June 24, 2013, 06:59
Default
  #6
Member
 
Join Date: Apr 2013
Posts: 32
Rep Power: 5
simt is on a distinguished road
Got rid of the spikes by limiting grad scheme, cellLimited leastSquares 1.0;.
simt is offline   Reply With Quote

Old   July 26, 2013, 12:14
Default
  #7
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 16
santiagomarquezd will become famous soon enough
It's been a long time since I started this thread. I'm solving the sloshing again, an slightly different case and the spikes are also present. I'm doing a parametric analysis, going up in maxCo. Things were good for small Co numbers, then, when I increased the Co number the spikes appeared, they seem to be related with a deficient p-U coupling, so that the problem desapeared increasing the PISO corrections and activating the mometum predictor.

Regards.
nero235 likes this.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   September 26, 2014, 18:04
Default
  #8
New Member
 
Hf
Join Date: Nov 2012
Posts: 24
Rep Power: 5
jasonchen is on a distinguished road
Quote:
Originally Posted by santiagomarquezd View Post
It's been a long time since I started this thread. I'm solving the sloshing again, an slightly different case and the spikes are also present. I'm doing a parametric analysis, going up in maxCo. Things were good for small Co numbers, then, when I increased the Co number the spikes appeared, they seem to be related with a deficient p-U coupling, so that the problem desapeared increasing the PISO corrections and activating the mometum predictor.
Hi Santiago,

Thanks a lot for your work on description of interFoam solver. Did you get good comparison now for the sloshing case, at the end of the tutorial? In another thread, you mentioned: "This spikes causes spurious deformations in the free surface that ought to be sinusoidal (is a mass pendulum, sloshing problem)."

I also found that the velocity in the air may be so large that the wave surface is distorted. Do you solve your problem by reducing maxCo and increasing PISO correctors?

Thanks,
Jason
jasonchen 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
How to modify interFoam to keep a constant velocity field thibault_pringuey OpenFOAM 0 January 9, 2009 06:59
Velocity in Porous medium : HELP! HELP! HELP! Kali Sanjay Phoenics 0 November 6, 2006 07:10
Variables Definition in CFX Solver 5.6 R P CFX 2 October 26, 2004 02:13
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13


All times are GMT -4. The time now is 16:36.