CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

gas-liquid two-phase flow in microchannel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 10, 2010, 07:04
Default gas-liquid two-phase flow in microchannel
  #1
New Member
 
Join Date: Nov 2010
Posts: 12
Rep Power: 6
LyngHoo is on a distinguished road
Hello everyone, I'm a newbie to the FLOW-3D, and trying to setup a simplified 2-D gas-liquid two-phase flow in microchannel to simulate the flow pattern. The channel is a T-shaped microchannel, its width is 0.5mm, the gas (air) and liquid (water) are introduced in the channel from the opposite inlets, the velocities of the gas and liquid are 0.7m/s and 0.5m/s, respectively. The channel for two-phase flow is 0.01m in the length. The outlet is open to atmospheric conditions. And the finish time is set to 10 sec. But the simulation always terminate unexpectedly.
Does anyone can tell me what goes wrong or share some similar examples with me.
LyngHoo is offline   Reply With Quote

Old   November 15, 2010, 13:35
Default
  #2
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
does it terminate with an error message? Does the solver run any distance or does it terminate right away?
MuxaB is offline   Reply With Quote

Old   November 15, 2010, 23:04
Default
  #3
New Member
 
Join Date: Nov 2010
Posts: 12
Rep Power: 6
LyngHoo is on a distinguished road
Quote:
Originally Posted by MuxaB View Post
does it terminate with an error message? Does the solver run any distance or does it terminate right away?
Yes the solver message is "excessive pressure iteration failures", the pressure iteration can't converge. I don't know where to find converge control options and how to control them. Could you please help me?
LyngHoo is offline   Reply With Quote

Old   November 16, 2010, 23:09
Default
  #4
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by LyngHoo View Post
Yes the solver message is "excessive pressure iteration failures", the pressure iteration can't converge. I don't know where to find converge control options and how to control them. Could you please help me?
All pressure solver options are listed on the Numerics tab, including the Convergence Controls. The first thing to check is the maximum residual when the solver does not converge. It is listed in the diagnostics message on the screen. If the residual is much larger than the convergence criterion epsi, then most likely there is something wrong in the setup - either fluid properties, boundary or initial conditions. Could be the mesh too.

If the difference is relatively small, ~ 2-3, then you may be able to achieve convergence by introducing limited compressibility, or switching to a different pressure solver.

Does it start failing right away? Have you talked to support?
MuxaB is offline   Reply With Quote

Old   November 17, 2010, 00:13
Default
  #5
New Member
 
Join Date: Nov 2010
Posts: 12
Rep Power: 6
LyngHoo is on a distinguished road
Quote:
Originally Posted by MuxaB View Post
All pressure solver options are listed on the Numerics tab, including the Convergence Controls. The first thing to check is the maximum residual when the solver does not converge. It is listed in the diagnostics message on the screen. If the residual is much larger than the convergence criterion epsi, then most likely there is something wrong in the setup - either fluid properties, boundary or initial conditions. Could be the mesh too.

If the difference is relatively small, ~ 2-3, then you may be able to achieve convergence by introducing limited compressibility, or switching to a different pressure solver.

Does it start failing right away? Have you talked to support?
Thank you very much for taking your time. I'll try them.

No, it doesn't start failing right away, and I haven't talked to support.
LyngHoo is offline   Reply With Quote

Old   November 17, 2010, 23:59
Default
  #6
New Member
 
Join Date: Nov 2010
Posts: 12
Rep Power: 6
LyngHoo is on a distinguished road
Quote:
Originally Posted by MuxaB View Post
All pressure solver options are listed on the Numerics tab, including the Convergence Controls. The first thing to check is the maximum residual when the solver does not converge. It is listed in the diagnostics message on the screen. If the residual is much larger than the convergence criterion epsi, then most likely there is something wrong in the setup - either fluid properties, boundary or initial conditions. Could be the mesh too.

If the difference is relatively small, ~ 2-3, then you may be able to achieve convergence by introducing limited compressibility, or switching to a different pressure solver.

Does it start failing right away? Have you talked to support?
MuxaB, I introduced limited compressibility to the gas phase, and problem solved.
I found this in the help contents, "Two-fluid problems may be composed of either two incompressible fluids or one incompressible and one compressible fluid". So I guess that's the problem I had.

Thank you very much for your help.
LyngHoo is offline   Reply With Quote

Old   November 19, 2010, 01:36
Default
  #7
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by LyngHoo View Post
MuxaB, I introduced limited compressibility to the gas phase, and problem solved.
I found this in the help contents, "Two-fluid problems may be composed of either two incompressible fluids or one incompressible and one compressible fluid". So I guess that's the problem I had.

Thank you very much for your help.
You are very welcome, glad you found a solution.

Limitted compressibility does not add the full equation-of-state compressibility which the full gas model does (ICMPRS=1). Instead it adds, the acoustic compressibility, where the density changes are assumed small, and pressure changes is a linear function of density changes: dP/dt=c^2drho/dt, where c is the speed of sound.

This is good for a) tracking acoustic waves, and b) softening stiff systems for better convergence. Looks like the latter worked out for you.
MuxaB is offline   Reply With Quote

Old   February 3, 2011, 06:07
Default
  #8
New Member
 
a
Join Date: Feb 2010
Posts: 11
Rep Power: 7
haghshenasfard is on a distinguished road
Dear LyngHoo
Please send me you email, maybe I can cooperte with you,
regards
Dr. M. Haghshenas

haghshenas@cc.iut.ac.ir
haghshenasfard 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
Advice on multi-phase flow modelling Martin Main CFD Forum 3 October 14, 2008 05:16
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02
Multiphase flow problem icedou FLUENT 6 July 10, 2005 02:52
Two phase flow models Atholl Main CFD Forum 2 May 7, 2002 03:49
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19


All times are GMT -4. The time now is 13:54.