CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLOW-3D (http://www.cfd-online.com/Forums/flow-3d/)
-   -   gas-liquid two-phase flow in microchannel (http://www.cfd-online.com/Forums/flow-3d/81910-gas-liquid-two-phase-flow-microchannel.html)

LyngHoo November 10, 2010 07:04

gas-liquid two-phase flow in microchannel
 
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.

MuxaB November 15, 2010 13:35

does it terminate with an error message? Does the solver run any distance or does it terminate right away?

LyngHoo November 15, 2010 23:04

Quote:

Originally Posted by MuxaB (Post 283520)
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?

MuxaB November 16, 2010 23:09

Quote:

Originally Posted by LyngHoo (Post 283553)
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?

LyngHoo November 17, 2010 00:13

Quote:

Originally Posted by MuxaB (Post 283707)
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 November 17, 2010 23:59

Quote:

Originally Posted by MuxaB (Post 283707)
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.

MuxaB November 19, 2010 01:36

Quote:

Originally Posted by LyngHoo (Post 283844)
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.

haghshenasfard February 3, 2011 06:07

Dear LyngHoo
Please send me you email, maybe I can cooperte with you,
regards
Dr. M. Haghshenas

haghshenas@cc.iut.ac.ir


All times are GMT -4. The time now is 22:01.