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

Problem with InterFoam.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 4, 2009, 19:56
Question Problem with InterFoam.
  #1
New Member
 
Yulong
Join Date: Oct 2009
Posts: 3
Rep Power: 7
miroder is on a distinguished road
Hi, I am trying to simulate a liquid droplet emerging from a pore on bottom of a cubic channel using interFoam(1.6.x). Gas was introduced from one side. But I didnot find any droplet at all, the total volume fraction of water did not change much (kept very small, e.g 1e-5).

Then I tried to increase the liquid velocity (from 0.1 to 1m/s), now I can get a droplet, the volume fraction was more than 0.1(makes sense). I was really confused by this result. Is there any limitation of InterFoam? Thanks a lot!


btw: fvscheme and fvsolution are the same as dambreak
=======0/alpha======
{
water_inlet
{
type fixedValue;
value uniform 1;
}
outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
gas_inlet
{
type fixedValue;
value uniform 0;
}
wall
{
type constantAlphaContactAngle;
theta0 140;
thetaA 170;
thetaR 90;
uTheta 1;
value uniform 1;
}
======0/U========
{
water_inlet
{
type fixedValue;
value uniform (0 0 0.0625);
}
outlet
{
type inletOutlet;
value uniform (0 0 0);
inletValue uniform ( 0 0 0 );
}
gas_inlet
{
type fixedValue;
value uniform (0 10 0);
}
wall
{
type fixedValue;
value uniform (0 0 0);
}
}
======0/p========
boundaryField
{
water_inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
gas_inlet
{
type zeroGradient;
}
wall
{
type zeroGradient;
}
}
miroder is offline   Reply With Quote

Old   November 5, 2009, 15:44
Default
  #2
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
I have done a similar work in my bachelor thesis.
The simulation was done by injecting a continous gas flow into a stagnant liquid.

During the simulation I encountered severe problems with "small" inflow rates.
It was evident that there was some loss of mass, as the liquid volume fraction was not changing although gas was flowing into the domain.

My "explanation" to this observation was the influence of parasitic currents in the proximity of the interface which was very close to the inflow in my case.

If the magnitude of the parasitic currents and the inflow velocity are close to each other (as it was in my case) some kind of interaction is highly probable!
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   November 5, 2009, 16:05
Default
  #3
New Member
 
Yulong
Join Date: Oct 2009
Posts: 3
Rep Power: 7
miroder is on a distinguished road
Thank you for your reply!

I used Fluent before, and these never happened even the flow rates was much lower. However, I really wanna use OPENFOAM for my research, is there any way to deal with that?

by the way, I am not quite understand the term "parasitic current", could you give me more explanation? Thanks a lot!
miroder is offline   Reply With Quote

Old   November 5, 2009, 16:47
Default
  #4
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
"Parasitic currents" are known as unphysical velocity fields in the proximity of a resting interface. Theoretically all velocities should be zero in a flow field if the interface is not moving. Yet you will allways examine a velocity field if you use the CSF-Model (Continuum-Surface-Modell) for the representation of surface-tension which is used in interFoam.

Have a look at this picture of a static drop which shows parasitic currents:



The CSF-model itself is introduced by Brackbill & al. "A Continuum Method for modeling Surface Tension" Journal of Compuational Physics, 100:335-354, 1992. The reasons of parasitic currents and its effects on the flow are discussend there.

The term "parasitic currents" was first introduced by Lafaurie et. al. "Modelling Merging and Fragmentation in Multiphase Flow with SURFER". Journal of Computational Physics. 113:134-147, 1994.

You will find a whole bunch of papers about this problem and even here it was discussed just yesterday:
parasitic currents

The magnitude of the parasitic currents scale with the fluid properties and with the "quality" of the solver. Please refer for the literature above for more details.

So maybe you will be able to simulate your cases with some restrictions on the fluid properties.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   November 5, 2009, 19:06
Default
  #5
New Member
 
Yulong
Join Date: Oct 2009
Posts: 3
Rep Power: 7
miroder is on a distinguished road
Really thanks your kind help. Seems I have a lot to learn
miroder 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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Incoherent problem table in hollow-fiber spinning Gianni FLUENT 0 April 5, 2008 10:33
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 09:16.