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

Droplet break-up in a t-junction

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 3, 2011, 12:51
Default Droplet break-up in a t-junction
  #1
New Member
 
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 5
deifobe is on a distinguished road
Hi foamers,
I try to simulate slug flow-droplet break-up in a t-junction to compare the results to those obtained with Comsol, but the simulation result is very different, the break-up in openFoam simulation is further, also the drop form and and the detach time
is very different but I don't understand what i do wrong. Any suggestion?
I use interfoam solver, this is my BC:
-0/alpha1
inletWater
{
type fixedValue;
value uniform 1;
}
inletOil
{
type fixedValue;
value uniform 0;
}
bottom
{
type symmetryPlane;
}
outlet
{
type zeroGradient;
}

walls
{
type constantAlphaContactAngle;
theta0 135;
limit gradient;
value uniform 0;
}
- 0/p_rgh
inletOil
{
type zeroGradient;
}

inletWater
{
type zeroGradient;
}

walls
{
type fixedFluxPressure;
adjoint no;
}
bottom
{
type symmetryPlane;
}
outlet
{
type fixedValue;
value uniform 0;
}
-0/U
inletWater
{
type flowRateInletVelocity;
flowRate 5.555e-11;
value uniform (0 0 0);
}
inletOil
{
type flowRateInletVelocity;
flowRate 1.111e-10;
value uniform (0 0 0);
}
walls
{
type fixedValue;
value uniform (0 0 0);
}

bottom
{
type symmetryPlane;
}
outlet
{
type zeroGradient;
}
test2.jpg
deifobe is offline   Reply With Quote

Old   November 3, 2011, 13:13
Default
  #2
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 240
Rep Power: 9
olivierG is on a distinguished road
hello,

Can you give your fvScheme / fvSolution, or better, the case with mesh ?

Anyway, i would first change your 0/p_rgh like:
- inletOil / inletWater: outletInlet
- walls : buoyantPressure
- outlet : totalPressure

for alpha1: are you sure about 135 ? (seem big, maybe the tetha definition is not the same as comsol)

for U
- outlet : try inletOutlet or pressure(Normal ?)InletOutletVelocity

regards,
olivier
olivierG is offline   Reply With Quote

Old   November 3, 2011, 17:03
Default
  #3
New Member
 
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 5
deifobe is on a distinguished road
Thanks a lot for your reply! I tried your BC but result is a continuos flow but, as you say,
the problem seems to be contact angle, I will have to find and compare this angle definition in OpenFoam and in Comsol.
Thank you again.
deifobe is offline   Reply With Quote

Old   November 4, 2011, 10:27
Default
  #4
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 201
Rep Power: 11
kwardle is on a distinguished road
Judging from your image, you are using a very coarse mesh. Unless you are trying to compare each code's results on the same mesh, you will want to use a much finer mesh to get anything right. Also, what kind of mesh is it? You should be able to easily use hex (blockMesh) for your geometry. You may also want to take a look at varying the cAlpha parameter in fvSolution--a value larger than 1 may result in some strange things on the interface which affect the accuracy. You have also not said what the dimensions of your problem are--different physics will affect the results depending on the scale. For example, if this is a micro channel flow (or even just 'milli' channel), then surface tension and wall contact angle will be much more important.
kwardle 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
droplet falling - VOF bohis FLUENT 1 July 10, 2013 04:28
DieselFoam Droplet Temperature Issues - OF 1.6 viv05 OpenFOAM 0 February 27, 2010 12:20
Importance of droplet size Itchie CFX 2 December 13, 2007 03:01
Droplet Evaporation Christian Main CFD Forum 2 February 27, 2007 07:27
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24


All times are GMT -4. The time now is 11:28.