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

Relaxation of a "Squared" Droplet using the Volume of Fluid method in interFoam

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

Like Tree1Likes
  • 1 Post By kmooney

Reply
 
LinkBack Thread Tools Display Modes
Old   February 3, 2015, 13:14
Default Relaxation of a "Squared" Droplet using the Volume of Fluid method in interFoam
  #1
New Member
 
Paolo Capobianchi
Join Date: Sep 2014
Posts: 28
Rep Power: 3
pablitobass is on a distinguished road
Hello everyone,

my name is Paolo, this is my first post and I would ask if someone can help me.

I am having some troubles with a simulation of a two-phase flow. More precisely, I am trying to simulate the relaxation of a 2D square shaped (see the attached pictures) volume of fluid immersed in another immiscible one. As you know, due to the surface tension the square should relax into a circular shape. It seems that it works, but after some iteration the shape starts to evolve into an irregular one.

I have done the following settings

Boundaries:
uniform 0 velocity
uniform 0 relative pressure

The two fluids have the same viscosity and same density (I have also tried different settings, but I had the same problem)

I have set 0 gravity

No settings about the contact angle.

I know that the VOF has the drawback of the spurious currents, and I thought that it could be the problem, thus I lowered the time step (I have actually imposed the Courant number) and refined the grid, but it does not work.
I have also tried to lower the surface tension and the only difference is that the fluid starts to become irregular after a longer time.

Does anyone has any clue about this problem, please?

Thank you very much!
Attached Images
File Type: jpg sq_drop_01.jpg (8.5 KB, 19 views)
File Type: jpg sq_drop_02.jpg (9.3 KB, 17 views)
File Type: jpg sq_drop_03.jpg (9.3 KB, 15 views)
File Type: jpg sq_drop_04.jpg (9.0 KB, 20 views)
File Type: jpg sq_drop_05.jpg (9.1 KB, 21 views)

Last edited by pablitobass; February 3, 2015 at 16:04.
pablitobass is offline   Reply With Quote

Old   February 5, 2015, 21:36
Default
  #2
Senior Member
 
kmooney's Avatar
 
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA - San Diego, CA USA
Posts: 310
Rep Power: 9
kmooney is on a distinguished road
Hi Paulo,

Unfortunately for VOF there is no guarantee that you'll end up with a perfectly balanced surface force at equilibrium.

There are, however, a few things that might improve your simulations results:
1. Try making a larger outer domain compared to the droplet. The interface is rather close to the boundary and it might be effecting the solution.
2. Increasing the viscosity (if thats allowed in your test, it will change the ohnesorge number...) will should damp the system faster
3. Try a larger gradient calculation stencil for the nHat term.

Something like this in fvSchemes:
Code:
gradSchemes
{
default linear;
nHat pointCellsLeastSquares 0.0;
}
If your in an older version of OF you might have to put 'extendedLeastSquares' 0.0 instead.

I hope that helps some!

Cheers,
Kyle
Cyp likes this.
kmooney is offline   Reply With Quote

Old   February 6, 2015, 07:09
Default
  #3
New Member
 
Paolo Capobianchi
Join Date: Sep 2014
Posts: 28
Rep Power: 3
pablitobass is on a distinguished road
Hi Kyle,

thank you very much for the tips!

In the meanwhile, I tried to change some parameters and seem that the solution is much better now.
I changed the following settings:

1. mesh refinement;
2. I lowered the max Co
3. I changed the level of compression (I have used C = 0) losing definition of the interface but in favour of lower parasite currents.

In the attached file you can see the evolution of the solution. The droplet become circular after some iteration, then seems to be stretched and move in the left corner down. After a while become again circular and eventually (no images for this) disintegrate to the walls).

I will try also the setting you proposed and I will see what happen. In fact, I am also trying to simulate other flows, such as segmented flows in a micro T-junction (fully 3D), and I am not allowed to use very low Co due to the very prohibitive time of calculation (with same setting I have estimated about 14 months... ).

Thanks again for your help!
I'll let you know what happen.

Cheers,
Paolo
Attached Images
File Type: jpg tau_328.jpg (10.0 KB, 7 views)
File Type: jpg tau_421.jpg (22.6 KB, 7 views)
File Type: jpg tau_1307.jpg (16.1 KB, 8 views)
pablitobass is offline   Reply With Quote

Old   February 6, 2015, 12:29
Default
  #4
Senior Member
 
kmooney's Avatar
 
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA - San Diego, CA USA
Posts: 310
Rep Power: 9
kmooney is on a distinguished road
Good news!

If you're looking to take larger time steps in interFoam be sure to try OpenFOAM-2.3.x's implicitMULES support. You can take much larger time steps while still keeping the simulation stable. You pay for it, however, in accuracy.

I did some quick benchmarks here in case you want to take a look:
http://sourceforge.net/projects/open...W09_P_0088.pdf

Implicit Mules:
http://www.openfoam.org/version2.3.0/multiphase.php
kmooney is offline   Reply With Quote

Old   February 7, 2015, 15:51
Default
  #5
New Member
 
Paolo Capobianchi
Join Date: Sep 2014
Posts: 28
Rep Power: 3
pablitobass is on a distinguished road
Hi Kyle,

thanks for the further advises!

I have run a simulation by doubling the domain and the droplet remain stable for a much longer time, but eventually, also in this case, it stretch and move to the corner.
I have also used the new setting for the gradient but I did not noticed a substantial variation in terms of parasite currents.
The least square gradient calculation serves just for a better reconstruction of the interface, or should have an impact also for the parasite currents?

About the viscosity, I have no particular restriction for my tests, thus I thought to perform different simulations by changing the Ohnesorge number and see what happen.
Plus, I would try keep the fluid parameters constant and change the "compression factor" C_alpha; unfortunately it seem that for c_alpha = 1 I cannot get a circular shape for a long time.

In any case, my goal is to have a better understanding of the solver because I am planning to simulate two-phase flows in microchannels, thus I have to evaluate how much the spurious currents affects my solutions. I also need to care about the resolution of the interface.

I would also think about a the 2.3-x version for the semi-implicit MULES; at the moment I am using other versions.

Thanks again for your kindness!

Cheers,
Paolo
pablitobass is offline   Reply With Quote

Old   June 9, 2015, 11:21
Default
  #6
Member
 
Saideep
Join Date: Apr 2015
Location: INDIA
Posts: 96
Rep Power: 2
Saideep is on a distinguished road
Hi guys;

I know there has been quite a gap between posts. I am working to reduce the spurious currents effects.

When I run the case over a static model domain, the bubble(or any fluid as a matter of fact) is just getting pushed to the corner of the domain and strangely I have a velocity for the 1st time step of 315m/s. Later it moves to the corner and magnitude of velocity reduces to e-1 orders.

I see the effect of these spurious currents are more pronounced for the static case problem. In my opinion it is bets to supress these where they are formed. So, I guess everything is dependent on the 'F' term in the NSE. Especially in the calculation of interface curvature 'k'.

Any ideas and helps to keep this active and solve this.

Saideep
Saideep 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 set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 12 December 12, 2011 05:16
My Revised "Time Vs Energy" Article For Review Abhi Main CFD Forum 2 July 9, 2002 09:08
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 13:07.