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

LinkBack  Thread Tools  Display Modes 
February 3, 2015, 13:14 
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 
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 twophase 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! Last edited by pablitobass; February 3, 2015 at 16:04. 

February 5, 2015, 21:36 

#2 
Senior Member
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA  San Diego, CA USA
Posts: 310
Rep Power: 9 
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; } I hope that helps some! Cheers, Kyle 

February 6, 2015, 07:09 

#3 
New Member
Paolo Capobianchi
Join Date: Sep 2014
Posts: 28
Rep Power: 3 
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 Tjunction (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 

February 6, 2015, 12:29 

#4 
Senior Member
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA  San Diego, CA USA
Posts: 310
Rep Power: 9 
Good news!
If you're looking to take larger time steps in interFoam be sure to try OpenFOAM2.3.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 

February 7, 2015, 15:51 

#5 
New Member
Paolo Capobianchi
Join Date: Sep 2014
Posts: 28
Rep Power: 3 
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 twophase 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 2.3x version for the semiimplicit MULES; at the moment I am using other versions. Thanks again for your kindness! Cheers, Paolo 

June 9, 2015, 11:21 

#6 
Member
Saideep
Join Date: Apr 2015
Location: INDIA
Posts: 96
Rep Power: 2 
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 e1 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 

Thread Tools  
Display Modes  


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 