
[Sponsors] 
October 30, 2009, 11:58 
parasitic currents

#1 
Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 81
Rep Power: 8 
Hi,
I have working with high weber number flows (capillary flows) and I am finding som important parasitic currents in the interface. I have read that Brackbill (1992) J. Comput. Phys. 100 335354, suggested to weight the surface tension force with the density in the cell in order to reduce this nonreal currents. I have modified this term in interFoam, fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1) multiplying by fvc::interpolate(rho/(twoPhaseProperties.rho1()twoPhaseProperties.r ho2()) The parasitic currents have been appreciably reduced. I am surprised than I so simple thing has not been before implemented in interFoam. Maybe there is some drawback that I don't know? Best regards 

October 30, 2009, 12:20 

#2 
Senior Member
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 8 
Hello Robert,
I agree with you, that we need a new thread for this discussion. I have a basic question, how do you usually visualize or calculate your parasitic flows at the interface. do you do this by just performing some post processing or is there any script based on some literature to calculate this. I need to know this because I am running some lesinterfoam calculations and it is really important for me to resolve the forces properly at the interface. I am using OF1.5, and if the implementation that you did is specified in some literature you can also let me know the paper, I will look in to it. I may also change the lesInterfoam solver and see if there is any major difference. But first of all i want to know how to find out if there are any currents acting at my interface, Hope you dont mind my basic question. I am new to the field of Multiphase flows. My Master thesis was in Incompressible flows, so i dont have much knowledge of Multiphase flows. bye with regards K.Suresh kumar 

October 31, 2009, 08:01 

#3  
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 9 
Hi Robert
Thanks for sharing this information. I have been hvaing some similar issues with the parasitic currents. Please post some pictures showing the comparison. According to you post: Quote:
phi = phiU + ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(g amma)* fvc::interpolate( rho / (twoPhaseProperties.rho1() twoPhaseProperties.rho2() )  ghf*fvc::snGrad(rho) )*rUAf*mesh.magSf(); Thanks once again for sharing the information. Best Regards jaswi 

November 4, 2009, 10:12 

#4 
Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 81
Rep Power: 8 
Hi,
kumar, the paper by Brackbill is, as far as I know, the first on parasitic currents. You can read also Harvie et al. Applied Mathematical Modelling, 30 (2006) 10561066. jaswi, not exactly, since I am using OF 1.6 and ghf is no more used. The modified pEqn.H is as follows: phi = phiU + ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1)* fvc::interpolate(rho/(twoPhaseProperties.rho1()twoPhaseProperties.r ho2()))*mesh.magSf() + fvc::interpolate(rho)*(g & mesh.Sf()) )*rUAf; Attached you can see the velocity vectors of one experiment, made with paraview. In the right side, with density correction, the parasitic currents have been appreciably reduced. Hope it can help you. with regards Robert 

November 4, 2009, 13:26 

#5 
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 9 
Dear Robert
Thanks for the answer and the pictures. They do show a substantial decrease in the spurious currents. I just can't wait to try that for my case :) BR jaswi 

February 28, 2010, 20:50 

#6  
New Member
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8 
Quote:
One drawback here is that now it will take more time to compute. How much? That is an another question. By the way, am I right that you did changes both in pEqn.H and UEqn.H ? BR Denis 

March 1, 2010, 11:09 

#7 
Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 81
Rep Power: 8 
Hi, Denis,
actually I have only modified the pEqn.H, since the Ueqn.H is only calculated if momentumPredicor is "true", which is not normally the case. Hope it will be useful for you. Best regards Robert 

March 1, 2010, 11:24 

#8 
New Member
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8 
I got your point. But to be on a safe side I modified both.
Ok, I got some intermediate results. It seems that such a simple modification completely cured that annoying effect when there is unwanted high velocities near the interface and now my OF model is much better follow the experimental data. Thank you, Robert one more time for posting this idea here. I do not know how, but I think this idea should be somehow more widely known, because, I think, a lot of people deal with capillary flows and might face the similar problem. Last edited by sundaero; March 2, 2010 at 15:22. 

March 4, 2010, 18:21 
has anybody applied this method for static problems?

#9 
New Member
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7 
today, I made similar changes to interFoam, but it seems that it produces higher parasitic currents in my case which is kind of calculating capillary pressure in a bubble trapped in a closed microscale 2D shape with some convex edges (all boundaries are noflow >static problem). it seems that the term "fvc::interpolate(rho/(twoPhaseProperties.rho1()twoPhaseProperties.rho2())" is greater than one and it causes higher surface tension force, and higher parasitic currents in my static problem.
has anybody applied this method for similar static problems? Last edited by aliqasemi; March 4, 2010 at 19:11. 

March 5, 2010, 12:07 

#10 
Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 81
Rep Power: 8 
I have mistyped the term. The suggestion of Brackbill is rho/<rho>, i.e.,
fvc::interpolate(2*rho/(twoPhaseProperties.rho1()+twoPhaseProperties.rho2 ()) This term has to be 1 in the interphase, and it has to reduce the force in the lighter phase. It can be greater than one in the heavier phase, but it should not increase the parasitic currents. Robert 

March 16, 2010, 04:09 

#11 
New Member
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8 
Thanks for the corrections.
It is noticeable that the previous version also worked fine for the gasliquid flow as it has value of 1 in the heavier phase and at the interface and a very small value in the lighter phase. 

April 19, 2010, 11:56 

#12 
Senior Member
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8 
Hi all,
I made the same modifications to a 2D static bubble problem with the result, that an original round bubble gets octagonal!! So the results get worse! Right now we performing some systematic test. The parasitic current problem is not that simple, since they depend on the physical problem (density ratio, viscosity ratio, We, Re, ...) and the numerical implementation of the VoF method. Regards Jens 

March 9, 2011, 12:15 

#13 
Senior Member
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 174
Rep Power: 8 

June 24, 2011, 08:53 

#14 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 289
Rep Power: 7 
Hi all,
i also made the same modification in pEqn.H, but i still get very high spurious velocity at the interface. if you remember, since one year passed, coul you please post your fvScheme and fvSolution. and what were the properties of your fluids? to have a look at my problem you can read here: Small time step in interFoam Thanks andrea 

February 20, 2012, 11:42 

#15 
New Member
Ivo
Join Date: Feb 2012
Posts: 22
Rep Power: 5 
Hi,
thanks for posting this. I implemented the change in OpenFOAM 2.1.0, but it seems to have no effect here. As a benchmark, I am using a sessile droplet (d = 1mm, semisphere) on a flat plate. After settling down due to the distortions caused by the initialisation of the alpha1 phase on the rectangular mesh (about 0.03s), the drop starts to move around over the plate. I suspect this behaviour is due to spurious currents, which I hoped to prevent with the measures described above. I will try to verify this result once more. 

April 23, 2012, 12:36 

#16 
New Member
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7 
We have solved the problem of spurious currents in our modified version of interFoam code, you can find the details in a paper (twophase flow at low capillary numbers / small scales) being published in JCP:
http://dx.doi.org/10.1016/j.jcp.2012.04.011 The Sharp Surafce Force part, described in the paper, is a one line code which any one can easily implement. Smoothing and filtering are also proposed in the paper. The paper is written for Cartesian meshes, but most parts are general, and now we are using the code for unstructured meshes with very few modifications / change of discretization algorithms. Hopefully these modifications will be published soon as well. Last edited by aliqasemi; May 2, 2012 at 12:00. 

April 23, 2012, 13:26 

#17 
Senior Member
Pablo
Join Date: Mar 2009
Posts: 102
Rep Power: 8 
Hello,
Can you send me the paper to pablodecastillo at gmail dot com or give here a few hints?? Thanks 

April 23, 2012, 15:02 

#18  
New Member
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7 
Quote:
in interFoam/pEqn.H change fvc::snGrad(alpha1) to fvc::snGrad( (1.0/(1.02.0*C)) * min( max(alpha1,C), (1.0C) ) ) For Static cases use C=0.470.49, for dynamic simulations (moving interfaces) use C=0.150.20, roughly speaking. (the definition of C here is different from the paper) Filtering is as important as sharpening the capillary force but it has a long story. I will be back to you later by email. 

April 23, 2012, 16:52 

#19 
Senior Member
Pablo
Join Date: Mar 2009
Posts: 102
Rep Power: 8 
Thanks Ali,
I will try tomorrow morning, and i will coment to you how it goes. 

April 24, 2012, 05:46 

#20 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 984
Rep Power: 17 
You linked to your email instead of doi.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oamtechnology 

Tags 
capillary flows, interfoam, parasitic currents 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to monitor free surface elevation vs time in OF?  ozgur  OpenFOAM PostProcessing  56  September 14, 2015 08:11 
parasitic currents  PeiYing Hsieh  Main CFD Forum  0  January 13, 2009 20:58 
Parasitic currents reduction  hsieh  OpenFOAM Running, Solving & CFD  0  January 13, 2009 16:44 
Parasitic currents reduction  hsieh  OpenFOAM Running, Solving & CFD  0  January 13, 2009 16:37 
Modelling ocean currents of the past Earth  pgm  Main CFD Forum  3  March 2, 2005 09:45 