parasitic currents
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 
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 
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 
1 Attachment(s)
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 
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 
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 
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 
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. 
has anybody applied this method for static problems?
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? 
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 
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. 
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 
Quote:
since one year passed, do you have any results of you investigation to share? Best Regards, Ilya 
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: http://www.cfdonline.com/Forums/ope...tml#post308969 Thanks andrea 
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. 
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. 
Hello,
Can you send me the paper to pablodecastillo at gmail dot com or give here a few hints?? Thanks 
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. 
Thanks Ali,
I will try tomorrow morning, and i will coment to you how it goes. 
You linked to your email instead of doi.

All times are GMT 4. The time now is 04:59. 