CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   parasitic currents (http://www.cfd-online.com/Forums/openfoam-programming-development/69673-parasitic-currents.html)

rcastilla October 30, 2009 11:58

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. 100 335-354, suggested to weight the surface tension force with the density in the cell in order to reduce this non-real 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

kumar October 30, 2009 12:20

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 OF-1.5, 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

jaswi October 31, 2009 08:01

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:

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())
Does that means that your final expression in pEqn.H for phi now lokks like this:

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

rcastilla November 4, 2009 10:12

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) 1056-1066.

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

jaswi November 4, 2009 13:26

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

sundaero February 28, 2010 20:50

Quote:

Originally Posted by rcastilla (Post 234662)
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?

Thank you, Robert. This one was a really important notice (why I did not found it out by myself?). I am also dealing with low Capillary number flows and my OF model is suffering from high unphysical velocities close to interface. I will try modified model and see what would be the difference in my case.

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

rcastilla March 1, 2010 11:09

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

sundaero March 1, 2010 11:24

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.

aliqasemi March 4, 2010 18:21

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 micro-scale 2D shape with some convex edges (all boundaries are no-flow ->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?

rcastilla March 5, 2010 12:07

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

sundaero March 16, 2010 04:09

Thanks for the corrections.
It is noticeable that the previous version also worked fine for the gas-liquid flow as it has value of 1 in the heavier phase and at the interface and a very small value in the lighter phase.

jens_klostermann April 19, 2010 11:56

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

linch March 9, 2011 12:15

Quote:

Originally Posted by jens_klostermann (Post 255301)
Right now we performing some systematic test.

Hi Jens,

since one year passed, do you have any results of you investigation to share?

Best Regards,
Ilya

Andrea_85 June 24, 2011 08:53

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.cfd-online.com/Forums/ope...tml#post308969

Thanks

andrea

Ivooo February 20, 2012 11:42

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, semi-sphere) 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.

aliqasemi April 23, 2012 12:36

We have solved the problem of spurious currents in our modified version of interFoam code, you can find the details in a paper (two-phase 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.

pablodecastillo April 23, 2012 13:26

Hello,
Can you send me the paper to pablodecastillo at gmail dot com or give here a few hints??

Thanks

aliqasemi April 23, 2012 15:02

Quote:

Originally Posted by pablodecastillo (Post 356446)
Hello,
Can you send me the paper to pablodecastillo at gmail dot com or give here a few hints??

Thanks

As a quick reply, the Sharp(er) Surface Force(SSF) formulation is as follows:

in interFoam/pEqn.H change
fvc::snGrad(alpha1)
to
fvc::snGrad( (1.0/(1.0-2.0*C)) * min( max(alpha1,C), (1.0-C) ) )

For Static cases use C=0.47-0.49, for dynamic simulations (moving interfaces) use C=0.15-0.20, 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.

pablodecastillo April 23, 2012 16:52

Thanks Ali,

I will try tomorrow morning, and i will coment to you how it goes.

akidess April 24, 2012 05:46

You linked to your email instead of doi.


All times are GMT -4. The time now is 20:25.