CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

parasitic currents

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

Like Tree22Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 30, 2009, 11:58
Default parasitic currents
  #1
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 80
Rep Power: 8
rcastilla is on a distinguished road
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
rcastilla is offline   Reply With Quote

Old   October 30, 2009, 12:20
Default
  #2
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 8
kumar is on a distinguished road
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
kumar is offline   Reply With Quote

Old   October 31, 2009, 08:01
Default
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 248
Rep Power: 9
jaswi is on a distinguished road
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
jaswi is offline   Reply With Quote

Old   November 4, 2009, 10:12
Default
  #4
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 80
Rep Power: 8
rcastilla is on a distinguished road
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
Attached Images
File Type: jpg parasitic_screenshot.jpg (86.0 KB, 626 views)
rcastilla is offline   Reply With Quote

Old   November 4, 2009, 13:26
Default
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 248
Rep Power: 9
jaswi is on a distinguished road
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
jaswi is offline   Reply With Quote

Old   February 28, 2010, 20:50
Default
  #6
New Member
 
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sundaero is on a distinguished road
Quote:
Originally Posted by rcastilla View Post
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
sundaero is offline   Reply With Quote

Old   March 1, 2010, 11:09
Default
  #7
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 80
Rep Power: 8
rcastilla is on a distinguished road
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
rcastilla is offline   Reply With Quote

Old   March 1, 2010, 11:24
Default
  #8
New Member
 
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sundaero is on a distinguished road
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.
sundaero is offline   Reply With Quote

Old   March 4, 2010, 18:21
Default has anybody applied this method for static problems?
  #9
New Member
 
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7
aliqasemi is on a distinguished road
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?

Last edited by aliqasemi; March 4, 2010 at 19:11.
aliqasemi is offline   Reply With Quote

Old   March 5, 2010, 12:07
Default
  #10
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 80
Rep Power: 8
rcastilla is on a distinguished road
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
amir_kb likes this.
rcastilla is offline   Reply With Quote

Old   March 16, 2010, 04:09
Default
  #11
New Member
 
Denis Semyonov
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sundaero is on a distinguished road
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.
sundaero is offline   Reply With Quote

Old   April 19, 2010, 11:56
Default
  #12
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
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
jens_klostermann is offline   Reply With Quote

Old   March 9, 2011, 12:15
Default
  #13
Senior Member
 
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 174
Rep Power: 7
linch is on a distinguished road
Quote:
Originally Posted by jens_klostermann View Post
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
linch is offline   Reply With Quote

Old   June 24, 2011, 08:53
Default
  #14
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Andrea_85 is offline   Reply With Quote

Old   February 20, 2012, 11:42
Default
  #15
New Member
 
Ivo
Join Date: Feb 2012
Posts: 22
Rep Power: 5
Ivooo is on a distinguished road
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.
Ivooo is offline   Reply With Quote

Old   April 23, 2012, 12:36
Default
  #16
New Member
 
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7
aliqasemi is on a distinguished road
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.

Last edited by aliqasemi; May 2, 2012 at 12:00.
aliqasemi is offline   Reply With Quote

Old   April 23, 2012, 13:26
Default
  #17
Senior Member
 
Pablo
Join Date: Mar 2009
Posts: 102
Rep Power: 8
pablodecastillo is on a distinguished road
Hello,
Can you send me the paper to pablodecastillo at gmail dot com or give here a few hints??

Thanks
pablodecastillo is offline   Reply With Quote

Old   April 23, 2012, 15:02
Default
  #18
New Member
 
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 7
aliqasemi is on a distinguished road
Quote:
Originally Posted by pablodecastillo View Post
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.
aliqasemi is offline   Reply With Quote

Old   April 23, 2012, 16:52
Default
  #19
Senior Member
 
Pablo
Join Date: Mar 2009
Posts: 102
Rep Power: 8
pablodecastillo is on a distinguished road
Thanks Ali,

I will try tomorrow morning, and i will coment to you how it goes.
pablodecastillo is offline   Reply With Quote

Old   April 24, 2012, 05:46
Default
  #20
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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...oam-technology
akidess is offline   Reply With Quote

Reply

Tags
capillary flows, interfoam, parasitic currents

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 monitor free surface elevation vs time in OF? ozgur OpenFOAM Post-Processing 55 October 31, 2013 10:33
parasitic currents Pei-Ying 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


All times are GMT -4. The time now is 05:31.