CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   how is parasitic current now? (http://www.cfd-online.com/Forums/openfoam/107861-how-parasitic-current-now.html)

houkensjtu October 8, 2012 10:07

how is parasitic current going now?
 
Hi foamers!
As you may known, parasitic current is unrealistic, vortex like velocity resides on two-phase interface when applying VOF method with CSF model.
About 3 years ago there was a thread discussing about this issue in here:

http://www.cfd-online.com/Forums/ope...-currents.html

it seems this problem still remains in current version of OF.
On the other hand, Brackbill et al.(who firstly introduced CSF model to VOF) published a paper dealing with this in about 2009. Also many other researchers paid great effort to reduce the "parasitic current" and much papers were published on this topic in the last 3 or 5 years.
In opensource world, the "Gerris" solver, created by Stephane popinet, also claimed to has solved this problem.

I am just wondering why OF still can not/did not release a parasitic current free interFoam solver. Is there any technical reason behind openfoam makes it difficult to solve?

ps:I will put some of my own test result here...plz comment!

nimasam October 8, 2012 10:43

Hello could you please share mentioned paper here

akidess October 8, 2012 11:39

OpenFoam's multiphase algorithms for two phase flows haven't seen any major changes, so the problems with parasitic currents are still there. OpenCFD is unlikely to release a major update without funding, and I'm guessing that's what's holding them back. Some researchers have published results with improved algorithms based on OpenFoam (e.g. Raeini et al 2012), but to my knowledge no one has released code.

kwardle October 8, 2012 13:29

Well, I am not familiar with the specific example cases of 'solutions' that you mention, but to some degree the issue of parasitic currents is inherent in the interface compression scheme that is used in interFoam (and related solvers). There is a nice paper by Gopala and van Wachem [2008] which compares an interFoam-like compressive scheme versus other methods. One thing I have found that helps significantly is to simply never use a value of cAlpha greater than 1. I don't know why it is higher than this in the tutorials and think this sets people on the wrong course (while I am at it--I NEVER use runTimeModifiable either, huge performance drag, which is also turned on in the tutorials).

Also, I want to mention that you implicitly are making the assumption that alternative methods which 'solve' the parasitic current issue are inherently better for all classes of problems (and that they don't have their own problems). While this may be true for certain surface tension-driven flows, this is certainly not the case for all problems--and not the ones I am personally interested in. OpenCFD HAS done paid development on interFoam-based solvers (e.g. multiphaseEulerFoam)--I have been involved in that--but there the simplicity of the interface compression method and the fact that it is phase volume conserving make it ideal for that solver.

All that said, I think it would be very interesting to see a PLIC version of interFoam with improved methods for surface tension--this would be useful for certain problems.

Just a few thoughts to consider.
-Kent

houkensjtu October 8, 2012 22:51

Quote:

Originally Posted by kwardle (Post 385577)
Well, I am not familiar with the specific example cases of 'solutions' that you mention, but to some degree the issue of parasitic currents is inherent in the interface compression scheme that is used in interFoam (and related solvers). There is a nice paper by Gopala and van Wachem [2008] which compares an interFoam-like compressive scheme versus other methods. One thing I have found that helps significantly is to simply never use a value of cAlpha greater than 1. I don't know why it is higher than this in the tutorials and think this sets people on the wrong course (while I am at it--I NEVER use runTimeModifiable either, huge performance drag, which is also turned on in the tutorials).

Also, I want to mention that you implicitly are making the assumption that alternative methods which 'solve' the parasitic current issue are inherently better for all classes of problems (and that they don't have their own problems). While this may be true for certain surface tension-driven flows, this is certainly not the case for all problems--and not the ones I am personally interested in. OpenCFD HAS done paid development on interFoam-based solvers (e.g. multiphaseEulerFoam)--I have been involved in that--but there the simplicity of the interface compression method and the fact that it is phase volume conserving make it ideal for that solver.

All that said, I think it would be very interesting to see a PLIC version of interFoam with improved methods for surface tension--this would be useful for certain problems.

Just a few thoughts to consider.
-Kent

Thanks for comment!
I do agree with u that reducing parasitic current may not be necessary for certain type of two-phase flow which is not surface-tension driven.
In fact, I noticed parasitic current problem when working on my master thesis. At that time I read several papers which all claimed that they "solved" the problem. I will list some of those papers here:
1. This paper is published by Los Alamos lab.'s research group, which I belive published RIPPLE- a very early two-phase flow solver.
http://www.sciencedirect.com/science...1999105003748#

2. This paper published by Stephane, who created Gerris
http://www.sciencedirect.com/science...199910900240X#

In these paper(though I still didn't fully understand), the problem seems to be oriented in the unbalance between surface tension & pressure force. While in last 3 years, more papers were published and the problem (also the solution method) is becoming more complicated, for example as you mentioned, some calculation tricks may affect the result more than I expected.

houkensjtu October 8, 2012 22:53

Quote:

Originally Posted by akidess (Post 385560)
OpenFoam's multiphase algorithms for two phase flows haven't seen any major changes, so the problems with parasitic currents are still there. OpenCFD is unlikely to release a major update without funding, and I'm guessing that's what's holding them back. Some researchers have published results with improved algorithms based on OpenFoam (e.g. Raeini et al 2012), but to my knowledge no one has released code.

Thanks for helpful information!
I think I need to read more papers because the problem may be not that simple and straight forward as I thought.

houkensjtu October 8, 2012 22:54

Quote:

Originally Posted by nimasam (Post 385550)
Hello could you please share mentioned paper here

Plz see my post above.

houkensjtu October 9, 2012 23:37

1 Attachment(s)
I made a simple test case to measure parasitic current in interFoam.
To be short, I put a static air bubble embed in water, and the radius of bubble is 250 um. All boundary is set as no-slip wall, means velocity are all 0. As initial condition, all velocity is 0.
After 0.0032 second physical time, the velocity field looks like:

Attachment 16108

It seems that the "current" is strongest at the very first of simulation, which I think is because in my initial condition, pressure inside the bubble is equal to pressure in the water, so strong unbalance cause a sudden boost of velocity. And after that, the current trends to be "stable", I mean the magnitude of velocity won't change suddenly, which is the condition I showed in this picture.

The max velocity here is about 0.345m/s.

I also did some simulation inside a microchannel. I will update soon. Plz comment! (especially if i made mistake or misunderstood in my boundary setting, plz point out!)

alberto October 18, 2012 23:03

Ken is correct. In interFoam cAlpha should be 1 for conservative compression (it's written also in the tutorial).

Definitely interFoam and the multiphase solvers in OpenFOAM have evolved quite a bit over the years, and in particular in 2.x.
One factor to consider when talking about VOF methods, is that implementing geometric-based methods on polyhedral grids is on one hand not trivial, on the other hand it's computationally expensive, and in some case it has limitations. Add to this the fact that in a good number of industrial applications a perfect interface reconstruction is not required, but users are more interested in a good estimate of the trends, and you should have a better idea why it often makes sense to use compressive schemes.

If you need higher accuracy there are level-set/VOF based approaches, which provide a much better quality of the interface reconstruction. Of course the computational cost and the complexity of the procedure are significantly higher.

alberto October 18, 2012 23:05

Quote:

Originally Posted by houkensjtu (Post 385832)
I made a simple test case to measure parasitic current in interFoam.
To be short, I put a static air bubble embed in water, and the radius of bubble is 250 um. All boundary is set as no-slip wall, means velocity are all 0. As initial condition, all velocity is 0.
After 0.0032 second physical time, the velocity field looks like:

Attachment 16108

It seems that the "current" is strongest at the very first of simulation, which I think is because in my initial condition, pressure inside the bubble is equal to pressure in the water, so strong unbalance cause a sudden boost of velocity. And after that, the current trends to be "stable", I mean the magnitude of velocity won't change suddenly, which is the condition I showed in this picture.

The max velocity here is about 0.345m/s.

I also did some simulation inside a microchannel. I will update soon. Plz comment! (especially if i made mistake or misunderstood in my boundary setting, plz point out!)

Maybe attach the test case, so we can take a look ;-)

aliqasemi May 15, 2013 15:44

An early version of my code - which may not be exactly what presented in my 2012 paper- was previously uploaded to our groups website:

http://www3.imperial.ac.uk/earthscie...tware/porefoam

It wasn't advertised because I wanted to release my new changes later for unstructured grids, but that is going to be done over this summer. The code also needs, I am speculating, improvements to handle density/viscosity contrasts efficiently, but I am not working on the code anymore. I may occasionally test new ideas to improve the efficiency of the code but not its accuracy, but now I am busy with other stuff.

Improving accuracy of the method for capillary pressure, in my opinion, is possible only through using surface-tracking methods, or using smoothing while applying some filters to keep the interface locally stable.


In any events, I really appreciate any useful feedbacks, either shared over forums, or done more professionally in peer-reviewed journals. I am submitting a paper on the application of the method now, and one other one over the summer, then I will be happy to share more code. The paper themselves should be interesting to those people studying capillary dominated flow too.

dl6tud December 13, 2013 12:39

Does anyone know some literature about the relation between spurious velocities and body forces (e.g. gravity)?


All times are GMT -4. The time now is 07:00.