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

how is parasitic current now?

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

Like Tree8Likes
  • 3 Post By houkensjtu
  • 1 Post By alberto
  • 2 Post By aliqasemi
  • 2 Post By JULIEN MAES

Reply
 
LinkBack Thread Tools Display Modes
Old   October 8, 2012, 09:07
Default how is parasitic current now?
  #1
Member
 
HouKen
Join Date: Jul 2011
Posts: 66
Rep Power: 7
houkensjtu is on a distinguished road
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:

parasitic currents

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!

Last edited by houkensjtu; October 8, 2012 at 10:04.
houkensjtu is offline   Reply With Quote

Old   October 8, 2012, 09:43
Default
  #2
Senior Member
 
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,208
Blog Entries: 1
Rep Power: 17
nimasam is on a distinguished road
Hello could you please share mentioned paper here
nimasam is offline   Reply With Quote

Old   October 8, 2012, 10:39
Default
  #3
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,163
Rep Power: 20
akidess will become famous soon enough
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.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2
akidess is offline   Reply With Quote

Old   October 8, 2012, 12:29
Default
  #4
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 208
Rep Power: 13
kwardle is on a distinguished road
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
kwardle is offline   Reply With Quote

Old   October 8, 2012, 21:51
Default
  #5
Member
 
HouKen
Join Date: Jul 2011
Posts: 66
Rep Power: 7
houkensjtu is on a distinguished road
Quote:
Originally Posted by kwardle View Post
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 is offline   Reply With Quote

Old   October 8, 2012, 21:53
Default
  #6
Member
 
HouKen
Join Date: Jul 2011
Posts: 66
Rep Power: 7
houkensjtu is on a distinguished road
Quote:
Originally Posted by akidess View Post
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 is offline   Reply With Quote

Old   October 8, 2012, 21:54
Default
  #7
Member
 
HouKen
Join Date: Jul 2011
Posts: 66
Rep Power: 7
houkensjtu is on a distinguished road
Quote:
Originally Posted by nimasam View Post
Hello could you please share mentioned paper here
Plz see my post above.
houkensjtu is offline   Reply With Quote

Old   October 9, 2012, 22:37
Default
  #8
Member
 
HouKen
Join Date: Jul 2011
Posts: 66
Rep Power: 7
houkensjtu is on a distinguished road
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:

22222.jpg

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!)
houkensjtu is offline   Reply With Quote

Old   October 18, 2012, 22:03
Default
  #9
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
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.
afshinb likes this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   October 18, 2012, 22:05
Default
  #10
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by houkensjtu View Post
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 ;-)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   May 15, 2013, 14:44
Default
  #11
New Member
 
Ali Q Raeini
Join Date: Feb 2010
Posts: 21
Rep Power: 8
aliqasemi is on a distinguished road
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.
hannes and Bernhard like this.
aliqasemi is offline   Reply With Quote

Old   December 13, 2013, 12:39
Default
  #12
Member
 
Join Date: May 2012
Location: Dresden, Germany
Posts: 32
Rep Power: 6
dl6tud is on a distinguished road
Does anyone know some literature about the relation between spurious velocities and body forces (e.g. gravity)?
dl6tud is offline   Reply With Quote

Old   April 15, 2015, 11:13
Default
  #13
Member
 
Vignesh
Join Date: Oct 2012
Location: Darmstadt, Germany
Posts: 63
Rep Power: 6
vigneshTG is on a distinguished road
Hi Ali Q Raeini !!
Did you publish the paper ? Can you tell us the title ??


Quote:
Originally Posted by aliqasemi View Post
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.
__________________
Thanks and Regards

Vignesh
vigneshTG is offline   Reply With Quote

Old   November 12, 2015, 12:47
Default
  #14
New Member
 
Julien Maes
Join Date: Sep 2015
Posts: 10
Rep Power: 3
JULIEN MAES is on a distinguished road
Hello,

I am new to this problem, and I downloaded interFoamSSF from github
https://github.com/aliozel/interFoamSSF

and poreFoam from the imperial college website (shared previously by Ali Raeini).
https://www.imperial.ac.uk/engineeri...e-flow-solver/

I found out that for both codes, the latest version do not kill spurious current for the static droplet case. I might have made a mistake so I will be grateful if other people try it and tell me what they found out.

For interFoamSSF, I switch to the explicit MULES solver for alpha and I am converging quite nicely. However, I realised that the flux of the interface normal vector, saved as nHatf_ in the interface properties class, is never calculated here, so always equal to zero. This vector is used when we calculate the artificial compression part in the equation for alpha. Therefore, this is equivalent to set cAlpha=0.

Does this mean that for SSF, we should not use any artificial compression?

Cheers,

Julien
JULIEN MAES is offline   Reply With Quote

Old   February 26, 2016, 08:30
Default
  #15
Member
 
Camille Bilger
Join Date: Jul 2013
Posts: 37
Rep Power: 5
kmou is on a distinguished road
Quote:
Originally Posted by JULIEN MAES View Post
Hello,

I am new to this problem, and I downloaded interFoamSSF from github
https://github.com/aliozel/interFoamSSF

and poreFoam from the imperial college website (shared previously by Ali Raeini).
https://www.imperial.ac.uk/engineeri...e-flow-solver/

I found out that for both codes, the latest version do not kill spurious current for the static droplet case. I might have made a mistake so I will be grateful if other people try it and tell me what they found out.


Julien
Hi Julien,
A few months later, do you have any luck with the static droplet case and spurious currents?
Camille
kmou is offline   Reply With Quote

Old   February 26, 2016, 08:45
Default
  #16
New Member
 
Julien Maes
Join Date: Sep 2015
Posts: 10
Rep Power: 3
JULIEN MAES is on a distinguished road
Hi Camille,

Yes, I did make some progress. For interFOAMSSF, I changed the MULES solver for alpha to explicit. I kill spurious current for the static droplet case. However I moved on to a moving droplet case and the results are not very good. Another important remark is that in the version of InterFOAMSSF I found on github, the interface normal vector nHatf_ is never updated in interfaceproperties.cpp. This vector is used for compressing the indicator alpha so it is very important to correct this problem.

For poreFOAM, I modified the code I found online so that it does exactly what's inside Ali Raeini's thesis and it works perfectly for static and moving droplet. However, it does not converge for more complex test case of pore invasion, while Ali's code that you find online seems to give me coherent results. We are currently working to get a code that would solve both droplet and more complex pore invasion test cases.

Regards,

Julien
Cyp and kmou like this.
JULIEN MAES is offline   Reply With Quote

Old   June 6, 2016, 07:29
Default
  #17
New Member
 
chubb87
Join Date: May 2011
Posts: 20
Rep Power: 7
chubb87 is on a distinguished road
Hi Julien,

what were the changes in poreFOAM you had to do compared to the paper? Are these changes now included in the source code that can be downloaded? I might also give it a try.
chubb87 is offline   Reply With Quote

Old   June 8, 2016, 02:26
Default
  #18
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,163
Rep Power: 20
akidess will become famous soon enough
Thanks for the hint Julien, I finally got around to pushing this change to the repository. Crazy noone (including me!) noticed the missing update of nHatf until now

poreFoam still contains a lot more stuff I don't have time to implement in interFoamSSF. You can find it here: https://figshare.com/articles/poreFoam_package/1155422

Quote:
Originally Posted by JULIEN MAES View Post
Hi Camille,

Yes, I did make some progress. For interFOAMSSF, I changed the MULES solver for alpha to explicit. I kill spurious current for the static droplet case. However I moved on to a moving droplet case and the results are not very good. Another important remark is that in the version of InterFOAMSSF I found on github, the interface normal vector nHatf_ is never updated in interfaceproperties.cpp. This vector is used for compressing the indicator alpha so it is very important to correct this problem.

For poreFOAM, I modified the code I found online so that it does exactly what's inside Ali Raeini's thesis and it works perfectly for static and moving droplet. However, it does not converge for more complex test case of pore invasion, while Ali's code that you find online seems to give me coherent results. We are currently working to get a code that would solve both droplet and more complex pore invasion test cases.

Regards,

Julien
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2
akidess is offline   Reply With Quote

Old   June 8, 2016, 05:13
Default
  #19
New Member
 
Julien Maes
Join Date: Sep 2015
Posts: 10
Rep Power: 3
JULIEN MAES is on a distinguished road
@chubb87 the changes I have made simply revert to a previous version of poreFOAM, which gives better results for the cases of single droplet, but not very good results for test cases in microchannels and micro-CT images, so it is not such a good idea to do them anyway. You should download poreFOAM and have a look at it, it is very interesting.
JULIEN MAES is offline   Reply With Quote

Reply

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
Turbidity current julien.n FLUENT 0 June 25, 2012 19:12
What is the difference between current time step and current time djing FLUENT 4 May 1, 2012 16:18
dilute gravity current at very flow base doronzo FLUENT 0 October 5, 2011 15:38
Interfoam Microchannel flow parasitic velocities cfd_user2011 OpenFOAM 2 June 12, 2011 15:43
Cells of current line in three dimensionnal flow GACEM_hatem Phoenics 2 June 18, 2001 09:38


All times are GMT -4. The time now is 21:34.