CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

trying to simulate the splashing phenomenon with multiphaseInterFoam

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

Like Tree2Likes
  • 2 Post By kwardle

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2012, 06:16
Default trying to simulate the splashing phenomenon with multiphaseInterFoam
  #1
New Member
 
Andrea Cristina
Join Date: May 2012
Location: Milano
Posts: 4
Rep Power: 5
AC87 is on a distinguished road
Hi to evrybody,

I'm working with droplets impingement on a thin liquid film, and I'm trying to simulate the splashing phenomenon with corolla rising and instability. So I succesfully use interFoam, but now I want to distinguish the drop liquid from the film liquid, and so i decided to use multiphaseInterFoam with the same boundary condition (that besides are the test case BC) .
This kind of simulation is not able to reproduce the splaching phenomenon.
Can anyone help me?
Thanks
AC87 is offline   Reply With Quote

Old   July 18, 2012, 09:56
Default
  #2
New Member
 
Andrea Cristina
Join Date: May 2012
Location: Milano
Posts: 4
Rep Power: 5
AC87 is on a distinguished road
is anyone familiar with multiphaseInterFoam?
AC87 is offline   Reply With Quote

Old   July 24, 2012, 10:05
Default
  #3
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
When you say it does not reproduce the splashing phenomenon do you mean that you see different results between your interFoam case and the one with multiphaseInterFoam on the same mesh? Which version are you using? Perhaps a few side-by-side comparisons of what you are seeing would be helpful. What about interfacial tension for your two liquids? Have you set this to zero to mimick interFoam behavior and match what you want to see?

Also, the newest version (2.1.1) should have much improved phase conservation in multiphaseInterFoam over older versions.
-Kent
kwardle is offline   Reply With Quote

Old   July 25, 2012, 11:50
Default
  #4
New Member
 
Andrea Cristina
Join Date: May 2012
Location: Milano
Posts: 4
Rep Power: 5
AC87 is on a distinguished road
First of all thanks for answering my post.
My intent is to use multiphaseinterFoam to distinguish different liquid (from drop anf film) in the corona formation.
I use the same mesh, the same initial and boundary condition in the interFoam and multiphase case. Moreover i set to zero the surface tension value for the drop and film mixture and to 1 the contactangle (however I've done different case in witch I've changed sigma and the contact angle).
I use the 2.0 OpenFoam version.


Recently I improved my results changing the solution scheme(now i can see the splash), but they are still different from interFoam.
AC87 is offline   Reply With Quote

Old   July 25, 2012, 13:42
Default
  #5
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
Yeah, I think I understand what you are trying to do. Does the version of multiphaseEulerFoam print out a line like, "Phase-sum volume fraction, min, max = 1 0.999909 1.00003"? The version with improved phase conservation should do this.

The other thing to consider (and it sounds like maybe you have) is that as part of the sharp interface tracking it uses interface compression along with an appropriate discretization scheme to keep the interface sharp. Have you change the divSchemes for alpha in fvScheme? The problem is that you cannot in multiphaseInterFoam change them independently for each phase pair. So, even if you are using the same fluid props, etc., it will keep a sharp interface between the two which might alter the results a little from the interFoam case. I wonder if you would get better results by using vanLeer/interfaceCompression only for the liquid-air part? Incidentally, you can do this in multiphaseEulerFoam, but I don't think that is what you need here.

What value for cAlpha are you using in fvSolution? The tutorials use 2, but I would not go more than 1 or 1.5 to avoid spurious interfacial currents. And 1 is sufficient in any case I have tried.
kwardle is offline   Reply With Quote

Old   July 30, 2012, 01:16
Default Hi Every Foamers:
  #6
Member
 
vahid
Join Date: Feb 2012
Location: Mashhad-Iran
Posts: 80
Rep Power: 4
vahid.najafi is an unknown quantity at this point
Hi Dear Foamers.
I want to add surfacetension in one solver(my solver is interPhsaeChangeFoam),for this reason I added :
fvc::interpolate(interface.sigma())
in this code:

#include ''fvCFD.H''



Foam::tmp<Foam::volScalarField>
Foam:haseChangeTwoPhaseMixtures::SchnerrSauer: Coeff
(
const volScalarField& p
) const
{
volScalarField limitedAlpha1(min(max(alpha1_, scalar(0)), scalar(1)));
volScalarField rho
(
limitedAlpha1*rho1() + (scalar(1) - limitedAlpha1)*rho2()
);
return

//......I want to change it( <<sigma>> surface tension multiple in it):
(3*rho1()*rho2())*sqrt(2/(3*rho1()))*(fvc::interpolate(interface.sigma()))
*rRb(limitedAlpha1)/(rho*sqrt(mag(p - pSat()) + 0.01*pSat()));
//.................................................. ......
}
dont successful wmake, and seen(was not declared ):
phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.C:113: error: 'interface' was not declared in this scope
make: *** [Make/linux64GccDPOpt/SchnerrSauer.o] Error 1
please help me,and tell me ,How to correct this problem???
vahid.najafi is offline   Reply With Quote

Old   May 14, 2014, 23:03
Default The interface become fuzzy with multiphaseinterFoam
  #7
New Member
 
zhanglei
Join Date: May 2013
Location: China
Posts: 19
Rep Power: 4
becklei is on a distinguished road
Quote:
Originally Posted by kwardle View Post
Yeah, I think I understand what you are trying to do. Does the version of multiphaseEulerFoam print out a line like, "Phase-sum volume fraction, min, max = 1 0.999909 1.00003"? The version with improved phase conservation should do this.

The other thing to consider (and it sounds like maybe you have) is that as part of the sharp interface tracking it uses interface compression along with an appropriate discretization scheme to keep the interface sharp. Have you change the divSchemes for alpha in fvScheme? The problem is that you cannot in multiphaseInterFoam change them independently for each phase pair. So, even if you are using the same fluid props, etc., it will keep a sharp interface between the two which might alter the results a little from the interFoam case. I wonder if you would get better results by using vanLeer/interfaceCompression only for the liquid-air part? Incidentally, you can do this in multiphaseEulerFoam, but I don't think that is what you need here.

What value for cAlpha are you using in fvSolution? The tutorials use 2, but I would not go more than 1 or 1.5 to avoid spurious interfacial currents. And 1 is sufficient in any case I have tried.
Hi, Kent!

I work with the Multiphaseinterfoam which is added energy equation and a viscosity model. Firstly, this solver have finished the two phase flow like the picture 1, and the interface between red and blue is good. secondly, I set the third phases with funkysetfields in a circle(to be a bubble) like the picture 2. Lastly, I run the Multiphaseinterfoam again to get the deformation of the bubble.

Unfortunately, the interface of the bubble become more and more fuzzy with the time going as shown as the picture 3. what's more, the interface between the early two phases is still good.

why the interface of bubble become fuzzy? Any answer is welcome! Thanks in advance!
Attached Images
File Type: jpg 1.jpg (29.8 KB, 34 views)
File Type: jpg 2.jpg (31.1 KB, 30 views)
File Type: jpg 3.jpg (32.3 KB, 32 views)
becklei is offline   Reply With Quote

Old   May 15, 2014, 10:30
Default
  #8
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
Just looks to me like your mesh resolution is too coarse. That is unless you have set cAlpha=0 for some reason in your setup.
kwardle is offline   Reply With Quote

Old   May 15, 2014, 22:56
Default
  #9
New Member
 
zhanglei
Join Date: May 2013
Location: China
Posts: 19
Rep Power: 4
becklei is on a distinguished road
Quote:
Originally Posted by kwardle View Post
Just looks to me like your mesh resolution is too coarse. That is unless you have set cAlpha=0 for some reason in your setup.
Thank you so much!

After correct the cAlpha as you told me, I got a quite sharp interface.

About the mesh resolution, I want to change the mesh tool,because the piontwise can not deal with the small size area(0.003m*0.01m*0.0001m) very well.

On the other hand, I find the sharp interface(cAlpha=1) will become unstable when the difference of physical properties of the two phase is large. About the "unstable", in my case, the interface become asymmetric as shown in the picture. Do you have any good way to deal with this "asymmetric" problem?
thanks in advance!
Attached Images
File Type: jpg asymmetric.jpg (91.2 KB, 34 views)
becklei is offline   Reply With Quote

Old   May 22, 2014, 15:53
Default
  #10
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
What you are seeing is a well-known issue with interface compression schemes such as used by interFoam. This has been discussed elsewhere--search for 'spurious currents' and have a look at this thread:
Suitability of interface compression scheme for interface rupture simulations
I mention there a paper by Gopala et al that compares the accuracy of various methods.
wyldckat and becklei like this.
kwardle is offline   Reply With Quote

Old   June 8, 2014, 23:13
Default
  #11
New Member
 
zhanglei
Join Date: May 2013
Location: China
Posts: 19
Rep Power: 4
becklei is on a distinguished road
Quote:
Originally Posted by kwardle View Post
What you are seeing is a well-known issue with interface compression schemes such as used by interFoam. This has been discussed elsewhere--search for 'spurious currents' and have a look at this thread:
Suitability of interface compression scheme for interface rupture simulations
I mention there a paper by Gopala et al that compares the accuracy of various methods.
thanks for your reply, I know a little about the 'spurious currents' and I found the greater the viscosity ratio, the greater the 'spurious currents' in my case
becklei 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
Dynamic contact angle calculation in multiphaseInterFoam rajeshchem OpenFOAM 2 January 31, 2014 08:52
a case which is very tough to simulate....... sharonyue OpenFOAM Running, Solving & CFD 6 November 22, 2012 02:20
how can simulate distilation water mustapha_alg FLUENT 0 August 5, 2012 06:55
Simulate the wind profile on a wind turbine---> HOW ???? mohammad Main CFD Forum 0 April 13, 2012 08:16
Simulate the wind profile on a wind turbine---> HOW ???? mohammad Main CFD Forum 0 April 13, 2012 08:07


All times are GMT -4. The time now is 15:23.