CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

interFoam : presence of strong spurious currents in static drop in equilibrium test

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

LinkBack Thread Tools Display Modes
Old   March 11, 2017, 12:12
Post interFoam : presence of strong spurious currents in static drop in equilibrium test
New Member
Join Date: Oct 2013
Posts: 7
Rep Power: 6
swap_9068 is on a distinguished road
I am new to OpenFoam. I am trying to study performance of openfoam to simulate two phase flow. I studied standard benchmark test case of staic drop in equilibrium.
A circular liquid drop (radius = 2) placed at the center of domain of size 8*8. The density and viscosity of liquid drop are 1 and 0.01 and of gas are 0.001 and 0.001 respectively. The surface tension coefficient is 73. Grid size is 40*40 and time step is 10^-6. This properties are same as described in reference of Francois et al. (2006).
I used interFoam flow solver and modified dam break test case given in tutorial. I used zerGradient boundary conditions for pressure, velocity and alpha. I used constant time step (10^-6) by commenting adjustTimeStep and set maxCo to be 0.01. Please find attached initial problem configuration described by contours of volume fraction field. Please find attached velocity contour after 10 steps (t =10^-5) and 100 steps (t=10^-4).

static_drop_in_equilibrium_problem_velocity_contour_after_10_steps.png static_drop_in_equilibrium_problem_velocity_contour_after_100_steps.png

Ideally there should be balance between pressure and surface tension forces and velocity magnitude should be as low as possible depending on numerical algorithm used for curvature and surface tension force calculation. But I observed development of large velocity field around the interface. This indicates presence of strong spurious currents. Do we generally obtain such spurious currents using interFoam.
I came across similar old post (6 years old) regarding same problem. strange curvature with interFoam (comparison with Brackbill work) I hope there will be some improvement in openrFoam solver over last 6 years.

Is there any other better algorithm in openfoam for solving two phase flows that provide better approximation for calculation of interface advection, interface curvature and surface tension force and whose results are approximately comparable to other solvers like coupled levelset VOF method, gerris which is based on VOF.

M. M. Francois, S. J. Cummins, E. D. Dendy, D. B. Kothe, J. M. Sicilian, M. W. Williams, A balanced-force algorithm for continuous and sharp interfacial surface tension models within a volume tracking framework, J. Comput. Phys. 213 (1) (2006) 141–173.
swap_9068 is offline   Reply With Quote

Old   March 11, 2017, 13:15
Senior Member
piu58's Avatar
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 444
Rep Power: 6
piu58 is on a distinguished road
I don't know interFoam. But it may be possible that you switched on some kind of turbulent wall function. This may cause such effects.t I would try to calculate with laminar wall model.

Sent from my HTC One SV using CFD Online Forum mobile app
Uwe Pilz
Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)
piu58 is offline   Reply With Quote

Old   March 12, 2017, 03:16
New Member
Join Date: Oct 2013
Posts: 7
Rep Power: 6
swap_9068 is on a distinguished road
Thank you very much for your response. interFoam can be used to solve unsteady, incompressible, immiscible two phase flow and is based on volume of fluid method. I used simulationType as laminar and set gravity as zero for this test case. I used zeroGradient boundary conditions for velocity, pressure and volume fraction along left, right, top and bottom walls.
swap_9068 is offline   Reply With Quote

Old   March 13, 2017, 07:36
Senior Member
akidess's Avatar
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,283
Rep Power: 23
akidess will become famous soon enough
interFoam has seen some improvement for ship-scale flows, but not regarding spurious currents. You can find community solvers on the web with other algorithms, and your mileage may vary with those.
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
akidess is offline   Reply With Quote

Old   March 14, 2017, 05:57
Post improved two phase flow solver from openfoam community
New Member
Join Date: Oct 2013
Posts: 7
Rep Power: 6
swap_9068 is on a distinguished road
Please provide me list of two phase flow solvers shared by openfoam community in public domain which improve performance of interFoam solver in terms of calculation of interface curvature, surface tension force, interface advection, volume conservation and avoids spurious currents. I am interested to study single drop dynamics.
swap_9068 is offline   Reply With Quote

Old   March 24, 2017, 06:28
New Member
Join Date: May 2009
Posts: 29
Rep Power: 10
Pedro24 is on a distinguished road
Spurious currents with the VOF method is a big issue discussed in many works.

Improvements on ship-scale have been made by H. Jasak and collaborators with a new method called isoAdvector :

IsoAdvector: A new interface advection scheme for interFoam type calculations

But this is not dedicated to the specific issue of capillary effects (objective is to keep sharp interface, whatever the interface displacements)

For capillary-driven flows, which induce strong parasitic currents (as your example), there are several partial solutions such as :

1) simple smoothing of alpha function for computing capillary forces

alpha1_smoothed  = coefSmoothing * fvc::average(linearInterpolate(alpha1)) + (1-coefSmoothing) * alpha1;
2) complex solutions such as one proposed by Raeini et al. (2012) using smoothing but also filtering capillary forces

The first solution can reduce parasitic currents but it is far from perfect.
The second solution is hard to use since Raeini's code is complicated and set up your own cases can be challenging.


Pedro24 is offline   Reply With Quote

Old   April 2, 2017, 06:03
New Member
Join Date: Oct 2013
Posts: 7
Rep Power: 6
swap_9068 is on a distinguished road
@Pedro24 Thank you very much for such a detailed response. I was eagerly waiting for such reply. These tips will definitely help me in solving my problems.
On openfoam forum, I found that there is not a single thread that lists down links for all available two phase solver developed and shared by openfoam community. Thus new thread is created on this forum for sharing links for two phase solver packages shared by openfoam community. Please find link for this thread. Sharing links for two phase solver packages developed by openfoam community
Listing of two phase solver on single thread will help new members to explore two phase flow using openfoam. I request Pedro24 to share his information related to two phase solver packages on this thread.
swap_9068 is offline   Reply With Quote

Old   May 19, 2017, 05:25
Super Moderator
Tobi's Avatar
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 2,033
Blog Entries: 6
Rep Power: 36
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi guys,

I moved the thread based on the fact that it does not belong to the validation sub-forum

To the topic

I mad some tests with interFoam and the smearing interface. It is a known problem that occur suddenly after some changes in the code. The problem is the interface oscillation. There should be a paper somewhere, but I cannot remember. However, my tests are given in that thread: Bug in OpenFOAM2.3 and 2.4: extra smearing of interface
Keep foaming,
Tobias Holzmann
Tobi is online now   Reply With Quote


interface advection, interface curvature, interfoam, surface tension, two phase flow

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
error: uninitialized local variable 't' used MASOUD Fluent UDF and Scheme Programming 5 October 17, 2016 04:24
enum MASOUD Fluent UDF and Scheme Programming 0 June 5, 2010 00:49
critical error during installation of openfoam Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 14:43
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 08:21

All times are GMT -4. The time now is 13:19.