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

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

 March 11, 2017, 12:12 interFoam : presence of strong spurious currents in static drop in equilibrium test #1 New Member   Nicky Join Date: Oct 2013 Posts: 4 Rep Power: 5 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_setup.png 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.

 March 11, 2017, 13:15 #2 Member     Uwe Pilz Join Date: Feb 2017 Location: Leipzig, Germany Posts: 78 Rep Power: 2 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 -- Sie ahnen nicht, wieviel Poesie in der Berechnung einer Logarithmentafel enthalten ist (Carl Friedrich Gauß)

 March 12, 2017, 03:16 #3 New Member   Nicky Join Date: Oct 2013 Posts: 4 Rep Power: 5 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.

 March 13, 2017, 07:36 #4 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,193 Rep Power: 21 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.

 March 14, 2017, 05:57 improved two phase flow solver from openfoam community #5 New Member   Nicky Join Date: Oct 2013 Posts: 4 Rep Power: 5 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.

 March 24, 2017, 06:28 #6 New Member   Pierre HORGUE Join Date: May 2009 Posts: 26 Rep Power: 9 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 Code: `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 https://figshare.com/articles/poreFoam_package/1155422 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. Sincerely, Pierre

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post MASOUD Fluent UDF and Scheme Programming 5 October 17, 2016 04:24 MASOUD Fluent UDF and Scheme Programming 0 June 5, 2010 00:49 Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01 piprus OpenFOAM Installation 22 February 25, 2010 14:43 chiven OpenFOAM Installation 3 December 1, 2009 08:21

All times are GMT -4. The time now is 23:32.