[swap_9068]

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.

[piu58]

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

[swap_9068]

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.

[akidess]

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.

[swap_9068]

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.

[Pedro24]

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 :

https://www.cfd-online.com/Forums/op...culations.html

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

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

[swap_9068]

@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.

[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

[suraj]

Originally Posted by swap_9068

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.

Hi Nicky,
Hope this response is not too late, but we have looked at this problem in the past. Here is our paper. Please look at section 3.3.3 in this paper. Specifically, we found that the key issue with spurious currents is the "stair-stepped" representation of the interface. This sets up an unphysical capillary flow in the vicinity of the interface. If left temporally unresolved, this flow grows unbounded leading to catastropic results! We have presented a "stable" time step condition with OpenFOAM.

Hope this helps.
Best,
Suraj