Coupled Level-Set / VOF Solver for OpenFOAM

interLevelSetFoam simulates two incompressible, immiscible fluids. The volume fraction is transported with VOF/MULES, which conserves mass. At every outer corrector, a signed-distance level set is rebuilt from that volume fraction. The level set then supplies the interface curvature and the smooth density and viscosity that the momentum equation uses.

How it works

All of the level-set work lives in one class, levelSetCoupledMixture (src/levelSetCoupledMixture). It extends OpenFOAM's immiscibleIncompressibleTwoPhaseMixture, so the rest of the solver (MULES, turbulence, fvOptions, dynamic meshes) is unchanged. With h the reference cell size, every rebuild does the following:

Step	Operation
Seed	d0 = (2 alpha1 - 1) * seedCoeff * h
Redistance	d <- d + dTau * sgn(d0) * (1 - |grad d|), dTau = pseudoTimeCoeff * h, nRedistanceIter times
Heaviside	H = (1 + x + sin(pi x)/pi) / 2, x = clamp(d/eps, -1, 1), eps = widthCoeff * h
Curvature	kappa = -div(n_f), n_f = (grad d)_f / |(grad d)_f|
Surface tension	f_f = sigma * kappa_f * snGrad(H)
Properties	rho = H rho1 + (1-H) rho2, mu = H mu1 + (1-H) mu2

The density and the mass flux rhoPhi both come from H. The momentum equation also removes the remaining mass imbalance, ddt(rho) + div(rhoPhi). Together, these keep ddt(rho U) and div(rhoPhi U) consistent with each other. The coupling follows the simple coupled level-set/VOF approach of Albadawi et al. (2013).

Settings

Every entry is optional. They all go in a levelSet sub-dictionary of constant/transportProperties. The surface tension coefficient is the usual sigma entry.

levelSet
{
    cellSize         0.00625;   // h [m]; default: smallest cell spacing
    widthCoeff       1.5;       // interface half-width eps / h
    seedCoeff        0.75;      // |seed distance| / h
    pseudoTimeCoeff  0.1;       // redistance pseudo-time step / h
    nRedistanceIter  15;        // default: ceil(widthCoeff/pseudoTimeCoeff)
    curvatureFrom    levelSet;  // levelSet | volumeFraction
    propertiesFrom   levelSet;  // levelSet | volumeFraction
}

On graded meshes, set cellSize explicitly to the cell size near the interface. The solver writes three extra fields: levelSet (signed distance), heaviside and levelSetCurvature.

Build

git clone https://github.com/cloner0110/LevelSet-VOF.git
cd LevelSet-VOF/src && wmake

Tested with OpenFOAM.com v2306, v2312 (CI), v2512 (CI) and v2606.

Tutorial: 2-D rising bubble

Tutorial/bubbleColumn is test case 2 of Hysing et al. (2009). A circular bubble of radius 0.25 starts at (0.5, 0.5) in a closed 1 × 2 box, with ρ1/ρ2 = 1000, μ1/μ2 = 100, σ = 1.96 and g = 0.98.

• The bubble is set with setAlphaField, which integrates the volume fraction in each cut cell.
• The top and bottom walls are no-slip, the side walls are free-slip, and p_rgh is fixedFluxPressure on all walls.
• The case writes the bubble's centre of mass and mean rise velocity at every time step, to postProcessing/bubble/0/volFieldValue.dat.

cd Tutorial/bubbleColumn && ./Allrun

The results below were run with OpenFOAM v2606. The 1/h = 160 runs are the tutorial as shipped, on 4 MPI ranks. The 1/h = 80 runs use (80 160 1) cells and deltaT 7.8125e-4. The reference is TP2D on its finest mesh, from Hysing et al. (2009), Tables XIII and XVI.

Run	Vmax,1 (t)	Vmax,2 (t)	yc(t = 3)
TP2D, 1/h = 640 (reference)	0.2524 (0.733)	0.2434 (2.071)	1.1380
FreeLIFE, 1/h = 160	0.2514 (0.728)	0.2440 (1.984)	1.1249
MooNMD	0.2502 (0.732)	0.2393 (2.060)	1.1376
this solver, 1/h = 80	0.2491 (0.734)	0.2287 (1.913)	1.1140
this solver, 1/h = 160	0.2472 (0.738)	0.2315 (1.982)	1.1174
volume-fraction coupling, 1/h = 160	0.2471 (0.734)	0.2309 (2.001)	1.1140

The phase volume is conserved to all printed digits.

• With curvatureFrom and propertiesFrom set to volumeFraction, the solver reproduces interFoam.
• The level-set coupling follows the reference more closely than that setting after the first maximum.

Results published for this tutorial before the setup fix (PR #4) came from a tilted, 3% oversized initial bubble and a top boundary that let fluid through. They should not be used.

References

• Taran, A. (2026). A consistent coupled level-set and volume-of-fluid solver for two-phase flow in OpenFOAM. arXiv preprint arXiv:2610.24225. https://arxiv.org/abs/2610.24225v1

License

This solver is derived from OpenFOAM's interFoam and links against OpenFOAM libraries. It is therefore distributed under the GNU General Public License v3, like OpenFOAM itself. Files that derive from OpenFOAM keep the original OpenFOAM Foundation and OpenCFD copyright lines.

OpenFOAM® is a registered trade mark of OpenCFD Ltd. This project is not approved or endorsed by OpenCFD Ltd.

Contact

• Email: amirhossein.taran@ucdconnect.ie
• Issues: GitHub Issues

Citation

If you use this solver, or want to cite it, please cite the following paper:

Taran, A. (2026). A consistent coupled level-set and volume-of-fluid solver for two-phase flow in OpenFOAM. arXiv preprint arXiv:2610.24225. https://arxiv.org/abs/2610.24225v1

@misc{taran2026interLevelSetFoam,
  author        = {Taran, Amirhossein},
  title         = {A consistent coupled level-set and volume-of-fluid solver
                   for two-phase flow in {OpenFOAM}},
  year          = {2026},
  eprint        = {2610.24225},
  archivePrefix = {arXiv},
  primaryClass  = {physics.flu-dyn},
  doi           = {10.48550/arXiv.2610.24225},
  url           = {https://arxiv.org/abs/2610.24225v1}
}