Difference between revisions of "The stationary droplet by Lionel Gamet"

From OpenFOAM Wiki
Jump to navigation Jump to search
Line 43: Line 43:
  
 
[[File:Gamet_Eq1.png|280px|center|]]
 
[[File:Gamet_Eq1.png|280px|center|]]
 +
 +
We use the stability criterion of Popinet . The time step must be bellow the following upper limit:
  
 
[[File:Gamet_Eq2.png|280px|center|]]
 
[[File:Gamet_Eq2.png|280px|center|]]
 +
 +
Computations are done by default at a constant time step and up to t= 100 t_σ. In practice, the time step is set constant to:
  
 
[[File:Gamet_Eq3.png|280px|center|]]
 
[[File:Gamet_Eq3.png|280px|center|]]

Revision as of 05:32, 17 September 2020

Go back to Multiphase modeling.

The stationary droplet

The starting cases case can be downloaded here:

Reference OpenFOAM results of the stationary droplet can be found here.

Introduction

This case is a reference test case for Volume-of-Fluid (VoF) simulations. This benchmark configuration allows for quantitative measurements of the spurious currents appearing in VoF simulations. The case consists in a single static droplet in a quiescent liquid under zero gravity. It is a widely used test case in the literature, described by Popinet [1]. More details can be found in the iterature [1,2,3,4,5] and in the article in press of Gamet et al. [6].

Configuration and boundary conditions for 2D static droplet case under zero gravity.

The 2D case setup is schematized in the Figure above. The phase 1 is the liquid, while the phase 2 is the gas. Both fluids have the same viscosity μ and density ρ. The volume fraction α is set to 1 inside the droplet near the bottom left corner, and to 0 outside. The density ρ and the surface tension σ between the two fluids are both taken as unitary constant values. The droplet has an initial diameter D_0 = 2R_0 = 0.8 m. Only a quarter of the 2D geometry is simulated in a domain of size 1x1 m. The droplet is placed at the bottom left corner of the domain. All boundary conditions are symmetries. This test case can easily be extended to 3D, where 1/8th of an initially spherical droplet is then simulated.

Ideally, the static droplet test case is not supposed to generate any velocity field and the pressure field should follow the Laplace pressure jump at the interface. However, parasitic velocities (also called spurious currents) can occur from a numerical imbalance between the discretization errors of the pressure gradient and surface tension terms.

Setting up the test case in OpenFOAM

This test case uses incompressible VoF solvers in OpenFOAM, namely interFoam or interIsoFoam solvers.

A uniform Cartesian grid built with blockMesh is used for the simulations. When running the sensitivity script, different grid levels and Laplace numbers are used (see section below). The droplet is initialized as a cylinder in 2D (as a sphere in 3D) using the setAlphaField utility.

In the fvSchemes file, a Crank-Nicolson second order time scheme with blending coefficient 0.9 is chosen. Gauss limitedLinearV 1 is used to treat the convective term, and Gauss vanLeer is used for the α convective term for MULES simulations. The Gauss linear scheme is used by default for all gradient terms.

In the fvSolution file, the GAMG implicit solver is used for pressure terms, while the smooth solver is used for the velocity. The PIMPLE algorithm uses 3 nOuterCorrectors in 2D (only 1 in 3D to save computational time) and 3 PISO correctors (nCorrectors=3). On other benchmark cases, it was found that momentumPredictor needed to be set to true to get a correct solution in terms of rising velocity and droplet circularity, in particular with isoAdvector. Both isoAdvector and MULES numerical parameters are present and appear separately in fvSolution, so that both interFoam and interIsoFoam can be run from the same input files.

The following reference time and velocity can be used to nondimensionalize results [5]:

Gamet Eq1.png

We use the stability criterion of Popinet . The time step must be bellow the following upper limit:

Gamet Eq2.png

Computations are done by default at a constant time step and up to t= 100 t_σ. In practice, the time step is set constant to:

Gamet Eq3.png
Gamet Eq4.png
Gamet Eq5.png


References

[1] S. Popinet: An accurate adaptive solver for surface-tension-driven interfacial flows," Journal of Computational Physics, vol. 228, no. 16, pp. 5838-5866, 2009.

[2] M. M. Francois, S. J. Cummins, E. D. Dendy, D. B. Kothe, J. M. Sicilian, and M. W. Williams: A balanced-force algorithm for continuous and sharp interfacial surface tension models within a volume tracking framework," Journal of Computational Physics, vol. 213, no. 1, pp. 141-173, 2006.

[3] S. Popinet: A quadtree-adaptive multigrid solver for the serre-green-naghdi equations," Journal of Computational Physics, vol. 302, pp. 336-358, 2015.

[4] --: Numerical models of surface tension," Annual Review of Fluid Mechanics, vol. 50, pp. 49-75, 2018.

[5] T. Abadie, J. Aubin, and D. Legendre: On the combined effects of surface tension force calculation and interface advection on spurious currents within volume of fluid and level set frameworks," Journal of Computational Physics, vol. 297, pp. 611-636, 2015.

[6] L. Gamet, M. Scala, J. Roenby, H. Scheufler, and J.-L. Pierson: Validation of volume-of-Fluid OpenFOAM isoAdvector solvers using single bubble benchmarks," Submitted to Computers and Fluids, 2020.

[7] H. Scheufler and J. Roenby: Accurate and effcient surface reconstruction from volume fraction data on general meshes," J. Comp. Phys., vol. 383, pp. 1 - 23, 2019.