A new volume-of-fluid method in OpenFOAM

Abstract

To realise the full potential of Computational Fluid Dynamics (CFD) within marine science and engineering, there is a need for continuous maturing as well as verification and validation of the numerical methods used for free surface and interfacial flows. One of the distinguishing features here is the existence of a water surface undergoing large deformations and topological changes during transient simulations e.g. of a breaking wave hitting an offshore structure. To date, the most successful method for advecting the water surface in marine applications is the Volume-of-Fluid (VOF) method. While VOF methods have become quite advanced and accurate on structured meshes, there is still room for improvement when it comes to unstructured meshes of the type needed to simulate flows in and around complex geometric structures. We have recently developed a new geometric VOF algorithm called isoAdvector for general meshes and implemented it in the OpenFOAM interfacial flow solver called interFoam. We have previously shown the advantages of isoAdvector for simple pure advection test cases on various mesh types. Here we test the effect of replacing the existing interface advection method in interFoam, based on MULES limited interface compression, with the new isoAd-vector method. Our test case is a steady 2D stream function wave propagating in a periodic domain. Based on a series of simulations with different numerical settings, we conclude that the introduction of isoAdvector has a significant effect on wave propagation with interFoam. There are several criteria of success: Preservation of water volume, of interface sharpness and shape, of crest kinematics and celerity, not to mention computational efficiency. We demonstrate how isoAdvector can improve on many of these parameters, but also that the success depends on the solver setup. Thus, we cautiously conclude that isoAdvector is a viable alternative to MULES when set up correctly, especially when interface sharpness, interface smoothness and calculation times are important. There is, however, still potential for improvement in the coupling of isoAdvector with interFoam's PISO based pressure-velocity solution algorithm.

Full text

VII International Conference on Computational Methods in Marine Engineering
MARINE 2017
M. Visonneau, P. Queutey and D. Le Touz´e (Eds)
A NEW VOLUME-OF-FLUID METHOD IN OPENFOAM
Johan Roenby∗, Bjarke Eltard Larsen?, Henrik Bredmose†AND Hrvoje
Jasak‡
∗DHI, Agern All 5, 2970 Hørsholm, Denmark, e-mail: jro@dhigroup.com
?DTU Mechanical Engineering, Richard Petersens Plads, 2800 Kgs. Lyngby, Denmark, e-mail:
bjelt@mek.dtu.dk
†DTU Wind Energy, Technical University of Denmark, Nils Koppels Alle, 2800 Lyngby,
Denmark
‡Faculty of Mechanical Engineering and Naval Architecture, University of Zagreb, Ivana
Lucica 5, Zagreb, Croatia
Key words: CFD, Marine Engineering, Interfacial Flows, IsoAdvector, VOF Methods, Surface
Gravity Waves
Abstract. To realise the full potential of Computational Fluid Dynamics (CFD) within ma-
rine science and engineering, there is a need for continuous maturing as well as verification
and validation of the numerical methods used for free surface and interfacial flows. One of the
distinguishing features here is the existence of a water surface undergoing large deformations
and topological changes during transient simulations e.g. of a breaking wave hitting an off-
shore structure. To date, the most successful method for advecting the water surface in marine
applications is the Volume-of-Fluid (VOF) method. While VOF methods have become quite
advanced and accurate on structured meshes, there is still room for improvement when it comes
to unstructured meshes of the type needed to simulate flows in and around complex geometric
structures. We have recently developed a new geometric VOF algorithm called isoAdvector for
general meshes and implemented it in the OpenFOAM interfacial flow solver called interFoam.
We have previously shown the advantages of isoAdvector for simple pure advection test cases
on various mesh types. Here we test the effect of replacing the existing interface advection
method in interFoam, based on MULES limited interface compression, with the new isoAd-
vector method. Our test case is a steady 2D stream function wave propagating in a periodic
domain. Based on a series of simulations with different numerical settings, we conclude that the
introduction of isoAdvector has a significant effect on wave propagation with interFoam. There
are several criteria of success: Preservation of water volume, of interface sharpness and shape,
of crest kinematics and celerity, not to mention computational efficiency. We demonstrate how
isoAdvector can improve on many of these parameters, but also that the success depends on the
solver setup. Thus, we cautiously conclude that isoAdvector is a viable alternative to MULES
when set up correctly, especially when interface sharpness, interface smoothness and calcula-
tion times are important. There is, however, still potential for improvement in the coupling of
isoAdvector with interFoam’s PISO based pressure-velocity solution algorithm.
1

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
1 INTRODUCTION
Computational Fluid Dynamics (CFD) is quickly gaining popularity as a tool for testing and
optimising marine structural designs and interaction with the surrounding water environment.
A concrete example is the assessment of extreme wave loads on offshore wind turbine founda-
tions of various types and shapes. From a numerical perspective, one of the great challenges
within marine CFD is accurate description and advection of a complex free surface, or air-water
interface. Various solution strategies have been developed to cope with this challenge[1]. The
most widely used within practical interfacial CFD is the Volume-of-Fluid (VOF) method. In
VOF, the interface is indirectly represented by a numerical field describing the volume fraction
of water within each computational cell. The game of VOF is then about “guessing” how much
water is floating across the faces between adjacent cells within a time step. VOF methods come
in two variants: 1) geometric VOF methods, using geometric operations to reconstruct the fluid
interface inside a cell and to approximate the water fluxes across faces, and 2) algebraic VOF
methods, relying on the limiter concept to blend first and higher order schemes in order to
retain sharpness and boundedness of the time advanced VOF field. Geometric VOF schemes are
typically much more accurate, but also computationally more expensive, complex to implement,
and restricted to certain types of computational meshes, such as hexahedral meshes. Algebraic
VOF schemes, on the other hand, are less accurate, but often faster, easier to implement, and
developed for general mesh types[2].
In marine applications, we often encounter complex geometries that are impossible, or at
least very difficult, to represent properly with a structured mesh. Hence, most free surface CFD
within marine engineering is based on algebraic VOF methods. Therefore, such simulations
often require excessive mesh resolution and therefore long calculation times to obtain the desired
solution quality.
To address the need for an improved computational interface advection method, we have
developed a new VOF approach called IsoAdvector[3]. It is geometric of nature both in the
interface reconstruction and advection step, but is applicable on general meshes consisting of
arbitrary polyhedral cells. In the interface reconstruction, we take a novel approach using
isosurface calculations to find the interface position and orientation in the intersected cells. In
the advection step, we rely on calculation of the face-interface intersection line sweeping a mesh
face during a time step. This avoids expensive calculations of intersections between cells and
flux polyhedra[4]. For a thorough description of the isoAdvector concept the reader is referred
to [3].
We have previously demonstrated using pure advection test cases that our new approach
leads to accurate interface advection on both structured and unstructured meshes without com-
promising calculation times[3]. In OpenFOAM’s interfacial flow solver, interFoam, each time
step starts by a MULES based update of the interface, followed by an update of the pressure
and velocity, using a variant of the PISO algorithm[2]. In this segregated solution approach
we can simply remove the MULES code snippet and replace it by a corresponding isoAdvector
based snippet. To complete the replacement of MULES with isoAdvector, we must also calculate
the mass flux across the faces – the quantity called rhoPhi in the interFoam code – based on
isoAdvector, since this is needed in the convection term for the velocity field in construction and
solution of the discretised momentum equations. In [5], we show how to derive a simple expres-
2

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
sion for rhoPhi from the mass fluxes provided by isoAdvector. The resulting solver is called
interFlow and is provided as open source together with the isoAdvector library and various test
cases at github.com/isoadvector.
In the following, we investigate the ability of interFlow and interFoam to propagate a stream
function wave for 10 wave periods across a computational domain, which is exactly one wave
length long and has periodic boundary conditions on the sides.
Figure 1: The initial wave shape. The defining wave parameters are the water depth: D = 20
m, wave height: H = 10 m, wave period: T = 14 s and mass transport velocity: ¯u2= 0 m/s.
Some derived quantities are the wave length: L = 193.23 m, steepness: H/L = 0.052, celerity:
c = 13.80 m/s, crest height: hcrest = 7.25 m, crest particle speed: ucrest = 5.95 m/s, trough
height: htrough = -2.75 m, trough particle speed: utroug h = -2.25 m/s.
2 PHYSICAL SETUP
A stream function wave is a periodic steady wave calculated from potential flow theory using
a truncated Fourier expansion of the surface and stream function describing the wave. The
Fourier coefficients are calculated using a numerical root finding method in parameter space
and by growing the wave height in steps so the solution procedure can be seeded with an Airy
wave. For details on the solution procedure the reader is referred to [6]. Here we adopt the
wave used in [7] and shown in Fig. 1, which also gives the wave parameters in the caption. The
advantage of using stream function wave theory as opposed to Stokes N’th order theory for the
input wave is that the former does not rely on the smallness of the wave amplitude, which is
the Taylor expansion parameter of Stokes wave theory.
One thing to keep in mind, when attempting to reproduce potential theory waves in CFD is
that these waves are calculated under the assumption of a free surface, i.e. zero pressure and
no air phase on top of the water surface. In our simulation we have a second phase above the
water and we are free to set the densities of the two phases. The water density will be set to
1000 kg/m3. Ideally, we would like to set the air density to zero for our stream function test
case, but numerical stability issues limit how low we can set the air density. We choose an air
density of 1 kg/m3, which is close to the real physical value. This is a good compromise, on one
hand high enough to limit high density ratio related instabilities at the interface, and on the
other hand low enough to make the air behaving like a “slave fluid” moving passively out of the
way in response to motion of the much heavier water surface.
The viscosities in both phases is set to zero in accordance with potential flow theory and we
have deactivated the turbulence model. This amounts to running the solver in “Euler equation
3

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
mode”, albeit the numerics will to some extend introduce an effective dissipation leading to a
lack of strict energy conservation.
For waves on the space and time scales considered here surface tension is irrelevant and we
set it to zero in our simulations.
3 NUMERICAL SETUP
The interFoam and interFlow solvers used in this study are based on the OpenFOAM-v1612+
version provided by ESI-OpenCFD. The details of the PISO algorithm implementation are
described in [2] and can be studied by inspecting the OpenFOAM code library, which is freely
available at openfoam.com.
For all simulations in the following the sides have periodic boundary conditions for both the
VOF-field, α, the velocity field, U, and the pressure, p. On the top and bottom we have zero
normal gradient for αand p, and a slip boundary condition for U.
The mesh type with square cells and two refinement zones covering the interface region is
show in Fig. 1. This is the finest mesh used in this study with 20 cells per wave height and
384 cells per wavelength in the interface region. Two coarser meshes with square cells were also
used: One with the finest refinement removed, yielding 10 cells per wave height, and a very
coarse mesh with no refinement at all and only 5 cells per wave height.
In all simulations we use adaptive time stepping based on a maximum allowed CFL number.
We show results with CFL = 0.1, 0.2 and 0.4. It should be noted that in water wave simulations
with interFoam the velocities in the air phase above the water surface are often higher than
the maximum velocities in the water volume. The air behaviour depends a lot on the choices
of numerical schemes and settings, but for our density ratio of 1:1000, it is not uncommon to
see air velocities that are 2-3 times higher than the velocity of the water particles in the wave
crests. Thus, in a simulation with a maximum allowed CLF number of 0.1 the actual maximum
CFL number in the water volume may in fact stay below 0.05. It might be fruitful to introduce
in the time stepping algorithm a separate CFL limit for each of the two phases.
Besides mesh and time resolution, the accuracy of wave propagation simulations depends
on the choices of schemes for the different terms in the momentum equations. In particular
the results are sensitive to the choice of time integration scheme. Therefore, in what follows,
we show results for both pure Euler time integration and a 50% mixture of Euler and Crank-
Nicolson. Another influential scheme is the momentum convection scheme. The convective term
is linearized and treated implicitly, so we use the face mass fluxes from a previous time step or
iteration to advect the updated velocity field through the face. For the cell-to-face interpolation
involved in the discretisation of the convective term we use a TVD method specialised for vector
fields, called limitedLinearV in OpenFOAM terminology. This scheme requires specification of
a coefficient in the range ψ∈[0,1], where 0 gives best accuracy and 1 gives best convergence[8].
In the following we use ψ= 1.
All discretisation schemes and solver settings used in the presented simulations are listed in
Appendix A and B to allow the reader to verify our results.
4

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
4 RESULTS
In the subsequent two sections we first vary the spatial resolution and then the CFL num-
ber to investigate its effect on the wave propagation properties of interFlow (isoAdvector) and
interFoam (MULES).
IsoAdvector
Euler
MULES
Crank–Nicolson 0.5
1
Figure 2: Surface elevation after 10 wave periods with CFL = 0.1. For convenience of plotting
the horizontal axis has been compressed by a factor of 10. Black: Exact, Green: H/dx = 5,
Blue: H/dx = 10, Red: H/dx = 20. Top panels: Euler time discretisation. Bottom panels: 50%
blended Crank-Nicolson and Euler time integration. Left panels: interFlow/IsoAdvector. Right
panels: interFoam/MULES.
4.1 Mesh refinement study
To investigate the effect of spatial resolution we simulate for L/dx = 5, 10 and 20 the prop-
agation of the wave through the periodic domain for 10 wave periods (140 s) and plot the final
surface curve compared to the exact theoretical solution. The results are shown in Fig. 2. We
observe that:
•In terms of surface shape preservation the best performance is obtained with isoAdvector
on the finest mesh where MULES gives a wiggly surface.
•In spite of the wiggly surface MULES is superior in terms celerity on the finest mesh with
5

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
almost no visible phase shift.
•Using isoAdvector on the coarsest mesh leads to excessive decay in wave height.
•On the intermediate mesh isoAdvector also has excessive wave height decay with Euler
but not with Crank-Nicolson.
•MULES with Euler looks surprisingly good on the coarsest mesh. Inspection of the time
series reveals that this is a “lucky” snapshot right after the wave has broken due to excessive
steepening. In general it can not be recommended to use meshes with only 5 cells per wave
height with the numerical setup used here.
In Table 1 we show the time it took for the simulation of the 10 periods to finish on a single
core for the different combinations of schemes and resolutions. IsoAdvector is significantly faster
than MULES for all combinations except for the H/dx = 10 with Euler. For the best settings,
H/dx=20 and Crank-Nicolson, isoAdvector is 32% faster than MULES and slightly faster than
the MULES-Euler combination.
H/dx isoAdvector MULES
5 314 335
10 1892 1228
20 4356 5741
(a) Euler
H/dx isoAdvector MULES
5 304 435
10 918 1669
20 5624 8151
(b) Crank-Nicolson 0.5
Table 1: Simulation times in seconds on a single core for 10 periods.
4.2 Time refinement study
As shown in [3], isoAdvector is accurate in pure advection test cases for CFL number up
to 0.5. It is our experience that isoAdvector works well for such cases even for CFL numbers
closer to (albeit not exceeding) 1. In [3] we also demonstrate how MULES requires CFL <0.1
to converge. We would therefore hope that replacing MULES with isoAdvector in interFoam
could allow more accurate solutions with larger time steps. In Fig. 3 we show the results of an
exercise where we keep the mesh resolution fixed at H/dx = 20 and vary the CFL time step
limit from 0.1 to 0.2 and on to 0.4. We observe that:
•IsoAdvector with Euler gives excessive wave damping for CFL = 0.2 and 0.4.
•IsoAdvector with Crank-Nicolson 0.5 gives slightly worse but acceptable results with CFL
= 0.2 with an increase in phase error and overprediction of wave height.
•IsoAdevctor with Crank-Nicolson and CFL = 0.4 causes severe wave breaking.
•MULES with Euler and CFL = 0.4 crashes before the simulation has finished.
•In spite of its wiggly surface MULES with CFL = 0.2 is very close to the CFL = 0.1 result
only differing by a small phase error.
6

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
IsoAdvector
Euler
MULES
Crank–Nicolson 0.5
1
Figure 3: Surface elevation after 10 wave periods. For convenience of plotting the horizontal
axis has been compressed by a factor of 10. Black: Exact, Green: CFL = 0.4, Blue: CFL =
0.2, Red: CFL = 0.1. Top panels: Euler time discretisation. Bottom panels: 50% blended
Crank-Nicolson and Euler time integration. Left panels: interFlow/IsoAdvector. Right panels:
interFoam/MULES.
This is somewhat disappointing for our hopes that isoAdvector would allow accurate simu-
lations with large time steps. It should be noted, that the current coupling of isoAdvector with
the pressure-velocity coupling is the simplest possible. Probably one should look for an improve-
ment in this coupling rather than for an improvement in the inner workings of the isoAdvector
method itself.
4.3 Crest velocity profiles
An important feature to be able to capture accurately in wave propagation simulations is
the particle kinematics in the wave crest. As for instance shown in [9], many solvers have issues
with overshooting in the particle velocities in the top of the crest. To investigate this, we show
in Fig. 4 the variation in the x-component of the velocity along a line of cells going up through
the wave crest. The results are shown for the simulations with H/dx = 20 and CFL = 0.1 at
time t = 70 s, i.e. after 5 wave periods. It is evident from this figure that with the current
implementation of isoAdvector into interFoam we get higher overshoots in the crest velocities
than the original interFoam solver with MULES which does a remarkably good job with the
7

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
IsoAdvector
Euler
MULES
Crank–Nicolson 0.5
1
Figure 4: Horizontal velocity in cell centres at wave crest after 5 wave periods of the simulation
with H/dx = 20 and CFL = 0.1. Red: Exact, Green: Simulation result. The α-field is shown
in a black-white colour map and the α= 0.001, 0.5 and 0.999 contours are plotted in blue. Top
panels: Euler time discretisation. Bottom panels: 50% blended Crank-Nicolson and Euler time
integration. Left panels: interFlow/IsoAdvector. Right panels: interFoam/MULES.
Crank-Nicolson 0.5 time integration. Since the surface is advected passively in the velocity field,
one should think that there was a strong correlation between a solver’s ability to represent these
velocities accurately near the surface and its ability to accurately propagate the surface and
preserve its shape. This does not seem to be the case here where isoAdvector, in spite of its
errors in crest kinematics, produces a better surface, and MULES, in spite of its accurate crest
kinematics, produces a wrinkled surface.
In Fig. 4, we show the interface width by plotting the α= 0.001, 0.5 and 0.999 contours in blue
colour. Careful inspection reveals that the distance between the 0.001 and 0.999 contours with
isoAdvector is 3 which is essentially the theoretical minimal interface width for a VOF method.
The corresponding distance with MULES is approximately twice as large, i.e. approximately 6
cells. This moves the stagnation point, where the air velocity above the crest changes direction,
8

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
one cell closer to the surface. In a true two-phase potential flow solution the tangential jump in
velocity should be right on the interface. In this sense the isoAdvector solution is closer to the
theoretical one.
4.4 Cell aspect ratio
It has previously been shown that the cell aspect ratio can have a significant effect on the
propagation of waves in OpenFOAM and on the breaking point of shoaling waves[10]. Clearly,
independence of simulation results on cell aspect ratios and cell shapes in general are highly
desirable features. To investigate how isoAdvector behaves with different cell aspect ratios we
have repeated the simulations on a mesh with flat cells (H/dx = 10 and H/dy = 20) and on a
mesh with tall cells (H/dx = 20 and H/dy = 10) in the interface region. The results are shown
in Fig. 5 where they are compared to the finest resolution results shown previously. We see that
the halving of the cell count in the interface region has only a small effect on the isoAdvector
simulation results. For MULES the surface wrinkles are exacerbated when using tall cells. For
flat cells the wrinkles completely disappear and a slight phase error is introduced.
IsoAdvector
Crank–Nicolson 0.5
MULES
1
Figure 5: Surface elevation after 10 wave periods. For convenience of plotting the horizontal
axis has been compressed by a factor of 10. Black: Exact. Red: square cells, H/dx = H/dy =
20. Blue: Flat cells, H/dx = 10, H/dy = 20. Green: Tall cells, H/dx = 20, H/dy = 10. Top
panels: Euler time discretisation. Bottom panels: 50% blended Crank-Nicolson and Euler time
integration. Left panels: interFlow/IsoAdvector. Right panels: interFoam/MULES.
5 CONCLUSION
We have demonstrated the feasibility of using the new geometric VOF algorithm, isoAdvector,
in the OpenFOAM interfacial flow solver, interFoam, to propagate a steady stream function wave
through a periodic domain. The benefits of using interFlow (interFoam with isoAdvector) as
opposed to MULES is a sharper and more smooth surface, shorter calculation times and less
sensitivity to cell aspect ratio. It is not recommended to use the solver with Euler integration
and fewer than 10 cells per wave height. Satisfactory results are obtained with a 50:50 blend of
Euler and Crank-Nicolson and 20 cells per wave height.
9

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
In spite of problems with a wrinkly surface the original interFoam solver with MULES per-
forms better than interFlow when it comes to phase error (celerity) on the finest mesh and
reproduction of the theoretical crest kinematics profile. Also, at this stage interFlow does not
produce satisfactory results when running with CFL number >0.2 as one might otherwise hope
due to its ability to advect interfaces accurately at CFL numbers close to 1. We expect that
higher accuracy at larger CFL numbers can be obtained by improving the way isoAdvector is
coupled with the PISO loop in the interFoam solver.
Finally a word of caution regarding this kind of numerical comparisons. Choosing schemes
and solver settings is a delicate procedure which requires some degree of informed guessing. It
may well be that one combination of schemes produces accurate results for a particular test
case because the energy that, say, the chosen time integration scheme erroneously injects into
the system is by pure luck equal to the energy erroneously taken out of the system due to the
coarseness of the mesh. Results may then look reasonable even though the numerical calculation
does not in reality represent the simulated physics properly. A professional CFD engineer should
always stress test her setup with an attitude of trying to prove it wrong, rather than trying to
prove it right.
Acknowledgements
This work was funded by JR’s Sapere Aude: DFF-Research Talent grant from The Danish
Council for Independent Research |Technology and Production Sciences (Grant DFF-1337-
00118) and by DHI’s GTS grant from the Danish Agency for Science, Technology and Innovation.
A Solver settings
PIMPLE isoAdvector
{ {
momentumPredictor yes; interfaceMethod isoAdvector;
nCorrectors 3; isoFaceTol 1e-8;
nOuterCorrectors 1; surfCellTol 1e-8;
nNonOrthogonalCorrectors 0; snapAlpha 1e-12;
nAlphaCorr 1; nAlphaBounds 3;
nAlphaSubCycles 1; clip true;
cAlpha 1; }
pRefPoint (1 0 16);
pRefValue 0;
}
"alpha.water.*" p_rgh
{ {
nAlphaCorr 2; solver GAMG;
nAlphaSubCycles 1; tolerance 1e-8;
cAlpha 1; relTol 0.01;
smoother DIC;
10

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
MULESCorr no; nPreSweeps 0;
nLimiterIter 3; nPostSweeps 2;
nFinestSweeps 2;
solver smoothSolver; cacheAgglomeration true;
smoother symGaussSeidel; nCellsInCoarsestLevel 10;
tolerance 1e-8; agglomerator faceAreaPair;
relTol 0; mergeLevels 1;
} }
pcorr p_rghFinal
{ {
solver PCG; solver PCG;
preconditioner preconditioner
{ {
preconditioner GAMG; preconditioner GAMG;
tolerance 1e-5; tolerance 1e-8;
relTol 0; relTol 0;
smoother DICGaussSeidel; nVcycles 2;
nPreSweeps 0; smoother DICGaussSeidel;
nPostSweeps 2; nPreSweeps 2;
nFinestSweeps 2; nPostSweeps 2;
cacheAgglomeration false; nFinestSweeps 2;
nCellsInCoarsestLevel 10; cacheAgglomeration true;
agglomerator faceAreaPair; nCellsInCoarsestLevel 10;
mergeLevels 1; agglomerator faceAreaPair;
} mergeLevels 1;
tolerance 1e-06; }
relTol 0;
maxIter 100; tolerance 1e-9;
} relTol 0;
maxIter 20;
}
U UFinal
{ {
solver smoothSolver; solver smoothSolver;
smoother GaussSeidel; smoother GaussSeidel;
tolerance 1e-7; tolerance 1e-8;
relTol 0.05; relTol 0;
nSweeps 2; nSweeps 2;
} }
B Discretisation schemes
ddtSchemes{default CrankNicolson 0.5;} //Euler
11

Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
gradSchemes{default Gauss linear;}
divSchemes
{
div(rhoPhi,U) Gauss limitedLinearV 1;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes{default Gauss linear corrected;}
interpolationSchemes{default linear;}
snGradSchemes{default corrected;}
REFERENCES
[1] G. Tryggvason, R. Scardovelli, and S. Zaleski, Direct numerical simulations of gas–liquid
multiphase flows. Cambridge University Press, 2011.
[2] S. S. Deshpande, L. Anumolu, and M. F. Trujillo, “Evaluating the performance of the two-
phase flow solver interFoam,” Computational Science & Discovery, vol. 5, no. 1, p. 014016,
2012.
[3] J. Roenby, H. Bredmose, and H. Jasak, “A computational method for sharp interface ad-
vection,” Royal Society Open Science, vol. 3, no. 11, p. 160405, 2016.
[4] J. Hern´andez, J. L´opez, P. G´omez, C. Zanzi, and F. Faura, “A new volume of fluid method
in three dimensions-part I: Multidimensional advection method with face-matched flux
polyhedra,” International Journal for Numerical Methods in Fluids, vol. 58, no. 8, pp. 897–
921, 2008.
[5] J. Roenby, H. Bredmose, and H. Jasak, “Isoadvector: Vof on general meshes,” in 11th Open-
FOAM Workshop (J. M. N´obrega and H. Jasak, eds.), Springer Nature, 2017. submitted.
[6] John D. Fenton, “Numerical methods for nonliner waves,” in Advances in Coastal and Ocean
Engineering, vol. 5, pp. 241–324, World Scientific, July 1999.
[7] B. T. Paulsen, H. Bredmose, H. Bingham, and N. Jacobsen, “Forcing of a bottom-mounted
circular cylinder by steep regular water waves at finite depth,” Journal of Fluid Mechanics,
vol. 755, pp. 1–34, Sept. 2014.
[8] C. J. Greenshields, “Openfoam user guide,” OpenFOAM Foundation Ltd, version, vol. 3,
no. 1, 2015.
[9] P. A. Wroniszewski, J. C. G. Verschaeve, and G. K. Pedersen, “Benchmarking of Navier-
Stokes codes for free surface simulations by means of a solitary wave,” Coastal Engineering,
vol. 91, pp. 1–17, Sept. 2014.
[10] N. G. Jacobsen, D. R. Fuhrman, and J. Fredsøe, “A wave generation toolbox for the open-
source CFD library: OpenFoam,” International Journal for Numerical Methods in Fluids,
vol. 70, no. 9, pp. 1073–1088, 2012.
12