Conference PaperPDF Available

A new volume-of-fluid method in OpenFOAM


Abstract and Figures

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.
Content may be subject to copyright.
VII International Conference on Computational Methods in Marine Engineering
M. Visonneau, P. Queutey and D. Le Touz´e (Eds)
Johan Roenby, Bjarke Eltard Larsen?, Henrik BredmoseAND Hrvoje
DHI, Agern All 5, 2970 Hørsholm, Denmark, e-mail:
?DTU Mechanical Engineering, Richard Petersens Plads, 2800 Kgs. Lyngby, Denmark, e-mail:
DTU Wind Energy, Technical University of Denmark, Nils Koppels Alle, 2800 Lyngby,
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.
Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
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-
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
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.
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
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.
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
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.
Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
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).
Crank–Nicolson 0.5
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
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.
Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
Crank–Nicolson 0.5
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:
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
Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
Crank–Nicolson 0.5
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,
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.
Crank–Nicolson 0.5
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.
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.
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.
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;
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
Johan Roenby, Bjarke Eltard Larsen, Henrik Bredmose and Hrvoje Jasak
gradSchemes{default Gauss linear;}
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;}
[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,
[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.
... Wroniszewski et al. (2014) compared the performance of several codes including interFoam in a test case with a progressive solitary wave and highlighted that interFoam over-predicts the velocity at the wave crest relative to the analytical solution. The same problem was also highlighted by Roenby et al. (2017), Amini Afshar (2010), Tomaselli (2016) and Larsen et al. (2019). Amini Afshar (2010) and Larsen et al. (2019) noted a second problem in interFoam, which is generation of wiggles in the interface between air and water. ...
... The improved interface reconstruction is however expected to improve the free surface advection and thereby also improve the overall performance of the DSD solvers. interIsoFoam has been used to propagate a stream function wave by Roenby et al. (2017Roenby et al. ( , 2018 and Larsen et al. (2019). The studies showed that isoAdvector improved the prediction of the surface elevation and eliminated the wiggly interface observed with interFoam. ...
... However, the velocity prediction by interIsoFoam has severe over-and underprediction, which is much larger than with interFoam. Roenby et al. (2017) used a fine resolution of 20 cells per wave height to get acceptable results, where significant errors could still be observed in both the surface elevation and velocity profile. Vukčević et al. (2017) showed that the continuous density field creates an imbalance in the momentum equation, which causes spurious velocities in absence of surface tension. ...
Full-text available
The solution procedure for two phases in OpenFOAM suffers from unphysical velocity oscillations at the free surface between the two phases. It is likely that this problem also exists in other two-phase Computational Fluid Dynamics (CFD) codes. We aim to solve this by imposing boundary conditions directly on the free surface. We have taken the first step towards a new two-phase solution method by first addressing the water phase alone. It is a free surface modelling method based on merging concepts from two existing methods: (1) A single-phase free surface method and (2) the solution method used in OpenFOAM. The underlying motivation is to enable more accurate estimation of wave induced load distributions from wave crest impacts on offshore structures. This first and foremost requires an accurate prediction of the kinematics near the free surface. We present a solution method with boundary conditions directly on the free surface, thereby the name: Direct Surface Description (DSD). Additionally it is the first time that the isoAdvector algorithm is combined with a single phase free surface method. The implementation is made in OpenFOAM, but may also relevant to other codes as well. First a still water level simulation is presented to illustrate the unphysical behavior of the existing solvers and validate the behaviour of the DSD method. The second test case is a moderately steep stream function wave in intermediate water depth. The DSD method is validated and compared to the existing solution methods of OpenFOAM: interFoam and interIsoFoam. We present a detailed comparison of surface elevations and velocity profiles. This is followed by a convergence study including wave height, velocity and phase shift. Additionally the influence of the Courant–Friedrichs–Lewy (CFL) number is studied. The stream function wave case demonstrates that the DSD method accurately predicts the free surface elevation and velocity fields without free surface undulations or oscillatory velocity fields. The convergence study underlines an increased accuracy of the DSD method. Finally, a 2D and a 3D showcase with breaking waves are presented to show that the DSD method is capable of simulating more complex and realistic cases.
... 29 The geometric VoF technique approximates the phase fraction fluxes over the cell surfaces and reconstructs the fluid interface within a cell using geometric operations. 30 By comparing the solution to the algebraic and geometric VoF as benchmarks for droplet deformation 31 and Taylor cone jets, 32 the enhancement of the interface resolution was demonstrated for our case. ...
... In our model, the WHM was just implemented in the electric properties, but in further investigations, the implementation on the hydrodynamic properties could also be tested. 21 Moreover, the simulation is considered laminar, and the interface reconstruction scheme is the plicRDF, 30 an improved geometric reconstruction method named isoAdvector algorithm is implemented using the OpenFOAM. Furthermore, the coupling of the pressure and velocity field is made with the PIMPLE algorithm, providing a very robust pressure-velocity coupling. ...
Full-text available
Electrohydrodynamic (EHD) jets are a highly promising technology for the generation of three-dimensional micro- and nanoscale structures, but the advancement of this technology is hindered by the insufficient understanding of many aspects of its flow mechanisms, such as the whipping behavior under larger electric potentials. A fully coupled numerical simulation of the three-dimensional electrohydrodynamic jet flow is used here since non-symmetric effects govern most of their EHD regimes. By applying considerable electric capillary numbers (CaE>0.25), we capture radial instabilities that until now no other numerical simulation was able to present. A comparison against previous two-dimensional axis-symmetric and validation with experimental studies of the Taylor cone jet is initially done. An exciting gain in accuracy was obtained, having an error of around 1.101% on the morphology against experimental results. Moreover, our numerical model takes into consideration the contact angle between the surface of the nozzle and the liquid, which is shown to be a very important variable for improved accuracy in the morphologic shape of the Taylor cone. Moreover, the three-dimensional structures and flow dynamics, under different electric capillary numbers, and their connection to the instabilities of the jet are studied. We present a novel visualization of the formation of droplet generation with the receded Taylor cone and the whipping dynamics.
... This is possible by coupling isoAdvector with interFoam's pressurevelocity solution algorithm. Roenby et al., (2017) mentioned that this is more advantageous than MULES and yields better results. ...
Conference Paper
The concept of oscillating water column (OWC) integrating with coastal structures is popular in marine engineering to extract energy from the ocean. The objective of the study is to numerically examine the newly proposed three different fixed oscillating water columns with a forward duct at the bottom of OWC named Forward Duct OWC (FD-OWC), a curved wall at the front side of OWC with a radius equal to the height of OWC called as Curved Front Lip Wall OWC (CFLW-OWC), and hybridization of the curved and vertical wall at the front portion of OWC named as Curved Vertical Front Lip Wall (CVFLW-OWC). This paper used a three-dimensional numerical model to investigate the hydrodynamic performance of three OWC devices under regular waves for constant wave steepness. The numerical model is based on the open-source computational fluid dynamics package OpenFOAM. The numerical results are validated with the available experimental results. The influence of the wave amplification factor, wave power absorption coefficient, the air pressure inside the three OWC chambers, hydrodynamic efficiency, and dynamic water pressure inside and outside the three OWC chambers are evaluated. The results show that the CVFLW-OWC exhibits better hydrodynamic efficiency.
... A first order, implicit, transient time scheme was specified for the temporal discretisation terms. The inherently stable nature of this discretisation scheme together with the small value of C max guarantees stability of the solution and improves accuracy of the results (Larsen et al., 2019;Roenby et al., 2016Roenby et al., , 2017. Additional details of the model verification procedure has previously been documented in Mayon et al. (2021). ...
Ocean wave energy is a rapidly developing sector and has the potential to contribute a significant share to the global green energy transformation. However, nearshore coastal regions, in which energy harvesting devices are most commonly installed, experience low wave energy densities compared with offshore regions. This is a significant impediment to the commercialisation of the wave energy sector. This study proposes a low cost solution to these low wave energy density distributions at nearshore environments whilst simultaneously providing an effective coastal protection system. A parabolic energy concentrator wall is coupled with an oscillating water column wave energy converter. The parabolic concentrator reflects and consolidates the incident wave energy to a focal point, at which the wave energy convertor is positioned. Experimental investigations, supported by numerical modelling results confirm energy conversion performances significantly exceeding hitherto recorded wave energy converter efficiencies, with wave-to-wire conversion efficiency in the laboratory model exceeding 70%. Furthermore, the parabolic concentrator wall has an ancillary purpose to act as a shoreline protection barrier. The simplicity of design, high energy conversion efficiencies, and inherent shoreline defensive aspect of the proposed system deems it particularly suitable for deployment to remote island nations, or coastal communities vulnerable to coastal erosion that presently rely on fossil fuel consumption for energy generation.
... 11,14 Interface reconstruction was performed geometrically using the isoAdvector concept. 15,16 Energy and species equations were solved separately for the two phases to estimate the phase change terms better. 17 The coupling of the energy jump condition and thermodynamic pseudo-equilibrium at the liquid-vapor interface was not implicitly resolved for simplicity. ...
Full-text available
Thermally induced secondary atomization (TISA) is a complex phenomenon that accelerates phase change in the combustion chamber. It occurs if multi-component fuels, having a wide boiling range, are exposed to high temperatures. Several airlines are recently experimenting with bio- and fossil fuels blends. However, the characteristics of droplet TISA are primarily unknown because of the challenges associated with experimental activities like suspended or falling droplets. In this scenario, numerical models become essential to study TISA. That is why a new multi-component, multi-phase volume of fluid computational fluid dynamics solver was developed to simulate droplets TISA. The solver takes advantage of the OpenFOAM framework and uses the isoAdvector methodology. The bio- and fossil fuels were represented by n-heptane and n-hexadecane, respectively, to simplify the problem. Evaporation was implemented by assuming that the mixture could only boil at that temperature. Surface tension and other relevant mixture properties were considered as a function of species concentration and temperature to replicate all phenomena comprehensively. An analysis of bubble expansion based on the Rayleigh–Plesset equation preceded the breakup tests. The test cases consisted of a droplet suspended in microgravity having a bubble initialized at the interface. The bubble eventually expanded, and the bubble cap collapsed, leading to the micro-explosion. A parametric study of breakup cases under different pressures and at a fixed temperature of 1200 K was performed. The atomization mechanism was tested at 1, 3, 10, and 20 bar and compared. It was observed that while high pressure slows down the process, it finally leads to a higher surface area. This behavior was confirmed by testing two different bubble sizes. Together with the atomization intensity, also the morphology of the particles changed. At atmospheric pressure, the maximum surface area was reached when the droplet had a disk-like shape, while at higher pressures, it evolved in an elongated shape.
... The "compressibleInterFoam" solver was applied to simulate the flow phenomena. The solver is appropriate for two compressible, non-isothermal, immiscible fluids and uses a VOF (Volume of Fluid) phase-fraction based on the interface capturing approach, Hirt and Nichols, 1981;Roenby et al., 2017. In VOF, phase fraction is determined as 1 in elements with solely one phase (e.g., water) and as 0 in elements with the second phase (e.g., air). ...
Full-text available
Removal of the accumulated liquid from jumpers of subsea gas production systems is essential to avoid possible hydrate creation and further damage to the pipeline. However, the displacement of high amounts of accumulated liquid during the production start-up leads to a gas pressure rise. Liquid plugs formed during the liquid displacement impact the structure's elbows. This in addition to cyclic pressure/forces fluctuations, may lead to harmful flow-induced vibrations (FIV). These flow phenomena that may endanger the jumper structure were explored in air-water experiments performed in a lab-scale jumper. The critical (minimal) gas velocity needed to purge the accumulated liquid was determined and the pressure and forces variations during the liquid removal were measured. In addition, the effects of the gas velocity, initial liquid amount, and gas flow ramp-up on the air-water flow phenomena were documented. Results of 3D and 2D numerical simulations (using OpenFOAM) were verified against the experimental data. The effects of employing different RANS turbulence models on the predictions were tested and demonstrated. A simple mechanistic model was established to predict the pressure and force variation during liquid displacement. The model enables inspecting the variation with the operational conditions of each pressure component (i.e., hydrostatic, friction, and acceleration) and examining their significance and contribution to the pressure rise.
... (2) the algorithm should be as stable as possible when the interface is unstable [35]. The interFOAM solver based on the VOF method is used to solve the interface of water-gas two-phase flow in OpenFOAM [36]. The interFOAM solver is based on incompressible, adiabatic, insoluble, non-mixing (mixing refers to the distribution of one fluid in another fluid, such as the movement of bubbles in liquid) two-phase interface capture to solve. ...
Full-text available
The problem of aircraft entering and exiting water is a complex, nonlinear, strongly disturbed, and multi-coupled multiphase flow problem, which involves the precise capture of the air/water interface and the multi-coupling interaction between aircraft, water, and air. Moreover, due to the large difference in medium properties during the crossing, the load on the body will suddenly change. In this paper, the VOF (volume of fluid) algorithm is used to capture the liquid surface at the air/water interface, and since body movement is involved in this process, the overset grid technology is used to avoid the traditional dynamic grid deformation problem. In the process of this numerical simulation prediction, the effects of different water-entry angles and different water-entry heights on the body load and attitude of the trans-medium aircraft, as well as the cavitation evolution law of the body water entry are analyzed. On this basis, to simulate the authenticity and complexity of the water-entry environment, numerical wave-making technology was introduced to analyze the water-entry load, posture, and cavitation evolution law of the body under different wave environments. The numerical parameters under the condition of wave and no wave are compared, and the difference in water-entry performance under the condition of wave and no wave is analyzed.
... during the simulations. Such a low number has been shown to increase the accuracy of such simulations using interFOAM (Roenby et al., 2017;Larsen et al., 2019). ...
Full-text available
The performance of a recently developed “stabilized” turbulence (k−ω) closure model, which avoids un-physical over-production of turbulence prior to wave breaking, is investigated in the computational fluid dynamics (CFD) simulation of cross-shore sediment transport and breaker bar morphology. Comparisons are made with experiments as well as results from simulations employing (otherwise identical) “standard” turbulence closure. The stabilized turbulence model is demonstrated to result in major (qualitative and quantitative) improvements of the predicted breaker bar position and height. Conversely, the established over-production of turbulence in the standard closure, coupled with associated inaccurate undertow structure in the outer surf zone, contribute to erroneous offshore migration of the breaker bar. By correcting these shortcomings, the stabilized turbulence closure model rightly predicts initial onshore morphological migration of the breaker bar without any calibration. This work thus establishes proper turbulence modeling as a prerequisite for accurate CFD prediction of cross-shore sediment transport and profile morphology.
This Ph.D. project was initially born from the motivation to contribute to the depth-averaged and 3D modeling of lava flows. Still, we can frame the work done in a broader and more generalist vision as we developed two models that may be used for generic viscous fluids, and we applied efficient numerical schemes for both cases, as explained in the following. The new solvers simulate free-surface viscous fluids whose temperature changes are due to radiative, convective, and conductive heat exchanges. A temperature-dependent viscoplastic model is used for the final application to lava flows. Both the models behind the solvers were derived from mass, momentum, and energy conservation laws. Still, one was obtained by following the depth-averaged model approach and the other by the 3D model approach. The numerical schemes adopted in both our models belong to the family of finite volume methods, based on the integral form of the conservation laws. This choice of methods family is fundamental because it allows the creation and propagation of discontinuities in the solutions and enforces the conservation properties of the equations. We propose a depth-averaged model for a viscous fluid in an incompressible and laminar regime with an additional transport equation for a scalar quantity varying horizontally and a variable density that depends on such transported quantity. Viscosity and non-constant vertical profiles for the velocity and the transported quantity are assumed, overtaking the classic shallow-water formulation. The classic formulation bases on several assumptions, such as the fact that the vertical pressure distribution is hydrostatic, that the vertical component of the velocity can be neglected, and that the horizontal velocity field can be considered constant with depth because the classic formulation accounts for non-viscous fluids. When the vertical shear is essential, the last assumption is too restrictive, so it must relax, producing a modified momentum equation in which a coefficient, known as the Boussinesq factor, appears in the advective term. The spatial discretization method we employed is a modified version of the central-upwind scheme introduced by Kurganov and Petrova in 2007 for the classical shallow water equations. This method is based on a semi-discretization of the computational domain, is stable, and, being a high-order method, has a low numerical diffusion. For the temporal discretization, we used an implicit-explicit Runge-Kutta technique discussed by Russo in 2005 that permits an implicit treatment of the stiff terms. The whole scheme is proved to preserve the positivity of flow thickness and the stationary steady-states. Several numerical experiments validate the proposed method, show the incidence on the numerical solutions of shape coefficients introduced in the model and present the effects of the viscosity-related parameters on the final emplacement of a lava flow. Our 3D model describes the dynamics of two incompressible, viscous, and immiscible fluids, possibly belonging to different phases. Being interested in the final application of lava flows, we also have an equation for energy that models the thermal exchanges between the fluid and the environment. We implemented this model in OpenFOAM, which employs a segregated strategy and the Finite Volume Methods to solve the equations. The Volume of Fluid (VoF) technique introduced by Hirt and Nichols in 1981 is used to deal with the multiphase dynamics (based on the Interphase Capturing strategy), and hence a new transport equation for the volume fraction of one phase is added. The challenging effort of maintaining an accurate description of the interphase between fluids is solved by using the Multidimensional Universal Limiter for Explicit Solution (MULES) method (described by Marquez Damian in 2013) that implements the Flux-Corrected Transport (FCT) technique introduced by Boris and Book in 1973, proposing a mix of high and low order schemes. The choice of the framework to use for any new numerical code is crucial. Our contribution consists of creating a new solver called interThermalRadConvFoam in the OpenFOAM framework by modifying the already existing solver interFoam (described by Deshpande et al. in 2012). Finally, we compared the results of our simulations with some benchmarks to evaluate the performances of our model.
Thermally-induced secondary atomization (TISA) enables enhanced atomization, better mixing and faster evaporation in multi-component sprays. Despite its importance in a number of applications, TISA is not yet well understood. In this work we study numerically the effects of key physical parameters on TISA dynamics, with particular emphasis on breakup. To this end, we simulated a series of cases for suspended droplets in microgravity conditions, varying the number of bubbles near the liquid-gas interface. We performed a total of 800 simulations with different fluid properties investigating a wide hyperspace. In particular, we varied viscosity, surface tension, number and size of bubbles, as well as the droplet size, identifying two main parameters necessary for modelling purposes: the breakup time, τb, and maximum normalized surface area, Sf. Here we defined the breakup time as the time between the beginning of the simulation and the maximum surface area observed. We also calculated the Pearson’s coefficient to estimate the influence of each variable on the parameters of interest, understanding that the size of the largest bubble controlled Sf while the Ohnesorge number strongly influenced τb. We further employed the dataset to formulate simple mathematical correlations for Sf and τb by performing a multi-variable regression. Moreover, we looked into the dynamics of the secondary droplets generated by the process, demonstrating that the velocity and size of the ejected droplets are linked to the size of the bubbles that generate them.
Full-text available
In a recent publication [1], we presented a novel geometric VOF algorithm , denoted isoAdvector. The OpenFOAM implementation of the method was publicly released[2] to allow more accurate and efficient multiphase flow simulations in OpenFOAM. In the present paper, we give a brief outline of the isoAd-vector method and test it with two pure advection cases. We show how to modify interFoam to use isoAdvector instead of the currently implemented MULES limited interface compression method. The properties of the new solver are tested with two simple interfacial flow cases, namely the damBreak case and a steady stream function wave. We find that the new solver is superior at keeping the interface sharp, but also that the sharper interface exacerbates the well-known spurious velocities in the air phase close to an air-water interface. To fully benefit from the accuracy of isoAdvector, there is a need to modify the pressure-velocity coupling algorithm of interFoam, so it more consistently takes into account the jump in fluid density at the interface. In our future research we aim at solving this problem by exploiting the sub cell information provided by isoAdvector.
Full-text available
We devise a numerical method for passive advection of a surface, such as the interface between two incompressible fluids, across a computational mesh. The method is called isoAdvector, and is developed for general meshes consisting of arbitrary polyhedral cells. The algorithm is based on the volume of fluid (VOF) idea of calculating the volume of one of the fluids transported across the mesh faces during a time step. The novelty of the isoAdvector concept consists in two parts: First, we exploit an isosurface concept for modelling the interface inside cells in a geometric surface reconstruction step. Second, from the reconstructed surface, we model the motion of the face-interface intersection line for a general polygonal face to obtain the time evolution within a time step of the submerged face area. Integrating this submerged area over the time step leads to an accurate estimate for the total volume of fluid transported across the face. The method was tested on simple 2D and 3D interface advection problems both on structured and unstructured meshes. The results are very satisfactory both in terms of volume conservation, boundedness, surface sharpness, and efficiency. The isoAdvector method was implemented as an OpenFOAM(R) extension and is published as open source.
Full-text available
The performance of the open source multiphase flow solver, interFoam, is evaluated in this work. The solver is based on a modified volume of fluid (VoF) approach, which incorporates an interfacial compression flux term to mitigate the effects of numerical smearing of the interface. It forms a part of the C + + libraries and utilities of OpenFOAM and is gaining popularity in the multiphase flow research community. However, to the best of our knowledge, the evaluation of this solver is confined to the validation tests of specific interest to the users of the code and the extent of its applicability to a wide range of multiphase flow situations remains to be explored. In this work, we have performed a thorough investigation of the solver performance using a variety of verification and validation test cases, which include (i) verification tests for pure advection (kinematics), (ii) dynamics in the high Weber number limit and (iii) dynamics of surface tension-dominated flows. With respect to (i), the kinematics tests show that the performance of interFoam is generally comparable with the recent algebraic VoF algorithms; however, it is noticeably worse than the geometric reconstruction schemes. For (ii), the simulations of inertia-dominated flows with large density ratios yielded excellent agreement with analytical and experimental results. In regime (iii), where surface tension is important, consistency of pressure–surface tension formulation and accuracy of curvature are important, as established by Francois et al (2006 J. Comput. Phys. 213 141–73). Several verification tests were performed along these lines and the main findings are: (a) the algorithm of interFoam ensures a consistent formulation of pressure and surface tension; (b) the curvatures computed by the solver converge to a value slightly (10%) different from the analytical value and a scope for improvement exists in this respect. To reduce the disruptive effects of spurious currents, we followed the analysis of Galusinski and Vigneaux (2008 J. Comput. Phys. 227 6140–64) and arrived at the following criterion for stable capillary simulations for interFoam: where . Finally, some capillary flows relevant to atomization were simulated, resulting in good agreement with the results from the literature.
Forcing by steep regular water waves on a vertical circular cylinder at finite depth was investigated numerically by solving the two-phase incompressible Navier-Stokes equations. Consistently with potential flow theory, boundary layer effects were neglected at the sea bed and at the cylinder surface, but the strong nonlinear motion of the free surface was included. The numerical model was verified and validated by grid convergence and by comparison to relevant experimental measurements. First-order convergence towards an analytical solution was demonstrated and an excellent agreement with the experimental data was found. Time-domain computations of the normalized inline force history on the cylinder were analysed as a function of dimensionless wave height, water depth and wavelength. Here the dependence on depth was weak, while an increase in wavelength or wave height both lead to the formation of secondary load cycles. Special attention was paid to this secondary load cycle and the flow features that cause it. By visual observation and a simplified analytical model it was shown that the secondary load cycle was caused by the strong nonlinear motion of the free surface which drives a return flow at the back of the cylinder following the passage of the wave crest. The numerical computations were further analysed in the frequency domain. For a representative example, the secondary load cycle was found to be associated with frequencies above the fifth and sixth-harmonic force component. For the third-harmonic force, a good agreement with the perturbation theories of Faltinsen, Newman & Vinje (J. Fluid Mech., vol. 289, 1995, pp. 179-198) and Malenica & Molin (J. Fluid Mech., vol. 302, 1995, pp. 203-229) was found. It was shown that the third-harmonic forces were estimated well by a Morison force formulation in deep water but start to deviate at decreasing depth.
The paper presents a benchmark of four freely available solvers for Navier–Stokes equations: Gerris, OpenFOAM, Thétis and Truchas. These models are selected because they have been reported to deal successfully with oceanographic and coastal engineering applications. The benchmark includes two free surface problems: propagation of a solitary wave and runup of a solitary wave on a plane beach. The fluids are inviscid, which allows a detailed study of energy conservation and comparison of the results with a reference solution given by a boundary integral solver. The Navier–Stokes solvers use the finite volume discretization and free surface capturing techniques based on the volume-of-fluid (VOF) method. In the first benchmark test, we investigate the influence of numerical dissipation and other spurious effects on the energy balance of the wave. In the second problem, we focus on the runup heights and compare them with the reference solution. The beach in the runup problem is represented with a solid body immersed in the Cartesian mesh. The solid boundaries are described with a VOF type approach or a staircase representation, depending on the features of the solver. In addition to the immersed boundary description a couple of body fitted meshes are tested for the runup case.
This Chapter gives a survey of numerical methods for solving fully-nonlinear problems of wave propagation in coastal and ocean engineering. While low-order theory may give insight, for accurate answers fully-nonlinear methods are becoming the norm. Such methods are often simpler than traditional methods, partly because the full equations are simpler than some of the approximations which are widely used. A lengthy description of the Fourier approximation method is given, which is the standard numerical method used to solve accurately the problem of steadily-propagating waves. This may be used to provide an approximate solution for waves in rather more general situations, or, as is often the case, to give initial conditions for methods which go on to simulate the propagation of waves over more general topography. The family of such propagation methods is then described, including Lagrangian methods, marker-and-cell methods, finite difference methods — including some exciting recent developments, boundary integral equation methods, spectral methods, Green-Naghdi Theory, and local polynomial approximation. Finally a review is given of methods for analysing laboratory and field data and extracting wave information.
Accurately predicting the behaviour of multiphase flows is a problem of immense industrial and scientific interest. Modern computers can now study the dynamics in great detail and these simulations yield unprecedented insight. This book provides a comprehensive introduction to direct numerical simulations of multiphase flows for researchers and graduate students. After a brief overview of the context and history the authors review the governing equations. A particular emphasis is placed on the ‘one-fluid’ formulation where a single set of equations is used to describe the entire flow field and interface terms are included as singularity distributions. Several applications are discussed, showing how direct numerical simulations have helped researchers advance both our understanding and our ability to make predictions. The final chapter gives an overview of recent studies of flows with relatively complex physics, such as mass transfer and chemical reactions, solidification and boiling, and includes extensive references to current work.
The open-source CFD library OpenFoam® contains a method for solving free surface Newtonian flows using the Reynolds averaged Navier–Stokes equations coupled with a volume of fluid method. In this paper, it is demonstrated how this has been extended with a generic wave generation and absorption method termed ‘wave relaxation zones’, on which a detailed account is given. The ability to use OpenFoam for the modelling of waves is demonstrated using two benchmark test cases, which show the ability to model wave propagation and wave breaking. Furthermore, the reflection coefficient from outlet relaxation zones is considered for a range of parameters. The toolbox is implemented in C++, and the flexibility in deriving new relaxation methods and implementing new wave theories along with other shapes of the relaxation zone is outlined. Subsequent to the publication of this paper, the toolbox has been made freely available through the OpenFoam-Extend Community. Copyright © 2011 John Wiley & Sons, Ltd.
A multidimensional advection scheme in 3D based on the use of face-matched flux polyhedra to integrate the volume fraction evolution equation is proposed. The algorithm tends to reduce the formation of ‘over/undershoots’ by alleviating the over/underlapping of flux polyhedra, thus diminishing the need to use local redistribution algorithms. The accuracy and efficiency of the proposed advection algorithm, which are analyzed using different tests with prescribed velocity field, compare well with other multidimensional advection methods proposed recently. The algorithm is also applied, in combination with a Navier–Stokes solver, to reproduce the impact of a water droplet falling through air on a pool of deep water. The interfacial curvature is calculated using a height-function technique with adaptive stencil adjustment, which provides improved accuracy in regions of low grid resolution. The comparison of the numerical results with experimental results shows a good degree of agreement. Copyright © 2008 John Wiley & Sons, Ltd.
Openfoam user guide OpenFOAM Foundation Ltd
  • C J Greenshields
C. J. Greenshields, " Openfoam user guide, " OpenFOAM Foundation Ltd, version, vol. 3, no. 1, 2015.