ChapterPDF Available

IsoAdvector: Geometric VOF on general meshes


Abstract and Figures

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.
Content may be subject to copyright.
IsoAdvector: Geometric VOF on general meshes
Johan Roenby, Henrik Bredmose and Hrvoje Jasak
Abstract In a recent publication [1], we presented a novel geometric VOF algo-
rithm, denoted isoAdvector. The OpenFOAM implementation of the method was
publicly released[2] to allow more accurate and efficient multiphase flow simula-
tions 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 func-
tion 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.
1 The interfacial flow equations
Let us start by writing the equations of motion governing the flow of two incom-
pressible, immiscible fluids. To keep things simple, we will ignore viscous effects
and surface tension. What remains are the passive advection equation,
Johan Roenby
DHI, Agern Alle 5, 2970 Horsholm, Denmark, e-mail:
Henrik Bredmose
DTU Wind Energy, Nils Koppels Alle, 2800 Kgs. Lyngby, Denmark e-mail:
Hrvoje Jasak, University of Zagreb, Faculty of Mechanical Engineering and Naval Architecture,
Ivana Lucica 5, Zagreb, Croatia, e-mail: (hrvoje,
2 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
∂ ρ
t+·(ρu) = 0,(1)
the incompressibility equation,
and the Euler equations,
∂ ρ u
t+·(ρuu) = p+ρg.(3)
Here ρis the fluid density field taking the constant value, ρ1, in the reference fluid
and the constant value ρ2in the other fluid, uis the velocity field, pis the fluid pres-
sure and gis the constant downward pointing gravity vector. In the interFoam solver
of OpenFOAM, these equations are discretized in the finite volume framework and
advanced in time in a segregated manner. Within a time step Eq. 1 is used to up-
date the density field in time, followed by a procedure for solving Eq. 2 and 3 to
update the pressure and velocity field in time. The details of the implementation is
well described in the paper [3]. This paper also gives an overview of the challenge
faced by the interfacial CFD community with keeping the density field sharp and
bounded, with spurious velocities at the interface and with handling of large density
ratios. The development of the isoAdvector interface advection method is a first step
in our efforts to solve these problems and increase the general performance and ac-
curacy of interfacial flow simulations. In the following we will briefly explain how
isoAdvector works.
2 isoAdvector for interface advection
The basic equation that we will solve, is Eq. 1 recast in the volume-of-fluid formu-
lation. We will let the computational domain be divided into cells, C1,C2,.... We
can then define the notation for the cell averaged value of a field, f(x,t), at time t,
where Viis the volume of cell i. Defining the indicator field
the volume fraction (of fluid 1) in cell iis then defined as
We will denote the mesh faces, F1,F2,..., and the list of labels of faces on the
boundary of cell iwill be denoted Bi. On the time axis the times, t1<t2< ... de-
IsoAdvector: Geometric VOF on general meshes 3
fine the time intervals (or steps), [tn,tn+1], over which the governing equations are
integrated. We will use superscripts to denote a function evaluated at one of these
times, fn=f(tn). With these definitions in place, we can now integrate Eq. 1 over
a cell volume and over a time interval. Using Gauss’ theorem, the following exact
equation governing the time evolution of the volume fraction in cell iis obtained,
i j,(7)
where the total volume of fluid 1 flowing from cell iduring the time interval [tn,tn+1]
into the neighbour cell with which it shares face jis
i j Ztn+1
H(x,τ)u(x,τ)·dSi jdτ.(8)
In this expression dSi j is the boundary element of face joriented so that it points out
of cell i, so if cell kis the other cell of face jthen dSk j =dSi j and Vn
k j =Vn
i j.
The art of constructing a volume of fluid algorithm is all about coming up with
the best possible approximation of Vn
i j given the incomplete available data, which
in our collocated finite volume framework consists of the volume fractions αn
i, the
cell averaged velocities, huin
i, and the volumetric face fluxes,
i j ZFj
u(x,tn)·dSi j.(9)
In the following we show how isoAdvector uses this data and a number of geometric
considerations to come up with an approximation for Vn
i j.
Fig. 1 Interpolation of volume fraction to a
vertex from all surrounding cells.
Fig. 2 Construction of the isoface inside a surface
4 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
2.1 Interface reconstruction
We start by noting that normally most cells will be fully immersed in either fluid
1 or fluid 2, and for such cells the advection problem is trivial, since there is only
one fluid fluxed through all faces during a time interval. The surface cells requiring
special treatment are those containing both fluid 1 and fluid 2. We will define a
surface cell as one with ε<αn
i<1ε, where we typically set ε=108in our
calculations. The first step in finding αn+1
ifor such cells is to reconstruct the fluid
interface inside the cell from the available data, αn
iat time tn. In the isoAdvector
method, this is done by calculating an isosurface inside the cell. For this purpose we
need to first interpolate the volume fractions from the cell centres to the vertices.
This process is illustrated in Fig.1. This interpolation can be done in various ways.
For convenience, we have chosen the inverse distance weighting provided by the
volPointInterpolation class.
With volume fractions interpolated to all vertices of cell i, we can choose an
isovalue, α0, and construct the α0-isosurface inside the cell. This we do by going
through all the cell’s edges and detect whether they are cut by the isosurface. An
edge is cut, if the interpolated volume fraction at one end is larger than α0and
the value at the other end is smaller than α0. If that is the case, we calculate the
edge-isosurface intersection point along the edge by linear interpolation. Connect-
ing these intersection points across the cell faces, we construct the cell-isosurface
intersection as illustrated in Fig. 2. The representation of this intersection will be
called an isoface, because it is really just an internal face cutting the cell into two
subcells. We can calculate the face centre, xS, and face unit normal vector, ˆ
nS, for
this isoface as for any other mesh face (black dot and vector in Fig. 2).
The choice of isovalue, α0, will clearly affect where the isoface will end up within
the cell and also its orientation. A general isovalue will not split the cell into two
subcells having volumes in accordance with the cell’s volume fraction, αn
i. But we
will exploit our freedom of choice of isovalue to make sure that this is actually the
case. We have implemented an efficient algorithm for finding the isovalue for the
isoface cutting a surface cell into subcells in accordance with αn
i. More details on
this can be found in [1]. This concludes our description of the interface reconstruc-
tion at time tn.
2.2 Interface advection
The next step is to exploit our new knowledge about the interface position inside
surface cells at time tnto estimate how much of the total fluid volume transported
across a face during a time step, [tn,tn+1]is fluid 1, and how much is fluid 2. We will
first make the assumption that u(x,τ)in Eq. 8 can be replaced by an appropriately
chosen constant vector ˜
j, which is representative for the velocity on the face during
the whole time interval. We also assume that we can write
IsoAdvector: Geometric VOF on general meshes 5
dSi j =ˆ
ni j(x)d A Si j
|Si j|d A,(10)
where ˆ
ni j is the (for a non-planar face spatially varying) unit normal vector and Si j
is the mean normal vector of face jpointing out of cell i. Then the volumetric face
flux can be defined as ˜
i j ˜
j·Si j and Vn
i j in Eq. 8 can be approximated by
i j
i j
In the current implementation, we simply use the volumetric face fluxes, φn
i j, at the
beginning of the time step for ˜
i j.1The remaining area integral in Eq. 11 is just the
time integral of the submerged area of face j,
If we want to be able to take time steps, where the interface moves a substantial
fraction of a cell size, we should come up with an estimate of how Ajvaries with
time within a time step. The topmost face of the polygonal prism cell in Fig. 2 is
reproduced in Fig. 3 with the initial face-interface intersection line at tnshown in
Fig. 3 Face-interface intersection line sweeping
the face.
Fig. 4 Submerged face are, Aj(τ), as a
piecewise quadratic polynomial.
To estimate how this line sweeps over the face as the isoface moves in the veloc-
ity field, we first interpolate the velocity field to the initial isoface centre, xs, shown
with a black dot in Fig. 2. We can then take the dot product of the interpolated ve-
locity with the isoface unit normal, ˆ
nS, to obtain the speed of the isoface motion
perpendicular to itself, US. For a vertex, xv, in Fig. 3, we can also estimate the per-
pendicular distance to the isoface by dv= (xvxS)·ˆ
nS. With the calculated isoface
1A future improvement could be to use φn1
i j in the backward time integration spirit to get an
estimate, φn+1
i j , for φn+1
i j , and then use ˜
i j =0.5(φn
i j +φn+1
i j )in Eq. 11. Similarly if the method is
used in a solver with outer correctors so we have an estimate of φn+1
i j from the previous iteration.
6 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
normal speed and vertex-to-isoface distance, we can then estimate the time of ar-
rival at vertex xvto be τv=dv/US. In this way we obtain the “vertex arrival times”,
τ1,τ2,... shown in Fig. 3. As illustrated, some of these will generally be outside the
integration interval, [tn,tn+1]and some will be inside. The crucial point is now that
between such two times, say τ2and τ3in Fig. 3, the face-interface intersection line
sweeps a quadrilateral. If we assume the line sweeps this quadrilateral steadily, we
can come up with an analytical expression for how Ajdepends on τon this sub time
interval. This expression is a quadratic polynomial in τand its coefficients depend
only on the shape of the quadrilateral. The resulting time variation of Aj(τ)as the
line sweeps the face is illustrated in Fig. 4
With a piecewise quadratic polynomial for Aj(τ)in Eq. 12, its time integral in
Eq. 11 is a piecewise cubic polynomial, and Vn
i j is finally obtained as the sum of the
contributions from these sub intervals. We note that a face of a surface cell may ini-
tially be fully immersed in fluid 1 or 2, and then become intersected during the time
interval [tn,tn+1]. With the calculated vertex arrival times this situation corresponds
to τ1>tn(the tnline in Fig. 4 would then be further to the left) and is treated by
making sure to flux pure fluid 1 or 2 through the face in the sub time interval [tn,τ1].
Similarly, if the interface leaves the face during [tn,tn+1], we will have τ5<tn+1for
a pentagonal face (the tn+1line would then be further to the right in Fig. 4), and we
must flux pure fluid 1 or 2 through the face during the last sub time interval [τ5,tn+1].
There is one final decision we must make before our advection routine is com-
plete: For a face j, both its owner and neighbour cell may be surface cells with their
isofaces not coinciding exactly on face jdue to the different isovalues used in the
two cells and not moving with exactly the same velocity due to the spatial variations
in the velocity field. Which cell should be used to calculate Vn
i j for this face? In our
current implementation, we have chosen to let Vn
i j be determined by the upwind
cell, i.e. the owner if φn
j>0 and the neighbour if φn
2.3 Bounding
The test cases provided with the released isoAdvector code [2] show that the method
outlined above generally gives very good estimates of Vn
i j and leads to accurate in-
terface advection as long as the interface is well resolved by the mesh and time step
size is limited to CFL <1. In some situations there may, however, arise small in-
accuracies, which can build up over time and lead to intolerable levels of unbound-
edness. To prevent the gradual build up of unboundedness, we have introduced a
bounding step which detects unboundedness and tries to adjust the Vn
i j’s of un-
bounded cells with a procedure that is described in detail in [1]. If this pure redistri-
bution step fails, the provided code also gives the option of brute-force non-volume
preserving chopping αn+1
iafter each advection step to guarantee boundedness. Acti-
vating this will ruin the machine precision volume conservation, but our experience
so far indicates that in many situations the resulting volume conservation error is
very small.
IsoAdvector: Geometric VOF on general meshes 7
In the current isoAdvector implementation we assume that there is only a single
isoface inside a cell. There are several occasions where one would expect more
isofaces inside a cell. On such situation is when a planar interface passes a non-
planar mesh face with which it is close to parallel. During the passage the face and
interface will intersect in more than two points and the face-interface intersection
cannot be represented by a single straight line. Proper treatment of such an event can
be implemented by on-the-fly decomposition of the non-planar face into triangular
subfaces sharing the face centre as their common apex. A face-interface intersection
line can then be calculated for each triangle separately2.
Another situation with more than one isoface inside a cell is when two separate
volumes of fluid approach each other and collide inside a cell. Then there will be a
time interval just before the collision where each volume has its own separate piece
of interface within the cell. In this event the solution is to decompose the whole
cell into tetrahedra sharing the cell centre as their common apex and separately
reconstruct the interface in each subcell.
We have experienced that due to these shortcomings of the current implemen-
tation the bounding errors can be substantial e.g. on polyhedral meshes with many
highly non-planar faces of the type obtained by generating the dual mesh of a ran-
dom tetrahedral mesh. The method still works on such meshes if switching on the
brute-force chopping described above but one may then experience substantial loss
of volume conservation. We plan to implement the fixes described above in a future
release of the code.
3 Pure advection tests
In this section we compare the performance of isoAdvector and MULES with two
standard test cases involving only advection in a pre-defined velocity field.
3.1 Notched disc in solid rotation flow
Our first test case is the notched disc which has become a standard test case since
its introduction in [4]. The domain is the unit square, the velocity field is the solid
body rotation around the point (0.5,0.5):
The initial volume fraction field is 1 within the disc of radius 0.15 centred at
(0.5,0.75)except in a slit of width 0.06 going up to y=0.85. The disc rotates around
(0.5,0.5)and return to its original position at time t = 1. The resulting interface
shape after such a rotation with isoAdvector and MULES is shown in Fig. 5 for
2We note that a triangular face can at most have two intersection points with the interface.
8 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
isoAdvector, CFL = 0.5
square cells
MULES, CFL = 0.5 MULES, CFL = 0.1
triangular cellspolygonal cells
Fig. 5 Notched disc advection test. Voluem fraction field shown after one full rotation. 0.5-contour
shown with a black curve.
three different mesh types with square, triangular and polygonal cells. All runs have
been performed with CFL = 0.1 and 0.5, but since the isoAdvector runs with CFL
= 0.1 and 0.5 are almost indistinguishable, we only show the latter. From the figure
and Tables 1 and 2, we remark that
IsoAdvector with CFL = 0.5 performs better than MULES with both CFL = 0.5
and 0.1 on square, triangular and polygonal meshes.
MULES performs bad on all mesh types with CFL = 0.5.
On square and polygonal meshes MULES improves dramatically when going
from CFL = 0.5 to 0.1, but not on the triangular mesh.
isoAdvector is 3 times faster than MULES with CFL = 0.5.
IsoAdvector: Geometric VOF on general meshes 9
Table 1 E1error for notched disc runs.
Mesh type isoAdvector CFL = 0.5 MULES CFL = 0.5 MULES CFL = 0.1
square 0.014 0.21 0.062
triangular 0.022 0.17 0.13
polygonal 0.022 0.14 0.064
Table 2 Calculation times in seconds for notched disc runs.
Mesh type isoAdvector CFL = 0.5 MULES CFL = 0.5 MULES CFL = 0.1
square 25 175 437
triangular 232 639 1929
polygonal 85 278 803
3.2 Sphere in shear flow
Our second pure advection case is from [5]. The domain is the unit box and the initial
volume fraction field is 1 within the sphere of radius 0.15 centred at (0.5,0.75,0.25)
and 0 elsewhere. The velocity field in which the interface is advected is
u(x,t) = cos2πt
where T=6 and r=p(x0.5)2+ (y0.5)2. In this flow the initial spherical
interface is sheared into a thin spiralling sheet until at t=1.5 it has reached its
maximum deformation and flows back to its initial shape and position at time t=3.
We run the case on a polyhedral mesh of the type generated with the polyMesh
tool of cfMesh [6]. In Fig. 6 we show the results obtained with isoAdevector and
MULES using CFL = 0.5 and 0.1.
Table 3 E1error (left) and calculation times (right) for sphere in 3D shear flow a polyhedral mesh.
CFL isoAdvector MULES
0.5 0.1 0.24
0.1 0.11 0.15
CFL isoAdvector MULES
0.5 146 s 439 s
0.1 513 s 1622 s
From Fig. 6 and Tables 3 we see that with this test case isoAdvector is still
more accurate and approximately three times faster than MULES, but also note that
MULES does a decent job even with CFL = 0.5. We also observe that the E1error
with isoAdvector actually increases slightly with smaller time steps.
10 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
CFL = 0.5
CFL = 0.1
Fig. 6 Sphere deformed in a 3D shear flow with isoAdvector and MULES for CFL = 0.5 and 0.1.
Initial sphere is shown in red. Interface shape at maximum deformation (t=1.5) and at the time
of return to spherical shape (t=3) shown in grey.
4 Using isoAdvector in interFoam
In interFoam, the MULES explicit solver code does not only provide the updated
volume fractions, αn+1
i. It also provides the quantity rhoPhi, which is used in the
convective term, fvm::div(rhoPhi, U), in the momentum matrix equation,
UEqn. To understand how we should construct rhoPhi from Vij , let us start by
looking at the convective term in the Euler equations in Eq. 3 formally integrated
over a small time interval and over a cell:
·[ρ(x,τ)u(x,τ)u(x,τ)]dV dτ+... (15)
We will denote this integrated convective term by Cn
iand use Gauss theorem to write
it as
We now approximate u(x,τ)with the constant representative velocity vector, ˜
use u·dS˜
i j/|Sj|d A as described in the beginning of Section 2. This allows us to
IsoAdvector: Geometric VOF on general meshes 11
i j
Now using the definition of H(x,t)in terms of ρ(x,t)in Eq. 5 and the definition of
the submerged face area, Aj, in terms of Hin Eq. 12, we can write Eq. 17 as
i j
[ρ2+ (ρ1ρ2)Aj(τ)]dτ.(18)
With the definition of Vn
i j in Eq. 8, we can finally write the convective term as
i jtn+ (ρ1ρ2)Vn
i j.(19)
Here the content of the square brackets is exactly the sought expression for rhoPhi.
The specific expression for ˜
ujin terms of the cell averaged velocities huin
iis deter-
mined by the settings in fvSchemes for the time integration and for the convective
5 The damBreak case
For an initial investigation of the behaviour of our new interFoam solver using
isoAdvector instead of MULES, we run a refined version of the standard dam break
tutorial shipped with OpenFOAM-4.0. The domain is a box of width and height
0.584 m with a small obstacle on the bottom and the water initially placed in a
square column in the left side of the domain. The case is run with adaptable time
steps using maxAlphaCo =maxCo = 0.5 . In Fig. 7, we show snapshots of the
volume fraction field at two times. In the top panels, where the water has just stum-
bled over the obstacle on the floor, we clearly see how isoAdvector – in contrast
to MULES – is capable of keeping the interface sharp even for droplets of only a
few cells width. In the bottom panels the water is starting to settle, and we see how
the interface produced with isoAdvector is only one cell wide, whereas the interface
produced with MULES covers many cells. Calculation times are similar for the two
This is to be thought of as a kind of “Hello World!” case for our new solver and
caution should be taken drawing quantitative conclusion from this setup. In future
work, we will make more quantitative investigations based e.g. on the experimental
data provided in [7].
We remark that a razor sharp interface is not always the best representation of
the physics water distribution on the given mesh. If the encounter with the obstacle
in a real physical damBreak experiment causes the interface to explode into a cloud
of sub cell sized droplets, then the smeared representation obtained with MULES
together with an appropriate dispersed flow model may be a better representation
12 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
Fig. 7 The damBreak case at times t=0.32 (top) and 1.1 (bottom) run with isoAdvector (left) and
MULES (right). Cells with 0.001 <αn
i<0.999 at t=1.1 are coloured yellow in the lower panels.
of the physical reality. To prevent unphysical sharpening of the interface in regions
with clouds of subcell droplets and bubbles, one could introduce a quantitative cri-
terion for detecting such regions and replace the isoAdvector interface treatment for
surface cells in these regions with a more appropriate dispersed model treatment.
6 Steady stream function wave
The purpose of our final test case is to investigae the effect it has on the propagation
of a steady stream function wave to change the interface advection method from
MULES to isoAdvector. The surface elevation, velocity pressure fields are found
IsoAdvector: Geometric VOF on general meshes 13
Fig. 8 Stream function wave with H = 10 m, D = 20 m and T = 14 s at time t = 10 s. From top:
MULES–Euler, MULES–Crank-Nicolson, isoAdvector–Euler, isoAdvector–Crank-Nicolson.
numerically using a Fourier approximation method which is well described in [8].
The derivation is based on potential flow theory with vacuum above the wave. This
corresponds to ρ2=0, which is not practically possible with the interFoam solver
because it involves division with ρ. We therefore use ρ2=0.1 kg/m3and ρ1=1000
kg/m3. As in [9], we use a wave with height H=10 m and period T=14 s on depth
D=20 m. This gives rise to a wave length of L=193.23 m which we choose as the
length of our rectangular domain with cyclic boundary conditions on the sides.
The cells in the interface region are squares of side length 0.5 m corresponding to 20
cells per wave height and 386 cells per wave length. Above and below the interface
region the mesh is coarser with cell size up to 2 m. For div(rho*phi,U) we use
Gauss limitedLinearV 1 as opposed to upwind used in [9]. Another differ-
ence is that in our setup we initialise the wave in a co-moving frame, and so the sur-
face elevation and velocity field should ideally not change throughout the transient
simulation. Also, we use a fixed time step of 0.002 s, which based on the theoretical
crest velocity of 5.95 m/s gives a CFL number of 0.0238. We run the setup with
MULES and isoAdvector using both Euler and crankNicolson 0.5 for time
14 Johan Roenby, Henrik Bredmose and Hrvoje Jasak
integration. The resulting wave shape and velocity magnitudes for the four combi-
nations a short time after the simulations have been started (t=10 s) are shown in
Fig. 8. The interface thickness is shown by plotting the 0.5 and 0.0001 contours of
the volume fraction field. We see that the interface is sharper and smoother in the
isoAdvector simulations than in the MULES simulations. But we also observe that
the velocities in a narrow air band just above the surface is almost twice as high in
the isoAdvector simulations (note the different colour scales in the different pan-
els). These larger air velocities do not seem to affected the interface significantly as
shown in Fig. 9, where we show the surface elevations from the four runs after 105
s corresponding to 7.5 wave periods.
Fig. 9 Stream function wave with H = 10 m, D = 20 m and T = 14 s at time 105 s. The x-axis has
been compressed by a factor 4. Black: exact elevation. Orange: MULES–Euler. Blue: MULES–
Crank-Nicolson. Red: isoAdvector–Euler. Green: isoAdvector–Crank-Nicolson.
All simulations have slightly too high celerity, causing all waves to be shifted
almost a quarter of a wave length to the right compared to the theoretical steady pro-
file crest centred in the middle of the domain. The MULES-Euler wave (orange) has
broken giving rise to a jerky profile. The MULES-Crank-Nicolson wave crest (blue)
has grown significantly and the trough is wrinkled. The isoAdvector waves with Eu-
ler (red) and Crank-Nicolson (green) also have slight overshoots in wave height but
much smaller and with much smoother profiles. This is a very preliminary test and
since many things can change if the case setup is adjusted one should not jump to
conclusions before a more thorough study has been conducted. It is, however, safe
to conclude that using isoAdvector instead of MULES in surface wave propagation
simulations does have a clear effect on the solution. It is also safe to conclude, that
the spurious tangential velocities observed at the interface for large density ratios
is not caused by MULES as such. More likely, the problem is caused by the PISO
loop implementation in interFoam not taking the large density jump properly into
account e.g. when interpolating density dependent quantities between cell centres
and face centres. We expect that an improved density jump treatment in this part of
the code can be achieved by using the information provided by isoAdvector about
the interface position inside surface cells.
IsoAdvector: Geometric VOF on general meshes 15
7 Summary
We have given a brief description of the isoAdvector algorithm for advection of a
sharp interface across general meshes. We added two pure advection cases to the
suite of test cases already presented in [1], demonstrating the superior behaviour
of isoAdvector compared to MULES with respect to accuracy and efficiency. We
derive an expression for the convective term in the momentum equation so that
isoAdvector can be used in interFoam instead of MULES. The resulting solver is
tested using the damBreak case and a steady stream function wave in a periodic do-
main. From these tests we conclude that using isoAdvector in interFoam is feasible
and leads to a sharper interface. Using isoAdvector for the tested wave propagation
case leads to significantly higher spurious tangential velocities in the lighter phase,
but nevertheless the solution quality is improved. In future work we will aim at ex-
ploiting the isoface data to impose consistent physical boundary conditions at the
interface in the PISO loop.
1. J. Roenby, H. Bredmose, and H. Jasak, “A computational method for sharp interface advection,
Royal Society Open Science, vol. 3, p. 160405, Nov. 2016.
2. Johan Roenby, “isoAdvector.”
3. 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.
GORITHMS FOR FLUIDS,” Journal of Computational Physics, vol. 31, no. 3, pp. 335–362,
5. J. L´
opez, C. Zanzi, P. G´
omez, F. Faura, and J. Hern´
andez, “A new volume of fluid method
in three dimensions–part II: Piecewise-planar interface reconstruction with cubic-b´
ezier fit,”
International Journal for Numerical Methods in Fluids, vol. 58, no. 8, pp. 923–944, 2008.
6. “cfMesh.” Accessed: 2016-12-09.
7. L. Lobovsk, E. Botia-Vera, F. Castellana, J. Mas-Soler, and A. Souto-Iglesias, “Experimental
investigation of dynamic pressure loads during dam break,Journal of Fluids and Structures,
vol. 48, pp. 407–434, July 2014.
in Coastal and Ocean Engineering, vol. 5 of Advances in Coastal and Ocean Engineering,
pp. 241–324, WORLD SCIENTIFIC, July 1999.
9. 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.
... was used to perform simulations of a fully three dimensional model. In this context, a numerical 305 method based in the Volume-of-fluid (VOF) approach was used, called IsoAdvector(Roenby et al., 2016(Roenby et al., , 2019. This method solves just one momentum equation, even though two fluids are present, as show in equation 18. ...
... then, it models how the face-interface intersection line moves to find out how the face area within a determined fluid changes during a time step(Roenby et al., 2016(Roenby et al., , 2019. O-H mesh grid used in the CFD simulations. ...
An one-dimensional model is developed for liquid-liquid flows considering a stratified flow where droplet entrainment is present. Two models from literature were used as a starting point: one that is well suited for stratified wavy flows and another that adds entrainment effects. In the development, an important intermediate step is introduced to correct wetted perimeters and interface position, which is particularly important when one of the phases has a high viscosity. The entrainment factors and rates are evaluated to assess their relevance for the typical flow case studied. Experimental data are gathered for comparison and validation purposes, and to act as closure information to the model. The predictions of the model are also compared against CFD simulations using a VOF based approach. The results are promising and suggest that the 1D model can be better suited for some applications, leading to great accuracy at a much lower processing cost than the CFD method applied.
... In the resolved SDF-CFD-DEM, the volume of fluid (VOF) method is employed to model multiphase fluids and the interface between two phases [54]. For DEM, the SDF-based DEM [50] recently proposed by the authors is adopted. ...
Full-text available
It is challenging to model granular particles with arbitrary shapes and related complications to fluid-particle interactions for granular flows which are widely encountered in nature and engineering. This paper presents an improved framework of the immersed boundary method (IBM)-based fully resolved computational fluid dynamics (CFD) and discrete element method (DEM), with an emphasis on irregular-shaped particles and the implications to particle-fluid interactions. The improved CFD-DEM framework is featured by two novel enhancements with signed distance field (SDF). First, an SDF-based formulation is employed to enable handling of granular particles with arbitrary shapes in DEM robustly and efficiently. Second, the IBM is modified to be consistent with SDF to fully resolve fluid-particle interactions in the presence of non-spherical particles. Such treatments leverage SDF as a generic interface to furnish a new SDF-CFD-DEM framework for universal modeling of arbitrarily shaped particles interacting with multiphase fluids with desired resolutions. Exemplified particle shape models include super-quadrics, spherical harmonics, polyhedron and level set, and new shape models can be flexibly developed by implementing the unified SDF-based shape interface. The proposed SDF-CFD-DEM is validated and showcased with examples including particle settling, drafting-kissing-tumbling, immersed granular collapse, and mudflow. The results demonstrate the good accuracy and robustness of the SDF-CFD-DEM and its potential for efficient computational modeling of multiphase granular flows involving granular particles with arbitrary shapes.
... This solver is based on the Volume Of Fluid solver interFoam with the advantage of a geometric interface reconstruction and sharp interface advection between two incompressible fluids known as IsoAdvector. 32 In the context of capillary flows with the introduction of wettability and consequent high interface curvatures in the vicinity of the wall, it is of great importance to keep curvature calculations precise with a low advection error to guarantee bounding of the scalar fields. The multiphase field is represented by an indicator function a, where a ¼ 0 is equivalent to the continuous phase and a ¼ 1 describes the disperse phase. ...
Full-text available
The objective of this research paper is to relate the influence of dynamic wetting in a liquid/liquid/solid system to the breakup of emulsion droplets in capillaries. Therefore, modeling and simulation of liquid/liquid flow through a capillary constriction have been performed with varying dynamic contact angles from highly hydrophilic to highly hydrophobic. Advanced advection schemes with geometric interface reconstruction (isoAdvector) are incorporated for high interface advection accuracy. A sharp surface tension force model is used to reduce spurious currents originating from the numerical treatment and geometric reconstruction of the surface curvature at the interface. Stress singularities from the boundary condition at the three-phase contact line are removed by applying a Navier-slip boundary condition. The simulation results illustrate the strong dependency of the wettability and the contact line and interface deformation.
... The volumetric source term S α accounts for the phase change between both phases. Based on iso-Advector, a method for geometric interface capturing and advection developed by Roenby et al. [28,29] and extended by Scheufler et al. [30], a piecewise linear interface reconstruction algorithm (PLIC) in combination with a reconstructed distance function (RDF) is used to reconstruct and advect the sharp interface between both fluid phases. ...
Full-text available
Surface structuring using nano-second lasers can be used to enhance certain properties of a material or even to introduce new ones. One way to create these structures efficiently is direct laser interference patterning using different polarization vector orientations of the interfering beams. However, experimentally measuring the fabrication process of these structures is very challenging due to small length and time scales. Therefore, a numerical model is developed and presented for resolving the physical effects during formation the predicting the resolidified surface structures. This three-dimensional, compressible computational fluid dynamics model considers the gas, liquid, and solid material phase and includes various physical effects, such as heating due to the laser beam for both parallel and radial polarization vector orientations, melting, solidification, and evaporation, Marangoni convection, and volumetric expansion. The numerical results reveal a very good qualitatively and quantitatively agreement with experimental reference data. Resolidified surface structures match both in overall shape as well as crater diameter and height, respectively. Furthermore, this model gives valuable insight on different quantities during the formation of these surface structures, such as velocity and temperature. In future, this model can be used to predict surface structures based on various process input parameters.
... The isoAdvection is a geometric VOF method; it can work on both structured and unstructured meshes; and there are no requirements for cell shapes. Different studies have been done by the isoAdvection method [42][43][44][45][46][47], showing that this method reduce the spurious flows close to the interface. ...
Full-text available
A benchmark study is conducted using isoAdvection as the interface description method. In different studies for the simulation of the thermal phase change of nanofluids, the Volume of Fluid (VOF) method is a contemporary standard to locate the interface position. One of the main drawbacks of VOF is the smearing of the interface, leading to the generation of spurious flows. To solve this problem, the VOF method can be supplemented with a recently introduced geometric method called isoAdvection. We study four benchmark cases that show how isoAdvection affects the simulation results and expose its relative strengths and weaknesses in different scenarios. Comparisons are made with VOF employing the Multidimensional Universal Limiter for Explicit Solution (MULES) limiter and analytical data and experimental correlations. The impact of nanoparticles on the base fluid are considered using empirical equations from the literature. The benchmark cases are 1D and 2D boiling and condensation problems. Their results show that isoAdvection (with isoAlpha reconstruct scheme) delivers a faster solution than MULES while maintaining nearly the same accuracy and convergence rate in the majority of thermal phase change scenarios.
... The gradient and divergence terms in the equations were discretized using second-order schemes. The sharp interface between oil and water was obtained using a geometric VOF algorithm, IsoAdvector (Roenby et al., 2016;Roenby et al., 2019). The discretization of the time derivative term was performed using a bounded, first-order implicit scheme that avoids the divergence and instability of the solver. ...
Experiments were performed to understand the impact of the orifice on droplet size in the shear breakup region. Oil jet was released vertically from two orifice types: a pipe and a converging nozzle. The roll-up vortices were observed clearly near the edge of the jet with nozzle orifice while elongated oil ligaments in the jet direction were mostly observed near the edge of the jet with pipe orifice. The size of the droplets shed from the near field shear layer increased along the jet direction for both orifice types. At different distances from the orifice, the characteristic shed droplet size (d50) was up to 40% larger with pipe orifice. Multiphase, large-eddy simulations (LES) with two orifice types were conducted to interpret the droplet size distribution (DSD) observed in the experiments. A thicker boundary layer that was initially formed inside the pipe dominated the near field of the jet with the pipe. The turbulent kinetic energy dissipation rate was higher with pipe orifice and the peak values of energy dissipation rate were found closer to the jet centerline with the pipe where oil holdup is larger. The viscous shear stress with the nozzle was higher than that of the pipe orifice within the initial two diameters from the orifice and slightly lower or higher at the following distances studied. The Reynolds shear stress was significantly larger with the nozzle at different distances from the orifice. The tangential vorticity within one diameter from the orifice was also dramatically higher with the nozzle. The key parameter in the shed droplet size of a liquid jet in liquid was found to be the shear layer thickness at the orifice, similar to prior works of a liquid jet in gas. A thicker shear layer at the pipe orifice induced a larger droplet size. The increase in the instabilities and shear layer thickness in the jet direction increased the droplet size in the jet direction.
Full-text available
The distribution of the gas-liquid interface is crucial to accurate calculation of the flow and heat transfer of in-orbit cryogenic propellants, for which the surface tension force overtakes the gravitational force. As an essential oxidant, liquid oxygen has a lower surface tension coefficient and viscosity than most room-temperature fluids, causing a greater possibility of interface instability and breakage. Conventional numerical methods have seldom been assessed in terms of cryogenic two-phase flows under microgravity, and commercial software cannot provide a consistent platform for the assessment. In this study, a unified code based on OpenFOAM has been developed for evaluating four interface-capturing methods for two-phase flows, namely, the algebraic volume of fluid (VoF), geometric VoF, coupled level set and VoF (CLSVoF), and density-scaled CLSVoF with a balanced force (CLSVoF-DSB) methods. The results indicate that the CLSVoF-DSB method is most accurate in predicting the interface motion, because it uses the level set function to represent the gas and liquid phases. The gas-liquid interface predicted by the CLSVoF-DSB method is the most stable because it adopts the scaling Heaviside function to weaken the effects of spurious currents and increases the stability. The numerical algorithm of the algebraic VoF method is the most simple, so it has the highest efficiency. And the geometric VoF uses the isoface to locate the gas-liquid interface in a grid cell, so it can obtain the thinnest interface. In applications of liquid oxygen, the CLSVoF-DSB method should be used if the overall accuracy is required.
Multiphase flows are ubiquitous in nature and industry. In order to fully describe multiphase systems, simulation approaches must be able to handle the interfaces separating the different phases properly. The Volume of Fluid (VOF) approach is widely used by researchers and engineers due to its intrinsic ability to conserve volume and handle large interface topology changes. A common problem that occurs in VOF Methods relates to the calculation of interfacial tension forces in the momentum equations while resolving a sharp interface. Common methods based on the gradients of the volume fraction field may lack accuracy due to the curvature and normal vector estimates through an abrupt transition. To address these points, the present work introduces a new proposal, where the VOF method based on a cloud of points for interface curvatures computation (PC-VOF) is extended by the coupling with the sharp-interface advection algorithm isoAdvector, implemented in the open source suite OpenFOAM®. The coupled method performs better than the ones implemented in the original solvers in a number of benchmark cases from the literature. It is shown to significantly reduce the spurious currents and also presents more stable and accurate results, especially for irregular triangular meshes.
Bubble geometric shape and hydrodynamic behavior affect directly mass, momentum and heat transfer at the interfacial area in the bubbly flow regime. A numerical model is developed to calculate instantaneous bubble interfacial area based on the VOF method. After data fitting, a new correlation is developed to associate the normalized bubble interfacial area with Eötvös and Galilei numbers. Considering the variation in liquid viscosity and surface tension of different gas–liquid systems, the influence of interface sharpening schemes on bubble hydrodynamics is illustrated comprehensively. With a moving reference frame, long-term bubble behavior is investigated in the air–water system and the temporal evolution of bubble hydrodynamics is analyzed in detail. Simulation results are validated by experimental data in terms of bubble rising velocity, aspect ratio and bubble deformation factor. The results indicated that the interface sharpening scheme affects the calculation of bubble interfacial area significantly. Both liquid viscosity and surface tension contribute to the formation of a stable terminal bubble interface. In the given range, the evolution of terminal interfacial area is found to agree well with the predicted correlation. Regarding long-term bubble behavior, three stages for instantaneous rising velocity and bubble interfacial area are observed, which are the damped oscillatory stage, the transition stage and the quasi-stable stage. Bubble deflection direction may be opposite to internal gas jet direction due to vortex shedding. In general, the numerical models applied in this study are proven to be feasible for bubble interfacial area calculation.
Full-text available
A novel test consisting on fast air injection into a vertical water column was experimentally and numerically studied. Measurements were focused on capturing the air-water interface as well as the volume of water evicted by the air, for a wide range of air flow rates. The numerical simulations, were performed with the Eulerian Two-Fluid (TF) and the Volume of Fluid (VOF) methods.For the TF method three topologies were considered: bubbly flow, dropUNR Universidad Nacional de Rosario flow, and blending. The last is a more smart methodology to automatically handle with the different flow regimes. For the VOF method, the standar VOF (SVOF), the Adaptive Mesh Refinement (AMR), and the high order Piecewise Linear Interface Calculation (PLIC) methods were assessed. SVOF and TF blending methods were choice to study the mesh convergence and turbulence modeling. Two-dimensional (2D) meshes of 2, 1 and 0.5 mm, and three-dimensional (3D) meshes of 2, 1 and 0.75 mm were considered. In all cases the standard VOF (SVOF) formulation showed mesh convergence and good agreement with experiments. The error for the finest 3D mesh was around 1%, but increased up to 20% for the finest 2D mesh. On the other hand, for the TF method mesh convergence was only evidenced for the 2D meshes. Regard the TF method, the bubbly and drop topology cases led to unacceptable solutions both in terms of inteface capturing as well as liquid evicted. On the other hand, the blending methodology clearly improved the estimations, although the interface was only partially captured because of the numerical diffusion. On the other hand, all the VOF methods were in relative good agreement both in terms of the liquid evicted as well as interface capturing. Errors were were reduced by refining the mesh. The initial swelling, with small bubbles and large slugs around the air injector was well captured, and the ligaments and drops spilled for high air flow rates were quite well estimated. The SVOF method showed low computational cost for coarse grids, but the computing time increased more than linearly with the mesh size. The AMR method showed accurate solutions, but the computing cost was largely increased with the refining level. Finally, the use of PLIC method for the coarser mesh reduced the error from 15% (SVOF) to 3.5% keeping low the computing cost.
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 objective of this research work has been to conduct experimental measurements on a dam break flow over a horizontal dry bed in order to provide a detailed insight, with emphasis on the pressure loads, into the dynamics of the dam break wave impacting a vertical wall downstream the dam. The experimental setup is described in detail, comprising state of the art miniaturized pressure sensors, high sampling rate data acquisition systems and high frame-rate video camera. It is a 1:2 scale of the highly cited (Lee et al., 2002, Journal of Fluids Engineering, 124) article experimental apparatus. Kinematics has been analyzed focusing on the free surface and wave front evolution. Experimental observations regarding liquid height and wave front speed have found to be in agreement with existing literature. This agreement enables the authors, assuming a similar framework, to discuss the measured pressure loads as a consequence of the dam break wave front impacting on the downstream wall. These loads show a substantial variability which has been statistically characterized. The measured quantities have been compared with the scarce available data in the literature, whose consistency is discussed. Measurements have been conducted with two filling heights. Scaling effects for such heights are also analyzed. As a direct result of the present initiative, an extensive set of data for computational tools validation is provided as Supplementary Materials, including pressure signals, wave height measurements and experimental videos.
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.
A new interface reconstruction method in 3D is presented. The method involves a conservative level-contour reconstruction coupled to a cubic-Bézier interpolation. The use of the proposed piecewise linear interface calculation (PLIC) reconstruction scheme coupled to a multidimensional time integration provides solutions of second-order spatial and temporal accuracy. The accuracy and efficiency of the proposed reconstruction algorithm are demonstrated through several tests, whose results are compared with those obtained with other recently proposed methods. An overall improvement in accuracy with respect to other recent methods has been achieved, along with a substantial reduction in the central processing unit time required. Copyright © 2008 John Wiley & Sons, Ltd.
  • S Zalesak
  • Fully
  • Flux-Corrected
  • Transport
  • For
  • Fluids
S. ZALESAK, " FULLY MULTIDIMENSIONAL FLUX-CORRECTED TRANSPORT ALGORITHMS FOR FLUIDS, " Journal of Computational Physics, vol. 31, no. 3, pp. 335–362, 1979.