Chapter 10. VOF Free Surface Model

Chapter 10. VOF Free Surface Model

Information about the VOF model is divided into the following
sections:

Section 10.1: Introduction
Section 10.2: Theory
Section 10.3: Using the VOF Model

10.1 Introduction

Two models are available in FLUENT for simulations where two or
more uids are present. The Volume of Fluid VOF model Hirt
and Nichols, 1981 49 is designed for two or more immiscible uids,
where the position of the interface between the uids is of interest.
The Eulerian model, described in Chapter 9, is designed for two or
more interpenetrating uids. Whereas the Eulerian model makes
use of multiple momentum equations to describe the individual u-
ids, the VOF model does not. In the VOF model, a single set
of momentum equations is shared by the uids, and the volume
fraction of each of the uids is tracked throughout the domain. Ap-
plications of the VOF model include the prediction of jet break-up,
the motion of large bubbles in a liquid, the motion of liquid after a
dam break, or the steady or transient tracking of any liquid-gas in-
terface. The Eulerian multiphase model, on the other hand, is best
suited for applications involving slurries or liquid-liquid and liquid-
gas mixtures involving small bubbles. The distinction between large
and small bubbles in these examples is based on the size of a typical
control volume. If a bubble is much smaller than a control volume,
many such bubbles can be treated as a separate uid in the Eu-
lerian multiphase model. If the bubble is so large that it extends
across several control volumes, the VOF formulation is appropriate
to track its boundary.
Example of a Dam To illustrate the capabilities of the VOF model, consider a rectan-
Break gular domain, 4 m long and 2.2 m high, in which water is initially
con ned to a region on the left side by the presence of a dam. At
time t=0, the dam breaks, and the water starts to ow to the right.

10-2 Chapter 10 | VOF Free Surface Model

Figures 10.1.1 and 10.1.2 illustrate the spread of the water during
the rst 0.7 seconds.
By 0.9 and 1.1 seconds, the water has reached the opposite side of
the container and is moving up the wall Figure 10.1.3.
If the grid is su ciently ne, FLUENT can predict the formation of
large water drops that separate from the water stream as it hits
the upper boundary of the domain. These drops will then fall to
the bottom of the container, where they will reattach to the water
there.
Auxiliary Models Most FLUENT models are available in combination with the VOF
and Limitations model. For example, the sliding-mesh model can be used to pre-
dict the shape of the surface of a liquid in a mixing tank. The
deforming mesh capability is also compatible with the VOF model.
The porous media model can be used to track the motion of the
interface between two uids through a packed bed or other porous
region. The e ects of surface tension may be included for one
speci ed phase only, and in combination with this model, you can
specify the wall adhesion angle. Heat transfer from walls to each
of the phases can be modeled, as can heat transfer between phases.
Turbulence modeling is available through the standard or the RNG
k - -model. Turbulence modeling with the Reynolds Stress model
is not available, however. For any of these applications, note that
all control volumes must be lled with either a single uid phase
or a combination of phases, since the model does not allow for void
regions where no uid of any type is present.
Some models are available for only one of the phases. Only one
phase's density can be calculated using the gas law. Species mix-
ing and reacting ow can be modeled in one of the phases, but
mass transfer between phases cannot be modeled without User-
De ned Subroutines. While temperature-dependent properties are
available for both phases, the kinetic theory option is only avail-
able for one of the phases, as is property de nition through User-
De ned-Subroutines. Only one of the phases can be modeled with
a non-Newtonian viscosity law.
If you model solidi cation using the phase change model described
in Chapter 8, the solidi cation can occur in only one phase. By
default, this solidifying phase is the rst secondary phase. You will
have the opportunity to specify a di erent phase for solidi cation
when you specify the phase change properties see Section 8.3.
Note also that solidi cation cannot take place in the vicinity of the
interface between two phases.

c Fluent Inc. May 10, 1997

10.1 Introduction 10-3

1.00E+00

5.00E-01

0.00E+00

Y Transient Simulation of a Dam Break Oct 20 1994
Z X Water Volume Fraction (Dim) Fluent 4.30
Lmax = 1.000E+00 Lmin = 0.000E+00 Time = 2.000E-01 Fluent Inc.

Figure 10.1.1: Transient Simulation of a Dam Break During the
First 0.2 Seconds
1.00E+00

5.00E-01

0.00E+00


Figure 10.1.2: Transient Simulation of a Dam Break at 0.5 and 0.7
Seconds



1.00E+00

5.00E-01

0.00E+00

Lmax = 1.000E+00 Lmin = 0.000E+00 Time = 1.100E+00 Fluent Inc.

Figure 10.1.3: Transient Simulation of a Dam Break at 0.9 and 1.1
Seconds

Steady State vs. The VOF formulation in FLUENT is, by default, time-dependent,
Time Dependence but for problems in which you are concerned only with a steady-
state solution, it is possible to perform a steady-state calculation.
A steady-state VOF calculation is sensible only when your solution
is independent of the initial conditions and there are distinct in ow
boundaries for the individual phases. For example, since the shape
of the free surface inside a rotating cup depends on the initial level of
the uid, such a problem must be solved using the time-dependent
formulation. On the other hand, the ow of water in a channel with
a region of air on top and a separate air inlet can be solved with
the steady-state formulation.


10.2 Theory 10-5

10.2 Theory

The VOF formulation relies on the fact that two or more uids
or phases are not interpenetrating. For each additional phase
that you add to your model, a variable is introduced, which is the
volume fraction of that phase. In each control volume, the volume
fractions of all phases add to unity. The elds for all variables and
properties are shared by the phases, as long as the volume fraction
of each of the phases is known at each location. Thus the variables
and properties in any given cell are either purely representative of
one of the phases, or are representative of a mixture of the phases,
depending upon the volume fraction values. In other words, if the
volume fraction of the kth uid in a multi- uid system is denoted
k , then the following three conditions are possible:

k = 0 the cell is empty of the kth uid
k = 1 the cell is full of the kth uid
0 k 1 the cell contains the interface between the uids
Based on the local value of k , the appropriate properties and vari-
ables will be assigned to each control volume within the domain.
The Volume The tracking of the interfaces between the phases is accomplished
Fraction Equation by the solution of a continuity equation for the volume fraction of
one or more of the phases. For the kth phase, this equation has
the form:
@ @
@t
k
+ uj @xk = S k 10.2-1
i

The source term on the right hand side of Equation 10.2-1 is nor-
mally zero, but can be constructed with a User-De ned Subroutine
to generate a source of the kth phase in one or more regions of the
solution domain to simulate mass transfer between phases. This
task requires the additional speci cation of a mass source.
Properties The properties appearing in the transport equations are determined
by the presence of the component phases in each control volume.
In a two-phase system, for example, if the phases are represented
by the subscripts 1 and 2, and if the volume fraction of the second
of these is being tracked, the density in each cell is given by:

= 2 2 + 1 , 2 1 10.2-2
In general, for an N-phase system, the volume-fraction averaged
density takes on the form:



X
= k k 10.2-3
All other properties are computed in this manner viscosity and
thermal conductivity, for example with the exception of the speci c
heat, which is mass fraction averaged:
P
k cp k
cp = P 10.2-4
k

k k

The basis for the mass-weighted averaging done for the speci c heat
lies in the manner in which the enthalpy is calculated at cells near
the interface. The enthalpy in general is dependent upon the ther-
mal mass of the uid. It follows, therefore, that a mass-averaged
enthalpy be computed at and near interface cells. For cells in this
region, the enthalpy at the node P is computed as follows:
P
k hk
hP = Pk 10.2-5
k k

The Momentum A single momentum equation is solved throughout the domain, and
Equation the resulting velocity eld is shared among the phases. The momen-
tum equation, shown below, is dependent on the volume fraction of
the kth phase through the properties and .
@ @
uj + ui uj
@t @xi

!
= , @x + @x
@P @ @ui
@xj
+ @x + @uj
gj + Fj 10.2-6
j i i

One limitation of the shared- elds approximation is that in cases
where large velocity di erences exist between the phases, the accu-
racy of the velocities computed near the interface can be adversely
a ected.
The Enthalpy The enthalpy equation, also shared between the phases, is shown
Equation below.
!
@ @ @ @T
@t
h + @x ui h = @x k
@xi
+ Sh 10.2-7
i i

The properties and k are shared by the phases, as discussed earlier.
The source term, Sh, contains contributions from radiation, and the


10.2 Theory 10-7

heat of reaction in the primary phase if reactions are a part of the
model.
As with the velocity eld, the accuracy of the enthalpy and conse-
quently the temperature near the interface is limited in cases where
large temperature di erences exist between the phases. Such prob-
lems also arise in cases where the properties vary by several orders
of magnitude. For example, if a model includes liquid metal in
combination with air, the conductivities of the materials can di er
by as much as 4 orders of magnitude. Such large discrepancies in
properties lead to equation sets with anisotropic coe cients, which
in turn lead to convergence and precision limitations.
Additional Scalar Depending upon your problem de nition, additional scalar equa-
Equations tions may be involved in your solution. In the case of turbulence
quantities, a single set of transport equations is solved, and the vari-
ables k and are shared by the phases throughout the eld. In the
case of species mixing, the species conservation equations are solved
throughout the eld, but only pertain to one of the phases. If a cell
is completely devoid of that phase, the mass fractions of the rst
N-1 species that you name will all take a value of zero in that cell.
Interpolation Near The control volume formulation requires that convection and dif-
the Interface fusion uxes through the control volume faces be computed and
balanced with source terms within the control volume itself. There
are two options in FLUENT for the calculation of face uxes for the
VOF model.
In the default method, which is an explicit approach, the standard
interpolation schemes that are used in FLUENT are used to obtain
the face uxes whenever a cell is completely lled with one phase or
another. When the cell is near the interface between two phases, a
donor-acceptor scheme is used to determine the amount of uid
advected through the face 49 . This scheme identi es one cell as a
donor of an amount of uid from one phase and another neighbor
cell as the acceptor of that same amount of uid, and is used to
prevent numerical di usion at the interface. The amount of uid
from one phase that can be convected across a cell boundary is
limited by the minimum of two values: the lled volume in the
donor cell or the free volume in the acceptor cell.
The orientation of the interface is also used in determining the face
uxes. It is determined by the direction of the gradient of the
volume fraction of the ith phase within the cell, and that of the
neighbor cell which shares the face in question. Depending upon
this as well as the motion of the interface, ux values are obtained by



pure upwinding, pure downwinding, or some combination of these.
In the alternative implicit interpolation method, FLUENT's stan-
dard interpolation schemes are used to obtain the face uxes for all
cells, including those near the interface. Thus, a standard scalar
transport equation is solved for each of the secondary-phase volume
fractions. The implicit formulation is valid for both steady-state
and time-dependent calculations. See Sections 10.1 and 10.3.2 for
more information.
Time Dependence The default VOF formulation in FLUENT is time-dependent, so
Equation 10.2-1 is solved using an explicit time-marching scheme.
Time dependence is automatically enabled as soon as you activate
the VOF model. A number of options are available for the control
of the time-dependent solution. You may use a single time step
for the calculation of all of the transport equations, or you can
use an automatic re nement of the time step for the multi-step
integration of the volume fraction equation. You may update the
volume fraction once for each time step, or once for each iteration
within each time step. These options are discussed in more detail
in the next section of this chapter.
If the explicit donor-acceptor interpolation method is disabled, it
is possible to turn o time dependence and perform a steady-state
calculation.

10.3 Using the VOF Model

10.3.1 Enabling VOF
The VOF model can be enabled in one of two ways. Either you
can enter the SETUP1 menu and use the DEFINE-MODELS command
from the text interface, or you can open the Models panel using the
graphical user interface.
Using the When you use the panel, the VOF Free Surface model can be chosen
Graphical Interface from among the options in the Model drop-down list under Multi-
phase on the right-hand side of the panel.


10.3 Using the VOF Model 10-9

Note that when you select the VOF model with the default donor-
acceptor scheme, the Time Dependent Flow model is activated au-
tomatically. If you wish to disable time dependence and perform
a steady-state calculation, you will need to rst disable the donor-
acceptor scheme, as described in Section 10.3.2.
When you click Apply in the Models panel, if you are just beginning
the problem setup, you may see the following question, which is
needed for the allocation of memory needed for the additional phase.



Once you have selected one of the multiphase models, the Multi-
phase Parameters... button becomes active, allowing you to specify
additional model parameters. In the case of the VOF model, this
panel allows you to select the optional Surface Tension and Wall Ad-
hesion models, disable the Donor-Acceptor Model, and set some of
the time-dependent solution control parameters.



The surface tension and wall-adhesion models and the time-dependence
parameters that are relevant to the VOF model are discussed later
in this chapter. The use of the implicit interpolation scheme rather
than the default donor-acceptor scheme is also discussed later.
Using the Text From the text interface, the VOF model can be enabled with the
Interface DEFINE-MODELS command in the SETUP1 menu. This command re-
sults in a menu where you can choose from among many models
that are available in FLUENT.
SETUP1 ,! DEFINE-MODELS



SETUP1-
DM

COMMANDS AVAILABLE FROM DEFINE-MODELS:
CYLINDRICAL-VELOCITIES HEAT-TRANSFER
TURBULENCE RADIATION
SPECIES-AND-CHEMISTRY MULTIPLE-PHASES
QUIT HELP
ENTER HELP COMMAND FOR MORE INFORMATION.
DEFINE-MODELS-

The option to perform either a VOF or an Eulerian multiphase
calculation is enabled with the MULTIPLE-PHASES command.
DEFINE-MODELS ,! MULTIPLE-PHASES

DEFINE-MODELS-
MP

MULTIPHASE MODELS SELECT ONLY ONE
NO EULERIAN-EULERIAN MULTIPHASE FLOW MODEL
NO EULERIAN-EULERIAN GRANULAR FLOW MODEL
YES VOF FREE SURFACE MODEL
D ACTION TOP,DONE,QUIT,REFRESH

After you select one of the multiphase models, a new menu appears
in which you can continue the model de nition. If you are just
beginning the problem setup, you may rst see the following ques-
tion, which is needed for the allocation of memory needed for the
additional phase.

MULTIPHASE MODEL SELECT ONLY ONE
*- ** MEMORY ALLOCATION **
I- NUMBER OF ADDITIONAL PHASES TO BE CONSIDERED
I- ++DEFAULT 1++
1
I- DEFAULT ASSUMED

COMMANDS AVAILABLE FROM MULTIPHASE:
DEFINE-PHASES MULTIPHASE-OPTIONS QUIT
HELP
MULTIPHASE-



The DEFINE-PHASES command is used to specify the number of
phases and their names, as described in Section 10.3.3. The
MULTIPHASE-OPTIONS command is used to enable the surface ten-
sion and wall adhesion models that may be used in conjunction with
the VOF calculation, or to disable the donor-acceptor scheme.
MULTIPHASE ,! MULTIPHASE-OPTIONS

MULTIPHASE-
MO

VOF OPTIONS
YES ENABLE DONOR-ACCEPTOR VOF MODEL
NO SURFACE TENSION
NO WALL ADHESION

These options are discussed in Section 10.3.2 and 10.3.9.
10.3.2 Choosing the VOF Formulation
The VOF formulations that are available in FLUENT are as follows:

time-dependent with the donor-acceptor interpolation scheme
default
time-dependent with the implicit interpolation scheme
steady-state with the implicit interpolation scheme

The time-dependent formulation with the donor-acceptor scheme is
the default scheme, and it should be used whenever you are inter-
ested in the time-accurate transient behavior of the VOF solution.
This formulation is activated automatically when you rst enable
the VOF model as described in Section 10.3.1.
The time-dependent formulation with the implicit interpolation scheme
can be used if you are looking for a steady-state solution and you
are not interested in the intermediate transient ow behavior, but
the nal steady-state solution is dependent on the initial ow con-
ditions and or you do not have a distinct in ow boundary for each
phase. To use this formulation, turn o the donor-acceptor model
as described below. While the implicit time-dependent formulation



may converge faster than the donor-acceptor formulation, the in-
terface between phases will not be as sharp as that predicted with
the donor-acceptor scheme. To reduce this di usivity, it is rec-
ommended that you use the QUICK discretization scheme for the
volume fraction equations. In addition, you may want to consider
turning the donor-acceptor scheme back on after calculating a solu-
tion with the implicit scheme, in order to obtain a sharper interface.
The steady-state formulation can be used if you are looking for
a steady-state solution, you are not interested in the intermedi-
ate transient ow behavior, and the nal steady-state solution is
not a ected by the initial ow conditions and there is a distinct
in ow boundary for each phase. To use this formulation, turn
o the donor-acceptor model as described below, and then disable
the time-dependent ow model in the Models panel or the EXPERT
TIME-DEPENDENCE table. As mentioned above, it is recommended
that you use the QUICK discretization scheme for the volume frac-
tion equations when you use the implicit interpolation scheme.
Examples To help you determine the best formulation to use for your problem,
examples which use each of the three formulations are listed below:

time-dependent with the donor-acceptor scheme: jet breakup
time-dependent with the implicit interpolation scheme: shape
of the liquid interface in a centrifuge
steady-state with the implicit interpolation scheme: ow around
a ship's hull

Disabling the In the GUI, you can turn o the donor-acceptor scheme in the Mul-
Donor-Acceptor tiphase Parameters panel. Click on the Multiphase Parameters... but-
Scheme ton in the Models panel, and then turn o the Donor-Acceptor Model
under VOF Free Surface Options:



If a steady-state formulation is desired, you can now turn o the
Time Dependent Flow option in the Models panel. When the Donor-
Acceptor Model is active, it is not possible to disable time depen-
dence.
When the donor-acceptor model is not active, FLUENT will solve
standard scalar transport equations for the secondary volume frac-
tions.



In the text interface, you can deactivate the donor-acceptor scheme
in the VOF OPTIONS table accessed when you use the MULTIPLE-
PHASES command in the DEFINE-MODELS menu to enable the VOF
model, as described in Section 10.3.1:

VOF OPTIONS
NO ENABLE DONOR-ACCEPTOR VOF MODEL
NO SURFACE TENSION
NO WALL ADHESION
ACTION TOP,DONE,QUIT,REFRESH

If a steady-state formulation is desired, you can now turn o TIME-
DEPENDENCE in the EXPERT menu. When the DONOR-ACCEPTOR VOF
MODEL is active, it is not possible to disable time dependence.

10.3.3 De ning the Phases
The next step in the problem setup is the naming of the phases.
Note that while this step is optional, it can facilitate the subse-
quent setup process in that the phases will be identi ed by name
rather than by number. To de ne the phases, you can use either
the DEFINE-PHASES text command in the SETUP1 menu, or the
DEFINE-PHASES command in the MULTIPHASE menu that appears
after you use the DEFINE-MODELS MULTIPLE-PHASES text command
to enable the VOF model.
You will be asked rst for the number of secondary phases in the
problem whether or not you were prompted for the number of
additional phases to be considered earlier, for memory allocation
purposes. You will only be allowed to input the same value as
before or a smaller value. A greater number of phases cannot be
enabled at this point. If you respond that there is 1 secondary
phase, a table will result in which you can input the name of the
PRIMARY PHASE and the secondary phase, PHASE 2.
SETUP1 ,! DEFINE-PHASES



SETUP1-
DP
I- NUMBER OF SECONDARY PHASES
I- ++DEFAULT 1++
1

PHASE NAMES
NOTE : PHASE NAMES CANNOT CONSIST OF
A SINGLE CHARACTER C OR X
PHASE 1 PRIMARY PHASE
PHASE 2 PHASE 2

Before you name the phases, it is important to give some thought
to which of the uids to identify as the PRIMARY PHASE. If you plan
to use the gas law, this model is only available for the primary
phase. In the same manner, any species mixing or chemical reac-
tions will take place only within the primary phase. It is only this
phase that allows for the complete spectrum of property model-
ing, including the use of kinetic theory, User-De ned Subroutines,
non-Newtonian ow, and composition-dependence. Temperature
dependence through polynomial or piecewise-linear pro les, on the
other hand, is available for all phases.
If your problem de nition does not require the gas law, species
mixing, or special property de nitions, you should identify the less
dense of the uids as the primary phase. This means that the vol-
ume fraction equations will be solved for the denser uids. The
motivation for this choice has to do with numerics. If, during the
course of the solution, small perturbations in the pressure eld occur
near the interface, these will translate into perturbations in the ve-
locity eld. Because of the increased inertia, velocity perturbations
are smaller and much less destabilizing in the denser uid than in
the lighter uid. If the volume fraction is computed for the denser
uid, the increased stability of the velocity eld leads to increased
stability in the volume fraction calculation.
Once you have determined which uid should be assigned to which
phase, the phases can be named, as shown below for a two-phase
system involving AIR and WATER.



PHASE NAMES
AIR PRIMARY PHASE
WATER PHASE 2

If you request 2 secondary phases, the table will ask for the names
of the primary and the two secondary phases.

SETUP1-
DP
I- ++DEFAULT 1++
2

PHASE NAMES
AIR PRIMARY PHASE
WATER PHASE 2
OIL PHASE 3

10.3.4 Time-Dependent Modeling Parameters
If you are using the time-dependent VOF formulation in FLUENT,
an explicit solution for the volume fraction is obtained either once
each time step or once each iteration, depending upon your inputs
to the model. You also have control over the time step used for the
volume fraction calculation. It can be either the same as that used
for the solution of the other transport equations in the model, or
it can be adjusted automatically by FLUENT, again based on your
inputs.
From the text interface, the time-dependent solution controls are
accessed from the EXPERT menu using the TIME-DEPENDENCE com-
mand.
EXPERT ,! TIME-DEPENDENCE



EXPERT-
TD

TIME DEPENDENT FLOW SOLUTION PARAMETERS
100 MAX. NO. ITNS PER TIME STEP
1.0000E-03 MIN. RESIDUAL SUM DIM
1.0000E-03 SET TIME STEP S
YES SOLVE VOF EVERY ITERATION
NO AUTOMATIC TIME STEP REFINEMENT FOR VOF
2.5000E-01 MAXIMUM COURANT NUMBER FOR VOF DIM
NO AUTOMATIC SAVING
NO ENABLE TIME VARYING GRAVITY VECTOR

The input lines in this table are the same as those appearing in
the table when the VOF model is not active, with the exception of
three. These are discussed below.
SOLVE VOF EVERY ITERATION: A response of yes or no to this
question allows you to request that FLUENT solve the vol-
ume fraction equations every iteration within a time step
or simply once a time step. If you solve these equations ev-
ery iteration, the convective ux coe cients appearing in the
other transport equations will be updated based on the up-
dated volume fraction each iteration. If you solve the VOF
equations once a time step, these coe cients will not be com-
pletely updated each iteration, since the volume fraction eld
will not change from iteration to iteration.
In general, if you anticipate that the location of the inter-
face will change as the other ow variables converge during
the time step, you should use a response of YES. This situa-
tion arises when large time steps are being used in hopes of
reaching a steady-state solution, for example. If small time
steps are being used, however, it is not necessary to perform
the additional work of solving for the volume fraction every
iteration, so an input of NO can be used. This choice is the
more stable of the two, and requires less computational e ort
per iteration than the rst choice, but the overall result is less
accurate in time.
AUTOMATIC TIME STEP REFINEMENT FOR VOF: Two options are
available for the choice of time step to be used for the volume
fraction calculation. If you respond NO to this option, FLU-
ENT will solve the VOF equations using the time step that



is set in this table on the SET TIME STEP S line. If you re-
spond YES, the time step will be re ned automatically, based
on your input for the maximum Courant Number allowed near
the free surface, discussed below.
MAXIMUM COURANT NUMBER FOR VOF DIM: The Courant Num-
ber is a dimensionless number that compares the time step in
a calculation to the characteristic time of transit of a uid
element across a control volume:
t 10.3-1
xcell =v uid
In the region near the uid interface, FLUENT divides the
volume of each cell by the sum of the outgoing uxes. The
resulting time represents the time it would take for the uid
to empty out of the cell. The smallest such time is used as
the characteristic time of transit for a uid element across a
control volume, as described above. Based upon this time
and your input for the maximum allowed Courant Number,
a time step is computed for use in the VOF calculation. For
example, if the maximum allowed Courant Number is 0.25,
the time step will be chosen to be at most one-fourth the
minimum transit time for any cell near the interface.

You can access the time-dependent ow parameters from the graph-
ical interface, as well. Recall that as soon as the VOF model is
enabled in the Models panel, the Time Dependent Flow option is en-
abled as well. If you open the Time Dependent Flow Parameters panel
from the Models panel, you can set the standard time-dependent
ow variables.



To set the time dependent ow parameters that are used in the
VOF model, you can use the Multiphase Parameters panel that can
be accessed once one of the multiphase models is enabled.



In this panel, you can choose whether or not to solve the VOF
equations every iteration, whether or not to use the automatic re-
nement of the time step, as described above, and set the limiting
Courant Number.
10.3.5 De ning the Properties
The uid properties are set up using the PHYSICAL-CONSTANTS com-
mand in the SETUP1 menu. The items appearing in the PHYSICAL-
CONSTANTS menu depend upon the scope of your problem de nition.



At the very least, options for setting the DENSITY and VISCOSITY
will appear. Thermal properties appear when temperature is being
calculated. Species-related properties appear when the calculation
involves two or more species. Kinetic theory parameters appear
when kinetic theory is active, and so forth. When the VOF model
is active, the same items appear in the menu, but the dialogue that
follows when you set the properties changes. This dialogue is de-
signed to allow you to set the properties for each of the active phases
in your problem. It is illustrated through a number of examples that
follow.
Setting the Density When the VOF model is active, the gas law can be used for the
density calculation for the primary phase only. Alternatively, the
phases can have temperature dependent densities. In the simplest
case, the phases have constant, but di erent densities. If such a
system consists of two phases, the following dialogue illustrates the
setup of constant densities.
SETUP1 ,! PHYSICAL-CONSTANTS ,! DENSITY



SETUP1-
PC

COMMANDS AVAILABLE FROM PHYSICAL-CONSTANTS:
DENSITY VISCOSITY OPERATING-PRESSURE
QUIT HELP
PHYSICAL-CONSTANTS-
DE

COMMANDS AVAILABLE FROM PHASE-SELECTION:
AIR WATER QUIT HELP
PHASE-SELECTION-
AIR
L- USE GAS LAW FOR AIR?
L- Y OR N ++DEFAULT-NO++
N
R- DENSITY OF AIR
R- UNITS= KG M3 ++DEFAULT 1.0000E+03++
1.0

AIR WATER QUIT HELP
PHASE-SELECTION-
WAT
R- DENSITY OF WATER
1000

PHASE-SELECTION-
Q

In the next example, consider a 3-phase system where the gas law is
to be used for the primary phase. As with any single phase system
involving a single species, FLUENT will ask for the molecular weight
for the material being modeled with the gas law.



PHYSICAL-CONSTANTS-
DE

AIR WATER QUIT HELP
PHASE-SELECTION-
AIR
Y
R- OPERATING PRESSURE
R- UNITS= PA ++DEFAULT 1.0132E+05++
X
R- DEFAULT ASSUMED

R- ENTER THE MOLECULAR WEIGHT FOR AIR
R- UNITS= DIM ++DEFAULT 2.8970E+01++
X
R- DEFAULT ASSUMED

PHASE-SELECTION-
WAT
R- DENSITY OF WATER
1000

PHASE-SELECTION-
Q

If you are modeling multiple species in the primary phase, you
will not be asked to input the molecular weight, but will be re-
minded to input molecular weights for all of the species using the
MOLECULAR-WEIGHTS command.
When you are solving for temperature, FLUENT asks for the tem-
perature dependence for all of the properties for all of the phases.
For example, for a 3-phase system, the dialogue for setting up the
densities would be similar to that shown below.



PHYSICAL-CONSTANTS-
DE

AIR OIL WATER QUIT HELP
PHASE-SELECTION-
AIR
Y
R- OPERATING PRESSURE
R- UNITS= PA ++DEFAULT 1.0132E+05++
X
R- DEFAULT ASSUMED

R- ENTER THE MOLECULAR WEIGHT FOR AIR
X
R- DEFAULT ASSUMED

PHASE-SELECTION-
WAT
*- DEFINE DENSITY OF WATER KG M3
*- AS A FUNCTION OF TEMPERATURE K
*-
I- NUMBER OF COEFFICIENTS +VE = POLYNOM., -VE = P.W.LINEAR
I- ++DEFAULT 1++
1
R- DENSITY OF WATER KG M3
X
R- DEFAULT ASSUMED



PHASE-SELECTION-
OIL
*- DEFINE DENSITY OF OIL KG M3
*-
I- ++DEFAULT 1++
2

POLYNOMIAL FIT FOR DENSITY OF OIL
8.0000E+02 ENTER COEFFICIENT - A1 KG M3
-1.0000E-02 ENTER COEFFICIENT - A2 -

Setting the The viscosities for the phases are input in the same manner. In an
Viscosity isothermal, 3-phase system, the viscosities would be input in the
manner shown below.
PHYSICAL-CONSTANTS ,! VISCOSITY
PHYSICAL-CONSTANTS-
VI

PHASE-SELECTION-
AIR
R- VISCOSITY OF AIR
R- UNITS= KG M-S ++DEFAULT 2.0000E-05++
1.7e-5

PHASE-SELECTION-
WAT
R- VISCOSITY OF WATER
X
R- DEFAULT ASSUMED

PHASE-SELECTION-
OIL
R- VISCOSITY OF OIL
.01

If you are calculating temperature, FLUENT will ask for the tem-
perature dependence of the viscosity for each phase, in the manner
shown above for the density.



Modeling a In the event that one of the phases is to be modeled as a non-
Non-Newtonian Newtonian uid, you must de ne this uid as the primary phase.
Viscosity Once the non-Newtonian model has been enabled in the EXPERT
OPTIONS table or the Models panel, the VISCOSITY command in the
PHYSICAL-CONSTANTS menu can be used to set the non-Newtonian
viscosity constants as well as the viscosity for the additional phases.

SETUP1-
PC

DENSITY VISCOSITY PROPERTY-OPTIONS
OPERATING-PRESSURE QUIT HELP
PHYSICAL-CONSTANTS-
VIS

PHASE-SELECTION-
AIR

NON-NEWTONIAN FLOW PARAMETERS POWER LAW FOR AIR
1.5 PARAMETER N DIM
1.0000E+00 PARAMETER K PA*S**N

PHASE-SELECTION-
WAT
R- VISCOSITY OF WATER
9E-4

Using Kinetic If you are using the gas law to model the primary phase, you will
Theory for have the option of using kinetic theory to model one or more of
Property De nition the other properties for that phase. The kinetic theory option is
enabled in the usual way, using the PROPERTY-OPTIONS table in the
PHYSICAL-CONSTANTS menu. Once enabled, you will be asked if
you want to use kinetic theory when you set the various properties.
For example, to use kinetic theory for the speci c heat, the dia-
logue would proceed as shown below. After setting the REFERENCE
TEMPERATURE FOR ENTHALPY and selecting the primary phase AIR
in the example below, you will be asked if you want to use kinetic
theory for the primary phase:



PHYSICAL-CONSTANTS-
CP
R- REFERENCE TEMPERATURE FOR ENTHALPY
R- UNITS= K ++DEFAULT 2.7300E+02++
X
R- DEFAULT ASSUMED

PHASE-SELECTION-
AIR
L- COMPUTE SPECIFIC HEAT FROM KINETIC THEORY?
L- Y OR N ++DEFAULT-YES++
Y

You can then de ne the optionally temperature-dependent speci c
heat for the remaining phases.

PHASE-SELECTION-
WAT
*- DEFINE SPECIFIC HEAT OF WATER J KG-K
*-
I- ++DEFAULT 1++
X
I- DEFAULT ASSUMED

R- SPECIFIC HEAT OF WATER J KG-K
R- UNITS= J KG-K ++DEFAULT 1.0000E+03++
4136

Before kinetic theory can be used, you will need to set the kinetic
theory parameters, appearing in the KINETIC-THEORY-PARMS. ta-
ble. The setting of these parameters is described in Chapter 15.
10.3.6 Including Body Forces in the VOF Calculation
In many instances, the motion of the uids you are tracking with the
VOF model is due, in part, to gravitational e ects. When you ac-
tivate a gravitational force in the BODY-FORCES table in the EXPERT
menu, you will be given a choice of whether to set the site of the
reference density or to set the reference density itself.
EXPERT ,! BODY-FORCES



SETUP1-
EX BF

BODY FORCES
YES IMPROVED TREATMENT OF BODY FORCE IN DISCRETE EQNS.
YES INCLUDE BODY FORCE TERMS IN VELOCITY INTERPOLATION
9.8000E+00 GRAVITY ACCELERATION IN X-DIRN - M S2
0.0000E+00 GRAVITY ACCELERATION IN Y-DIRN - M S2
YES USER DEFINED REFERENCE DENSITY

If you respond YES to the option to input a USER DEFINED REFERENCE
DENSITY, a second table will appear, where you will be able to input
the value of this density.

USER DEFINED REFERENCE DENSITY
1.0000E+00 REFERENCE DENSITY KG M3

If you respond NO to the input of a USER DEFINED REFERENCE DENSITY,
a second table will appear asking you to input the location of the
cell from which the reference density will be taken.

REFERENCE DENSITY LOCATION
2 REFERENCE DENSITY : I - LOCATION
2 REFERENCE DENSITY : J - LOCATION

While either selection works well for most single phase applications,
the option to set the reference density rather than the site of the
reference density is preferred when the VOF model is in use. The
aim is to have a reference density value that is stable throughout
the calculation. Since many VOF applications involve a change
from one phase to another in any given control volume throughout
the course of the calculation, it is better to set the density value
itself, rather than assume that one cell in particular will always be
lled with one particular phase.
In terms of selecting the appropriate reference density value, the
best strategy is to use the density of the predominant uid. If,
in a two-phase system, for example, water occupies over 50 of



the volume, the density of water should be used. This strategy
minimizes the round-o in the density uctuations that are the
source of the buoyancy forces in the domain.
If your model has in ow out ow boundaries and you prefer to set
the reference density site, you should do so at an in ow boundary
where the predominant uid enters the domain. This is because
the density will be constant throughout the calculation at this site.
If you choose an interior site, convergence problems will arise if
uctuations of the density occur at the site that you choose.
10.3.7 Setting Boundary Conditions
Boundary conditions may be input using either the text interface
command for BOUNDARY-CONDITIONS in the SETUP1 menu, or the
Boundary Conditions panel through the graphical user interface. At
inlets, one additional scalar, the volume fraction, must be set when
the VOF model is active. Note that this scalar can only be set for
the non-primary phases.
In a 2-phase system, for example, where the primary phase is air and
the second phase is water, the steps for setting the inlet boundary
conditions from the graphical user interface are as follows. From the
Boundary Conditions panel, choose an INLET cell type and select the
appropriate zone ID. When you press the Set... button the Velocity
or Pressure Inlet Boundary Conditions panel appears.



In the Inlet Boundary Conditions panel, the rst Phase that you
named appears in the upper left corner, and the elds for the rel-
evant velocities and scalars are active. The Volume Fraction eld
under Multiphase is not active at this time.
The speci cation of the boundary conditions requires two steps.
First, enter the velocity and other scalar values in the appropriate
elds and click on Apply. Second, choose one of the secondary phases
from the Phase drop-down list. When you do this, the velocity and



scalar elds become inactive, and the Volume Fraction eld becomes
active. Set the appropriate Volume Fraction and click on Apply. If,
in a two-phase system, the inlet is to have a volume fraction of 1
for the rst phase, you will need to choose the second phase and set
a volume fraction of 0.

Note that with the VOF Model, only values of 0 or 1 are meaningful
at any given inlet. If an inlet is to introduce a strati ed layer of
two uids into a domain, it should be replaced by two inlets, each
carrying a single uid.



From the text interface, the VOLUME-FRACTION appears in the inlet
zone boundary conditions menu as shown below.
SETUP1 ,! BOUNDARY-CONDITIONS

SETUP1-
BC

COMMANDS AVAILABLE FROM BOUNDS:
W-WALL Z-WALL SYMMETRY .LIVE
CYCLIC OUTLET INLET AXIS
QUIT HELP
BOUNDS-
I 1

COMMANDS AVAILABLE FROM I1-ZONE-BOUNDARY-CONDITIONS:
NORMAL-VELOCITY U-VELOCITY V-VELOCITY
VOLUME-FRACTION QUIT HELP
I1-ZONE-BOUNDARY-CONDITIONS-

As with the graphical interface, the VOLUME-FRACTION command
will prompt you for the volume fraction of the secondary phases
only. Thus, if you are solving a problem in which there is one sec-
ondary phase, FLUENT will ask for the volume fraction of only that
phase. Volume fractions of either 0 or 1.0 are the only meaningful
choices for the VOF model, even though any value between these
two will be accepted.
BOUNDARY-CONDITIONS ,! VOLUME-FRACTION

VF
R- VOLUME FRACTION OF WATER
1.0

Because the velocity and turbulence and enthalpy elds are shared,
there is no need to specify a separate velocity boundary condition
for the various phases. This is in contrast to the setting of bound-
ary conditions in the Eulerian multiphase model, where each phase



carries its own velocity eld. Wall boundary condition options
are not expanded by the presence of multiple phases within the
domain. A zero normal gradient boundary condition is imposed for
the volume fraction.
10.3.8 Solution Strategies
In addition to the appropriate choice for the primary phase uid
and the time stepping technique to use, other steps can be taken to
improve the accuracy of the VOF calculation.
Setting the The site of the reference pressure can be moved to a location that
Reference Pressure will result in less round-o in the pressure calculation. The option
Location to set the reference pressure location is in the EXPERT SOLUTION-
PARAMETERS table. If you respond YES, as shown below, a second
table appears in which the location of the reference pressure can be
chosen.
EXPERT ,! SOLUTION-PARAMETERS

SOLUTION PARAMETERS
NO MONITOR SOLVER
NO ALLOW PATCHING OF BOUNDARY VALUES
YES CONVERGENCE-DIVERGENCE CHECK ON
1.0000E-03 SET MINIMUM RESIDUAL SUM DIM
YES NORMALIZE RESIDUALS
YES CONTINUITY CHECK
NO ENABLE HIGHER ORDER SCHEME
NO ENABLE LINEAR INTERPOLATION FOR PRESSURE
NO VISCOSITY WEIGHTED VELOCITY INTERPOLATION
NO ENABLE SIMPLEC METHOD DEFAULT IS SIMPLE
NO ENABLE FIX VARIABLE OPTION
YES SET PRESSURE REFERENCE LOCATION

REFERENCE PRESSURE LOCATION
2 I-VALUE
10 J-VALUE

The cell that you choose should be in a region that will always
contain the less dense of the two uids. This is because variations
in the static pressure are larger in a more dense uid than in a less
dense uid, given the same velocity distribution. If the zero of the
relative pressure eld is in a region where the pressure variations are



small, less round-o will occur than if the variations occur in a eld
of large non-zero values. Thus in systems containing air and water,
for example, it is important that the reference pressure location be
in the portion of the domain lled with air rather than that lled
with water.
Setting the The calculation of pressure is perhaps the most important among all
Multigrid of the variables in a VOF simulation in terms of having an in uence
Parameters on the prediction of volume fraction. Whenever possible, the multi-
grid solver should be enabled for pressure. To extract the most work
from the multigrid solver each iteration, you should decrease the
TERMINATION-CRITERIA to its minimum value, 1 10,3 , at least
during the rst few time steps, using the TERMINATION-CRITERIA
command in the MULTIGRID-PARAMETERS menu or the Termination
Criterion eld in the Multigrid Parameters panel.
EXPERT ,! LINEAR-EQN.-SOLVERS ,! MULTIGRID-PARAMETERS
Solve ,! Controls ,!Multigrid...
Reduction of this value leads to the maximum volume conservation
condition that can be imposed during each iteration, leading to the
most accurate prediction of the volume fraction.
Underrelaxation A third change that you may want to make to the solver settings is
for the in the underrelaxation factors that you use. Typically, the default
Time-Dependent time-dependent VOF formulation allows for increased values on all
Donor-Acceptor underrelaxation factors, provided a small time step is used, without
Formulation a loss of solution stability. In simple geometries with little grid
skew, you can generally increase the underrelaxation factors for all
variables to 1.0 and expect stability and a rapid rate of convergence
in the form of few iterations required per time step. The default
underrelaxation factor of 1.0 on the body forces need not be reduced
except in cases where gravity and strong swirl or other user-de ned
momentum sources are involved.
EXPERT ,! UNDERRELAX1
Solve ,! Controls ,!Underrelaxation...
As with any FLUENT simulation, the underrelaxation factors can
and should be increased as the solution exhibits stable, convergent
behavior. You should always save a Data File beforehand, however,
in case the increase you specify destabilizes the solution process.
Underrelaxation If you have deactivated the donor-acceptor model as described in
for the Implicit Section 10.3.2, you will be able to set underrelaxation parame-
Formulations ters for each secondary-phase volume-fraction transport equation.



This is true for both the time-dependent and steady-state implicit
formulations. By default, these underrelaxation factors are set to
0.2. For improved convergence, you can set these as well as the
underrelaxation factors for all other equations to 0.5.
Linear Solver As mentioned earlier, if you have deactivated the donor-acceptor
Parameters for the model as described in Section 10.3.2, FLUENT will solve trans-
Implicit port equations for the secondary-phase volume fractions. It is not
Formulations possible to use the multigrid solver for these volume fraction equa-
tions, so you must always use the linear LGS solver.
Discretization When the implicit scheme is used instead of the donor-acceptor
Scheme Selection scheme, you should use the QUICK discretization scheme for the
for the Implicit volume fraction equations in order to improve the sharpness of the
Formulations interface between phases.
10.3.9 The Surface Tension Model
It is possible to include the e ects of surface tension along the in-
terface between two uids. The model can be augmented by the
additional speci cation of a contact angle that one of the uids
makes with the container wall.
Surface tension arises as a result of attractive forces between molecules
in a uid. Consider an air bubble in water, for example. Within
the bubble, the net force on a molecule due to its neighbors is zero.
At the surface, however, the net force is radially inward, and the
combined e ect of the radial components of force across the entire
spherical surface is to make the surface contract, thereby increasing
the pressure on the concave side of the surface. The surface tension
is a force, acting only at the surface, that is required to maintain
equilibrium in such instances. It acts to balance the radially inward
inter-molecular attractive force with the radially outward pressure
gradient force across the surface. In regions where two uids are
separated, but one of them is not in the form of spherical bubbles,
the surface tension acts to decrease the area of the interface.
The surface tension model in FLUENT is the Continuum Surface
Force CSF model proposed by Brackbill et al. 14 . With this
model, the addition of surface tension to the VOF calculation results
in a source term to the momentum equation. To understand the
origin of the source term, consider the special case where the surface
tension is constant along the surface, and where only the forces
normal to the interface are considered. It can be shown that the
pressure drop across the surface depends upon the surface tension
coe cient, , and the surface curvature as measured by two radii



in orthogonal directions, R1 and R2:

1 1
p2 , p1 = R1
+R 10.3-2
2

where p1 and p2 are the pressures in the two uids on either side of
the interface.
In FLUENT, a more general formulation is used, where the surface
curvature is computed from local gradients in the surface normal at
the interface. Let n be the surface normal, de ned as the gradient
in 2 , the secondary phase volume fraction.

n =r 2 10.3-3
The curvature, , is de ned in terms of the divergence of the unit
normal, n:
^
!
=rn =
1
jnj r jnj , r n
n
^ jnj 10.3-4

where
n
^ = jnj
n 10.3-5

The surface tension can be written in terms of the pressure jump
across the surface. The force at the surface can be expressed as a
volume force using the divergence theorem. It is this volume force
that is the source term which is added to the momentum equation.
It has the following form:

= 2 x 2 r 2
Fvol x 10.3-6
Note that the source term is only added on one side of the inter-
face: the side on which the volume fraction calculation is being
performed. In the FLUENT VOF model, this corresponds to the
secondary phase.
Example: As an example of the surface tension model, consider a section of a
Prediction of a stationary cylinder of water in a zero gravitational eld. The sec-
Capillary Jet tion is 5.236 cm in length, and roughly 1 cm in diameter, following
Breakup an example proposed in Reference 65 . A region of air, 3 cm in
diameter, surrounds the cylinder of water. A 41 31 grid is used



in the axisymmetric model, which employs a symmetry boundary
condition on the axis and both ends, and a pressure boundary to
model the plenum of air surrounding the water.
The liquid surface is initially perturbed at t=0 so that the diameter
at the left side is 5 larger than that at the right Figure 10.3.1,
with the transition modeled using a cosine function.
1.00E+00

5.00E-01

0.00E+00

Y Initial Conditions for Capillary Jet Breakup Nov 03 1994
Max = 1.000E+00 Min = 0.000E+00 Time = 5.000E-04 Fluent Inc.

Figure 10.3.1: Initial Conditions for Capillary Jet Breakup Problem

As time evolves, the perturbation in the surface grows, as can be
seen in Figure 10.3.2.
The reason that the perturbation grows in this manner is that the
curvature in the surface gives rise to di erent pressure gradients
across the surface in di erent regions. Where the surface is concave
as seen from the water side, the pressure is higher on the water side
than on the air side, forcing the boundary to move outward. Where
the surface is convex, the opposite is true, so that the boundary
moves inward. At t = 0.75 seconds Figure 10.3.3, the perturbation
has advanced to the point where the jet is about to break. Within
the next 15 ms, the break up has occurred.
Enabling the The surface tension model can be enabled three di erent ways.
Surface Tension First, you can open the Multiphase Parameters panel and turn on
Model the Surface Tension check button.


1.00E+00

5.00E-01

0.00E+00

Y Capillary Jet Breakup at t = 0.5 / 0.7 sec Nov 03 1994

Figure 10.3.2: Capillary Jet Breakup at T = 0.5 top and 0.7
bottom sec



1.00E+00

5.00E-01

0.00E+00

Y Capillary Jet Breakup at t = 0.75 / 0.765 sec Nov 03 1994

Figure 10.3.3: Capillary Jet Breakup at T = 0.75 top and 0.765
bottom sec



Alternatively, you can use the text interface. In the SETUP1 menu,
you can start with the DEFINE-MODELS command and select the
MULTIPLE-PHASES option to turn on the VOF FREE SURFACE MODEL.

DEFINE-MODELS-
MP

MULTIPHASE MODELS SELECT ONLY ONE
NO EULERIAN-EULERIAN MULTIPHASE FLOW MODEL
NO EULERIAN-EULERIAN GRANULAR FLOW MODEL
YES VOF FREE SURFACE MODEL

After you select one of the multiphase models, a new menu ap-
pears in which you can name the phases, as described earlier, or
choose MULTIPHASE-OPTIONS that are relevant to the VOF model:
the SURFACE TENSION model with the optional addition of WALL
ADHESION described later in this section.

COMMANDS AVAILABLE FROM MULTIPHASE:
DEFINE-PHASES MULTIPHASE-OPTIONS QUIT
HELP
MULTIPHASE-
MO

VOF OPTIONS
YES SURFACE TENSION
NO WALL ADHESION

Finally, you can use the OPTIONS command in the EXPERT menu.
EXPERT ,! OPTIONS



EXPERT-
OP

MODELING OPTIONS
NO ALLOW LINK SETTING
NO ALLOW PROFILE SETTING
NO ENABLE NON-NEWTONIAN FLOW MODEL
NO ENABLE POROUS FLOW MODEL
NO ENABLE FAN RADIATOR MODEL
NO ALLOW FIXED PRESSURE BOUNDARIES
NO ALLOW SETTING FLOW ANGLES FOR PRESSURE-INLETS
NO ENABLE STEADY CORIOLIS FORCE
NO ENABLE TIME-DEPENDENT CORIOLIS FORCE
NO ENABLE MULTIPLE ROTATING REFERENCE FRAMES
YES SURFACE TENSION
NO WALL ADHESION
NO ENABLE SLIDING MESH CALCULATION
NO ACTIVATE PHASE CHANGE MODELING
NO ENABLE DEFORMING MESH CALCULATION

The setting of the surface tension coe cient is illustrated along with
the setting of the contact angle that the uid makes with the wall.
This so-called wall adhesion angle is discussed below.
Wall Adhesion An option to specify a wall adhesion angle in conjunction with the
surface tension model is also available in the VOF model. The
model is taken from work done by Brackbill et al. 14 . Rather than
impose this boundary condition at the wall itself, the contact angle
that the uid is assumed to make with the wall is used to adjust
the surface normal in cells near the wall. This so-called dynamic
boundary condition results in the adjustment of the curvature of
the surface near the wall.
If

w is the contact angle at the wall, then the surface normal at the
live cell next to the wall is

n ^ ^
^ = nw cos

w 10.3-7
^
where nw and tw are the unit vectors normal and tangential to
^
the wall, respectively. The combination of this contact angle with
the normally calculated surface normal one cell away from the wall
determine the local curvature of the surface, and this curvature is
used to adjust the body force term in the surface tension calculation.



Enabling the Wall The ability to set the contact angle that the uid makes with the
Adhesion Model wall is set using one of the three methods discussed earlier for en-
abling surface tension. You can use the Multiphase Parameters panel,
the MULTIPHASE-OPTIONS menu command, or the EXPERT OPTIONS
table.
Example: As an example, consider a cylindrical container, partially lled with
Formation of a water, in a zero gravity eld. The container is 10 cm tall and 10
Water Bubble cm in diameter. An axisymmetric model is solved using a 51 31
grid.
At time t=0, the water lls the bottom 2 cm of the container, with
air above it Figure 10.3.4, left frame. The air is modeled as the
primary phase, which means that the surface tension value 0.07
N m will be applied to the second phase, water. A contact angle
of 175 is used. This contact angle is applied to the water, which
means that an obtuse angle, as measured in the water, will form at
the walls. For this condition to be met, the water level must rise in
the middle of the container and drop at the edges. The start of this
process is shown in Figure 10.3.4 right frame, where the boundary
condition at the wall acts to change the water level nearby. Note
that the water level at the center of the vessel is not yet a ected at
this time.
After 0.7 sec have passed Figure 10.3.5 left frame, the uid in the
center of the container has responded, and the water at the edges
continues to try to satisfy the contact angle boundary condition. By
1.3 sec Figure 10.3.5 right frame, the water has become detached
from the bottom of the vessel and is moving slowly upward.
Setting the Surface The surface tension coe cient and contact angle at the wall are set
Tension and Wall in the PHYSICAL-CONSTANTS menu, using the VOF-SURFACE-TENSION
Adhesion command. Note that you can specify the surface tension coe cient
Properties for only one phase. The contact angle is that between the inter-
face and the wall as measured inside the speci ed phase uid. In
the example below, a contact angle of 45 corresponds to the water
creeping up the side of its container, as is common with water in a
glass.
SETUP1 ,! PHYSICAL-CONSTANTS ,! VOF-SURFACE-TENSION



1.00E+00

5.00E-01

0.00E+00

Formation of a Bubble in a Zero Gravity Field Oct 21 1994
Z Y Water Volume Fraction (Dim) Fluent 4.30
X

Figure 10.3.4: Initial Water Level in a Container Left and Altered
Water Level After 0.2 sec Right



1.00E+00

5.00E-01

0.00E+00

Formation of a Bubble in a Zero Gravity Field Oct 21 1994
X
Max = 1.000E+00 Min = 0.000E+00 Time = 1.300E+00 Fluent Inc.

Figure 10.3.5: Formation of a Water Bubble Before Left and After
Right it Separates from the Wall



SETUP1-
PC

DENSITY VISCOSITY
PROPERTY-OPTIONS OPERATING-PRESSURE
VOF-SURFACE-TENSION QUIT
HELP
PHYSICAL-CONSTANTS-
VOF

*- SELECT PHASE FOR SURFACE TENSION

*- DEFAULT PHASE - WATER

AIR WATER QUIT HELP
PHASE-SELECTION-
WAT

R- ENTER SURFACE TENSION COEFFICIENT FOR WATER
R- UNITS= N M ++DEFAULT 7.3050E-02++
X
R- DEFAULT ASSUMED

R- ENTER CONTACT ANGLE IN DEGREES
45
R- DEFAULT ASSUMED

The default setting for surface tension coe cient corresponds to
water at room temperature and atmospheric pressure. The contact
angle is the angle between each boundary wall and the uid interface
as measured in the speci ed phase here, water. The default value
90 corresponds to a surface which is at all times normal to the
surrounding walls.
10.3.10 Using the VOF Model with Porous Media
The VOF model is compatible with the porous media model in
FLUENT. If you have a region that needs to be described as a porous
media, the setup begins in the normal way. First, you need to enable
the porous media model in the EXPERT OPTIONS table in the text



interface. The next step is to set the cell types appropriately so as
to belong to one or more porous zones.
When you set the porous media constants from the PHYSICAL-CONSTANTS
menu, FLUENT will prompt you for the PERMEABILITY and INERTIAL-
RESISTANCE-FACTOR for each of the phases separately.
PHYSICAL-CONSTANTS ,! POROUS-MEDIA

PHYSICAL-CONSTANTS-
PM
*- POROUS MEDIA INPUTS...
*- ENTER QUIT WHEN FINISHED

SELECT-ZONE-
1

COMMANDS AVAILABLE FROM * POROUS MEDIA INPUTS FOR ZONE 1 *:
PERMEABILITY INERTIAL-RESISTANCE-FACTOR
POROSITY QUIT
HELP
* POROUS MEDIA INPUTS FOR ZONE 1 *-
PER

PERMEABILITY FOR ZONE 1
1.0000E-08 PERMEABILITY IN THE I-DIRN. FOR PHASE 1 M2
1.0000E-08 PERMEABILITY IN THE J-DIRN. FOR PHASE 1 M2
5.0000E-09 PERMEABILITY IN THE I-DIRN. FOR PHASE 2 M2
5.0000E-09 PERMEABILITY IN THE J-DIRN. FOR PHASE 2 M2

* POROUS MEDIA INPUTS FOR ZONE 1 *-
IRF

INERTIAL RESISTANCE FACTOR FOR ZONE 1
4.0000E+02 INERTIAL FACTOR IN THE I-DIRN. FOR PHASE 1 M
4.0000E+02 INERTIAL FACTOR IN THE J-DIRN. FOR PHASE 1 M
1.0000E+02 INERTIAL FACTOR IN THE I-DIRN. FOR PHASE 2 M
1.0000E+02 INERTIAL FACTOR IN THE J-DIRN. FOR PHASE 2 M
NO INERTIAL TERM =C2*DEN*Vi*ABSVi 2 ELSE =C2*DEN*Vi*Vmag 2



Example As an example, consider a long narrow channel that is completely
lled with a porous material.

CELL TYPES:
J I= 2 4 6 8 10 12 14 16 18 20
10 W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1 10
9 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 9
8 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 8
7 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 7
6 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 6
5 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 5
4 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 4
3 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 3
2 I1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1*1I2 2
1 W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1W1 1
J I= 2 4 6 8 10 12 14 16 18 20

The duct is initially lled with oil with a density of 800 kg m3 and
a viscosity of 0.01 kg m-sec. At t=0, water is allowed to enter the
domain from the left under the action of a total pressure of 104
Pascals. The water has a density of 1000 kg m3 and a viscosity of
9e-4 kg m-sec. A zero pressure boundary serves as the exit for the
duct on the right.
In this example, the porous media is modeled with a permeability
only. Under these conditions, the source term contribution to the
momentum equation in the porous region has the form:

S = ,v
k
10.3-8
Using permeability values of 5 10,7 m2 for oil and 1 10,8 m2
for water, the transient solution shows the front moving steadily
through the domain Figure 10.3.6.
The velocity is continuous across the interface, but the pressure
drop is not, due to the permeabilities speci ed for the two uids.
10.3.11 Using the VOF Model in Mixing Tank Simulations
There are many industrial applications of mixing tanks involving
impellers and a tank lled partially with liquid. In these cases,
the shape of the liquid surface can be of interest. At low impeller
speeds, the liquid surface will remain at. As the speed increases,
the surface will be pulled downward near the impeller shaft. If the



1.00E+00

5.00E-01

0.00E+00

Y Motion of an Oil-Water Interface through a Porous Region Oct 20 1994

Figure 10.3.6: Motion of an Oil-Water Interface Through a Porous
Region



impeller speed is too great, the surface can break, resulting in the
entrainment of air or other gas from above.
The following model combinations are possible for simulating mix-
ing tanks with impellers in FLUENT:

Time-dependent VOF|with the default donor-acceptor scheme|
and the sliding mesh model described in Section 13.1.
Time-dependent VOF|with either the donor-acceptor or the
implicit interpolation scheme see Section 10.3.2 to determine
which is more appropriate|and the multiple reference frames
model described in Section 12.4.
Time-dependent VOF|with either the donor-acceptor or the
implicit interpolation scheme|and the x option described
in Section 14.16.

If the mixing tank problem includes in ow and out ow boundaries
for the liquid, and a pressure boundary for the air on top of the
tank, the following combinations are possible:

Steady-state VOF and the multiple reference frames model.
Steady-state VOF and the x option.

Using the Sliding In combining the VOF and sliding mesh models, two time-dependent
Mesh Model phenomena must be treated in a compatible manner. The standard
technique to use in the sliding mesh model Chapter 13 is one where
coarse time stepping is done to reach the steady-state, after which
the time step is reduced to obtain a well converged periodic solution.
In combination with the VOF model, coarse time-stepping can lead
to convergence di culties with the volume fraction equation. It is
advisable, therefore, that the impeller grid move no more than two
grid lines per time step in the early stages of the calculation.
Once you have created a 3D grid that represents a section of a mix-
ing tank with one or more impellers, the sliding mesh model requires
a number of inputs in the EXPERT ROTOR-PARAMETERS table. This
table can only be accessed from the SETUP1 menu.
SETUP1 ,! EXPERT ,! ROTOR-PARAMETERS



SETUP1-
EX

EXPERT-
RP

ROTOR PARAMETERS
30 ROTOR ANGULAR VELOCITY RAD S
15 SLIP LINE IN RADIAL DIRECTION
25 SLIP PLANE 1 IN AXIAL DIRECTION
49 SLIP PLANE 2 IN AXIAL DIRECTION
2 NUMBER OF GRID SPACE PER TIME STEP

The inputs to the table are the same that would be used for any
standard sliding-mesh calculation with two exceptions unless you
are interested in modeling the rotor free-surface interaction, which
is discussed below. First, the axial slip planes must not be such
that the free surface interface crosses at any point. Whereas in any
non-VOF simulation the axial slip planes can be anywhere from the
top of the vessel to the bottom with the exception of the boundary
planes themselves, with the VOF model active they must both be
completely contained within one of the uids. Second, the number
of grid lines that the model can traverse within a time step should
not exceed 2. As the solution reaches a periodic steady-state, this
value should be reduced further, as is advised in any sliding-mesh
calculation.
The next step in the setting of the ROTOR-PARAMETERS is the choice
to be made between automatic or manual time-step adjustment. As
with any sliding-mesh calculation, an automatic time-step adjust-
ment is advised, particularly in the early stages of the calculation.

L- AUTOMATIC TIME STEP ADJUSTMENT? NO=MANUAL?
Y
*- ** TIME STEP IS RE-ADJUSTED FOR MOVING MESH **

The nal step is the setting of the TIME-DEPENDENT FLOW SOLUTION
PARAMETERS. As with other VOF simulations, the choice can be
made to use the same global time step for the volume fraction cal-
culation, or use an automatic re nement based upon the maximum
allowable Courant Number at the interface. Since the sliding-mesh



calculation is by nature one in which the ow eld changes with
each time step, it is advisable to choose the automatic re nement
scheme.

TIME DEPENDENT FLOW SOLUTION PARAMETERS
10 MAX. NO. ITNS PER TIME STEP
1.0000E-03 MIN. RESIDUAL SUM DIM
1.3523E-03 SET TIME STEP S
YES SOLVE VOF EVERY ITERATION
YES AUTOMATIC TIME STEP REFINEMENT FOR VOF
2.5000E-01 MAXIMUM COURANT NUMBER FOR VOF DIM
NO AUTOMATIC SAVING
NO ENABLE TIME VARYING GRAVITY VECTOR

At the start of the calculation, it is recommended to request fewer
than the default value of 100 iterations per time step, so as to reach
the steady state condition as quickly as possible. Once the steady
state has been reached, this value should be increased.
Modeling It is possible to use the sliding-mesh model in combination with the
Rotor Free-Surface VOF model to simulate the action of an impeller in a mixing tank
Interaction which is lled only to the level of the impeller. In such instances,
one axial slip plane will be immersed in one uid while the other
will be immersed in the other. A very small time step is required for
this kind of model. You can keep the default entry for the NUMBER
OF GRID SPACE PER TIME STEP prompt in the ROTOR-PARAMETERS
table and request a manual time step adjustment in the question
that follows:

L- AUTOMATIC TIME STEP ADJUSTMENT? NO=MANUAL?
N

You should then choose a small time step in the TIME DEPENDENT
FLOW SOLUTION PARAMETERS table, such that several time steps are
required for the sliding mesh to traverse a typical control volume.
In Figure 10.3.7, a sliding-mesh simulation is illustrated with a par-
tially lled tank. The impeller rotates with an angular speed of 26.4
rad.sec. After roughly a half second, the surface of the water begins
to change shape as a result of the rotation in the liquid phase.



1.00E+00

5.00E-01

0.00E+00

Sliding Mesh Model of a Partially Filled Mixing Tank Nov 07 1994
X

Figure 10.3.7: Sliding-Mesh Model of a Partially Filled Cylindrical
Vessel

Using the Fix If the time-averaged e ects of an impeller are su cient for your
Option model, the FIX-OPTION can be used in place of the sliding mesh
model. With this choice, the velocity components in the vicinity
of the impeller can be xed for the duration of the calculation.
This model, described in detail in Section 14.16, is enabled in the
SOLUTION-PARAMETERS table in the EXPERT menu.
In the example below, a cylindrical vessel is modeled using an ax-
isymmetric grid with 50 23 cells. A central shaft rotates with
an angular velocity of 26.4 rad sec. At the end of the shaft, u,,
v ,, and w , components of velocity are xed to simulate the time-
averaged action of an impeller rotating at the same frequency. At
time t=0, the vessel is half- lled with water. After slightly more
than 1.5 seconds have passed, the surface of the water becomes dis-
torted as shown in Figure 10.3.8, due to the action of the impeller.
Note that the location of the live cells where the xes are applied
for this problem are highlighted by setting these cells to be porous
cells. If the loss factors for these porous cells are not changed from
their default values, the porous cells will function as regular live
cells.



1.00E+00

5.00E-01

0.00E+00

Water in a Mixing Tank Modeled with the Fix Option Nov 07 1994
X

Figure 10.3.8: Water Level in a Mixing Tank Modeled with Velocity
Fixes



10.3.12 Using the VOF Model with Species Mixing
If your model involves the calculation of species mixing or reacting
ow, this can be accomplished in the primary phase uid only. To
set up a model of this type, begin with the Models panel and choose
both the Calculate Species and the VOF Free Surface options.

The next steps are to de ne the phases as well as the species. These
steps can be accomplished in the SETUP1 menu, using the text in-
terface, with the DEFINE-PHASES and DEFINE-SPECIES commands.



SETUP1-
DP
I- ++DEFAULT 1++
1

PHASE NAMES
LIQUID PRIMARY PHASE
AIR PHASE 2

SETUP1-
DS

SPECIES NAMES
NOTE : SPECIES NAMES CANNOT CONSIST OF
OIL-A SPECIES 1
OIL-B SPECIES 2

You can also use the graphical user interface to name the species. In
the De ne pull-down menu, choose Species.... The resulting De ne
Species panel can be edited to name the species.



Note that the setup of multiple phases and multiple species can be
done entirely with the text interface, if you prefer. The setup of the
multiple phases is illustrated in Section 10.3; the additional setup of
species is shown below. Begin by selecting SPECIES-AND-CHEMISTRY
from the DEFINE-MODELS menu.
SETUP1 ,! DEFINE-MODELS ,! SPECIES-AND-CHEMISTRY



SETUP1-
DM

COMMANDS AVAILABLE FROM DEFINE-MODELS:
W-VELOCITY HEAT-TRANSFER TURBULENCE
RADIATION SPECIES-AND-CHEMISTRY MULTIPLE-PHASES
QUIT HELP
DEFINE-MODELS-
SP

CHEMISTRY MODEL SELECT ONLY ONE
YES NON-REACTING SPECIES
NO FINITE RATE REACTIONS
NO PDF DIFFUSION
NO PREMIXED FRONT TRACKING

After choosing between reacting and non-reacting ow options, set
the number of species, and then name them.



COMMANDS AVAILABLE FROM NON-REACTING SPECIES:
NUMBER-OF-SPECIES DEFINE-SPECIES QUIT
HELP
NON-REACTING SPECIES-
NU

SPECIES
2 TOTAL NUMBER OF CHEMICAL SPECIES
NO ENABLE MOLE FRACTION INPUTS OTHERWISE MASS FRACTION

COMMANDS AVAILABLE FROM NON-REACTING SPECIES:
NUMBER-OF-SPECIES DEFINE-SPECIES QUIT
HELP
NON-REACTING SPECIES-
DE

SPECIES NAMES
NOTE : SPECIES NAMES CANNOT CONSIST OF
OIL-A SPECIES 1
OIL-B SPECIES 2

Setting the To set the properties, commands in the PHYSICAL-CONSTANTS menu
Properties are used in the usual manner. The following dialogue illustrates the
setting of the density when the gas law is not in use.

PHYSICAL-CONSTANTS-
DE

PHASE-SELECTION-
LIQ
L- USE GAS LAW FOR LIQUID?
N

COMMANDS AVAILABLE FROM SPECIES-SELECTION:
OIL-A OIL-B QUIT HELP
SPECIES-SELECTION-



As with any problem involving species mixing, a menu appears con-
taining the species names. The densities for each are set by selecting
each species in turn.

SPECIES-SELECTION-
OIL-A
R- DENSITY OF OIL-A
800

COMMANDS AVAILABLE FROM SPECIES-SELECTION:
OIL-A OIL-B QUIT HELP
SPECIES-SELECTION-
OIL-B
R- DENSITY OF OIL-B
810

Once the species densities are set, you can QUIT from the
SPECIES-SELECTION menu and set the density of the second phase.

SPECIES-SELECTION-
Q

PHASE-SELECTION-
AIR
R- DENSITY OF AIR
1.0

The gas law can only be used in the primary phase, which means
that species mixing in combination with the gas law can only be
done when the species are a part of the gaseous phase. In this
event, the setting of the density proceeds as it normally does when
the gas law is elected with multiple species. The dialogue is followed
by input of the density for the second phase, as shown above.
The viscosity is set in the usual way. By default, you will need to
de ne the viscosity of each of the phases.



PHYSICAL-CONSTANTS-
VI

PHASE-SELECTION-
LIQ
R- VISCOSITY OF LIQUID
X
R- DEFAULT ASSUMED

PHASE-SELECTION-
AIR
R- VISCOSITY OF AIR
X
R- DEFAULT ASSUMED

Note that if you want to set the viscosity for each of the species indi-
vidually, you need to enable the COMPOSITION DEPENDENT VISCOSITY
option in the PROPERTY-OPTIONS table.
The setting of other properties, such as thermal conductivity and
speci c heat, is done in a manner similar to that shown for the
viscosity.
Setting the The boundary conditions are set for the phases and species in the
Boundary same manner as when only one of these models is active. For ex-
Conditions ample, consider the setting of boundary conditions at an inlet. To
set the VOLUME-FRACTION, you only need to specify it for the second
phase if it is not zero, the default value.

SETUP1-
BC I 1

COMMANDS AVAILABLE FROM I1-ZONE-BOUNDARY-CONDITIONS:
CHEMICAL-SPECIES NORMAL-VELOCITY U-VELOCITY
V-VELOCITY VOLUME-FRACTION QUIT
HELP
VF
R- VOLUME FRACTION OF AIR
0



To set the CHEMICAL-SPECIES you need to specify the value of the
rst species named for this example. If you have N species, you
will have to set all non-zero values for the rst N-1 species.

CS
R- OIL-A MASS FRACTION
.5

Boundary conditions may also be set in the Boundary Conditions
panel. Choose the boundary from the Active Zones list and click
the Set... button. The Phase information is set in the resulting
boundary conditions panel, as shown below.



To set the species, click on the Species... button, and provide the
inputs to the chemical species panel.

10.3.13 Postprocessing with the VOF Model
Postprocessing with the VOF model includes the display of the vol-
ume fractions of the phases, as well as integral reports that are
relative to a single phase at a time. These features are discussed in
this section.
Display of the The volume fraction of the primary or one of the secondary phases
Volume Fraction may be examined using alphanumerics or graphically using con-
tours, lled contours, or pro les. As an example, consider a bowl
which is partially lled with water and spinning on its axis. To
request a display of the volume fraction of water, begin with the
Display pull-down menu and select the Contours... item. In the
Contours panel, choose Multiphase in the Contours Of box. To select
lled contours, click on the Filled check button. Note that WATER
is the current selection from the Phase drop-down list so does not
need to be changed. The default number of Contour Levels is 30.
For a crisp display of the interface, it is best to choose 2 levels
instead.



The resulting gure, shown in Figure 10.3.9 has been mirrored about
the y-min boundary, rotated about the z axis, and reduced in size
to t in the graphics window.
Note that the air-water interface occurs at a value of 2 = 0.5, which
is a common practice in the viewing of volume fraction results. The
maximum is light in color and the minimum is dark in this gure.
Had AIR been chosen from the Phase drop-down list on the Contours
panel, the colors would be switched Figure 10.3.10.
Alphanumeric Alphanumeric reporting is available from the *MAIN* menu using
Reporting the VIEW-ALPHA command. Once in the VIEW-ALPHA menu, the
SELECT-VARIABLE command results in a large selection of variables
from which to choose. The VOLUME-FRACTION command results in
the display of one phase at a time, which you can choose from the
PHASE-SELECTION menu.



1.00E+00

5.00E-01

0.00E+00

Water in a Spinning Bowl Oct 26 1994
X

Figure 10.3.9: Volume Fraction of Water

1.00E+00

5.00E-01

0.00E+00

Water in a Spinning Bowl Oct 26 1994
Z Y Air Volume Fraction (Dim) Fluent 4.30
X

Figure 10.3.10: Volume Fraction of Air



VIEW-ALPHANUMERICS-
SV

COMMANDS AVAILABLE FROM VARIABLE-SELECTION:
DENSITY EXCHANGE-MASS
EXCHANGE-X EXCHANGE-Y
MASS-FRACTION MOLE-FRACTION
MOLECULAR-VISCOSITY STATIC-PRESSURE-REL
STATIC-PRESSURE-ABS STREAM-FUNCTION
SURFACE-MASS-FLUX TOTAL-PRESSURE-REL
TOTAL-PRESSURE-ABS U-VELOCITY
V-VELOCITY VELOCITY-MAGNITUDE
VOLUME-FRACTION XMOM-SOURCE
YMOM-SOURCE INTEGRALS-I-DIRECTION
INTEGRALS-J-DIRECTION INTEGRAL-RANGES
WALL-FORCES XTENDED-XOPTIONS
QUIT HELP
VARIABLE-SELECTION-
VF

AIR WATER QUIT HELP
PHASE-SELECTION-
AIR

VIEW ALPHA: AIR VOLUME FRACTION DIM AT TIME T = 5.000E-01
J I= 1 2 3 4 5 6
33 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00
32 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00
31 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00
30 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00
29 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00 1.00E+00
. . . . . . .
. . . . . . .
. . . . . . .

Integral reports are also available for a single phase at a time. For
example, to examine the I-direction integrals for the top surface of
the cup, where only air is present, the corresponding inlet zone is
chosen, and AIR is chosen from the PHASE-SELECTION menu.


Chapter 10. VOF Free Surface Model

More Related Content

What's hot

Viewers also liked

Similar to Chapter 10. VOF Free Surface Model

Recently uploaded

Chapter 10. VOF Free Surface Model