Chapter 20. General Multiphase Models

Transcription

Chapter 20.
Models
General Multiphase
This chapter discusses the general multiphase models that are available
in FLUENT. Chapter 18 provides a brief introduction to multiphase modeling, Chapter 19 discusses the Lagrangian dispersed phase model, and
Chapter 21 describes FLUENT’s model for solidification and melting.
• Section 20.1: Choosing a General Multiphase Model
• Section 20.2: Volume of Fluid (VOF) Model
• Section 20.3: Mixture Model
• Section 20.4: Eulerian Model
• Section 20.5: Cavitation Effects
• Section 20.6: Setting Up a General Multiphase Problem
• Section 20.7: Solution Strategies for General Multiphase Problems
• Section 20.8: Postprocessing for General Multiphase Problems
20.1
Choosing a General Multiphase Model
As discussed in Section 18.4, the VOF model is appropriate for stratified
or free-surface flows, and the mixture and Eulerian models are appropriate for flows in which the phases mix or separate and/or dispersed-phase
volume fractions exceed 10%. (Flows in which the dispersed-phase volume fractions are less than or equal to 10% can be modeled using the
discrete phase model described in Chapter 19.)
To choose between the mixture model and the Eulerian model, you
should consider the following, in addition to the detailed guidelines in
Section 18.4:
c Fluent Inc. November 28, 2001
20-1
General Multiphase Models
• If there is a wide distribution of the dispersed phases, the mixture
model may be preferable. If the dispersed phases are concentrated
just in portions of the domain, you should use the Eulerian model
instead.
• If interphase drag laws that are applicable to your system are
available (either within FLUENT or through a user-defined function), the Eulerian model can usually provide more accurate results
than the mixture model. If the interphase drag laws are unknown
or their applicability to your system is questionable, the mixture
model may be a better choice.
• If you want to solve a simpler problem, which requires less computational effort, the mixture model may be a better option, since
it solves a smaller number of equations than the Eulerian model.
If accuracy is more important than computational effort, the Eulerian model is a better choice. Keep in mind, however, that the
complexity of the Eulerian model can make it less computationally
stable than the mixture model.
Brief overviews of the three models, including their limitations, are provided in Sections 20.1.1, 20.1.2, and 20.1.3. Detailed descriptions of the
models are provided in Sections 20.2, 20.3, and 20.4.
20.1.1
Overview and Limitations of the VOF Model
Overview
The VOF model can model two or more immiscible fluids by solving a
single set of momentum equations and tracking the volume fraction of
each of the fluids throughout the domain. Typical applications include
the prediction of jet breakup, the motion of large bubbles in a liquid, the
motion of liquid after a dam break, and the steady or transient tracking
of any liquid-gas interface.
Limitations
The following restrictions apply to the VOF model in FLUENT:
20-2
20.1 Choosing a General Multiphase Model
• You must use the segregated solver. The VOF model is not available with either of the coupled solvers.
• All control volumes must be filled with either a single fluid phase
or a combination of phases; the VOF model does not allow for void
regions where no fluid of any type is present.
• Only one of the phases can be compressible.
• Streamwise periodic flow (either specified mass flow rate or specified pressure drop) cannot be modeled when the VOF model is
used.
• Species mixing and reacting flow cannot be modeled when the VOF
model is used.
• The LES turbulence model cannot be used with the VOF model.
• The second-order implicit time-stepping formulation cannot be used
with the VOF model.
• The VOF model cannot be used for inviscid flows.
• The shell conduction model for walls cannot be used with the VOF
model.
Steady-State and Transient VOF Calculations
The VOF formulation in FLUENT is generally used to compute a timedependent solution, 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 inflow 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
fluid, such a problem must be solved using the time-dependent formulation. On the other hand, the flow 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.
20-3
20.1.2
Overview and Limitations of the Mixture Model
Overview
The mixture model is a simplified multiphase model that can be used to
model multiphase flows where the phases move at different velocities, but
assume local equilibrium over short spatial length scales. The coupling
between the phases should be strong. It can also be used to model
homogeneous multiphase flows with very strong coupling and the phases
moving at the same velocity.
The mixture model can model n phases (fluid or particulate) by solving the momentum, continuity, and energy equations for the mixture,
the volume fraction equations for the secondary phases, and algebraic
expressions for the relative velocities. Typical applications include sedimentation, cyclone separators, particle-laden flows with low loading, and
bubbly flows where the gas volume fraction remains low.
The mixture model is a good substitute for the full Eulerian multiphase
model in several cases. A full multiphase model may not be feasible
when there is a wide distribution of the particulate phase or when the
interphase laws are unknown or their reliability can be questioned. A
simpler model like the mixture model can perform as well as a full multiphase model while solving a smaller number of variables than the full
multiphase model.
Limitations
The following limitations apply to the mixture model in FLUENT:
• You must use the segregated solver. The mixture model is not
available with either of the coupled solvers.
• Only one of the phases can be compressible.
• Streamwise periodic flow (either specified mass flow rate or specified pressure drop) cannot be modeled when the mixture model is
used.
20-4
• Species mixing and reacting flow cannot be modeled when the mixture model is used.
• Solidification and melting cannot be modeled in conjunction with
the mixture model.
• The LES turbulence model cannot be used with the mixture model.
with the mixture model.
• The mixture model cannot be used for inviscid flows.
• The shell conduction model for walls cannot be used with the mixture model.
20.1.3
Overview and Limitations of the Eulerian Model
Overview
The Eulerian multiphase model in FLUENT allows for the modeling of
multiple separate, yet interacting phases. The phases can be liquids,
gases, or solids in nearly any combination. An Eulerian treatment is
used for each phase, in contrast to the Eulerian-Lagrangian treatment
that is used for the discrete phase model.
With the Eulerian multiphase model, the number of secondary phases
is limited only by memory requirements and convergence behavior. Any
number of secondary phases can be modeled, provided that sufficient
memory is available. For complex multiphase flows, however, you may
find that your solution is limited by convergence behavior. See Section 20.7.3 for multiphase modeling strategies.
FLUENT’s Eulerian multiphase model differs from the Eulerian model in
FLUENT 4 in that there is no global distinction between fluid-fluid and
fluid-solid (granular) multiphase flows. A granular flow is simply one
that involves at least one phase that has been designated as a granular
phase.
The FLUENT solution is based on the following:
20-5
• A single pressure is shared by all phases.
• Momentum and continuity equations are solved for each phase.
• The following parameters are available for granular phases:
– Granular temperature (solids fluctuating energy) can be calculated for each solid phase. This is based on an algebraic
relation.
– Solid-phase shear and bulk viscosities are obtained from application of kinetic theory to granular flows. Frictional viscosity
is also available.
• Several interphase drag coefficient functions are available, which
are appropriate for various types of multiphase regimes. (You can
also modify the interphase drag coefficient through user-defined
functions, as described in the separate UDF Manual.)
• All of the k- turbulence models are available, and may apply to
all phases or to the mixture.
Limitations
All other features available in FLUENT can be used in conjunction with
the Eulerian multiphase model, except for the following limitations:
• Only the k- models can be used for turbulence.
• Particle tracking (using the Lagrangian dispersed phase model)
interacts only with the primary phase.
• Streamwise periodic flow (either specified mass flow rate or specified pressure drop) cannot be modeled when the Eulerian model is
used.
• Compressible flow is not allowed.
• Inviscid flow is not allowed.
with the Eulerian model.
20-6
• Melting and solidification are not allowed.
• Species transport and reactions are not allowed.
• Heat transfer cannot be modeled.
• The only type of mass transfer between phases that is allowed is
cavitation; evaporation, condensation, etc. are not allowed.
Stability and Convergence
The process of solving a multiphase system is inherently difficult, and
you may encounter some stability or convergence problems, although
the current algorithm is more stable than that used in FLUENT 4. If
a time-dependent problem is being solved, and patched fields are used
for the initial conditions, it is recommended that you perform a few
iterations with a small time step, at least an order of magnitude smaller
than the characteristic time of the flow. You can increase the size of the
time step after performing a few time steps. For steady solutions it is
recommended that you start with a small under-relaxation factor for the
volume fraction.
Stratified flows of immiscible fluids should be solved with the VOF model
(see Section 20.2). Some problems involving small volume fractions can
be solved more efficiently with the Lagrangian discrete phase model (see
Chapter 19).
Many stability and convergence problems can be minimized if care is
taken during the setup and solution processes (see Section 20.7.3).
20-7
20.2
Volume of Fluid (VOF) Model
The VOF formulation relies on the fact that two or more fluids (or
phases) are not interpenetrating. For each additional phase that you
add to your model, a variable is introduced: the volume fraction of the
phase in the computational cell. In each control volume, the volume
fractions of all phases sum to unity. The fields for all variables and properties are shared by the phases and represent volume-averaged values,
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 representative of a mixture of the phases, depending upon the volume fraction values. In other
words, if the qth fluid’s volume fraction in the cell is denoted as αq , then
the following three conditions are possible:
• αq = 0: the cell is empty (of the qth fluid).
• αq = 1: the cell is full (of the qth fluid)
• 0 < αq < 1: the cell contains the interface between the qth fluid
and one or more other fluids.
Based on the local value of αq , the appropriate properties and variables
will be assigned to each control volume within the domain.
20.2.1
The Volume Fraction Equation
The tracking of the interface(s) between the phases is accomplished by
the solution of a continuity equation for the volume fraction of one (or
more) of the phases. For the qth phase, this equation has the following
form:
Sα
∂αq
+ ~v · ∇αq = q
∂t
ρq
(20.2-1)
By default, the source term on the right-hand side of Equation 20.2-1 is
zero, but you can specify a constant or user-defined mass source for each
phase.
20-8
20.2 Volume of Fluid (VOF) Model
The volume fraction equation will not be solved for the primary phase;
the primary-phase volume fraction will be computed based on the following constraint:
n
X
αq = 1
(20.2-2)
q=1
20.2.2
Properties
The properties appearing in the transport equations are determined by
the presence of the component phases in each control volume. In a twophase 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
ρ = α2 ρ2 + (1 − α2 )ρ1
(20.2-3)
In general, for an n-phase system, the volume-fraction-averaged density
takes on the following form:
ρ=
X
αq ρq
(20.2-4)
All other properties (e.g., viscosity) are computed in this manner.
20.2.3
The Momentum Equation
A single momentum equation is solved throughout the domain, and the
resulting velocity field is shared among the phases. The momentum
equation, shown below, is dependent on the volume fractions of all phases
through the properties ρ and µ.
h i
∂
(ρ~v ) + ∇ · (ρ~v~v ) = −∇p + ∇ · µ ∇~v + ∇~v T + ρ~g + F~
∂t
(20.2-5)
20-9
One limitation of the shared-fields approximation is that in cases where
large velocity differences exist between the phases, the accuracy of the
velocities computed near the interface can be adversely affected.
20.2.4
The Energy Equation
The energy equation, also shared among the phases, is shown below.
∂
(ρE) + ∇ · (~v (ρE + p)) = ∇ · (keff ∇T ) + Sh
∂t
(20.2-6)
The VOF model treats energy, E, and temperature, T , as mass-averaged
variables:
n
X
E=
αq ρq Eq
q=1
n
X
(20.2-7)
αq ρq
q=1
where Eq for each phase is based on the specific heat of that phase and
the shared temperature.
The properties ρ and keff (effective thermal conductivity) are shared by
the phases. The source term, Sh , contains contributions from radiation,
as well as any other volumetric heat sources.
As with the velocity field, the accuracy of the temperature near the interface is limited in cases where large temperature differences exist between
the phases. Such problems 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
differ by as much as four orders of magnitude. Such large discrepancies
in properties lead to equation sets with anisotropic coefficients, which in
turn can lead to convergence and precision limitations.
20-10
20.2.5
Additional Scalar Equations
Depending upon your problem definition, additional scalar equations
may be involved in your solution. In the case of turbulence quantities,
a single set of transport equations is solved, and the turbulence variables (e.g., k and or the Reynolds stresses) are shared by the phases
throughout the field.
20.2.6
Interpolation Near the Interface
FLUENT’s control-volume formulation requires that convection and diffusion fluxes through the control volume faces be computed and balanced with source terms within the control volume itself. There are four
schemes in FLUENT for the calculation of face fluxes for the VOF model:
geometric reconstruction, donor-acceptor, Euler explicit, and implicit.
In the geometric reconstruction and donor-acceptor schemes,
applies a special interpolation treatment to the cells that lie
interface between two phases. Figure 20.2.1 shows an actual
shape along with the interfaces assumed during computation
two methods.
FLUENT
near the
interface
by these
The Euler explicit scheme and the implicit scheme treat these cells with
the same interpolation as the cells that are completely filled with one
phase or the other (i.e., using the standard upwind, second-order, or
QUICK scheme), rather than applying a special treatment.
The Geometric Reconstruction Scheme
In the geometric reconstruction approach, the standard interpolation
schemes that are used in FLUENT are used to obtain the face fluxes
whenever a cell is completely filled with one phase or another. When the
cell is near the interface between two phases, the geometric reconstruction scheme is used.
The geometric reconstruction scheme represents the interface between
fluids using a piecewise-linear approach. In FLUENT this scheme is the
most accurate and is applicable for general unstructured meshes. The
geometric reconstruction scheme is generalized for unstructured meshes
20-11
actual interface shape
interface shape represented by
the geometric reconstruction
(piecewise-linear) scheme
interface shape represented by
the donor-acceptor scheme
Figure 20.2.1: Interface Calculations
20-12
from the work of Youngs [273]. It assumes that the interface between
two fluids has a linear slope within each cell, and uses this linear shape
for calculation of the advection of fluid through the cell faces. (See
Figure 20.2.1.)
The first step in this reconstruction scheme is calculating the position
of the linear interface relative to the center of each partially-filled cell,
based on information about the volume fraction and its derivatives in
the cell. The second step is calculating the advecting amount of fluid
through each face using the computed linear interface representation and
information about the normal and tangential velocity distribution on the
face. The third step is calculating the volume fraction in each cell using
the balance of fluxes calculated during the previous step.
! When the geometric reconstruction scheme is used, a time-dependent
solution must be computed. Also, if you are using a conformal grid
(i.e., if the grid node locations are identical at the boundaries where two
subdomains meet), you must ensure that there are no two-sided (zerothickness) walls within the domain. If there are, you will need to slit
them, as described in Section 5.7.8.
The Donor-Acceptor Scheme
In the donor-acceptor approach, the standard interpolation schemes that
are used in FLUENT are used to obtain the face fluxes whenever a cell
is completely filled 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 fluid advected through the face [93]. This
scheme identifies one cell as a donor of an amount of fluid from one phase
and another (neighbor) cell as the acceptor of that same amount of fluid,
and is used to prevent numerical diffusion at the interface. The amount
of fluid from one phase that can be convected across a cell boundary is
limited by the minimum of two values: the filled 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 fluxes.
The interface orientation is either horizontal or vertical, depending on
the direction of the volume fraction gradient of the qth phase within
the cell, and that of the neighbor cell that shares the face in question.
20-13
Depending on the interface’s orientation as well as its motion, flux values
are obtained by pure upwinding, pure downwinding, or some combination
of the two.
! When the donor-acceptor scheme is used, a time-dependent solution
must be computed. Also, the donor-acceptor scheme can be used only
with quadrilateral or hexahedral meshes. In addition, if you are using a
conformal grid (i.e., if the grid node locations are identical at the boundaries where two subdomains meet), you must ensure that there are no
two-sided (zero-thickness) walls within the domain. If there are, you will
need to slit them, as described in Section 5.7.8.
The Euler Explicit Scheme
In the Euler explicit approach, FLUENT’s standard finite-difference interpolation schemes are applied to the volume fraction values that were
computed at the previous time step.
X
αn+1
− αnq
q
(Ufn αnq,f ) = 0
V +
∆t
f
where
n+1
n
αq,f
=
=
=
V
Uf
=
=
(20.2-8)
index for new (current) time step
index for previous time step
face value of the qth volume fraction, computed
from the first- or second-order upwind or
QUICK scheme
volume of cell
volume flux through the face, based on
normal velocity
This formulation does not require iterative solution of the transport equation during each time step, as is needed for the implicit scheme.
! When the Euler explicit scheme is used, a time-dependent solution must
be computed.
20-14
The Implicit Scheme
In the implicit interpolation method, FLUENT’s standard finite-difference
interpolation schemes are used to obtain the face fluxes for all cells, including those near the interface.
X
αn+1
− αnq
q
(Ufn+1 αn+1
V +
q,f ) = 0
∆t
f
(20.2-9)
Since this equation requires the volume fraction values at the current
time step (rather than at the previous step, as for the Euler explicit
scheme), a standard scalar transport equation is solved iteratively for
each of the secondary-phase volume fractions at each time step.
The implicit scheme can be used for both time-dependent and steadystate calculations. See Section 20.6.4 for details.
20.2.7
Time Dependence
For time-dependent VOF calculations, Equation 20.2-1 is solved using an
explicit time-marching scheme. FLUENT automatically refines the time
step for the integration of the volume fraction equation, but you can
influence this time step calculation by modifying the Courant number.
You can choose to 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 Section 20.6.12.
20.2.8
Surface Tension and Wall Adhesion
The VOF model can also include the effects of surface tension along the
interface between each pair of phases. The model can be augmented by
the additional specification of the contact angles between the phases and
the walls.
Surface Tension
Surface tension arises as a result of attractive forces between molecules
in a fluid. Consider an air bubble in water, for example. Within the
20-15
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
effect 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 fluids are separated, but one of them is not in the form
of spherical bubbles, the surface tension acts to minimize free energy by
decreasing the area of the interface.
The surface tension model in FLUENT is the continuum surface force
(CSF) model proposed by Brackbill et al. [25]. With this model, the
addition of surface tension to the VOF calculation results in a source
term in 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 coefficient, σ, and the surface curvature
as measured by two radii in orthogonal directions, R1 and R2 :
1
1
p2 − p1 = σ
+
R1 R2
(20.2-10)
where p1 and p2 are the pressures in the two fluids on either side of the
interface.
In FLUENT, a formulation of CSF model is used, where the surface curvature is computed from local gradients in the surface normal at the
interface. Let n be the surface normal, defined as the gradient of αq , the
volume fraction of the qth phase.
n = ∇αq
(20.2-11)
The curvature, κ, is defined in terms of the divergence of the unit normal,
n̂ [25]:
20-16
κ = ∇ · n̂
(20.2-12)
where
n̂ =
n
|n|
(20.2-13)
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:
Fvol =
X
σij
pairs ij, i<j
αi ρi κj ∇αj + αj ρj κi ∇αi
1
2 (ρi + ρj )
(20.2-14)
This expression allows for a smooth superposition of forces near cells
where more than two phases are present. If only two phases are present in
a cell, then κi = −κj and ∇αi = −∇αj , and Equation 20.2-14 simplifies
to
Fvol = σij
1
2
ρκi ∇αi
(ρi + ρj )
(20.2-15)
where ρ is the volume-averaged density computed using Equation 20.2-4.
Equation 20.2-15 shows that the surface tension source term for a cell is
proportional to the average density in the cell.
Note that the calculation of surface tension effects on triangular and
tetrahedral meshes is not as accurate as on quadrilateral and hexahedral
meshes. The region where surface tension effects are most important
should therefore be meshed with quadrilaterals or hexahedra.
When Surface Tension Effects are Important
The importance of surface tension effects is determined based on the
value of two dimensionless quantities: the Reynolds number, Re, and
20-17
the capillary number, Ca; or the Reynolds number, Re, and the Weber number, We. For Re 1, the quantity of interest is the capillary
number:
Ca =
µU
σ
(20.2-16)
and for Re 1, the quantity of interest is the Weber number:
We =
σ
ρLU 2
(20.2-17)
where U is the free-stream velocity. Surface tension effects can be neglected if Ca 1 or We 1.
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. [25]. Rather than impose this
boundary condition at the wall itself, the contact angle that the fluid 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 θw is the contact angle at the wall, then the surface normal at the live
cell next to the wall is
n̂ = n̂w cos θw + t̂w sin θw
(20.2-18)
where n̂w and t̂w 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.
The contact angle θw is the angle between the wall and the tangent to
the interface at the wall, measured inside the first phase of the pair listed
in the Wall panel, as shown in Figure 20.2.2.
20-18
second phase
interface
θw
first phase
wall
Figure 20.2.2: Measuring the Contact Angle
20-19
20.3
Mixture Model
The mixture model, like the VOF model, uses a single-fluid approach.
It differs from the VOF model in two respects:
• The mixture model allows the phases to be interpenetrating. The
volume fractions αq and αp for a control volume can therefore be
equal to any value between 0 and 1, depending on the space occupied by phase q and phase p.
• The mixture model allows the phases to move at different velocities,
using the concept of slip velocities. (Note that the phases can also
be assumed to move at the same velocity, and the mixture model
is then reduced to a homogeneous multiphase model.)
The mixture model solves the continuity equation for the mixture, the
momentum equation for the mixture, the energy equation for the mixture, and the volume fraction equation for the secondary phases, as well
as algebraic expressions for the relative velocities (if the phases are moving at different velocities).
20.3.1
Continuity Equation for the Mixture
The continuity equation for the mixture is
∂
(ρm ) + ∇ · (ρm~vm ) = ṁ
∂t
(20.3-1)
where ~vm is the mass-averaged velocity:
Pn
~vm =
vk
k=1 αk ρk ~
ρm
(20.3-2)
and ρm is the mixture density:
ρm =
n
X
αk ρk
(20.3-3)
k=1
20-20
20.3 Mixture Model
αk is the volume fraction of phase k.
ṁ represents mass transfer due to cavitation (described in Section 20.5)
or user-defined mass sources.
20.3.2
Momentum Equation for the Mixture
The momentum equation for the mixture can be obtained by summing
the individual momentum equations for all phases. It can be expressed
as
h
i
∂
T
+
(ρm~vm ) + ∇ · (ρm~vm~vm ) = −∇p + ∇ · µm ∇~vm + ∇~vm
∂t
ρm~g + F~ + ∇ ·
n
X
!
αk ρk~vdr,k~vdr,k
(20.3-4)
k=1
where n is the number of phases, F~ is a body force, and µm is the
viscosity of the mixture:
µm =
n
X
αk µk
(20.3-5)
k=1
~vdr,k is the drift velocity for secondary phase k:
~vdr,k = ~vk − ~vm
20.3.3
(20.3-6)
Energy Equation for the Mixture
The energy equation for the mixture takes the following form:
n
n
X
∂ X
(αk ρk Ek ) + ∇ ·
(αk ~vk (ρk Ek + p)) = ∇ · (keff ∇T ) + SE (20.3-7)
∂t k=1
k=1
where keff is the effective conductivity (k + kt , where kt is the turbulent
thermal conductivity, defined according to the turbulence model being
20-21
used). The first term on the right-hand side of Equation 20.3-7 represents
energy transfer due to conduction. SE includes any other volumetric heat
sources.
In Equation 20.3-7,
Ek = hk −
p
v2
+ k
ρk
2
(20.3-8)
for a compressible phase, and Ek = hk for an incompressible phase,
where hk is the sensible enthalpy for phase k.
20.3.4
Relative (Slip) Velocity and the Drift Velocity
The relative velocity (also referred to as the slip velocity) is defined as the
velocity of a secondary phase (p) relative to the velocity of the primary
phase (q):
~vqp = ~vp − ~vq
(20.3-9)
The drift velocity and the relative velocity (~vqp ) are connected by the
following expression:
~vdr,p = ~vqp −
n
X
αk ρk
k=1
ρm
~vqk
(20.3-10)
FLUENT’s mixture model makes use of an algebraic slip formulation. The
basic assumption of the algebraic slip mixture model is that, to prescribe
an algebraic relation for the relative velocity, a local equilibrium between
the phases should be reached over short spatial length scales. The form
of the relative velocity is given by
~vqp = τqp~a
(20.3-11)
where ~a is the secondary-phase particle’s acceleration and τqp is the particulate relaxation time. Following Manninen et al. [150] τqp is of the
form:
20-22
20.3 Mixture Model
τqp =
(ρm − ρp )d2p
18µq fdrag
(20.3-12)
where dp is the diameter of the particles (or droplets or bubbles) of
secondary phase p, and the drag function fdrag is taken from Schiller
and Naumann [202]:
(
fdrag =
1 + 0.15Re0.687 Re ≤ 1000
0.0183Re
Re > 1000
(20.3-13)
and the acceleration ~a is of the form
~a = ~g − (~vm · ∇)~vm −
∂~vm
∂t
(20.3-14)
The simplest algebraic slip formulation is the so-called drift flux model,
in which the acceleration of the particle is given by gravity and/or a
centrifugal force and the particulate relaxation time is modified to take
into account the presence of other particles.
Note that, if the slip velocity is not solved, the mixture model is reduced
to a homogeneous multiphase model. In addition, the mixture model can
be customized (using user-defined functions) to use a formulation other
than the algebraic slip method for the slip velocity. See the separate
UDF Manual for details.
20.3.5
Volume Fraction Equation for the Secondary Phases
From the continuity equation for secondary phase p, the volume fraction
equation for secondary phase p can be obtained:
∂
(αp ρp ) + ∇ · (αp ρp~vm ) = −∇ · (αp ρp~vdr,p )
∂t
(20.3-15)
20-23
20.4
Eulerian Model
To change from a single-phase model, where a single set of conservation equations for momentum and continuity is solved, to a multiphase
model, additional sets of conservation equations must be introduced. In
the process of introducing additional sets of conservation equations, the
original set must also be modified. The modifications involve, among
other things, the introduction of the volume fractions α1 , α2 , . . . αn for
the multiple phases, as well as a mechanism for the exchange of momentum between the phases.
Details about the Eulerian multiphase model are presented in the following subsections:
• Section 20.4.1: Volume Fractions
• Section 20.4.2: Conservation Equations
• Section 20.4.3: Interphase Exchange Coefficients
• Section 20.4.4: Solids Pressure
• Section 20.4.5: Solids Shear Stresses
• Section 20.4.6: Granular Temperature
• Section 20.4.7: Turbulence Models
• Section 20.4.8: Solution Method in FLUENT
20.4.1
Volume Fractions
The description of multiphase flow as interpenetrating continua incorporates the concept of phasic volume fractions, denoted here by αq . Volume fractions represent the space occupied by each phase, and the laws
of conservation of mass and momentum are satisfied by each phase individually. The derivation of the conservation equations can be done
by ensemble averaging the local instantaneous balance for each of the
phases [3] or by using the mixture theory approach [22].
The volume of phase q, Vq , is defined by
20-24
20.4 Eulerian Model
Z
Vq =
αq dV
(20.4-1)
V
where
n
X
αq = 1
(20.4-2)
ρ̂q = αq ρq
(20.4-3)
q=1
The effective density of phase q is
where ρq is the physical density of phase q.
20.4.2
Conservation Equations
The general conservation equations from which the equations solved by
FLUENT are derived are presented in this section, followed by the solved
equations themselves.
Equations in General Form
Conservation of Mass
The continuity equation for phase q is
n
X
∂
ṁpq
(αq ρq ) + ∇ · (αq ρq ~vq ) =
∂t
p=1
(20.4-4)
where ~vq is the velocity of phase q and ṁpq characterizes the mass transfer
from the pth to q th phase. From the mass conservation one can obtain
ṁpq = −ṁqp
(20.4-5)
and
20-25
ṁpp = 0
(20.4-6)
Conservation of Momentum
The momentum balance for phase q yields
n
X
∂
~ pq + ṁpq~vpq ) +
(R
(αq ρq ~vq ) + ∇ · (αq ρq~vq~vq ) = −αq ∇p + ∇ · τ q +
∂t
p=1
αq ρq (F~q + F~lift,q + F~vm,q )
(20.4-7)
where τ q is the q th phase stress-strain tensor
2
τ q = αq µq (∇~vq + ∇~vqT ) + αq (λq − µq )∇ · ~vq I
3
(20.4-8)
Here µq and λq are the shear and bulk viscosity of phase q, F~q is an
external body force, F~lift,q is a lift force, F~vm,q is a virtual mass force,
~ pq is an interaction force between phases, and p is the pressure shared
R
by all phases.
~vpq is the interphase velocity, defined as follows. If ṁpq > 0 (i.e., phase
p mass is being transferred to phase q), ~vpq = ~vp ; if ṁpq < 0 (i.e., phase
q mass is being transferred to phase p), ~vpq = ~vq ; and ~vpq = ~vqp .
Equation 20.4-7 must be closed with appropriate expressions for the in~ pq . This force depends on the friction, pressure, cohesion,
terphase force R
~ pq = −R
~ qp and
and other effects, and is subject to the conditions that R
~
Rqq = 0.
FLUENT uses a simple interaction term of the following form:
n
X
p=1
~ pq =
R
n
X
Kpq (~vp − ~vq )
(20.4-9)
p=1
where Kpq (= Kqp ) is the interphase momentum exchange coefficient
(described in Section 20.4.3).
20-26
20.4 Eulerian Model
Lift Forces
For multiphase flows, FLUENT can include the effect of lift forces on
the secondary phase particles (or droplets or bubbles). These lift forces
act on a particle mainly due to velocity gradients in the primary-phase
flow field. The lift force will be more significant for larger particles, but
the FLUENT model assumes that the particle diameter is much smaller
than the interparticle spacing. Thus, the inclusion of lift forces is not
appropriate for closely packed particles or for very small particles.
The lift force acting on a secondary phase p in a primary phase q is
computed from [57]
Flift = −0.5ρq αp |~vq − ~vp | × (∇ × ~vq )
(20.4-10)
The lift force Flift will be added to the right-hand side of the momentum
equation for both phases (Flift,q = −Flift,p ).
In most cases, the lift force is insignificant compared to the drag force, so
there is no reason to include this extra term. If the lift force is significant
(e.g., if the phases separate quickly), it may be appropriate to include this
term. By default, Flift is not included. The lift force and lift coefficient
can be specified for each pair of phases, if desired.
Virtual Mass Force
For multiphase flows, FLUENT includes the “virtual mass effect” that
occurs when a secondary phase p accelerates relative to the primary
phase q. The inertia of the primary-phase mass encountered by the
accelerating particles (or droplets or bubbles) exerts a “virtual mass
force” on the particles [57]:
Fvm = 0.5αp ρq
The term
dq
dt
dq vq
dp vp
−
dt
dt
(20.4-11)
denotes the phase material time derivative of the form
dq (φ)
∂(φ)
=
+ (~vq · ∇)φ
dt
∂t
(20.4-12)
20-27
The virtual mass force Fvm will be added to the right-hand side of the
momentum equation for both phases (Fvm,q = −Fvm,p ).
The virtual mass effect is significant when the secondary phase density
is much smaller than the primary phase density (e.g., for a transient
bubble column). By default, Fvm is not included.
Equations Solved by FLUENT
The equations for fluid-fluid and granular multiphase flows, as solved by
FLUENT, are presented here for the general case of an n-phase flow.
Continuity Equation
The volume fraction of each phase is calculated from a continuity equation:


n
∂
dq ρq 
1 X
ṁpq − αq
(αq ) + ∇ · (αq ~vq ) =
∂t
ρq p=1
dt
(20.4-13)
The solution of this equation for each secondary phase, along with the
condition that the volume fractions sum to one (given by Equation 20.4-2),
allows for the calculation of the primary-phase volume fraction. This
treatment is common to fluid-fluid and granular flows.
Fluid-Fluid Momentum Equations
The conservation of momentum for a fluid phase q is
∂
(αq ρq ~vq ) + ∇ · (αq ρq~vq~vq ) = −αq ∇p + ∇ · τ q + αq ρq ~g +
∂t
αq ρq (F~q + F~lift,q + F~vm,q ) +
n
X
(Kpq (~vp − ~vq ) + ṁpq~vpq )
p=1
(20.4-14)
20-28
20.4 Eulerian Model
Here ~g is the acceleration due to gravity and F~q , F~lift,q , and F~vm,q are as
defined for Equation 20.4-7.
Fluid-Solid Momentum Equations
Following the work of [2, 32, 50, 76, 131, 145, 167, 235], FLUENT uses a
multi-fluid granular model to describe the flow behavior of a fluid-solid
mixture. The solid-phase stresses are derived by making an analogy between the random particle motion arising from particle-particle collisions
and the thermal motion of molecules in a gas, taking into account the
inelasticity of the granular phase. As is the case for a gas, the intensity of
the particle velocity fluctuations determines the stresses, viscosity, and
pressure of the solid phase. The kinetic energy associated with the particle velocity fluctuations is represented by a “pseudothermal” or granular
temperature which is proportional to the mean square of the random
motion of particles.
The conservation of momentum for the fluid phases is similar to Equation 20.4-14, and that for the sth solid phase is
∂
(αs ρs~vs ) + ∇ · (αs ρs~vs~vs ) = −αs ∇p − ∇ps + ∇ · τ s + αs ρs~g +
∂t
αs ρs (F~s + F~lift,s + F~vm,s ) +
N
X
(Kls (~vl − ~vs ) + ṁls~vls ) (20.4-15)
l=1
where ps is the sth solids pressure, Kls = Ksl is the momentum exchange
coefficient between fluid or solid phase l and solid phase s, N is the
total number of phases, and F~q , F~lift,q , and F~vm,q are as defined for
Equation 20.4-7.
20.4.3
Interphase Exchange Coefficients
It can be seen in Equations 20.4-14 and 20.4-15 that momentum exchange
between the phases is based on the value of the fluid-fluid exchange
coefficient Kpq and, for granular flows, the fluid-solid and solid-solid
exchange coefficients Kls .
20-29
Fluid-Fluid Exchange Coefficient
For fluid-fluid flows, each secondary phase is assumed to form droplets
or bubbles. This has an impact on how each of the fluids is assigned
to a particular phase. For example, in flows where there are unequal
amounts of two fluids, the predominant fluid should be modeled as the
primary fluid, since the sparser fluid is more likely to form droplets or
bubbles. The exchange coefficient for these types of bubbly, liquid-liquid
or gas-liquid mixtures can be written in the following general form:
Kpq =
αp ρp f
τp
(20.4-16)
where f , the drag function, is defined differently for the different exchangecoefficient models (as described below) and τp , the “particulate relaxation time”, is defined as
τp =
ρp d2p
18µq
(20.4-17)
where dp is the diameter of the bubbles or droplets of phase p.
Nearly all definitions of f include a drag coefficient (CD ) that is based on
the relative Reynolds number (Re). It is this drag function that differs
among the exchange-coefficient models.
• For the model of Schiller and Naumann [202]
f=
CD Re
24
(20.4-18)
where
(
CD =
24(1 + 0.15Re0.687 )/Re Re ≤ 1000
0.44
Re > 1000
(20.4-19)
and Re is the relative Reynolds number. The relative Reynolds
number for the primary phase q and secondary phase p is obtained
from
20-30
20.4 Eulerian Model
Re =
ρq |~vp − ~vq |dp
µq
(20.4-20)
The relative Reynolds number for secondary phases p and r is
obtained from
Re =
ρrp |~vr − ~vp |drp
µrp
(20.4-21)
where µrp = αp µp + αr µr is the mixture viscosity of the phases p
and r.
The Schiller and Naumann model is the default method, and it is
acceptable for general use for all fluid-fluid pairs of phases.
• For the Morsi and Alexander model [163]
f=
CD Re
24
(20.4-22)
where
CD = a1 +
a2
a3
+
Re Re2
(20.4-23)
and Re is defined by Equation 20.4-20 or 20.4-21. The a’s are
defined as follows:














a1 , a2 , a3 =













0, 18, 0
3.690, 22.73, 0.0903
1.222, 29.1667, −3.8889
0.6167, 46.50, −116.67
0.3644, 98.33, −2778
0.357, 148.62, −47500
0.46, −490.546, 578700
0.5191, −1662.5, 5416700
0 < Re < 0.1
0.1 < Re < 1
1 < Re < 10
10 < Re < 100
100 < Re < 1000
1000 < Re < 5000
5000 < Re < 10000
Re ≥ 10000
(20.4-24)
The Morsi and Alexander model is the most complete, adjusting
the function definition frequently over a large range of Reynolds
20-31
numbers, but calculations with this model may be less stable than
with the other models.
• For the symmetric model
Kpq =
αp (αp ρp + αq ρq )f
τpq
(20.4-25)
where
d +d
τpq =
(αp ρp + αq ρq )( p 2 q )2
18(αp µp + αq µq )
(20.4-26)
CD Re
24
(20.4-27)
and
f=
where
(
CD =
24(1 + 0.15Re0.687 )/Re Re ≤ 1000
0.44
Re > 1000
(20.4-28)
and Re is defined by Equation 20.4-20 or 20.4-21.
The symmetric model is recommended for flows in which the secondary (dispersed) phase in one region of the domain becomes the
primary (continuous) phase in another. For example, if air is injected into the bottom of a container filled halfway with water,
the air is the dispersed phase in the bottom half of the container;
in the top half of the container, the air is the continuous phase.
This model can also be used for the interaction between secondary
phases.
You can specify different exchange coefficients for each pair of phases.
It is also possible to use user-defined functions to define exchange coefficients for each pair of phases. If the exchange coefficient is equal to zero
(i.e., if no exchange coefficient is specified), the flow fields for the fluids
will be computed independently, with the only “interaction” being their
complementary volume fractions within each computational cell.
20-32
20.4 Eulerian Model
Fluid-Solid Exchange Coefficient
The fluid-solid exchange coefficient Ksl can be written in the following
general form:
Ksl =
αs ρs f
τs
(20.4-29)
where f is defined differently for the different exchange-coefficient models
(as described below), and τs , the “particulate relaxation time”, is defined
as
τs =
ρs d2s
18µl
(20.4-30)
where ds is the diameter of particles of phase s.
All definitions of f include a drag function (CD ) that is based on the
relative Reynolds number (Res ). It is this drag function that differs
among the exchange-coefficient models.
• For the Syamlal-O’Brien model [234]
f=
CD Res αl
2
24vr,s
(20.4-31)
where the drag function has a form derived by Dalla Valle [47]

2
4.8

CD = 0.63 + q
Res /vr,s
(20.4-32)
This model is based on measurements of the terminal velocities of
particles in fluidized or settling beds, with correlations that are a
function of the volume fraction and relative Reynolds number [193]:
Res =
ρl ds |~vs − ~vl |
µl
(20.4-33)
20-33
where the subscript l is for the lth fluid phase, s is for the sth solid
phase, and ds is the diameter of the sth solid phase particles.
The fluid-solid exchange coefficient has the form
3αs αl ρl
Ksl =
CD
2 d
4vr,s
s
Res
vr,s
!
|~vs − ~vl |
(20.4-34)
where vr,s is the terminal velocity correlation for the solid phase [73]:
vr,s = 0.5 A − 0.06Res +
q
2
(0.06Res ) + 0.12Res (2B − A) +
A2
(20.4-35)
with
A = α4.14
l
(20.4-36)
B = 0.8α1.28
l
(20.4-37)
B = α2.65
l
(20.4-38)
and
for αl ≤ 0.85, and
for αl > 0.85.
This model is appropriate when the solids shear stresses are defined
according to Syamlal et al. [235] (Equation 20.4-52).
• For the model of Wen and Yu [262], the fluid-solid exchange coefficient is of the following form:
αs αl ρl |~vs − ~vl | −2.65
3
Ksl = CD
αl
4
ds
(20.4-39)
where
20-34
20.4 Eulerian Model
CD =
i
24 h
1 + 0.15(αl Res )0.687
αl Res
(20.4-40)
and Res is defined by Equation 20.4-33.
This model is appropriate for dilute systems.
• The Gidaspow model [76] is a combination of the Wen and Yu
model [262] and the Ergun equation [62].
When αl > 0.8, the fluid-solid exchange coefficient Ksl is of the
following form:
αs αl ρl |~vs − ~vl | −2.65
3
Ksl = CD
αl
4
ds
(20.4-41)
where
CD =
i
24 h
1 + 0.15(αl Res )0.687
αl Res
(20.4-42)
αs (1 − αl )µl
ρl αs |~vs − ~vl |
+ 1.75
2
αl ds
ds
(20.4-43)
When αl ≤ 0.8,
Ksl = 150
This model is recommended for dense fluidized beds.
Solid-Solid Exchange Coefficient
The solid-solid exchange coefficient Kls has the following form [233]:
Kls =
3 (1 + els )
π
2
2
+ Cfr,ls π8
αs ρs αl ρl (dl + ds )2 g0,ls
2π ρl d3l + ρs d3s
|~vl − ~vs |
(20.4-44)
20-35
where
20.4.4
els
=
Cfr,ls
=
dl
g0,ls
=
=
the coefficient of restitution (described in
Section 20.4.4)
the coefficient of friction between the lth and sth
solid-phase particles (Cfr,ls = 0)
the diameter of the particles of solid l
the radial distribution coefficient (described in
Section 20.4.4)
Solids Pressure
For granular flows in the compressible regime (i.e., where the solids volume fraction is less than its maximum allowed value), a solids pressure is
calculated independently and used for the pressure gradient term, ∇ps ,
in the granular-phase momentum equation. Because a Maxwellian velocity distribution is used for the particles, a granular temperature is
introduced into the model, and appears in the expression for the solids
pressure and viscosities. The solids pressure is composed of a kinetic
term and a second term due to particle collisions:
ps = αs ρs Θs + 2ρs (1 + ess )α2s g0,ss Θs
(20.4-45)
where ess is the coefficient of restitution for particle collisions, g0,ss is the
radial distribution function, and Θs is the granular temperature. FLUENT uses a default value of 0.9 for ess , but the value can be adjusted
to suit the particle type. The granular temperature Θs is proportional
to the kinetic energy of the fluctuating particle motion, and will be described later in this section. The function g0,ss (described below in more
detail) is a distribution function that governs the transition from the
“compressible” condition with α < αs,max , where the spacing between
the solid particles can continue to decrease, to the “incompressible” condition with α = αs,max , where no further decrease in the spacing can
occur. A value of 0.63 is the default for αs,max , but you can modify it
during the problem setup.
20-36
20.4 Eulerian Model
Radial Distribution Function
The radial distribution function, g0 , is a correction factor that modifies
the probability of collisions between grains when the solid granular phase
becomes dense. This function may also be interpreted as the nondimensional distance between spheres:
g0 =
s + dp
s
(20.4-46)
where s is the distance between grains. From Equation 20.4-46 it can be
observed that for a dilute solid phase s → ∞, and therefore g0 → 1. In
the limit when the solid phase compacts, s → 0 and g0 → ∞. The radial
distribution function is closely connected to the factor χ of Chapman
and Cowling’s [32] theory of non-uniform gases. χ is equal to one for a
rare gas, and increases and tends to infinity when the molecules are so
close together that motion is not possible.
In the literature there is no unique formulation for the radial distribution
function. FLUENT employs that proposed in [167]:

g0 = 1 −
αs
! 1 −1
αs,max
3

(20.4-47)
When the number of solid phases is greater than 1, Equation 20.4-47 is
extended to

g0,ll = 1 −
αl
αl,max
! 1 −1
3

(20.4-48)
where αl,max is specified by you during the problem setup, and
g0,lm =
dm g0,ll + dl g0,mm
dm + dl
(20.4-49)
20-37
20.4.5
Solids Shear Stresses
The solids stress tensor contains shear and bulk viscosities arising from
particle momentum exchange due to translation and collision. A frictional component of viscosity can also be included to account for the
viscous-plastic transition that occurs when particles of a solid phase reach
the maximum solid volume fraction.
The collisional and kinetic parts, and the optional frictional part, are
added to give the solids shear viscosity:
µs = µs,col + µs,kin + µs,fr
(20.4-50)
Collisional Viscosity
The collisional part of the shear viscosity is modeled as [76, 235]
µs,col
Θs
4
= αs ρs ds g0,ss (1 + ess )
5
π
1/2
(20.4-51)
Kinetic Viscosity
FLUENT provides two expressions for the kinetic part.
The default expression is from Syamlal et al. [235]:
µs,kin
√
αs ds ρs Θs π
2
=
1 + (1 + ess ) (3ess − 1) αs g0,ss
6 (3 − ess )
5
(20.4-52)
The following optional expression from Gidaspow et al. [76] is also available:
µs,kin
20-38
√
2
10ρs ds Θs π
4
=
1 + g0,ss αs (1 + ess )
96αs (1 + ess ) g0,ss
5
(20.4-53)
20.4 Eulerian Model
Bulk Viscosity
The solids bulk viscosity accounts for the resistance of the granular particles to compression and expansion. It has the following form from Lun
et al. [145]:
Θs
4
λs = αs ρs ds g0,ss (1 + ess )
3
π
1/2
(20.4-54)
Note that the bulk viscosity is set to a constant value of zero, by default.
It is also possible to select the Lun et al. expression or use a user-defined
function.
Frictional Viscosity
In dense flow at low shear, where the secondary volume fraction for
a solid phase nears the packing limit, the generation of stress is mainly
due to friction between particles. The solids shear viscosity computed by
FLUENT does not, by default, account for the friction between particles.
If the frictional viscosity is included in the calculation, FLUENT uses
Schaeffer’s [200] expression:
ps sin φ
µs,fr = √
2 I2D
(20.4-55)
where ps is the solids pressure, φ is the angle of internal friction, and I2D
is the second invariant of the deviatoric stress tensor. It is also possible
to specify a constant or user-defined frictional viscosity.
20.4.6
Granular Temperature
The granular temperature for the sth solids phase is proportional to the
kinetic energy of the random motion of the particles. The transport
equation derived from kinetic theory takes the form [50]
3 ∂
(ρs αs Θs ) + ∇ · (ρs αs~vs Θs )
2 ∂t
= (−ps I + τ s ) : ∇~vs
20-39
∇ · (kΘs ∇Θs ) − γΘs +
φls
(20.4-56)
where
(−ps I + τ s ) : ∇~vs
=
kΘs ∇Θs
=
γΘs
φls
=
=
the generation of energy by the
solid stress tensor
the diffusion of energy (kΘs is the
diffusion coefficient)
the collisional dissipation of energy
the energy exchange between the lth
fluid or solid phase and the sth solid
phase
Equation 20.4-56 contains the term kΘs ∇Θs describing the diffusive flux
of granular energy.
The collisional dissipation of energy, γΘs , represents the rate of energy
dissipation within the sth solids phase due to collisions between particles.
This term is represented by the expression derived by Lun et al. [145]
γΘm =
12(1 − e2ss )g0,ss
√
ρs α2s Θ3/2
s
ds π
(20.4-57)
The transfer of the kinetic energy of random fluctuations in particle
velocity from the sth solids phase to the lth fluid or solid phase is represented by φls [76]:
φls = −3Kls Θs
(20.4-58)
FLUENT currently uses an algebraic relation for the granular temperature. This has been obtained by neglecting convection and diffusion in
the transport equation, Equation 20.4-56 [235].
20.4.7
Turbulence Models
To describe the effects of turbulent fluctuations of velocities and scalar
quantities in a single phase, FLUENT uses various types of closure models, as described in Chapter 10. In comparison to single-phase flows,
20-40
20.4 Eulerian Model
the number of terms to be modeled in the momentum equations in multiphase flows is large, and this makes the modeling of turbulence in
multiphase simulations extremely complex.
FLUENT provides three methods for modeling turbulence in multiphase
flows within the context of the k- models:
• mixture turbulence model (default)
• dispersed turbulence model
• turbulence model for each phase
The choice of model depends on the importance of the secondary-phase
turbulence in your application.
! Note that the descriptions of each method below are presented based
on the standard k- model. The multiphase modifications to the RNG
and realizable k- models are similar, and are therefore not presented
explicitly.
Mixture Turbulence Model
The mixture turbulence model is the default multiphase turbulence model.
It represents the first extension of the single-phase k- model, and it is
applicable when phases separate, for stratified (or nearly stratified) multiphase flows, and when the density ratio between phases is close to 1. In
these cases, using mixture properties and mixture velocities is sufficient
to capture important features of the turbulent flow.
The k and equations describing this model are as follows:
∂
µt,m
∇k + Gk,m − ρm (ρm k) + ∇ · (ρm~vm k) = ∇ ·
∂t
σk
(20.4-59)
and
20-41
∂
µt,m
∇ + (C1 Gk,m −C2 ρm ) (20.4-60)
(ρm )+∇·(ρm~vm ) = ∇·
∂t
σ
k
where the mixture density and velocity, ρm and ~vm , are computed from
ρm =
N
X
αi ρi
(20.4-61)
i=1
and
N
X
~vm =
αi ρi~vi
i=1
N
X
(20.4-62)
αi ρi
i=1
the turbulent viscosity, µt,m , is computed from
µt,m = ρm Cµ
k2
(20.4-63)
and the production of turbulence kinetic energy, Gk,m , is computed from
Gk,m = µt,m (∇~vm + (∇~vm )T ) : ∇~vm
(20.4-64)
The constants in these equations are the same as those described in
Section 10.4.1 for the single-phase k- model.
Dispersed Turbulence Model
The dispersed turbulence model is the appropriate model when the concentrations of the secondary phases are dilute. In this case, interparticle
collisions are negligible and the dominant process in the random motion
of the secondary phases is the influence of the primary-phase turbulence.
Fluctuating quantities of the secondary phases can therefore be given in
20-42
20.4 Eulerian Model
terms of the mean characteristics of the primary phase and the ratio of
the particle relaxation time and eddy-particle interaction time.
The model is applicable when there is clearly one primary continuous
phase and the rest are dispersed dilute secondary phases.
Assumptions
The dispersed method for modeling turbulence in FLUENT involves the
following assumptions:
• A modified k- model for the continuous phase: Turbulent predictions for the continuous phase are obtained using the standard k-
model supplemented with extra terms that include the interphase
turbulent momentum transfer.
• Tchen-theory correlations for the dispersed phases: Predictions for
turbulence quantities for the dispersed phases are obtained using
the Tchen theory of dispersion of discrete particles by homogeneous
turbulence [91].
• Interphase turbulent momentum transfer: In turbulent multiphase
flows, the momentum exchange terms contain the correlation between the instantaneous distribution of the dispersed phases and
the turbulent fluid motion. It is possible to take into account the
dispersion of the dispersed phases transported by the turbulent
fluid motion.
• A phase-weighted averaging process: The choice of averaging process has an impact on the modeling of dispersion in turbulent multiphase flows. A two-step averaging process leads to the appearance
of fluctuations in the phase volume fractions. When the two-step
averaging process is used with a phase-weighted average for the turbulence, however, turbulent fluctuations in the volume fractions do
not appear. FLUENT uses phase-weighted averaging, so no volume
fraction fluctuations are introduced into the continuity equations.
20-43
Turbulence in the Continuous Phase
The eddy viscosity model is used to calculate averaged fluctuating quantities. The Reynolds stress tensor for continuous phase q takes the following form:
2
00
~ q )I + ρq µt,q (∇U
~ q + ∇U
~qT )
τ q = − (ρq kq + ρq µt,q ∇ · U
3
(20.4-65)
~ q is the phase-weighted velocity.
where U
The turbulent viscosity µt,q is written in terms of the turbulent kinetic
energy of phase q:
µt,q = ρq Cµ
kq2
q
(20.4-66)
and a characteristic time of the energetic turbulent eddies is defined as
τt,q =
3 kq
Cµ
2
q
(20.4-67)
where q is the dissipation rate and Cµ = 0.09.
The length scale of the turbulent eddies is
r
Lt,q =
3
3 kq2
Cµ
2
q
(20.4-68)
Turbulent predictions are obtained from the modified k- model:
∂
~ q kq ) = ∇ · (αq µt,q ∇kq ) + αq Gk,q − αq ρq q +
(αq ρq kq ) + ∇ · (αq ρq U
∂t
σk
αq ρq Πkq
(20.4-69)
and
20-44
20.4 Eulerian Model
∂
~ q q ) = ∇ · (αq µt,q ∇q ) +
(αq ρq q ) + ∇ · (αq ρq U
∂t
σ
q
αq (C1 Gk,q − C2 ρq q ) +
kq
αq ρq Πq
(20.4-70)
Here Πkq and Πq represent the influence of the dispersed phases on
the continuous phase q, and Gk,q is the production of turbulent kinetic
energy, as defined in Section 10.4.4. All other terms have the same
meaning as in the single-phase k- model.
The term Πkq can be derived from the instantaneous equation of the
continuous phase and takes the following form, where M represents the
number of secondary phases:
Πkq =
M
X
Kpq
α ρ
p=1 q q
~p − U
~ q ) · ~vdr )
(< ~vq00 · ~vp00 > +(U
(20.4-71)
which can be simplified to
Πkq =
M
X
Kpq
p=1
αq ρq
(kpq − 2kq + ~vpq · ~vdr )
(20.4-72)
where klq is the covariance of the velocities of the continuous phase q and
the dispersed phase l (calculated from Equation 20.4-80 below), ~vpq is the
relative velocity, and ~vdr is the drift velocity (defined by Equation 20.4-85
below).
Πq is modeled according to Elgobashi et al. [61]:
Πq = C3
q
Πk
kq q
(20.4-73)
where C3 = 1.2.
20-45
Turbulence in the Dispersed Phase
Time and length scales that characterize the motion are used to evaluate
dispersion coefficients, correlation functions, and the turbulent kinetic
energy of each dispersed phase.
The characteristic particle relaxation time connected with inertial effects
acting on a dispersed phase p is defined as
τF,pq =
−1
αp ρp Kpq
ρp
+ CV
ρq
!
(20.4-74)
The Lagrangian integral time scale calculated along particle trajectories,
mainly affected by the crossing-trajectory effect [43], is defined as
τt,q
τt,pq = q
(1 + Cβ ξ 2 )
(20.4-75)
where
ξ=
|~vpq |τt,q
Lt,q
(20.4-76)
and
Cβ = 1.8 − 1.35 cos2 θ
(20.4-77)
where θ is the angle between the mean particle velocity and the mean
relative velocity. The ratio between these two characteristic times is
written as
ηpq =
τt,pq
τF,pq
(20.4-78)
Following Simonin [212], FLUENT writes the turbulence quantities for
dispersed phase p as follows:
20-46
20.4 Eulerian Model
kp = kq
kpq = 2kq
Dt,pq =
b2 + ηpq
1 + ηpq
b + ηpq
1 + ηpq
1
kpq τt,pq
3
Dp = Dt,pq +
!
(20.4-79)
!
(20.4-80)
(20.4-81)
2
1
kp − b kpq τF,pq
3
3
ρp
b = (1 + CV )
+ CV
ρq
(20.4-82)
!−1
(20.4-83)
and CV = 0.5 is the added-mass coefficient.
Interphase Turbulent Momentum Transfer
The turbulent drag term for multiphase flows (Kpq (~vp − ~vq ) in Equation 20.4-9) is modeled as follows, for dispersed phase p and continuous
phase q:
~p − U
~ q ) − Kpq ~vdr
Kpq (~vp − ~vq ) = Kpq (U
(20.4-84)
The second term on the right-hand side of Equation 20.4-84 contains the
drift velocity:
~vdr = −
Dp
Dq
∇αp −
∇αq
σpq αp
σpq αq
!
(20.4-85)
Here Dp and Dq are diffusivities, and σpq is a turbulent Schmidt number.
When using Tchen theory in multiphase flows, FLUENT assumes Dp =
Dq = Dt,pq and the default value for σpq is 0.67.
The drift velocity results from turbulent fluctuations in the volume fraction. When multiplied by the exchange coefficient Kpq , it serves as a
correction to the momentum exchange term for turbulent flows. This
20-47
correction is not included, by default, but you can enable it during the
problem setup.
Turbulence Model for Each Phase
The most general multiphase turbulence model solves a set of k and transport equations for each phase. This turbulence model is the appropriate choice when the turbulence transfer among the phases plays a
dominant role.
Note that, since FLUENT is solving two additional transport equations
for each secondary phase, the per-phase turbulence model is more computationally intensive than the dispersed turbulence model.
Transport Equations
The Reynolds stress tensor and turbulent viscosity are computed using
Equations 20.4-65 and 20.4-66. Turbulence predictions are obtained from
∂
~ q kq ) = ∇ · (αq µt,q ∇kq ) + (αq Gk,q − αq ρq q ) +
(αq ρq kq ) + ∇ · (αq ρq U
∂t
σk
N
X
l=1
N
X
l=1
N
X
Klq (Clq kl − Cql kq ) −
~l − U
~q) ·
Klq (U
µt,l
∇αl +
αl σl
~l − U
~ q ) · µt,q ∇αq
Klq (U
αq σq
l=1
(20.4-86)
and
∂
~ q q ) = ∇ · (αq µt,q ∇q ) +
(αq ρq q ) + ∇ · (αq ρq U
∂t
σ
q
(C1 αq Gk,q − C2 αq ρq q +
kq
20-48
20.4 Eulerian Model
N
X
C3 (
Klq (Clq kl − Cql kq ) −
l=1
N
X
~l − U
~ q ) · µt,l ∇αl +
Klq (U
αl σl
l=1
N
X
~l − U
~ q ) · µt,q ∇αq ))
Klq (U
αq σq
l=1
(20.4-87)
The terms Clq and Cql can be approximated as
Clq = 2
Cql = 2
ηlq
1 + ηlq
!
(20.4-88)
where ηlq is defined by Equation 20.4-78.
Interphase Turbulent Momentum Transfer
The turbulent drag term (Kpq (~vp −~vq ) in Equation 20.4-9) is modeled as
follows, where l is the dispersed phase (replacing p in Equation 20.4-9)
and q is the continuous phase:
N
X
Klq (~vl − ~vq ) =
l=1
N
X
l=1
~l − U
~q) −
Klq (U
N
X
Klq~vdr,lq
(20.4-89)
l=1
~ l and U
~ q are phase-weighted velocities, and ~vdr,lq is the drift veHere U
locity for phase l (computed using Equation 20.4-85, substituting l for
p). Note that FLUENT will compute the diffusivities Dl and Dq directly
from the transport equations, rather than using Tchen theory (as it does
for the dispersed turbulence model).
As noted above, the drift velocity results from turbulent fluctuations in
the volume fraction. When multiplied by the exchange coefficient Klq ,
it serves as a correction to the momentum exchange term for turbulent
20-49
flows. This correction is not included, by default, but you can enable it
during the problem setup.
The turbulence model for each phase in FLUENT accounts for the effect
of the turbulence field of one phase on the other(s). If you want to
modify or enhance the interaction of the multiple turbulence fields and
interphase turbulent momentum transfer, you can supply these terms
using user-defined functions.
20.4.8
Solution Method in FLUENT
For Eulerian multiphase calculations, FLUENT uses the Phase Coupled
SIMPLE (PC-SIMPLE) algorithm [244] for the pressure-velocity coupling. PC-SIMPLE is an extension of the SIMPLE algorithm [172] to
multiphase flows. The velocities are solved coupled by phases, but in a
segregated fashion. The block algebraic multigrid scheme used by the
coupled solver described in [260] is used to solve a vector equation formed
by the velocity components of all phases simultaneously. Then, a pressure correction equation is built based on total volume continuity rather
than mass continuity. Pressure and velocities are then corrected so as to
satisfy the continuity constraint.
The Pressure-Correction Equation
For incompressible multiphase flow, the pressure-correction equation takes
the form
n
X
k=1
(
n
∂
1 X
ṁlk
αk + ∇ · αk ~vk0 + ∇ · αk~vk∗ −
∂t
ρk l=1
)
=0
(20.4-90)
where ~vk0 is the velocity correction for the kth phase and ~vk∗ is the value
of ~vk at the current iteration. The velocity corrections are themselves
expressed as functions of the pressure corrections.
Volume Fractions
The volume fractions are obtained from the phase continuity equations.
In discretized form, the equation of the kth volume fraction is
20-50
20.5 Cavitation Effects
ap,k αk =
X
(anb,k αnb,k ) + bk = Rk
(20.4-91)
nb
In order to satisfy the condition that all the volume fractions sum to
one,
n
X
αk = 1
(20.4-92)
k=1
20.5
Cavitation Effects
Cavitation effects can be included in two-phase flows when the mixture
model or Eulerian model is used. This section provides information
about the cavitation model used in FLUENT.
20.5.1
Overview and Limitations of the Cavitation Model
A liquid at constant temperature can be subjected to a decreasing pressure, which may fall below the saturated vapor pressure. The process of
rupturing the liquid by a decrease of pressure at constant temperature
is called cavitation. The liquid contains micro-bubbles of air or nuclei,
and under decreasing pressure these may grow and form cavities.
The cavitation model, designed for two interpenetrating fluids, models
the formation of bubbles when the local pressure becomes less than the
vaporization pressure. The cavitation model can be used with the mixture model (with or without slip velocities) or the Eulerian multiphase
model.
The following assumptions are made in the cavitation model:
• The system under investigation involves only two phases.
• Bubbles are neither created nor destroyed.
• The population or number of bubbles per unit volume is known in
advance.
20-51
The following limitations apply to the cavitation model in FLUENT:
• The cavitation model cannot be used with the VOF model, because
the surface tracking schemes for the VOF model are incompatible
with the interpenetrating continua assumption of the cavitation
model.
• The cavitation model can be used only for multiphase simulations that use the mixture or Eulerian model and involve only
two phases. It is always preferable to solve for cavitation using the
mixture model without slip velocity; Eulerian multiphase or slip
velocities can be turned on if the problem suggests that there is
significant slip between phases.
• With the cavitation model, only the secondary phase can be compressible; the primary phase must be incompressible.
Volume and Number of Bubbles
The volume of the individual bubbles is changing with respect to space
and time and denoted by
4
φ(~r, t) = πR3
3
(20.5-1)
where R is the bubble radius.
The volume fraction of vapor is defined as
αv =
φη
1 + φη
(20.5-2)
where η is the population or number of bubbles per unit volume of liquid.
The Volume Fraction Equation
The volume fraction equation is derived from the continuity equation for
the mixture (m). After some manipulation, assuming an incompressible
liquid (l), the following expression can be obtained:
20-52
20.5 Cavitation Effects
∂
η
dφ αρv dρv
ρl
(αp ) + ∇(αp~vm ) =
+
∂t
ρm (1 + ηφ)2 dt
ρm dt
(20.5-3)
Bubble Dynamics
Since cavitation bubbles will form in a liquid at low temperatures, FLUENT models the cavitating flow as isothermal, neglecting the latent heat
of vaporization. The Rayleigh-Plesset equation relates the pressure and
the bubble volume φ:
R
d2 R 3 dR
+
dt2
2 dt
2
=
pB − p
2σ
µl dR
−
−4
ρl
ρl R
ρl R dt
(20.5-4)
Here pB denotes the pressure within the bubble, represented by the sum
of a partial pressure (pv ) of the vapor and a partial pressure of noncondensable gas (p), and σ is the surface tension coefficient.
To simplify the calculation, FLUENT assumes that the process of bubble
growth and collapse is given by

q
2(pB −p)
, pv > p
dR  q 3ρ
l
=
2(p
−p)
B

dt
−
, pv < p
3ρl
(20.5-5)
20-53
20.6
Setting Up a General Multiphase Problem
This section provides instructions and guidelines for using the VOF,
mixture, and Eulerian multiphase models. Information is presented in
the following subsections:
• Section 20.6.1: Steps for Using the General Multiphase Models
• Section 20.6.2: Additional Guidelines for Eulerian Multiphase Simulations
• Section 20.6.3: Enabling the Multiphase Model and Specifying the
Number of Phases
• Section 20.6.4: Selecting the VOF Formulation
• Section 20.6.5: Defining a Homogeneous Multiphase Flow
• Section 20.6.6: Including Cavitation Effects
• Section 20.6.7: Overview of Defining the Phases
• Section 20.6.8: Defining Phases for the VOF Model
• Section 20.6.9: Defining Phases for the Mixture Model
• Section 20.6.10: Defining Phases for the Eulerian Model
• Section 20.6.11: Including Body Forces
• Section 20.6.12: Setting Time-Dependent Parameters for the VOF
Model
• Section 20.6.13: Selecting a Turbulence Model for an Eulerian Multiphase Calculation
• Section 20.6.14: Setting Boundary Conditions
• Section 20.6.15: Setting Initial Volume Fractions
• Section 20.6.16: Inputs for Compressible VOF and Mixture Model
Calculations
• Section 20.6.17: Inputs for Solidification/Melting VOF Calculations
20-54
20.6 Setting Up a General Multiphase Problem
20.6.1
Steps for Using the General Multiphase Models
The procedure for setting up and solving a general multiphase problem
is outlined below, and described in detail in the subsections that follow. Remember that only the steps that are pertinent to general multiphase calculations are shown here. For information about inputs related
to other models that you are using in conjunction with the multiphase
model, see the appropriate sections for those models.
See also Section 20.6.2 for guidelines on simplifying Eulerian multiphase
simulations.
1. Enable the multiphase model you want to use (VOF, mixture, or
Eulerian) and specify the number of phases. For the VOF model,
specify the VOF formulation as well.
Define −→ Models −→Multiphase...
See Sections 20.6.3 and 20.6.4 for details.
2. Copy the material representing each phase from the materials database.
Define −→Materials...
If the material you want to use is not in the database, create a
new material. See Section 7.1.2 for details about copying from
the database and creating new materials. See Section 20.6.16 for
additional information about specifying material properties for a
compressible phase (VOF and mixture models only).
!
If your model includes a particulate (granular) phase, you will need
to create a new material for it in the fluid materials category (not
the solid materials category).
3. Define the phases, and specify any interaction between them (e.g.,
surface tension if you are using the VOF model, slip velocity functions if you are using the mixture model, or drag functions if you
are using the Eulerian model).
Define −→Phases...
See Sections 20.6.7–20.6.10 for details.
20-55
4. (Eulerian model only) If the flow is turbulent, define the multiphase
turbulence model.
Define −→ Models −→Viscous...
See Section 20.6.13 for details.
5. If body forces are present, turn on gravity and specify the gravitational acceleration.
Define −→Operating Conditions...
6. Specify the boundary conditions, including the secondary-phase
volume fractions at flow boundaries and (if you are modeling wall
adhesion in a VOF simulation) the contact angles at walls.
Define −→Boundary Conditions...
7. Set any model-specific solution parameters.
Solve −→ Controls −→Solution...
See Sections 20.6.12 and 20.7 for details.
8. Initialize the solution and set the initial volume fractions for the
secondary phases.
Solve −→ Initialize −→Patch...
9. Calculate a solution and examine the results.
See Sections 20.7 and 20.8 for details.
20.6.2
Additional Guidelines for Eulerian Multiphase
Simulations
Once you have determined that the Eulerian multiphase model is appropriate for your problem (as described in Sections 18.4 and 20.1), you
should consider the computational effort required to solve your multiphase problem. The required computational effort depends strongly on
20-56
the number of transport equations being solved and the degree of coupling. For the Eulerian multiphase model, which has a large number of
highly coupled transport equations, computational expense will be high.
Before setting up your problem, try to reduce the problem statement to
the simplest form possible.
Instead of trying to solve your multiphase flow in all of its complexity
on your first solution attempt, you can start with simple approximations
and work your way up to the final form of the problem definition. Some
suggestions for simplifying a multiphase flow problem are listed below:
• Use a hexahedral or quadrilateral mesh (instead of a tetrahedral
or triangular mesh).
• Reduce the number of phases.
You may find that even a very simple approximation will provide you
with useful information about your problem.
See Section 20.7.3 for more solution strategies for Eulerian multiphase
calculations.
20.6.3
Enabling the Multiphase Model and Specifying the
Number of Phases
To enable the VOF, mixture, or Eulerian multiphase model, select Volume of Fluid, Mixture, or Eulerian as the Model in the Multiphase Model
panel (Figure 20.6.1).
Define −→ Models −→Multiphase...
The panel will expand to show the relevant inputs for the selected multiphase model.
If you selected the VOF model, the inputs are as follows:
• number of phases
• VOF formulation (see Section 20.6.4)
20-57
Figure 20.6.1: The Multiphase Model Panel
• (optional) implicit body force formulation (see Section 20.6.11)
If you selected the mixture model, the inputs are as follows:
• whether or not to compute the slip velocities (see Section 20.6.5)
• (optional) implicit body force formulation (see Section 20.6.11)
• (optional) cavitation effects (see Section 20.6.6)
20-58
If you selected the Eulerian model, the inputs are as follows:
• (optional) cavitation effects (see Section 20.6.6)
To specify the number of phases for the multiphase calculation, enter the
appropriate value in the Number of Phases field. You can specify up to
20 phases.
20.6.4
Selecting the VOF Formulation
To specify the VOF formulation to be used, select the appropriate VOF
Scheme under VOF Parameters in the Multiphase Model panel.
The VOF formulations that are available in FLUENT are as follows:
• Time-dependent with the geometric reconstruction interpolation
scheme: This formulation should be used whenever you are interested in the time-accurate transient behavior of the VOF solution.
To use this formulation, select Geo-Reconstruct (the default) as the
VOF Scheme. FLUENT will automatically turn on the unsteady
formulation with first-order discretization for time in the Solver
panel.
• Time-dependent with the donor-acceptor interpolation scheme:
This formulation should be used instead of the time-dependent
formulation with the geometric reconstruction scheme if your mesh
contains highly twisted hexahedral cells. For such cases, the donoracceptor scheme may provide more accurate results.
To use this formulation, select Donor-Acceptor as the VOF Scheme.
FLUENT will automatically turn on the unsteady formulation with
first-order discretization for time in the Solver panel.
• Time-dependent with the Euler explicit interpolation scheme: Since
the donor-acceptor scheme is available only for quadrilateral and
hexahedral meshes, it cannot be used for a hybrid mesh containing
20-59
twisted hexahedral cells. For such cases, you should use the timedependent Euler explicit scheme. This formulation can also be
used for other cases in which the geometric reconstruction scheme
does not give satisfactory results, or the flow calculation becomes
unstable.
To use this formulation, select Euler Explicit as the VOF Scheme.
FLUENT will automatically turn on the unsteady formulation with
first-order discretization for time in the Solver panel.
While the Euler explicit time-dependent formulation is less computationally expensive than the geometric reconstruction scheme,
the interface between phases will not be as sharp as that predicted
with the geometric reconstruction scheme. To reduce this diffusivity, it is recommended that you use the second-order discretization
scheme for the volume fraction equations. In addition, you may
want to consider turning the geometric reconstruction scheme back
on after calculating a solution with the implicit scheme, in order
to obtain a sharper interface.
• Time-dependent with the implicit interpolation scheme: This formulation can be used if you are looking for a steady-state solution
and you are not interested in the intermediate transient flow behavior, but the final steady-state solution is dependent on the initial
flow conditions and/or you do not have a distinct inflow boundary
for each phase.
To use this formulation, select Implicit as the VOF Scheme, and
enable an Unsteady calculation in the Solver panel (opened with
the Define/Models/Solver... menu item).
!
The issues discussed above for the Euler explicit time-dependent
formulation also apply to the implicit time-dependent formulation.
You should take the precautions described above to improve the
sharpness of the interface.
• Steady-state with the implicit interpolation scheme: This formulation can be used if you are looking for a steady-state solution,
you are not interested in the intermediate transient flow behavior,
and the final steady-state solution is not affected by the initial flow
conditions and there is a distinct inflow boundary for each phase.
20-60
To use this formulation, select Implicit as the VOF Scheme.
!
The issues discussed above for the Euler explicit time-dependent
formulation also apply to the implicit steady-state formulation.
You should take the precautions described above to improve the
sharpness of the interface.
! For the geometric reconstruction and donor-acceptor schemes, if you are
using a conformal grid (i.e., if the grid node locations are identical at the
boundaries where two subdomains meet), you must ensure that there are
no two-sided (zero-thickness) walls within the domain. If there are, you
will need to slit them, as described in Section 5.7.8.
Examples
To help you determine the best formulation to use for your problem,
examples that use different formulations are listed below:
• jet breakup: time-dependent with the geometric reconstruction
scheme (or the donor-acceptor or Euler explicit scheme if problems occur with the geometric reconstruction scheme)
• shape of the liquid interface in a centrifuge: time-dependent with
the implicit interpolation scheme
• flow around a ship’s hull: steady-state with the implicit interpolation scheme
20.6.5
Defining a Homogeneous Multiphase Flow
If you are using the mixture model, you have the option to disable the
calculation of slip velocities and solve a homogeneous multiphase flow
(i.e., one in which the phases all move at the same velocity). By default,
FLUENT will compute the slip velocities for the secondary phases, as described in Section 20.3.4. If you want to solve a homogeneous multiphase
flow, turn off Slip Velocity under Mixture Parameters.
20-61
20.6.6
Including Cavitation Effects
For mixture and Eulerian calculations, it is possible to include the effects
of cavitation. To enable the cavitation model, turn on Cavitation under
Interphase Mass Transfer in the Multiphase Model panel.
Next you will specify two parameters to be used in the calculation of mass
transfer due to cavitation. Specification of these parameters should be in
agreement with the characteristic parameters of the flow under investigation: Reynolds number and cavitation number. Under Cavitation Parameters in the Multiphase Model panel, set the Vaporization Pressure (pv in
Equation 20.5-5) and the Bubble Number Density (η in Equation 20.5-2).
The default value of η is 10000, as recommended by Kubota et al. [119].
The default value of pv is 2367.8, the vaporization pressure for water at
ambient temperature.
See Section 20.5 for details about modeling cavitation.
20.6.7
Overview of Defining the Phases
To define the phases (including their material properties) and any interphase interaction (e.g., surface tension and wall adhesion for the VOF
model, slip velocity function for the mixture model, drag functions for
the Eulerian model), you will use the Phases panel (Figure 20.6.2).
Define −→Phases...
Each item in the Phase list in this panel is one of two types, as indicated
in the Type list: primary-phase indicates that the selected item is the
primary phase, and secondary-phase indicates that the selected item is a
secondary phase. To specify any interaction between the phases, click
the Interaction... button.
Instructions for defining the phases and interaction are provided in Sections 20.6.8, 20.6.9, and 20.6.10 for the VOF, mixture, and Eulerian
models, respectively.
20-62
Figure 20.6.2: The Phases Panel
20.6.8
Defining Phases for the VOF Model
Instructions for specifying the necessary information for the primary and
secondary phases and their interaction in a VOF calculation are provided
below.
! In general, you can specify the primary and secondary phases whichever
way you prefer. It is a good idea, especially in more complicated problems, to consider how your choice will affect the ease of problem setup.
For example, if you are planning to patch an initial volume fraction of 1
for one phase in a portion of the domain, it may be more convenient to
make that phase a secondary phase. Also, if one of the phases is compressible, it is recommended that you specify it as the primary phase to
improve solution stability.
! Recall that only one of the phases can be compressible. Be sure that
you do not select a compressible material (i.e., a material that uses the
compressible ideal gas law for density) for more than one of the phases.
20-63
Defining the Primary Phase
To define the primary phase in a VOF calculation, follow these steps:
1. Select phase-1 in the Phase list.
2. Click Set..., and the Primary Phase panel (Figure 20.6.3) will open.
Figure 20.6.3: The Primary Phase Panel
3. In the Primary Phase panel, enter a Name for the phase.
4. Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.
5. Define the material properties for the Phase Material.
(a) Click Edit..., and the Material panel will open.
(b) In the Material panel, check the properties, and modify them
if necessary. (See Chapter 7 for general information about
setting material properties, Section 20.6.16 for specific information related to compressible VOF calculations, and Section 20.6.17 for specific information related to melting/solidification VOF calculations.)
!
If you make changes to the properties, remember to click
Change before closing the Material panel.
6. Click OK in the Primary Phase panel.
20-64
Defining a Secondary Phase
To define a secondary phase in a VOF calculation, follow these steps:
1. Select the phase (e.g., phase-2) in the Phase list.
2. Click Set..., and the Secondary Phase panel (Figure 20.6.4) will
open.
Figure 20.6.4: The Secondary Phase Panel for the VOF Model
3. In the Secondary Phase panel, enter a Name for the phase.
5. Define the material properties for the Phase Material, following the
procedure outlined above for setting the material properties for the
primary phase.
6. Click OK in the Secondary Phase panel.
Including Surface Tension and Wall Adhesion Effects
As discussed in Section 20.2.8, the importance of surface tension effects
depends on the value of the capillary number, Ca (defined by Equation 20.2-16), or the Weber number, We (defined by Equation 20.2-17).
Surface tension effects can be neglected if Ca 1 or We 1.
! Note that the calculation of surface tension effects will be more accuc Fluent Inc. November 28, 2001
20-65
rate if you use a quadrilateral or hexahedral mesh in the area(s) of the
computational domain where surface tension is significant. If you cannot use a quadrilateral or hexahedral mesh for the entire domain, then
you should use a hybrid mesh, with quadrilaterals or hexahedra in the
affected areas.
If you want to include the effects of surface tension along the interface
between one or more pairs of phases, as described in Section 20.2.8, click
Interaction... to open the Phase Interaction panel (Figure 20.6.5).
Figure 20.6.5: The Phase Interaction Panel for the VOF Model
Follow the steps below to include surface tension (and, if appropriate,
wall adhesion) effects along the interface between one or more pairs of
phases:
1. Turn on the Surface Tension option.
20-66
2. If you want to include wall adhesion, turn on the Wall Adhesion option. (When Wall Adhesion is enabled, you will need to specify the
contact angle at each wall as a boundary condition (as described
in Section 20.6.14.)
3. For each pair of phases between which you want to include the
effects of surface tension, specify a constant surface tension coefficient. All surface tension coefficients are equal to 0 by default,
representing no surface tension effects along the interface between
the two phases.
! For calculations involving surface tension, it is recommended that you
also turn on the Implicit Body Force treatment for the Body Force Formulation in the Multiphase Model panel. This treatment improves solution
convergence by accounting for the partial equilibrium of the pressure
gradient and surface tension forces in the momentum equations. See
Section 22.3.3 for details.
20.6.9
Defining Phases for the Mixture Model
Instructions for specifying the necessary information for the primary and
secondary phases and their interaction for a mixture model calculation
are provided below.
! Recall that only one of the phases can be compressible. Be sure that
you do not select a compressible material (i.e., a material that uses the
compressible ideal gas law for density) for more than one of the phases.
The procedure for defining the primary phase in a mixture model calculation is the same as for a VOF calculation. See Section 20.6.8 for
details.
Defining a Secondary Phase
To define a secondary phase in a mixture model calculation, follow these
steps:
20-67
open.
Figure 20.6.6: The Secondary Phase Panel for the Mixture Model
same procedure you used to set the material properties for the
primary phase (see Section 20.6.8). For a particulate phase (which
must be placed in the fluid materials category, as mentioned in
Section 20.6.1), you need to specify only the density; you can ignore
the values for the other properties, since they will not be used.
20-68
6. In the Secondary Phase panel, specify the Diameter of the bubbles,
droplets, or particles of this phase (dp in Equation 20.3-12). You
can specify a constant value, or use a user-defined function. See
the separate UDF Manual for details about user-defined functions.
Defining the Slip Velocity
If you are solving for slip velocities during the mixture calculation, and
you want to modify the slip velocity definition, click Interaction... to
open the Phase Interaction panel (Figure 20.6.7).
Figure 20.6.7: The Phase Interaction Panel for the Mixture Model
Under Slip Velocity, you can specify the slip velocity function for each
secondary phase with respect to the primary phase by choosing the appropriate item in the adjacent drop-down list.
• Select maninnen-et-al (the default) to use the algebraic slip method
of Manninen et al. [150], described in Section 20.3.4.
20-69
• Select none if the secondary phase has the same velocity as the
primary phase (i.e., no slip velocity).
• Select user-defined to use a user-defined function for the slip velocity. See the separate UDF Manual for details.
20.6.10
Defining Phases for the Eulerian Model
Instructions for specifying the necessary information for the primary
and secondary phases and their interaction for an Eulerian multiphase
calculation are provided below.
The procedure for defining the primary phase in an Eulerian multiphase
calculation is the same as for a VOF calculation. See Section 20.6.8 for
details.
Defining a Non-Granular Secondary Phase
To define a non-granular (i.e., liquid or vapor) secondary phase in an
Eulerian multiphase calculation, follow these steps:
open.
primary phase (see Section 20.6.8).
6. In the Secondary Phase panel, specify the Diameter of the bubbles
or droplets of this phase. You can specify a constant value, or use
a user-defined function. See the separate UDF Manual for details
about user-defined functions.
20-70
Figure 20.6.8: The Secondary Phase Panel for a Non-Granular Phase
Defining a Granular Secondary Phase
To define a granular (i.e., particulate) secondary phase in an Eulerian
multiphase calculation, follow these steps:
open.
20-71
Figure 20.6.9: The Secondary Phase Panel for a Granular Phase
primary phase (see Section 20.6.8). For a granular phase (which
must be placed in the fluid materials category, as mentioned in
Section 20.6.1), you need to specify only the density; you can ignore
the values for the other properties, since they will not be used.
6. In the Secondary Phase panel, specify the following properties of
the particles of this phase:
Diameter specifies the diameter of the particles. You can select
20-72
constant in the drop-down list and specify a constant value, or
select user-defined to use a user-defined function. See the separate UDF Manual for details about user-defined functions.
Granular Viscosity specifies the kinetic part of the granular viscosity of the particles (µs,kin in Equation 20.4-50). You can select
constant (the default) in the drop-down list and specify a constant value, select syamlal-obrien to compute the value using
Equation 20.4-52, select gidaspow to compute the value using
Equation 20.4-53, or select user-defined to use a user-defined
function.
Granular Bulk Viscosity specifies the solids bulk viscosity (λq in Equation 20.4-8). You can select constant (the default) in the dropdown list and specify a constant value, select lun-et-al to compute the value using Equation 20.4-54, or select user-defined
to use a user-defined function.
Frictional Viscosity specifies a shear viscosity based on the viscousplastic flow (µs,fr in Equation 20.4-50). By default, the frictional viscosity is neglected, as indicated by the default selection of none in the drop-down list. If you want to include
the frictional viscosity, you can select constant and specify
a constant value, select schaeffer to compute the value using
Equation 20.4-55, or select user-defined to use a user-defined
function.
Angle of Internal Friction specifies a constant value for the angle φ
used in Schaeffer’s expression for frictional viscosity (Equation 20.4-55). This parameter is relevant only if you have
selected schaeffer or user-defined for the Frictional Viscosity.
Packing Limit specifies the maximum volume fraction for the granular phase (αs,max ). For monodispersed spheres the packing
limit is about 0.63, which is the default value in FLUENT. In
polydispersed cases, however, smaller spheres can fill the small
gaps between larger spheres, so you may need to increase the
maximum packing limit.
20-73
Defining the Interaction Between Phases
For both granular and non-granular flows, you will need to specify the
drag function to be used in the calculation of the momentum exchange
coefficients. For granular flows, you will also need to specify the restitution coefficient(s) for particle collisions. It is also possible to include an
optional lift force and/or virtual mass force (described below) for both
granular and non-granular flows.
To specify these parameters, click Interaction... to open the Phase Interaction panel (Figure 20.6.10).
Figure 20.6.10: The Phase Interaction Panel for the Eulerian Model
Specifying the Drag Function
FLUENT allows you to specify a drag function for each pair of phases.
Follow the steps below:
20-74
1. Click the Drag tab to display the Drag Function inputs.
2. For each pair of phases, select the appropriate drag function from
the corresponding drop-down list.
• Select schiller-naumann to use the fluid-fluid drag function
described by Equation 20.4-19. The Schiller and Naumann
model is the default method, and it is acceptable for general
use in all fluid-fluid multiphase calculations.
• Select morsi-alexander to use the fluid-fluid drag function described by Equation 20.4-23. The Morsi and Alexander model
is the most complete, adjusting the function definition frequently over a large range of Reynolds numbers, but calculations with this model may be less stable than with the other
models.
• Select symmetric to use the fluid-fluid drag function described
by Equation 20.4-28. The symmetric model is recommended
for flows in which the secondary (dispersed) phase in one region of the domain becomes the primary (continuous) phase
in another. For example, if air is injected into the bottom of
a container filled halfway with water, the air is the dispersed
phase in the bottom half of the container; in the top half of
the container, the air is the continuous phase.
• Select wen-yu to use the fluid-solid drag function described by
Equation 20.4-40. The Wen and Yu model is applicable for
dilute phase flows, in which the total secondary phase volume
fraction is significantly lower than that of the primary phase.
• Select gidaspow to use the fluid-solid drag function described
by Equation 20.4-42. The Gidaspow model is recommended
for dense fluidized beds.
• Select syamlal-obrien to use the fluid-solid drag function described by Equation 20.4-32. The Syamlal-O’Brien model is
recommended for use in conjunction with the Syamlal-O’Brien
model for granular viscosity.
• Select syamlal-obrien-symmetric to use the solid-solid drag function described by Equation 20.4-44. The symmetric Syamlal-
20-75
O’Brien model is appropriate for a pair of solid phases.
• Select constant to specify a constant value for the drag function, and then specify the value in the text field.
• Select user-defined to use a user-defined function for the drag
function (see the separate UDF Manual for details).
• If you want to temporarily ignore the interaction between two
phases, select none.
Specifying the Restitution Coefficients (Granular Flow Only)
For granular flows, you need to specify the coefficients of restitution for
collisions between particles (els in Equation 20.4-44 and ess in Equation 20.4-45). In addition to specifying the restitution coefficient for
collisions between each pair of granular phases, you will also specify the
restitution coefficient for collisions between particles of the same phase.
Follow the steps below:
1. Click the Collisions tab to display the Restitution Coefficient inputs.
2. For each pair of phases, specify a constant restitution coefficient.
All restitution coefficients are equal to 0.9 by default.
Including the Lift Force
For both granular and non-granular flows, it is possible to include the
effect of lift forces (Flift in Equation 20.4-10) on the secondary phase
particles, droplets, or bubbles. These lift forces act on a particle, droplet,
or bubble mainly due to velocity gradients in the primary-phase flow
field. In most cases, the lift force is insignificant compared to the drag
force, so there is no reason to include it. If the lift force is significant
(e.g., if the phases separate quickly), you may want to include this effect.
! Note that the lift force will be more significant for larger particles, but
the FLUENT model assumes that the particle diameter is much smaller
than the interparticle spacing. Thus, the inclusion of lift forces is not
appropriate for closely packed particles or for very small particles.
To include the effect of lift forces, follow these steps:
20-76
1. Click the Lift tab to display the Lift Coefficient inputs.
2. For each pair of phases, select the appropriate specification method
from the corresponding drop-down list. Note that, since the lift
forces for a particle, droplet, or bubble are due mainly to velocity
gradients in the primary-phase flow field, you will not specify lift
coefficients for pairs consisting of two secondary phases; lift coefficients are specified only for pairs consisting of a secondary phase
and the primary phase.
• Select none (the default) to ignore the effect of lift forces.
• Select constant to specify a constant lift coefficient, and then
specify the value in the text field.
• Select user-defined to use a user-defined function for the lift
coefficient (see the separate UDF Manual for details).
Including the Virtual Mass Force
For both granular and non-granular flows, it is possible to include the
“virtual mass force” (Fvm in Equation 20.4-11) that is present when
a secondary phase accelerates relative to the primary phase. The virtual mass effect is significant when the secondary phase density is much
smaller than the primary phase density (e.g., for a transient bubble column).
To include the effect of the virtual mass force, turn on the Virtual Mass
option in the Phase Interaction panel. The virtual mass effect will be
included for all secondary phases; it is not possible to enable it just for
a particular phase.
20.6.11
Including Body Forces
In many cases, the motion of the phases is due, in part, to gravitational
effects. To include this body force, turn on Gravity in the Operating
Conditions panel and specify the Gravitational Acceleration.
20-77
For VOF calculations, you should also turn on the Specified Operating
Density option in the Operating Conditions panel, and set the Operating Density to be the density of the lightest phase. (This excludes the
buildup of hydrostatic pressure within the lightest phase, improving the
round-off accuracy for the momentum balance.) If any of the phases is
compressible, set the Operating Density to zero.
! For VOF and mixture calculations involving body forces, it is recommended that you also turn on the Implicit Body Force treatment for the
Body Force Formulation in the Multiphase Model panel. This treatment
improves solution convergence by accounting for the partial equilibrium
of the pressure gradient and body forces in the momentum equations.
20.6.12
Setting Time-Dependent Parameters for the VOF
Model
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.
To compute a time-dependent VOF solution, you will need to enable
the Unsteady option in the Solver panel (and choose the appropriate
Unsteady Formulation, as discussed in Section 22.15.1). If you choose the
Geo-Reconstruct, Donor-Acceptor, or Euler Explicit scheme, FLUENT will
turn on the first-order unsteady formulation for you automatically, so
you need not visit the Solver panel yourself.
Define −→ Models −→Solver...
There are two inputs for the time-dependent calculation in the Multiphase
Model panel:
• By default, FLUENT will solve the volume fraction equation(s) once
for each time step. This means that the convective flux coefficients
appearing in the other transport equations will not be completely
20-78
updated each iteration, since the volume fraction fields will not
change from iteration to iteration.
If you want FLUENT to solve the volume fraction equation(s) at
every iteration within a time step, turn on the Solve VOF Every
Iteration option under VOF Parameters. When FLUENT solves these
equations every iteration, the convective flux coefficients in the
other transport equations will be updated based on the updated
volume fractions at each iteration.
In general, if you anticipate that the location of the interface will
change as the other flow variables converge during the time step,
you should enable the Solve VOF Every Iteration option. This situation 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 you can leave
this option turned off. This choice is the more stable of the two,
and requires less computational effort per time step than the first
choice.
!
If you are using sliding meshes, using the Solve VOF Every Iteration option may yield more accurate results, although at a greater
computational cost.
• When FLUENT performs a time-dependent VOF calculation, the
time step used for the volume fraction calculation will not be the
same as the time step used for the rest of the transport equations.
FLUENT will refine the time step for VOF automatically, based
on your input for the maximum Courant Number allowed near the
free surface. The Courant number is a dimensionless number that
compares the time step in a calculation to the characteristic time
of transit of a fluid element across a control volume:
∆t
∆xcell /vfluid
(20.6-1)
In the region near the fluid interface, FLUENT divides the volume
of each cell by the sum of the outgoing fluxes. The resulting time
represents the time it would take for the fluid to empty out of the
20-79
cell. The smallest such time is used as the characteristic time of
transit for a fluid 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 default), the time step will be chosen to be
at most one-fourth the minimum transit time for any cell near the
interface.
Note that these inputs are not required when the implicit scheme is used.
20.6.13
Selecting a Turbulence Model for an Eulerian
Multiphase Calculation
If you are using the Eulerian model to solve a turbulent flow, you will
need to choose one of the three turbulence models described in Section 20.4.7 in the Viscous Model panel (Figure 20.6.11).
The procedure is as follows:
1. Select k-epsilon under Model.
2. Select the desired k-epsilon Model and any other related parameters,
as described for single-phase calculations in Section 10.10.
3. Under k-epsilon Multiphase Model, indicate the desired multiphase
turbulence model (see Section 20.4.7 for details about each):
• Select Mixture to use the mixture turbulence model. This is
the default model.
• Select Dispersed to use the dispersed turbulence model. This
model is applicable when there is clearly one primary continuous phase and the rest are dispersed dilute secondary phases.
• Select Per Phase to use a k- turbulence model for each phase.
This model is appropriate when the turbulence transfer among
the phases plays a dominant role.
20-80
Figure 20.6.11: The Viscous Model Panel for an Eulerian Multiphase
Calculation
Including Source Terms
By default, the interphase momentum, k, and sources are not included
in the calculation. If you want to include any of these source terms,
you can enable them using the multiphase-options command in the
define/models/viscous/multiphase-turbulence/ text menu. Note
that the inclusion of these terms can slow down convergence noticeably.
If you are looking for additional accuracy, you may want to compute a
solution first without these sources, and then continue the calculation
with these terms included. In most cases these terms can be neglected.
20-81
20.6.14
Setting Boundary Conditions
Multiphase boundary conditions are set in the Boundary Conditions panel
(Figure 20.6.12), but the procedure for setting multiphase boundary conditions is slightly different than for single-phase models. You will need
to set some conditions separately for individual phases, while other conditions are shared by all phases (i.e., the mixture), as described in detail
below.
Define −→Boundary Conditions...
Figure 20.6.12: The Boundary Conditions Panel
Boundary Conditions for the Mixture and the Individual Phases
The conditions you need to specify for the mixture and those you need
to specify for the individual phases will depend on which of the three
multiphase models you are using. Details for each model are provided
below.
20-82
VOF Model
If you are using the VOF model, the conditions you need to specify for
each type of zone are listed below and summarized in Table 20.6.1.
• For an exhaust fan, inlet vent, intake fan, mass flow inlet, outlet
vent, pressure inlet, pressure outlet, or velocity inlet, there are no
conditions to be specified for the primary phase. For each secondary phase, you will need to set the volume fraction as a constant, a profile (see Section 6.25), or a user-defined function (see
the separate UDF Manual). All other conditions are specified for
the mixture.
• For an axis, fan, outflow, periodic, porous jump, radiator, solid,
symmetry, or wall zone, all conditions are specified for the mixture;
there are no conditions to be set for the individual phases.
• For a fluid zone, mass sources are specified for the individual phases,
and all other sources are specified for the mixture.
If the fluid zone is not porous, all other conditions are specified for
the mixture.
If the fluid zone is porous, you will enable the Porous Zone option
in the Fluid panel for the mixture. The porosity inputs (if relevant) are also specified for the mixture. The resistance coefficients
and direction vectors, however, are specified separately for each
phase. See Section 6.19.6 for details about these inputs. All other
conditions are specified for the mixture.
See Chapter 6 for details about the relevant conditions for each type of
boundary. Note that the pressure far-field boundary is not available with
the VOF model.
20-83
Table 20.6.1: Phase-Specific and Mixture Conditions for the VOF Model
Type
exhaust fan
inlet vent
intake fan
mass flow inlet
outlet vent
pressure inlet
pressure outlet
velocity inlet
axis
fan
outflow
periodic
porous jump
radiator
solid
symmetry
wall
pressure far-field
fluid
20-84
Primary Phase
nothing
Secondary Phase
volume fraction
Mixture
all others
nothing
nothing
all others
not available
mass source;
other porous
inputs
not available
mass source;
other porous
inputs
not available
porous zone;
porosity;
all others
Mixture Model
If you are using the mixture model, the conditions you need to specify
for each type of zone are listed below and summarized in Table 20.6.2.
• For an exhaust fan, outlet vent, or pressure outlet, there are no conditions to be specified for the primary phase. For each secondary
phase, you will need to set the volume fraction as a constant, a profile (see Section 6.25), or a user-defined function (see the separate
UDF Manual). All other conditions are specified for the mixture.
• For an inlet vent, intake fan, mass flow inlet, or pressure inlet, you
will specify for the mixture which direction specification method
will be used at this boundary (Normal to Boundary or Direction
Vector). If you select the Direction Vector specification method,
you will specify the coordinate system (3D only) and flow-direction
components for the individual phases. For each secondary phase,
you will need to set the volume fraction (as described above). All
other conditions are specified for the mixture.
• For a velocity inlet, you will specify the velocity for the individual
phases. For each secondary phase, you will need to set the volume
fraction (as described above). All other conditions are specified for
the mixture.
• For an axis, fan, outflow, periodic, porous jump, radiator, solid,
symmetry, or wall zone, all conditions are specified for the mixture;
there are no conditions to be set for the individual phases.
• For a fluid zone, mass sources are specified for the individual phases,
and all other sources are specified for the mixture.
the mixture.
20-85
See Chapter 6 for details about the relevant conditions for each type of
boundary. Note that the pressure far-field boundary is not available with
the mixture model.
Table 20.6.2: Phase-Specific and Mixture Conditions for the Mixture Model
Type
exhaust fan
outlet vent
pressure outlet
inlet vent
intake fan
mass flow inlet
pressure inlet
velocity inlet
Primary Phase
nothing
Secondary Phase
volume fraction
Mixture
all others
coord. system;
flow direction
coord. system;
flow direction;
volume fraction
dir. spec.
method;
all others
velocity
all others
axis
fan
outflow
periodic
porous jump
radiator
solid
symmetry
wall
pressure far-field
fluid
nothing
velocity;
volume fraction
nothing
all others
not available
mass source;
other porous
inputs
not available
mass source;
other porous
inputs
not available
porous zone;
porosity;
all others
20-86
Eulerian Model
If you are using the Eulerian model, the conditions you need to specify
for each type of zone are listed below and summarized in Tables 20.6.3,
20.6.4, 20.6.5, and 20.6.6. Note that the specification of turbulence parameters will depend on which of the three multiphase turbulence models
you are using, as indicated in Tables 20.6.4–20.6.6. See Sections 20.4.7
and 20.6.13 for more information about multiphase turbulence models.
• For an exhaust fan, outlet vent, or pressure outlet, there are no
conditions to be specified for the primary phase if you are modeling
laminar flow or using the mixture turbulence model (the default
multiphase turbulence model).
For each secondary phase, you will need to set the volume fraction
as a constant, a profile (see Section 6.25), or a user-defined function
(see the separate UDF Manual). If the phase is granular, you will
also need to set its granular temperature.
If you are using the mixture turbulence model, you will need to
specify the turbulence boundary conditions for the mixture; if you
are using the dispersed turbulence model, you will need to specify
them for the primary phase; if you are using the per-phase turbulence model, you will need to specify them for the primary phase
and for each secondary phase.
All other conditions are specified for the mixture.
• For an inlet vent, intake fan, mass flow inlet, or pressure inlet, you
will specify for the mixture which direction specification method
will be used at this boundary (Normal to Boundary or Direction
Vector). If you select the Direction Vector specification method,
you will specify the coordinate system (3D only) and flow-direction
components for the individual phases.
(as described above). If the phase is granular, you will also need
to set its granular temperature.
20-87
• For a velocity inlet, you will specify the velocity for the individual
phases.
(as described above). If the phase is granular, you will also need
to set its granular temperature.
• For an axis, outflow, periodic, solid, or symmetry zone, all conditions are specified for the mixture; there are no conditions to be
set for the individual phases.
• For a wall zone, shear conditions are specified for the individual
phases; all other conditions are specified for the mixture.
• For a fluid zone, all source terms and fixed values are specified for
the individual phases, unless you are using the mixture turbulence
model or the dispersed turbulence model. If you are using the mixture turbulence model, source terms and fixed values for turbulence
are specified instead for the mixture; if you are using the dispersed
turbulence model, they are specified only for the primary phase.
the mixture.
20-88
See Chapter 6 for details about the relevant conditions for each type
of boundary. Note that the pressure far-field, fan, porous jump, and
radiator boundaries are not available with the Eulerian model.
20-89
Table 20.6.3: Phase-Specific and Mixture Conditions for the Eulerian Model
(for Laminar Flow)
Type
exhaust fan
outlet vent
pressure outlet
inlet vent
intake fan
mass flow inlet
pressure inlet
velocity inlet
Primary Phase
nothing
Secondary Phase
volume fraction;
gran. temperature
Mixture
all others
coord. system;
flow direction
dir. spec.
method;
all others
axis
outflow
periodic
solid
symmetry
wall
pressure far-field
fan
porous jump
radiator
fluid
nothing
coord. system;
flow direction;
volume fraction;
gran. temperature
velocity;
volume fraction;
gran. temperature
nothing
shear condition
not available
shear condition
not available
all others
not available
all source terms;
all fixed values;
other porous
inputs
all source terms;
all fixed values;
other porous
inputs
porous zone;
porosity;
all others
20-90
velocity
all others
all others
(with the Mixture Turbulence Model)
Type
exhaust fan
outlet vent
pressure outlet
inlet vent
intake fan
mass flow inlet
pressure inlet
velocity inlet
Primary Phase
nothing
Secondary Phase
volume fraction;
gran. temperature
Mixture
all others
coord. system;
flow direction
dir. spec.
method;
all others
axis
outflow
periodic
solid
symmetry
wall
pressure far-field
fan
porous jump
radiator
fluid
nothing
coord. system;
flow direction;
volume fraction;
gran. temperature
velocity;
volume fraction;
gran. temperature
nothing
shear condition
not available
shear condition
not available
all others
not available
other source
terms;
other fixed
values;
other porous
inputs
other source
terms;
other fixed
values;
other porous
inputs
source terms
for turbulence;
fixed values
for turbulence;
porous zone;
porosity;
all others
velocity
all others
all others
20-91
(with the Dispersed Turbulence Model)
Type
exhaust fan
outlet vent
pressure outlet
inlet vent
intake fan
mass flow inlet
pressure inlet
velocity inlet
axis
outflow
periodic
solid
symmetry
wall
pressure far-field
fan
porous jump
radiator
fluid
20-92
Primary Phase
turb. parameters
Secondary Phase
volume fraction;
gran. temperature
Mixture
all others
coord. system;
flow direction;
turb. parameters;
dir. spec.
method
all others
nothing
coord. system;
flow direction;
volume fraction;
gran. temperature
velocity;
volume fraction;
gran. temperature
nothing
shear condition
not available
shear condition
not available
all others
not available
momentum, mass,
turb. sources;
momentum, mass,
turb. fixed values;
other porous
inputs
momentum and
mass sources;
momentum and
mass fixed values;
other porous
inputs
porous zone;
porosity;
all others
velocity;
turb. parameters
all others
all others
(with the Per-Phase Turbulence Model)
Type
exhaust fan
outlet vent
pressure outlet
inlet vent
intake fan
mass flow inlet
pressure inlet
Primary Phase
turb. parameters
Mixture
all others
nothing
Secondary Phase
volume fraction;
turb. parameters;
gran. temperature
coord. system;
flow direction;
volume fraction;
turb. parameters;
gran. temperature
velocity;
volume fraction;
turb. parameters;
gran. temperature
nothing
velocity inlet
velocity;
turb. parameters
axis
outflow
periodic
solid
symmetry
wall
pressure far-field
fan
porous jump
radiator
fluid
shear condition
not available
shear condition
not available
all others
not available
momentum, mass,
turb. sources;
momentum, mass,
turb. fixed values;
other porous
inputs
momentum, mass,
turb. sources;
momentum, mass,
turb. fixed values;
other porous
inputs
porous zone;
porosity;
all others
coord. system;
flow direction;
turb. parameters
dir. spec.
method;
all others
all others
all others
20-93
Steps for Setting Boundary Conditions
The steps you need to perform for each boundary are as follows:
1. Select the boundary in the Zone list in the Boundary Conditions
panel.
2. Set the conditions for the mixture at this boundary, if necessary.
(See above for information about which conditions need to be set
for the mixture.)
(a) In the Phase drop-down list, select mixture.
(b) If the current Type for this zone is correct, click Set... to open
the corresponding panel (e.g., the Pressure Inlet panel); otherwise, choose the correct zone type in the Type list, confirm
the change (when prompted), and the corresponding panel
will open automatically.
(c) In the corresponding panel for the zone type you have selected
(e.g., the Pressure Inlet panel, shown in Figure 20.6.13), specify
the mixture boundary conditions.
Figure 20.6.13: The Pressure Inlet Panel for a Mixture
Note that only those conditions that apply to all phases, as
described above, will appear in this panel.
!
20-94
For a VOF calculation, if you enabled the Wall Adhesion opc Fluent Inc. November 28, 2001
tion in the Phase Interaction panel, you can specify the contact angle at the wall for each pair of phases (as shown in
Figure 20.6.14).
The contact angle (θw in Figure 20.2.2) is the angle between
the wall and the tangent to the interface at the wall, measured
inside the first phase of the pair listed in the Wall panel. For
example, if you are setting the contact angle between the oil
and air phases in the Wall panel shown in Figure 20.6.14, θw
is measured inside the oil phase.
The default value for all pairs is 90 degrees, which is equivalent to no wall adhesion effects (i.e., the interface is normal
to the adjacent wall). A contact angle of 45◦ , for example,
corresponds to water creeping up the side of a container, as
is common with water in a glass.
(d) Click OK when you are done setting the mixture boundary
conditions.
3. Set the conditions for each phase at this boundary, if necessary.
(See above for information about which conditions need to be set
for the individual phases.)
(a) In the Phase drop-down list, select the phase (e.g., water).
!
Note that, when you select one of the individual phases (rather
than the mixture), only one type of zone appears in the Type
list. It is not possible to assign phase-specific zone types at
a given boundary; the zone type is specified for the mixture,
and it applies to all of the individual phases.
(b) Click Set... to open the panel for this phase’s conditions (e.g.,
the Pressure Inlet panel, shown in Figure 20.6.15).
(c) Specify the conditions for the phase. Note that only those
conditions that apply to the individual phase, as described
above, will appear in this panel.
(d) Click OK when you are done setting the phase-specific boundary conditions.
20-95
Figure 20.6.14: The Wall Panel for a Mixture in a VOF Calculation with
Wall Adhesion
20-96
Figure 20.6.15: The Pressure Inlet Panel for a Phase
Steps for Copying Boundary Conditions
The steps for copying boundary conditions for a multiphase flow are
slightly different from those described in Section 6.1.5 for a single-phase
flow. The modified steps are listed below:
1. In the Boundary Conditions panel, click the Copy... button. This
will open the Copy BCs panel.
2. In the From Zone list, select the zone that has the conditions you
want to copy.
3. In the To Zones list, select the zone or zones to which you want to
copy the conditions.
4. In the Phase drop-down list, select the phase for which you want to
copy the conditions (either mixture or one of the individual phases).
!
Note that copying the boundary conditions for one phase does
not automatically result in the boundary conditions for the other
phases and the mixture being copied as well. You need to copy the
conditions for each phase on each boundary of interest.
5. Click Copy. FLUENT will set all of the selected phase’s (or mixture’s) boundary conditions on the zones selected in the To Zones
20-97
list to be the same as that phase’s conditions on the zone selected
in the From Zone list. (You cannot copy a subset of the conditions,
such as only the thermal conditions.)
See Section 6.1.5 for additional information about copying boundary
conditions, including limitations.
20.6.15
Setting Initial Volume Fractions
Once you have initialized the flow (as described in Section 22.13), you
can define the initial distribution of the phases. For a transient simulation, this distribution will serve as the initial condition at t = 0; for a
steady-state simulation, setting an initial distribution can provide added
stability in the early stages of the calculation.
You can patch an initial volume fraction for each secondary phase using
the Patch panel.
Solve −→ Initialize −→Patch...
If the region in which you want to patch the volume fraction is defined
as a separate cell zone, you can simply patch the value there. Otherwise,
you can create a cell “register” that contains the appropriate cells and
patch the value in the register. See Section 22.13.2 for details.
20.6.16
Inputs for Compressible VOF and Mixture Model
Calculations
If you are using the VOF or mixture model for a compressible flow, note
the following:
• Only one of the phases can be compressible (i.e., you can select the
ideal gas law for the density of only one phase’s material).
• If you are using the VOF model, for stability reasons it is better
(although not required) if the primary phase is compressible.
• If you specify the total pressure at a boundary (e.g., for a pressure
inlet or intake fan) the specified value for temperature at that
20-98
boundary will be used as total temperature for the compressible
phase, and as static temperature for the other phases (which are
incompressible).
See Section 8.5 for more information about compressible flows.
20.6.17
Inputs for Solidification/Melting VOF Calculations
If you are including melting or solidification in your VOF calculation,
note the following:
• It is possible to model melting or solidification in a single phase or
in multiple phases.
• For phases that are not melting or solidifying, you must set the
latent heat (L), liquidus temperature (Tliquidus ), and solidus temperature (Tsolidus ) to zero.
See Chapter 21 for more information about melting and solidification.
20-99
20.7
Solution Strategies for General Multiphase Problems
Solution strategies for the VOF, mixture, and Eulerian models are provided in Sections 20.7.1, 20.7.2, and 20.7.3, respectively.
20.7.1
Solution Strategies for the VOF Model
Several recommendations for improving the accuracy and convergence of
the VOF solution are presented here.
Setting the Reference Pressure Location
The site of the reference pressure can be moved to a location that will
result in less round-off in the pressure calculation. By default, the reference pressure location is the center of the cell at or closest to the point
(0,0,0). You can move this location by specifying a new Reference Pressure Location in the Operating Conditions panel.
The position that you choose should be in a region that will always
contain the least dense of the fluids (e.g., the gas phase, if you have a
gas phase and one or more liquid phases). This is because variations in
the static pressure are larger in a more dense fluid than in a less dense
fluid, given the same velocity distribution. If the zero of the relative
pressure field is in a region where the pressure variations are small, less
round-off will occur than if the variations occur in a field of large nonzero 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 filled with air rather than that filled with water.
Pressure Interpolation Scheme
For all VOF calculations, you should use the body-force-weighted pressure interpolation scheme or the PRESTO! scheme.
20-100
20.7 Solution Strategies for General Multiphase Problems
Discretization Scheme Selection for the Implicit and Euler
Explicit Formulations
When the implicit or Euler explicit scheme is used you should use the
second-order or QUICK discretization scheme for the volume fraction
equations in order to improve the sharpness of the interface between
phases.
Pressure-Velocity Coupling and Under-Relaxation for the
Time-Dependent Formulations
Another change that you should make to the solver settings is in the
pressure-velocity coupling scheme and under-relaxation factors that you
use. The PISO scheme is recommended for transient calculations in
general. Using PISO allows for increased values on all under-relaxation
factors, without a loss of solution stability. You can generally increase
the under-relaxation factors for all variables to 1 and expect stability
and a rapid rate of convergence (in the form of few iterations required
per time step). For calculations on tetrahedral or triangular meshes,
an under-relaxation factor of 0.7–0.8 for pressure is recommended for
improved stability with the PISO scheme.
As with any FLUENT simulation, the under-relaxation factors will need
to be decreased if the solution exhibits unstable, divergent behavior with
the under-relaxation factors set to 1. Reducing the time step is another
way to improve the stability.
Under-Relaxation for the Steady-State Formulation
If you are using the steady-state implicit VOF scheme, the under-relaxation
factors for all variables should be set to values between 0.2 and 0.5 for
improved stability.
20-101
20.7.2
Solution Strategies for the Mixture Model
Setting the Under-Relaxation Factor for the Slip Velocity
You should begin the mixture calculation with a low under-relaxation
factor for the slip velocity. A value of 0.2 or less is recommended. If the
solution shows good convergence behavior, you can increase this value
gradually.
Calculating an Initial Solution
For some cases (e.g., cyclone separation), you may be able to obtain a
solution more quickly if you compute an initial solution without solving
the volume fraction and slip velocity equations. Once you have set up
the mixture model, you can temporarily disable these equations and
compute an initial solution.
In the Solution Controls panel, deselect Volume Fraction and Slip Velocity
in the Equations list. You can then compute the initial flow field. Once
a converged flow field is obtained, turn the Volume Fraction and Slip
Velocity equations back on again, and compute the mixture solution.
20.7.3
Solution Strategies for the Eulerian Model
Calculating an Initial Solution
To improve convergence behavior, you may want to compute an initial
solution before solving the complete Eulerian multiphase model. There
are two methods you can use to obtain an initial solution for an Eulerian
multiphase calculation:
• Set up and solve the problem using the mixture model (with or
without slip velocities) instead of the Eulerian model. You can then
enable the Eulerian model, complete the setup, and continue the
calculation using the mixture-model solution as a starting point.
• Set up the Eulerian multiphase calculation as usual, but compute
the flow for only the primary phase. To do this, deselect Volume
20-102
20.8 Postprocessing for General Multiphase Problems
Fraction in the Equations list in the Solution Controls panel. Once
you have obtained an initial solution for the primary phase, turn
the volume fraction equations back on and continue the calculation
for all phases.
! You should not try to use a single-phase solution obtained without the
mixture or Eulerian model as a starting point for an Eulerian multiphase
calculation. Doing so will not improve convergence, and may make it
even more difficult for the flow to converge.
Temporarily Ignoring Lift and Virtual Mass Forces
If you are planning to include the effects of lift and/or virtual mass
forces in a steady-state Eulerian multiphase simulation, you can often
reduce stability problems that sometimes occur in the early stages of the
calculation by temporarily ignoring the action of the lift and the virtual
mass forces. Once the solution without these forces starts to converge,
you can interrupt the calculation, define these forces appropriately, and
continue the calculation.
20.8
Postprocessing for General Multiphase Problems
Each of the three general multiphase models provides a number of additional field functions that you can plot or report. You can also report
flow rates for individual phases for all three models, and display velocity
vectors for the individual phases in a mixture or Eulerian calculation.
Information about these postprocessing topics is provided in the following subsections:
• Section 20.8.1: Available Postprocessing Variables
• Section 20.8.2: Displaying Velocity Vectors for Individual Phases
• Section 20.8.3: Reporting Fluxes for Individual Phases
• Section 20.8.4: Reporting Forces on Walls for Individual Phases
• Section 20.8.5: Reporting Flow Rates for Individual Phases
20-103
20.8.1
Available Postprocessing Variables
When you use one of the general multiphase models, several additional
field functions will be available for postprocessing, as listed in this section. See Chapter 27 for a complete list of field functions and their definitions. Chapters 25 and 26 explain how to generate graphics displays
and reports of data.
VOF Model
For VOF calculations you can generate graphical plots or alphanumeric
reports of the following additional items:
• Volume fraction of phase-n (in the Phases... category)
• Density of phase-n (in the Density... category)
• Molecular Viscosity of phase-n (in the Properties... category)
• Thermal Conductivity of phase-n (in the Properties... category)
• Specific Heat of phase-n (in the Properties... category)
• Enthalpy of phase-n (in the Temperature... category)
• Total Enthalpy of phase-n (in the Temperature... category)
• Total Energy of phase-n (in the Temperature... category)
• Internal Energy of phase-n (in the Temperature... category)
The non-phase-specific variables that are available (e.g., Molecular Viscosity and Thermal Conductivity) represent mixture quantities. The thermal
quantities listed above will be available only for calculations that include
the energy equation.
20-104
Mixture Model
For calculations with the mixture model, you can generate graphical
plots or alphanumeric reports of the following additional items:
• phase-n Velocity Magnitude (in the Velocity... category)
• phase-n Relative Velocity Magnitude (in the Velocity... category)
• phase-n X, Y, Z, etc. Velocity (in the Velocity... category)
• phase-n Relative X, Y, Z, etc. Velocity (in the Velocity... category)
• phase-n Stream Function (in the Velocity... category)
• Diameter of phase-n (in the Properties... category)
• Thermal Conductivity of phase-n (in the Properties... category)
• Specific Heat of phase-n (in the Properties... category)
• Enthalpy of phase-n (in the Temperature... category)
• Total Enthalpy of phase-n (in the Temperature... category)
• Total Energy of phase-n (in the Temperature... category)
• Internal Energy of phase-n (in the Temperature... category)
The non-phase-specific variables that are available (e.g., Velocity Magnitude and X Velocity) represent mixture quantities. The thermal quantities listed above will be available only for calculations that include the
energy equation.
! Note that if you read a mixture-model data file into FLUENT, you will
need to run the solver for one iteration before plotting or reporting the
items listed above. (This is not necessary if you plot or report these
variables for a data set that you just computed in the current FLUENT
session.)
20-105
Eulerian Model
For Eulerian multiphase calculations you can generate graphical plots or
alphanumeric reports of the following additional items:
• phase-n Velocity Magnitude (in the Velocity... category)
• phase-n Relative Velocity Magnitude (in the Velocity... category)
• phase-n X, Y, Z, etc. Velocity (in the Velocity... category)
• phase-n Relative X, Y, Z, etc. Velocity (in the Velocity... category)
• phase-n Stream Function (in the Velocity... category)
• phase-n Turbulent Viscosity (in the Turbulence... category)
• phase-n Wall Yplus (in the Turbulence... category)
• phase-n Turbulent Kinetic Energy (in the Turbulence... category)
• phase-n Turbulent Dissipation Rate (in the Turbulence... category)
• phase-n Production of k (in the Turbulence... category)
• Diameter of phase-n (in the Properties... category)
• phase-n Wall Shear Stress (in the Wall Fluxes... category)
• phase-n X, Y, Z Wall Shear Stress (in the Wall Fluxes... category)
• phase-n Skin Friction Coefficient (in the Wall Fluxes... category)
The availability of the turbulence quantities listed above will depend on
which multiphase turbulence model you used in the calculation.
! Note that if you read an Eulerian multiphase data file into FLUENT, you
20-106
will need to run the solver for one iteration before plotting or reporting
the items listed above. (This is not necessary if you plot or report these
variables for a data set that you just computed in the current FLUENT
session.)
20.8.2
Displaying Velocity Vectors for Individual Phases
For mixture and Eulerian calculations, it is possible to display velocity
vectors for the individual phases using the Vectors panel.
Display −→Vectors...
To display the velocity of a particular phase, select phase-n Velocity
(where phase-n is replaced by the name of the phase of interest, e.g., airbubbles Velocity) in the Vectors Of drop-down list. You can also choose
Relative phase-n Velocity to display the phase velocity relative to a moving reference frame. To display the mixture velocity ~vm (relevant for
mixture model calculations only), select Velocity (or Relative Velocity for
the mixture velocity relative to a moving reference frame).
20.8.3
Reporting Fluxes for Individual Phases
When you use the Flux Reports panel to compute fluxes through boundaries, you will be able to specify whether the report is for the mixture
or for an individual phase.
Report −→Fluxes...
Select mixture in the Phase drop-down list at the bottom of the panel
to report fluxes for the mixture, or select the name of a phase to report
fluxes just for that phase.
20.8.4
Reporting Forces on Walls for Individual Phases
For Eulerian calculations, when you use the Force Reports panel to compute forces or moments on wall boundaries, you will be able to specify
the individual phase for which you want to compute the forces.
Report −→Forces...
20-107
Select the name of the desired phase in the Phase drop-down list on the
left side of the panel.
20.8.5
Reporting Flow Rates for Individual Phases
You can obtain a report of mass flow rate for each phase (and the mixture) through each flow boundary using the report/mass-flow text
command:
report −→mass-flow
When you specify the phase of interest (the mixture or an individual
phase), FLUENT will list each zone, followed by the mass flow rate
through that zone for the specified phase. An example is shown below.
/report> mf
(mixture water air)
domain id/name [mixture] air
zone 10 (spiral-press-outlet): -1.2330244
zone 3 (pressure-outlet): -9.7560663
zone 11 (spiral-vel-inlet): 0.6150589
zone 8 (spiral-wall): 0
zone 1 (walls): 0
zone 4 (velocity-inlet): 4.9132133
net mass-flow: -5.4608185
20-108

Chapter 20. General Multiphase Models

Transcription

Documents pareils

CV Anglais COLIN Elodie

216 F09-E1

Caramel Popcorn Clusters

GLYCEROL

fractionation of hydrocarbons between oil and gas phases

Application Form - Executive Education

Chapter 21. Modeling Solidification and Melting

Resale Range Professional Range

MSDS - HQ POWER - SCENT PASSION -VDLSLF3

Using the Models TA-460, PVM610, and PVM620 to Measure