Section 20.1: Choosing a General Multiphase Model. Section 20.2: Volume of Fluid (VOF) Model. Section 20.6: Setting Up a General Multiphase Problem

Transcription

1 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,

2 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 , , and Detailed descriptions of the models are provided in Sections 20.2, 20.3, and 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 c Fluent Inc. November 28, 2001

3 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. c Fluent Inc. November 28,

4 General Multiphase Models 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 c Fluent Inc. November 28, 2001

5 20.1 Choosing a General Multiphase Model 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. The second-order implicit time-stepping formulation cannot be used 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 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 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: c Fluent Inc. November 28,

6 General Multiphase Models 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-ɛ 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-ɛ 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. The second-order implicit time-stepping formulation cannot be used with the Eulerian model c Fluent Inc. November 28, 2001

7 20.1 Choosing a General Multiphase Model 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 ). c Fluent Inc. November 28,

8 General Multiphase Models 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 α q,then the following three conditions are possible: α q = 0: the cell is empty (of the qth fluid). α q = 1: the cell is full (of the qth fluid) 0 <α q < 1: the cell contains the interface between the qth fluid and one or more other fluids. Based on the local value of α q, the appropriate properties and variables will be assigned to each control volume within the domain 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: α q t + v α q = S α q ρ q (20.2-1) By default, the source term on the right-hand side of Equation is zero, but you can specify a constant or user-defined mass source for each phase c Fluent Inc. November 28, 2001

9 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: Properties n α q = 1 (20.2-2) q=1 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 = α 2 ρ 2 +(1 α 2 )ρ 1 (20.2-3) In general, for an n-phase system, the volume-fraction-averaged density takes on the following form: ρ = α q ρ q (20.2-4) All other properties (e.g., viscosity) are computed in this manner 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. ( (ρ v)+ (ρ v v) = p + [ µ v + v T)] + ρ g + F t (20.2-5) c Fluent Inc. November 28,

10 General Multiphase Models 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 The Energy Equation The energy equation, also shared among the phases, is shown below. t (ρe)+ ( v(ρe + p)) = (k eff T )+S h (20.2-6) The VOF model treats energy, E, and temperature, T, as mass-averaged variables: E = n α q ρ q E q q=1 (20.2-7) n α q ρ q q=1 where E q for each phase is based on the specific heat of that phase and the shared temperature. The properties ρ and k eff (effective thermal conductivity) are shared by the phases. The source term, S h, 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 c Fluent Inc. November 28, 2001

11 20.2 Volume of Fluid (VOF) Model 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 ɛ or the Reynolds stresses) are shared by the phases throughout the field 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, FLUENT applies a special interpolation treatment to the cells that lie near the interface between two phases. Figure shows an actual interface shape along with the interfaces assumed during computation by these two methods. 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 c Fluent Inc. November 28,

12 General Multiphase Models actual interface shape interface shape represented by the geometric reconstruction (piecewise-linear) scheme interface shape represented by the donor-acceptor scheme Figure : Interface Calculations c Fluent Inc. November 28, 2001

13 20.2 Volume of Fluid (VOF) Model! 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 ) 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 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. c Fluent Inc. November 28,

14 General Multiphase Models! 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 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. α n+1 q α n q t V + f (U n f αn q,f ) = 0 (20.2-8)! where n + 1 = index for new (current) time step n = index for previous time step α q,f = face value of the qth volume fraction, computed from the first- or second-order upwind or QUICK scheme V = volume of cell U f = 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 c Fluent Inc. November 28, 2001

15 20.2 Volume of Fluid (VOF) Model The Implicit Scheme In the implicit interpolation method, FLUENT s standardfinite-difference interpolation schemes are used to obtain the face fluxes for all cells, including those near the interface. α n+1 q α n q t V + f (U n+1 f α n+1 q,f ) = 0 (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 for details Time Dependence For time-dependent VOF calculations, Equation 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 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 c Fluent Inc. November 28,

16 General Multiphase Models 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, R 1 and R 2 : ( 1 p 2 p 1 = σ + 1 ) R1 R2 ( ) where p 1 and p 2 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 α q,the volume fraction of the qth phase. n = α q ( ) The curvature, κ, is defined in terms of the divergence of the unit normal, ˆn [25]: c Fluent Inc. November 28, 2001

17 20.2 Volume of Fluid (VOF) Model κ = ˆn ( ) where ˆn = n n ( ) 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: F vol = pairs ij, i<j σ ij α i ρ i κ j α j + α j ρ j κ i α i 1 2 (ρ i + ρ j ) ( ) 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 κ i = κ j and α i = α j, and Equation simplifies to F vol = σ ij ρκ i α i 1 2 (ρ i + ρ j ) ( ) where ρ is the volume-averaged density computed using Equation Equation 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 c Fluent Inc. November 28,

18 General Multiphase Models 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 ( ) and for Re 1, the quantity of interest is the Weber number: We = σ ρlu 2 ( ) where U is the free-stream velocity. Surface tension effects can be neglected if Ca 1orWe 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 θ w is the contact angle at the wall, then the surface normal at the live cell next to the wall is ˆn =ˆn w cos θ w + ˆt w sin θ w ( ) where ˆn w and ˆt w 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 θ w 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 c Fluent Inc. November 28, 2001

19 20.2 Volume of Fluid (VOF) Model second phase interface θ w first phase wall Figure : Measuring the Contact Angle c Fluent Inc. November 28,

20 General Multiphase Models 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 α q and α p 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) Continuity Equation for the Mixture The continuity equation for the mixture is where v m is the mass-averaged velocity: t (ρ m)+ (ρ m v m )=ṁ (20.3-1) v m = nk=1 α k ρ k v k ρ m (20.3-2) and ρ m is the mixture density: n ρ m = α k ρ k (20.3-3) k= c Fluent Inc. November 28, 2001

21 20.3 Mixture Model α k is the volume fraction of phase k. ṁ represents mass transfer due to cavitation (described in Section 20.5) or user-defined mass sources 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 ( )] t (ρ m v m )+ (ρ m v m v m )= p + [µ m v m + v m T + ( n ) ρ m g + F + α k ρ k v dr,k v dr,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: n µ m = α k µ k (20.3-5) k=1 v dr,k is the drift velocity for secondary phase k: Energy Equation for the Mixture v dr,k = v k v m (20.3-6) The energy equation for the mixture takes the following form: t n (α k ρ k E k )+ k=1 n (α k v k (ρ k E k + p)) = (k eff T )+S E (20.3-7) k=1 where k eff is the effective conductivity (k + k t,wherek t is the turbulent thermal conductivity, defined according to the turbulence model being c Fluent Inc. November 28,

22 General Multiphase Models used). The first term on the right-hand side of Equation represents energy transfer due to conduction. S E includes any other volumetric heat sources. In Equation , E k = h k p ρ k + v2 k 2 (20.3-8) for a compressible phase, and E k = h k for an incompressible phase, where h k is the sensible enthalpy for phase k 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): v qp = v p v q (20.3-9) The drift velocity and the relative velocity ( v qp ) are connected by the following expression: v dr,p = v qp n k=1 α k ρ k ρ m v qk ( ) 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 v qp = τ qp a ( ) where a is the secondary-phase particle s acceleration and τ qp is the particulate relaxation time. Following Manninen et al. [150] τ qp is of the form: c Fluent Inc. November 28, 2001

23 20.3 Mixture Model τ qp = (ρ m ρ p )d 2 p 18µ q f drag ( ) where d p is the diameter of the particles (or droplets or bubbles) of secondary phase p, and the drag function f drag is taken from Schiller and Naumann [202]: f drag = { Re Re Re Re > 1000 ( ) and the acceleration a is of the form a = g ( v m ) v m v m t ( ) 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 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: t (α pρ p )+ (α p ρ p v m )= (α p ρ p v dr,p ) ( ) c Fluent Inc. November 28,

24 General Multiphase Models 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 α 1,α 2,... α n 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 : Volume Fractions Section : Conservation Equations Section : Interphase Exchange Coefficients Section : Solids Pressure Section : Solids Shear Stresses Section : Granular Temperature Section : Turbulence Models Section : Solution Method in FLUENT Volume Fractions The description of multiphase flow as interpenetrating continua incorporates the concept of phasic volume fractions, denoted here by α q. 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, V q, is defined by c Fluent Inc. November 28, 2001

25 20.4 Eulerian Model V q = V α q dv (20.4-1) where n α q = 1 (20.4-2) q=1 The effective density of phase q is where ρ q is the physical density of phase q Conservation Equations ˆρ q = α q ρ q (20.4-3) 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 t (α qρ q )+ (α q ρ q v q )= n ṁ pq (20.4-4) p=1 where v q is the velocity of phase q and ṁ pq characterizes the mass transfer from the p th to q th phase. From the mass conservation one can obtain and ṁ pq = ṁ qp (20.4-5) c Fluent Inc. November 28,

26 General Multiphase Models ṁ pp = 0 (20.4-6) Conservation of Momentum The momentum balance for phase q yields t (α qρ q v q )+ (α q ρ q v q v q ) = α q p + τ q + n ( R pq +ṁ pq v pq )+ p=1 α q ρ q ( F q + F lift,q + F vm,q ) (20.4-7) where τ q is the q th phase stress-strain tensor τ q = α q µ q ( v q + v T q )+α q(λ q 2 3 µ q) v q I (20.4-8) Here µ q and λ q are the shear and bulk viscosity of phase q, Fq is an external body force, Flift,q is a lift force, Fvm,q is a virtual mass force, R pq is an interaction force between phases, and p is the pressure shared by all phases. v pq is the interphase velocity, defined as follows. If ṁ pq > 0 (i.e., phase p mass is being transferred to phase q), v pq = v p ;ifṁ pq < 0 (i.e., phase q mass is being transferred to phase p), v pq = v q ;and v pq = v qp. Equation must be closed with appropriate expressions for the interphase force R pq. This force depends on the friction, pressure, cohesion, and other effects, and is subject to the conditions that R pq = R qp and R qq =0. FLUENT uses a simple interaction term of the following form: n n R pq = K pq ( v p v q ) (20.4-9) p=1 p=1 where K pq (= K qp ) is the interphase momentum exchange coefficient (described in Section ) c Fluent Inc. November 28, 2001

27 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] F lift = 0.5ρ q α p v q v p ( v q ) ( ) The lift force F lift will be added to the right-hand side of the momentum equation for both phases (F lift,q = F lift,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, F lift 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]: F vm =0.5α p ρ q ( dq v q dt d ) pv p dt ( ) The term dq dt denotes the phase material time derivative of the form d q (φ) dt = (φ) t +( v q )φ ( ) c Fluent Inc. November 28,

28 General Multiphase Models The virtual mass force F vm will be added to the right-hand side of the momentum equation for both phases (F vm,q = F vm,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, F vm 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: t (α q)+ (α q v q )= 1 ρ q n p=1 ṁ pq α q d q ρ q dt ( ) The solution of this equation for each secondary phase, along with the condition that the volume fractions sum to one (given by Equation ), 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 t (α qρ q v q )+ (α q ρ q v q v q ) = α q p + τ q + α q ρ q g + α q ρ q ( F q + F lift,q + F vm,q )+ n (K pq ( v p v q )+ṁ pq v pq ) p=1 ( ) c Fluent Inc. November 28, 2001

29 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 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 , and that for the s th solid phase is t (α sρ s v s )+ (α s ρ s v s v s ) = α s p p s + τ s + α s ρ s g + α s ρ s ( F s + F lift,s + F vm,s )+ N (K ls ( v l v s )+ṁ ls v ls ) ( ) where p s is the s th solids pressure, K ls = K sl 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, Flift,q, and F vm,q are as defined for Equation l= Interphase Exchange Coefficients It can be seen in Equations and that momentum exchange between the phases is based on the value of the fluid-fluid exchange coefficient K pq and, for granular flows, the fluid-solid and solid-solid exchange coefficients K ls. c Fluent Inc. November 28,

30 General Multiphase Models 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: K pq = α pρ p f τ p ( ) where f, the drag function, is defined differently for the different exchangecoefficient models (as described below) and τ p, the particulate relaxation time, is defined as τ p = ρ pd 2 p 18µ q ( ) where d p is the diameter of the bubbles or droplets of phase p. Nearly all definitions of f includeadragcoefficient(c D )thatisbasedon 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] where f = C DRe 24 ( ) C D = { 24( Re )/Re Re Re > 1000 ( ) and Re is the relative Reynolds number. The relative Reynolds number for the primary phase q and secondary phase p is obtained from c Fluent Inc. November 28, 2001

31 20.4 Eulerian Model Re = ρ q v p v q d p µ q ( ) The relative Reynolds number for secondary phases p and r is obtained from Re = ρ rp v r v p d rp µ rp ( ) where µ rp = α p µ p + α r µ r 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] where f = C DRe 24 ( ) C D = a 1 + a 2 Re + a 3 Re 2 ( ) and Re is defined by Equation or The a s are defined as follows: a 1,a 2,a 3 = 0, 18, 0 0 <Re< , 22.73, <Re< , , <Re< , 46.50, <Re< , 98.33, <Re< , , <Re< , , <Re< , , Re ( ) The Morsi and Alexander model is the most complete, adjusting the function definition frequently over a large range of Reynolds c Fluent Inc. November 28,

32 General Multiphase Models numbers, but calculations with this model may be less stable than with the other models. For the symmetric model where K pq = α p(α p ρ p + α q ρ q )f τ pq ( ) τ pq = (α pρ p + α q ρ q )( dp+dq 2 ) 2 18(α p µ p + α q µ q ) ( ) and where f = C DRe 24 ( ) C D = { 24( Re )/Re Re Re > 1000 ( ) and Re is defined by Equation or 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 c Fluent Inc. November 28, 2001

33 20.4 Eulerian Model Fluid-Solid Exchange Coefficient The fluid-solid exchange coefficient K sl can be written in the following general form: K sl = α sρ s f τ s ( ) where f is defined differently for the different exchange-coefficient models (as described below), and τ s, the particulate relaxation time, is defined as where d s is the diameter of particles of phase s. τ s = ρ sd 2 s 18µ l ( ) All definitions of f include a drag function (C D )thatisbasedonthe relative Reynolds number (Re s ). It is this drag function that differs among the exchange-coefficient models. For the Syamlal-O Brien model [234] f = C DRe s α l 24v 2 r,s ( ) where the drag function has a form derived by Dalla Valle [47] C D = Re s /v r,s 2 ( ) 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]: Re s = ρ ld s v s v l µ l ( ) c Fluent Inc. November 28,

34 General Multiphase Models where the subscript l is for the l th fluid phase, s is for the s th solid phase, and d s is the diameter of the s th solid phase particles. The fluid-solid exchange coefficient has the form K sl = 3α ( ) sα l ρ l Res 4vr,s 2 d C D v s v l ( ) s v r,s where v r,s is the terminal velocity correlation for the solid phase [73]: ( ) v r,s =0.5 A 0.06Re s + (0.06Re s ) Re s (2B A)+A 2 with and ( ) A = α 4.14 l ( ) for α l 0.85, and B =0.8α 1.28 l ( ) B = α 2.65 l ( ) for α l > This model is appropriate when the solids shear stresses are defined according to Syamlal et al. [235] (Equation ). For the model of Wen and Yu [262], the fluid-solid exchange coefficient is of the following form: where K sl = 3 4 C α s α l ρ l v s v l D α 2.65 l ( ) d s c Fluent Inc. November 28, 2001

35 20.4 Eulerian Model C D = 24 α l Re s [ (α l Re s ) 0.687] ( ) and Re s is defined by Equation 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 α l > 0.8, the fluid-solid exchange coefficient K sl is of the following form: where When α l 0.8, K sl = 3 4 C α s α l ρ l v s v l D αl 2.65 ( ) d s C D = 24 α l Re s [ (α l Re s ) 0.687] ( ) K sl = 150 α s(1 α l )µ l α l d 2 s ρ lα s v s v l d s ( ) This model is recommended for dense fluidized beds. Solid-Solid Exchange Coefficient The solid-solid exchange coefficient K ls has the following form [233]: K ls = 3(1+e ls) ( ) π 2 + C fr,ls π2 8 α s ρ s α l ρ l (d l + d s ) 2 g 0,ls 2π ( ρ l d 3 l + ρ sd 3 ) v l v s s ( ) c Fluent Inc. November 28,

36 General Multiphase Models where e ls = the coefficient of restitution (described in Section ) C fr,ls = the coefficient of friction between the l th and s th solid-phase particles (C fr,ls =0) d l = the diameter of the particles of solid l g 0,ls = the radial distribution coefficient (described in Section ) 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, p s, 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: p s = α s ρ s Θ s +2ρ s (1 + e ss )α 2 sg 0,ss Θ s ( ) where e ss is the coefficient of restitution for particle collisions, g 0,ss is the radial distribution function, and Θ s is the granular temperature. FLU- ENT uses a default value of 0.9 for e ss, but the value can be adjusted to suit the particle type. The granular temperature Θ s is proportional to the kinetic energy of the fluctuating particle motion, and will be described later in this section. The function g 0,ss (described below in more detail) is a distribution function that governs the transition from the compressible condition with α<α s,max, where the spacing between the solid particles can continue to decrease, to the incompressible condition with α = α s,max, where no further decrease in the spacing can occur. A value of 0.63 is the default for α s,max, but you can modify it during the problem setup c Fluent Inc. November 28, 2001

37 20.4 Eulerian Model Radial Distribution Function The radial distribution function, g 0, 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: g 0 = s + d p s ( ) where s is the distance between grains. From Equation it can be observed that for a dilute solid phase s, and therefore g 0 1. In the limit when the solid phase compacts, s 0andg 0. 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]: g 0 = 1 ( αs α s,max ) ( ) When the number of solid phases is greater than 1, Equation is extended to g 0,ll = 1 ( αl α l,max ) ( ) where α l,max is specified by you during the problem setup, and g 0,lm = d mg 0,ll + d l g 0,mm d m + d l ( ) c Fluent Inc. November 28,

38 General Multiphase Models 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: µ s = µ s,col + µ s,kin + µ s,fr ( ) Collisional Viscosity The collisional part of the shear viscosity is modeled as [76, 235] µ s,col = 4 5 α sρ s d s g 0,ss (1 + e ss ) Kinetic Viscosity ( Θs FLUENT provides two expressions for the kinetic part. The default expression is from Syamlal et al. [235]: π ) 1/2 ( ) µ s,kin = α sd s ρ s Θs π 6(3 e ss ) [1+ 25 (1 + e ss)(3e ss 1) α s g 0,ss ] ( ) The following optional expression from Gidaspow et al. [76] is also available: µ s,kin = [ 10ρ s d s Θs π α s (1 + e ss ) g 0,ss 5 g 0,ssα s (1 + e ss )] ( ) c Fluent Inc. November 28, 2001

39 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]: λ s = 4 3 α sρ s d s g 0,ss (1 + e ss ) ( Θs π ) 1/2 ( ) 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: µ s,fr = p s sin φ 2 I 2D ( ) where p s is the solids pressure, φ is the angle of internal friction, and I 2D is the second invariant of the deviatoric stress tensor. It is also possible to specify a constant or user-defined frictional viscosity Granular Temperature The granular temperature for the s th 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 2 t (ρ sα s Θ s )+ (ρ s α s v s Θ s ) = ( p s I + τ s ): v s c Fluent Inc. November 28,

40 General Multiphase Models where (k Θs Θ s ) γ Θs + φ ls ( ) ( p s I + τ s ): v s = the generation of energy by the solid stress tensor k Θs Θ s = the diffusion of energy (k Θs is the diffusion coefficient) γ Θs = the collisional dissipation of energy φ ls = the energy exchange between the l th fluid or solid phase and the s th solid phase Equation contains the term k Θs Θ s describing the diffusive flux of granular energy. The collisional dissipation of energy, γ Θs, represents the rate of energy dissipation within the s th solids phase due to collisions between particles. This term is represented by the expression derived by Lun et al. [145] γ Θm = 12(1 e2 ss)g 0,ss d s π ρ s α 2 s Θ3/2 s ( ) The transfer of the kinetic energy of random fluctuations in particle velocity from the s th solids phase to the l th fluid or solid phase is represented by φ ls [76]: φ ls = 3K ls Θ s ( ) FLUENT currently uses an algebraic relation for the granular temperature. This has been obtained by neglecting convection and diffusion in the transport equation, Equation [235] 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, c Fluent Inc. November 28, 2001

41 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-ɛ 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-ɛ model. The multiphase modifications to the RNG and realizable k-ɛ 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-ɛ 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 ɛ equations describing this model are as follows: and ( ) t (ρ µt,m mk)+ (ρ m v m k)= k + G k,m ρ m ɛ ( ) σ k c Fluent Inc. November 28,

42 General Multiphase Models ( ) t (ρ µt,m mɛ)+ (ρ m v m ɛ)= ɛ + ɛ σ ɛ k (C 1ɛG k,m C 2ɛ ρ m ɛ) ( ) where the mixture density and velocity, ρ m and v m, are computed from N ρ m = α i ρ i ( ) i=1 and v m = N α i ρ i v i i=1 ( ) N α i ρ i i=1 the turbulent viscosity, µ t,m, is computed from µ t,m = ρ m C µ k 2 ɛ ( ) and the production of turbulence kinetic energy, G k,m, is computed from G k,m = µ t,m ( v m +( v m ) T ): v m ( ) The constants in these equations are the same as those described in Section for the single-phase k-ɛ 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 c Fluent Inc. November 28, 2001

43 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: Amodifiedk-ɛ model for the continuous phase: Turbulent predictions for the continuous phase are obtained using the standard k-ɛ 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. c Fluent Inc. November 28,

44 General Multiphase Models 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: τ q = 2 3 (ρ qk q + ρ q µ t,q U q )I + ρ q µ t,q ( U q + U q T ) ( ) where U q is the phase-weighted velocity. The turbulent viscosity µ t,q is written in terms of the turbulent kinetic energy of phase q: µ t,q = ρ q C µ k 2 q ɛ q ( ) and a characteristic time of the energetic turbulent eddies is defined as where ɛ q is the dissipation rate and C µ =0.09. The length scale of the turbulent eddies is τ t,q = 3 2 C k q µ ( ) ɛ q L t,q = 3 2 C k 3 2 q µ ( ) ɛ q Turbulent predictions are obtained from the modified k-ɛ model: t (α qρ q k q )+ (α q ρ quq µ t,q k q ) = (α q k q )+α q G k,q α q ρ q ɛ q + σ k α q ρ q Π kq ( ) and c Fluent Inc. November 28, 2001

45 20.4 Eulerian Model t (α qρ q ɛ q )+ (α q ρ q Uq ɛ q ) = (α q µ t,q σ ɛ ɛ q )+ α q ɛ q k q (C 1ɛ G k,q C 2ɛ ρ q ɛ q )+ α q ρ q Π ɛq ( ) Here Π kq and Π ɛq represent the influence of the dispersed phases on the continuous phase q, andg k,q is the production of turbulent kinetic energy, as defined in Section All other terms have the same meaning as in the single-phase k-ɛ model. The term Π kq can be derived from the instantaneous equation of the continuous phase and takes the following form, where M represents the number of secondary phases: Π kq = M p=1 which can be simplified to K pq α q ρ q (< v q v p > +( U p U q ) v dr ) ( ) Π kq = M p=1 K pq α q ρ q (k pq 2k q + v pq v dr ) ( ) where k lq is the covariance of the velocities of the continuous phase q and the dispersed phase l (calculated from Equation below), v pq is the relative velocity, and v dr is the drift velocity (defined by Equation below). Π ɛq is modeled according to Elgobashi et al. [61]: where C 3ɛ =1.2. Π ɛq = C 3ɛ ɛ q k q Π kq ( ) c Fluent Inc. November 28,

46 General Multiphase Models 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 τ F,pq = α p ρ p K 1 pq ( ) ρp + C V ρ q ( ) The Lagrangian integral time scale calculated along particle trajectories, mainly affected by the crossing-trajectory effect [43], is defined as τ t,pq = τ t,q (1 + C β ξ 2 ) ( ) where ξ = v pq τ t,q L t,q ( ) and C β = cos 2 θ ( ) 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 η pq = τ t,pq τ F,pq ( ) Following Simonin [212], FLUENT writes the turbulence quantities for dispersed phase p as follows: c Fluent Inc. November 28, 2001

47 20.4 Eulerian Model ( b 2 ) + η pq k p = k q 1+η pq ( ) b + ηpq k pq = 2k q 1+η pq ( ) ( ) D t,pq = 1 3 k pqτ t,pq ( ) ( 2 D p = D t,pq + 3 k p b 1 ) 3 k pq τ F,pq ( ) b = (1+C V ) ( ρp ρ q + C V ) 1 ( ) and C V =0.5 is the added-mass coefficient. Interphase Turbulent Momentum Transfer The turbulent drag term for multiphase flows (K pq ( v p v q )inequation ) is modeled as follows, for dispersed phase p and continuous phase q: K pq ( v p v q )=K pq ( U p U q ) K pq v dr ( ) The second term on the right-hand side of Equation contains the drift velocity: v dr = ( Dp α p D ) q α q σ pq α p σ pq α q ( ) Here D p and D q are diffusivities, and σ pq is a turbulent Schmidt number. When using Tchen theory in multiphase flows, FLUENT assumes D p = D q = D t,pq and the default value for σ pq is The drift velocity results from turbulent fluctuations in the volume fraction. When multiplied by the exchange coefficient K pq,itservesasa correction to the momentum exchange term for turbulent flows. This c Fluent Inc. November 28,

48 General Multiphase Models 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 ɛ 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 and Turbulence predictions are obtained from t (α qρ q k q )+ (α q ρ q Uq k q ) = (α q µ t,q σ k k q )+(α q G k,q α q ρ q ɛ q )+ and N K lq (C lq k l C ql k q ) l=1 N l=1 N l=1 K lq ( U l U q ) µt,l α l σ l α l + K lq ( U l U q ) µ t,q α q σ q α q ( ) t (α qρ q ɛ q )+ (α q ρ q Uq ɛ q ) = (α q µ t,q σ ɛ ɛ q )+ ɛ q k q (C 1ɛ α q G k,q C 2ɛ α q ρ q ɛ q c Fluent Inc. November 28, 2001

49 20.4 Eulerian Model N C 3ɛ ( K lq (C lq k l C ql k q ) N l=1 N l=1 l=1 K lq ( U l U q ) µt,l α l σ l α l + K lq ( U l U q ) µ t,q α q σ q α q )) ( ) The terms C lq and C ql can be approximated as C lq = 2 C ql = 2 ( ηlq 1+η lq ) ( ) where η lq is defined by Equation Interphase Turbulent Momentum Transfer The turbulent drag term (K pq ( v p v q ) in Equation ) is modeled as follows, where l is the dispersed phase (replacing p in Equation ) and q is the continuous phase: N K lq ( v l v q )= l=1 N K lq ( U l U N q ) K lq v dr,lq ( ) l=1 Here U l and U q are phase-weighted velocities, and v dr,lq is the drift velocity for phase l (computed using Equation , substituting l for p). Note that FLUENT will compute the diffusivities D l and D q 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 K lq, it serves as a correction to the momentum exchange term for turbulent l=1 c Fluent Inc. November 28,

50 General Multiphase Models 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 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 k=1 { t α k + α k v k + α k v k 1 ρ k } n ṁ lk = 0 ( ) where v k is the velocity correction for the kth phase and v k is the value of v k 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 k th volume fraction is l= c Fluent Inc. November 28, 2001

51 20.5 Cavitation Effects a p,k α k = nb (a nb,k α nb,k )+b k = R k ( ) In order to satisfy the condition that all the volume fractions sum to one, 20.5 Cavitation Effects n α k = 1 ( ) k=1 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 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. c Fluent Inc. November 28,

52 General Multiphase Models 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 where R is the bubble radius. The volume fraction of vapor is defined as φ( r, t) = 4 3 πr3 (20.5-1) α v = 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: c Fluent Inc. November 28, 2001

53 20.5 Cavitation Effects t (α p)+ (α p v m )= ρ l η dφ ρ m (1 + ηφ) 2 dt + αρ v dρ v ρ m dt (20.5-3) Bubble Dynamics Since cavitation bubbles will form in a liquid at low temperatures, FLU- ENT 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 dt ( ) dr 2 = p B p 2σ 2 dt ρ l ρ l R 4 µ l dr ρ l R dt (20.5-4) Here p B denotes the pressure within the bubble, represented by the sum of a partial pressure (p v ) 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 dr dt = 2(pB p) 3ρ l, p v >p 2(pB p) 3ρ l, p v <p (20.5-5) c Fluent Inc. November 28,

54 General Multiphase Models 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 : Steps for Using the General Multiphase Models Section : Additional Guidelines for Eulerian Multiphase Simulations Section : Enabling the Multiphase Model and Specifying the Number of Phases Section : Selecting the VOF Formulation Section : Defining a Homogeneous Multiphase Flow Section : Including Cavitation Effects Section : Overview of Defining the Phases Section : Defining Phases for the VOF Model Section : Defining Phases for the Mixture Model Section : Defining Phases for the Eulerian Model Section : Including Body Forces Section : Setting Time-Dependent Parameters for the VOF Model Section : Selecting a Turbulence Model for an Eulerian Multiphase Calculation Section : Setting Boundary Conditions Section : Setting Initial Volume Fractions Section : Inputs for Compressible VOF and Mixture Model Calculations Section : Inputs for Solidification/Melting VOF Calculations c Fluent Inc. November 28, 2001

55 20.6 Setting Up a General Multiphase Problem 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 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 and 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 for details about copying from the database and creating new materials. See Section 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 for details. c Fluent Inc. November 28,

56 General Multiphase Models 4. (Eulerian model only) If the flow is turbulent, define the multiphase turbulence model. Define Models Viscous... See Section for details. 5. If body forces are present, turn on gravity and specify the gravitational acceleration. Define Operating Conditions... See Section for details. 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... See Section for details. 7. Set any model-specific solution parameters. Solve Controls Solution... See Sections and 20.7 for details. 8. Initialize the solution and set the initial volume fractions for the secondary phases. Solve Initialize Patch... See Section for details. 9. Calculate a solution and examine the results. See Sections 20.7 and 20.8 for details 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 c Fluent Inc. November 28, 2001

57 20.6 Setting Up a General Multiphase Problem 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 for more solution strategies for Eulerian multiphase calculations Enabling the Multiphase Model and Specifying the Number of Phases To enable the VOF, mixture, or Eulerian multiphase model, select Volume of Fluid, Mixture, oreulerian as the Model in the Multiphase Model panel (Figure ). 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 ) c Fluent Inc. November 28,

58 General Multiphase Models Figure : The Multiphase Model Panel (optional) implicit body force formulation (see Section ) If you selected the mixture model, the inputs are as follows: number of phases whether or not to compute the slip velocities (see Section ) (optional) implicit body force formulation (see Section ) (optional) cavitation effects (see Section ) c Fluent Inc. November 28, 2001

59 20.6 Setting Up a General Multiphase Problem If you selected the Eulerian model, the inputs are as follows: number of phases (optional) cavitation effects (see Section ) 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 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 c Fluent Inc. November 28,

60 General Multiphase Models 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 c Fluent Inc. November 28, 2001

61 20.6 Setting Up a General Multiphase Problem! 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 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 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 If you want to solve a homogeneous multiphase flow, turn off Slip Velocity under Mixture Parameters. c Fluent Inc. November 28,

62 General Multiphase Models 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 (p v in Equation ) and the Bubble Number Density (η in Equation ). The default value of η is 10000, as recommended by Kubota et al. [119]. The default value of p v is , the vaporization pressure for water at ambient temperature. See Section 20.5 for details about modeling cavitation 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 ). 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 , , and for the VOF, mixture, and Eulerian models, respectively c Fluent Inc. November 28, 2001

63 20.6 Setting Up a General Multiphase Problem Figure : The Phases Panel 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. See Section for details. c Fluent Inc. November 28,

64 General Multiphase Models 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 ) will open. Figure : 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..., andthematerial 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 for specific information related to compressible VOF calculations, and Section 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 c Fluent Inc. November 28, 2001

65 20.6 Setting Up a General Multiphase Problem 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 ) will open. Figure : The Secondary Phase Panel for the VOF Model 3. In the Secondary 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, 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 , the importance of surface tension effects depends on the value of the capillary number, Ca (defined by Equation ), or the Weber number, We (defined by Equation ). Surface tension effects can be neglected if Ca 1orWe 1. Note that the calculation of surface tension effects will be more accu- c Fluent Inc. November 28,

66 General Multiphase Models 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 , click Interaction... to open the Phase Interaction panel (Figure ). Figure : 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 c Fluent Inc. November 28, 2001

67 20.6 Setting Up a General Multiphase Problem 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 ) 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 for details 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. See Section for details. Defining the Primary Phase The procedure for defining the primary phase in a mixture model calculation is the same as for a VOF calculation. See Section for details. Defining a Secondary Phase To define a secondary phase in a mixture model calculation, follow these steps: c Fluent Inc. November 28,

68 General Multiphase Models 1. Select the phase (e.g., phase-2) in the Phase list. 2. Click Set..., and the Secondary Phase panel (Figure ) will open. Figure : The Secondary Phase Panel for the Mixture Model 3. In the Secondary 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, following the same procedure you used to set the material properties for the primary phase (see Section ). For a particulate phase (which must be placed in the fluid materials category, as mentioned in Section ), you need to specify only the density; you can ignore the values for the other properties, since they will not be used c Fluent Inc. November 28, 2001

69 20.6 Setting Up a General Multiphase Problem 6. In the Secondary Phase panel, specify the Diameter of the bubbles, droplets, or particles of this phase (d p in Equation ). You can specify a constant value, or use a user-defined function. See the separate UDF Manual for details about user-defined functions. 7. Click OK in the Secondary Phase panel. 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 ). Figure : 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 c Fluent Inc. November 28,

70 General Multiphase Models 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 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. Defining the Primary Phase The procedure for defining the primary phase in an Eulerian multiphase calculation is the same as for a VOF calculation. See Section 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: 1. Select the phase (e.g., phase-2) in the Phase list. 2. Click Set..., and the Secondary Phase panel (Figure ) will open. 3. In the Secondary 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, following the same procedure you used to set the material properties for the primary phase (see Section ). 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 c Fluent Inc. November 28, 2001

71 20.6 Setting Up a General Multiphase Problem Figure : The Secondary Phase Panel for a Non-Granular Phase 7. Click OK in the Secondary Phase panel. Defining a Granular Secondary Phase To define a granular (i.e., particulate) secondary phase in an Eulerian multiphase 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 ) will open. 3. In the Secondary Phase panel, enter a Name for the phase. c Fluent Inc. November 28,

72 General Multiphase Models Figure : The Secondary Phase Panel for a Granular 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, following the same procedure you used to set the material properties for the primary phase (see Section ). For a granular phase (which must be placed in the fluid materials category, as mentioned in Section ), 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 c Fluent Inc. November 28, 2001

73 20.6 Setting Up a General Multiphase Problem 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 (µ s,kin in Equation ). 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 , select gidaspow to compute the value using Equation , or select user-defined to use a user-defined function. Granular Bulk Viscosity specifies the solids bulk viscosity (λ q in Equation ). 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 , or select user-defined to use a user-defined function. Frictional Viscosity specifies a shear viscosity based on the viscousplastic flow (µ s,fr in Equation ). 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 , 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 ). 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 (α s,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. 7. Click OK in the Secondary Phase panel. c Fluent Inc. November 28,

74 General Multiphase Models 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 ). Figure : 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: c Fluent Inc. November 28, 2001

75 20.6 Setting Up a General Multiphase Problem 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 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 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 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 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 The Gidaspow model is recommended for dense fluidized beds. Select syamlal-obrien to use the fluid-solid drag function described by Equation The Syamlal-O Brien model is recommended for use in conjunction with the Syamlal-O Brien model for granular viscosity. Select syamlal-obrien-symmetric tousethesolid-solid dragfunction described by Equation The symmetric Syamlalc Fluent Inc. November 28,

76 General Multiphase Models 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 (e ls in Equation and e ss in Equation ). 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 (F lift in Equation ) 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: c Fluent Inc. November 28, 2001

77 20.6 Setting Up a General Multiphase Problem 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 (F vm in Equation ) 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 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. Define Operating Conditions... c Fluent Inc. November 28,

78 General Multiphase Models! 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. See Section for details 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 ). If you choose the Geo-Reconstruct, Donor-Acceptor, oreuler 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 c Fluent Inc. November 28, 2001

79 20.6 Setting Up a General Multiphase Problem! 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. WhenFLUENT 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 x cell /v fluid (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 c Fluent Inc. November 28,

80 General Multiphase Models 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 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 in the Viscous Model panel (Figure ). 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 Under k-epsilon Multiphase Model, indicate the desired multiphase turbulence model (see Section 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-ɛ turbulence model for each phase. This model is appropriate when the turbulence transfer among the phases plays a dominant role c Fluent Inc. November 28, 2001

81 20.6 Setting Up a General Multiphase Problem Figure : Calculation The Viscous Model Panel for an Eulerian Multiphase Including Source Terms By default, the interphase momentum, k, andɛ 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. c Fluent Inc. November 28,

82 General Multiphase Models Setting Boundary Conditions Multiphase boundary conditions are set in the Boundary Conditions panel (Figure ), 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 : 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 c Fluent Inc. November 28, 2001

83 20.6 Setting Up a General Multiphase Problem 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 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 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. c Fluent Inc. November 28,

84 General Multiphase Models Table : Phase-Specific and Mixture Conditions for the VOF Model Type Primary Phase Secondary Phase Mixture exhaust fan nothing volume fraction all others inlet vent intake fan mass flow inlet outlet vent pressure inlet pressure outlet velocity inlet axis nothing nothing all others fan outflow periodic porous jump radiator solid symmetry wall pressure far-field not available not available not available fluid mass source; mass source; porous zone; other porous other porous porosity; inputs inputs all others c Fluent Inc. November 28, 2001

85 20.6 Setting Up a General Multiphase Problem 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 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. 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 for details about these inputs. All other conditions are specified for the mixture. c Fluent Inc. November 28,

86 General Multiphase Models 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 : Phase-Specific and Mixture Conditions for the Mixture Model Type Primary Phase Secondary Phase Mixture exhaust fan nothing volume fraction all others outlet vent pressure outlet inlet vent coord. system; coord. system; dir. spec. intake fan flow direction flow direction; method; mass flow inlet volume fraction all others pressure inlet velocity inlet velocity velocity; all others volume fraction axis nothing nothing all others fan outflow periodic porous jump radiator solid symmetry wall pressure far-field not available not available not available fluid mass source; mass source; porous zone; other porous other porous porosity; inputs inputs all others c Fluent Inc. November 28, 2001

87 20.6 Setting Up a General Multiphase Problem 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 , , , and Note that the specification of turbulence parameters will depend on which of the three multiphase turbulence models you are using, as indicated in Tables See Sections and 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. For each secondary phase, you will need to set the volume fraction (as described above). 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 c Fluent Inc. November 28,

88 General Multiphase Models 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 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). 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 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. 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 c Fluent Inc. November 28, 2001

89 20.6 Setting Up a General Multiphase Problem and direction vectors, however, are specified separately for each phase. See Section 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, fan, porous jump, and radiator boundaries are not available with the Eulerian model. c Fluent Inc. November 28,

90 General Multiphase Models Table : Phase-Specific and Mixture Conditions for the Eulerian Model (for Laminar Flow) Type Primary Phase Secondary Phase Mixture exhaust fan nothing volume fraction; all others outlet vent gran. temperature pressure outlet inlet vent coord. system; coord. system; dir. spec. intake fan flow direction flow direction; method; mass flow inlet volume fraction; all others pressure inlet gran. temperature velocity inlet velocity velocity; all others volume fraction; gran. temperature axis nothing nothing all others outflow periodic solid symmetry wall shear condition shear condition all others pressure far-field not available not available not available fan porous jump radiator fluid all source terms; all source terms; porous zone; all fixed values; all fixed values; porosity; other porous other porous all others inputs inputs c Fluent Inc. November 28, 2001

91 20.6 Setting Up a General Multiphase Problem Table : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Mixture Turbulence Model) Type Primary Phase Secondary Phase Mixture exhaust fan nothing volume fraction; all others outlet vent gran. temperature pressure outlet inlet vent coord. system; coord. system; dir. spec. intake fan flow direction flow direction; method; mass flow inlet volume fraction; all others pressure inlet gran. temperature velocity inlet velocity velocity; all others volume fraction; gran. temperature axis nothing nothing all others outflow periodic solid symmetry wall shear condition shear condition all others pressure far-field not available not available not available fan porous jump radiator fluid other source other source source terms terms; terms; for turbulence; other fixed other fixed fixed values values; values; for turbulence; other porous other porous porous zone; inputs inputs porosity; all others c Fluent Inc. November 28,

92 General Multiphase Models Table : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Dispersed Turbulence Model) Type Primary Phase Secondary Phase Mixture exhaust fan turb. parameters volume fraction; all others outlet vent gran. temperature pressure outlet inlet vent coord. system; coord. system; dir. spec. intake fan flow direction; flow direction; method mass flow inlet turb. parameters; volume fraction; all others pressure inlet gran. temperature velocity inlet velocity; velocity; all others turb. parameters volume fraction; gran. temperature axis nothing nothing all others outflow periodic solid symmetry wall shear condition shear condition all others pressure far-field not available not available not available fan porous jump radiator fluid momentum, mass, momentum and porous zone; turb. sources; mass sources; porosity; momentum, mass, momentum and all others turb. fixed values; mass fixed values; other porous other porous inputs inputs c Fluent Inc. November 28, 2001

93 20.6 Setting Up a General Multiphase Problem Table : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Per-Phase Turbulence Model) Type Primary Phase Secondary Phase Mixture exhaust fan turb. parameters volume fraction; all others outlet vent turb. parameters; pressure outlet gran. temperature inlet vent coord. system; coord. system; dir. spec. intake fan flow direction; flow direction; method; mass flow inlet turb. parameters volume fraction; all others pressure inlet turb. parameters; gran. temperature velocity inlet velocity; velocity; all others turb. parameters volume fraction; turb. parameters; gran. temperature axis nothing nothing all others outflow periodic solid symmetry wall shear condition shear condition all others pressure far-field not available not available not available fan porous jump radiator fluid momentum, mass, momentum, mass, porous zone; turb. sources; turb. sources; porosity; momentum, mass, momentum, mass, all others turb. fixed values; turb. fixed values; other porous other porous inputs inputs c Fluent Inc. November 28,

94 General Multiphase Models 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 ), specify the mixture boundary conditions. Figure : 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. For a VOF calculation, if you enabled the Wall Adhesion op c Fluent Inc. November 28, 2001

95 20.6 Setting Up a General Multiphase Problem tion in the Phase Interaction panel, you can specify the contact angle at the wall for each pair of phases (as shown in Figure ). The contact angle (θ w in Figure ) 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 , θ w 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 ). (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. c Fluent Inc. November 28,

96 General Multiphase Models Figure : The Wall Panel for a Mixture in a VOF Calculation with Wall Adhesion c Fluent Inc. November 28, 2001

97 20.6 Setting Up a General Multiphase Problem Figure : 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 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 c Fluent Inc. November 28,