Figure 26.3: Multiphase Model Dialog Box for the Eulerian Model

To specify the number of phases for the multiphase calculation, enter the appropriate value in the Number of Eulerian Phases field. You can specify up to 20 phases.

For the VOF and Mixture multiphase models and for the Eulerian multiphase model with Multi-Fluid VOF enabled, you must specify the interface regime that you will be modeling. This will determine the availability of the various volume fraction discretization schemes (Spatial Discretization Schemes for Volume Fraction). The following options are available for Interface Modeling Type:

Interfacial Anti-Diffusion

If you are using the Sharp interface modeling type, you can optionally enable the Interfacial Anti-Diffusion treatment. This treatment is applied only in interfacial cells and attempts to suppress the numerical diffusion that can arise from the volume fraction advection schemes.

The use of this treatment can have adverse effects on convergence, especially with aggressive settings and large time step size. Therefore, it should be used in cases that use a coarse mesh, that have high aspect-ratio cells, that have large cell-volume jumps in the vicinity of the fluid-fluid interface, or that suffer from excess numerical diffusion.

The strength of the anti-diffusion treatment can be specified using the define/models/multiphase/interface-modeling-options text command. The strength can range between 0 (none) and 1 (maximum).

The anti-diffusion treatment can sometimes produce artificial waves due to excessive sharpening. The dynamic anti-diffusion strength option may help in such cases by reducing the anti-diffusion strength in the direction tangential to the interface. Dynamic strength can be enabled using the following text commands.

solve/set/multiphase-numerics/advanced-stability-controls/anti-diffusion/
enable-dynamic-strength?

solve/set/multiphase-numerics/advanced-stability-controls/anti-diffusion/enable-dynamic-strength?
Enable anti-diffusion treatment with dynamic strength? [no] yes

Dynamic strength is specified as:

(26–1)

where

= anti diffusion strength

= interface unit normal

= area unit normal

= angle between the area and interface unit normals

= exponent (default = 1.5)

= maximum value of anti-diffusion strength ranging between 0 and 0.95 (default = 0.75)

Values of the exponent and maximum strength can be adjusted using the following text commands, if needed:

Sharp/Dispersed Interface Modeling Options

Selecting Sharp/Dispersed will make available some additional discretization options. To access these, click Interface Modeling Options... in the Multiphase Model dialog box.

These options allow you to adjust the discretization behavior on a per-zone and/or per-phase-pair basis for cases in which it is important to simultaneously model dispersed and sharp interfaces.

You can choose from various spatial discretization schemes for volume fraction depending on the multiphase model in use, the interface regime type, and the volume fraction formulation chosen. The available discretization schemes for each combination of model, formulation, and interface regime are summarized in the following tables:

The Geo-Reconstruct scheme is an interface tracking scheme based on geometrical information. It is the most accurate scheme, but is more computationally expensive than the other schemes. Geo-Reconstruct is the preferred scheme when solving on meshes of poor quality.

The CICSAM, Modified HRIC, and Compressive schemes are interface capturing schemes based on algebraic information.

The Donor-Acceptor discretization is a scheme applicable only to quad- and hex-meshes. As it is considered obsolete, it does not appear by default in the graphical user interface. However, it can be made available if required using the following text command: solve/set/advanced/show-all-discretization-schemes. This command can also be used to expose discretization schemes that may be applicable, but are hidden by default according to the tables above.

For more details about the implementations of the volume fraction discretization schemes, refer to Interpolation Near the Interface in the Fluent Theory Guide.

The Volume Fraction Cutoff allows you to specify a cutoff limit for the volume fraction values. The value that you provide is used as the lower cutoff for the volume fraction. All volume fraction values in the domain below this cutoff value are set to zero. The upper cutoff is calculated as (1.0 - lower cutoff). All volume fraction values above the upper cutoff value are set to 1.0. The default value is 1e-6, which is the recommended value. Using a higher value may lead to a higher volume imbalance.

When using the Explicit formulation, there are several additional options that you can access in the Expert Options dialog box that opens by clicking Expert Options... in the Multiphase Model dialog box (Models tab).

Figure 26.4: Expert Options Dialog Box

For a more detailed discussion of how to use these options, refer to Setting Time-Dependent Parameters for the Explicit Volume Fraction Formulation.

In addition, you can enable Advanced Volume Fraction Filtering if you want to filter out small values of the volume fraction, which may be purely numerical causing solution instability. Small-scale numerical errors in the volume fraction field may arise due to the various reasons:

Ansys Fluent uses the flotsam filtering method to identify whether these errors are physical or numerical. The method is based on a principle that an interface cannot be constructed in a single cell.

Figure 26.5: Numerical Flotsams in the Volume Fraction Field depicts generation of a numerical flotsam. In scenario A, the neighboring cells are completely full, while the central cell is not full. In scenario B, the neighboring cells are completely void, but the central cell contains a non-zero volume fraction. Both scenarios cannot exist unless there is a mass source/sink present in a single cell.

Figure 26.5: Numerical Flotsams in the Volume Fraction Field

Once a cell is identified as a flotsam, its volume fraction is removed from the cell and distributed to the partial cells (that is, cells with the volume fraction between 0 and 1).

You can select one of the following Filtering Options:

Ansys Fluent provides the following methods for calculation of operating density for a buoyancy-driven flow. These options appear in the Operating Density drop-down list in the Operating Conditions dialog box (Variable-Density Parameters group box).

Figure 26.9: The Operating Conditions Dialog Box for Multiphase Flows

The default method, minimum-phase-averaged, is appropriate for most cases, and typically you do not need to change it. It automatically handles the operating density requirements for both incompressible and compressible flows by resolving the correct hydrostatic pressure gradient distribution.

If you are interested only in the pressure gradient (rather than the hydrostatic pressure values), you can use either the primary-phase-averaged or mixture-averaged method.

When using the Boussinesq approximation for density variation in multiphase flows, there are several important items to consider:

For additional information on the Boussinesq approximation, see The Boussinesq Model.

The existing formulation of sensible enthalpy for interphase mass transfer includes the formation enthalpy, which could be problematic for some cases, such as cases that involve species transport and reactions. The alternative treatment, which is available with the VOF and Mixture multiphase models, is based on the explicit modeling of the energy source driven by mass transfer. You can enable the alternative formulation by using the following text command:

solve/set/multiphase-numerics/heat-mass-transfer/alternative-energy-treatment?

enable alternative treatment of handling latent heat source [no] y

Energy Source Treatment

The energy source is modeled explicitly as:

(26–2)

where is the mass transfer rate, and is latent heat of vaporization. If you are using the tabular-ptl-sat method to specify saturation temperature for the Evaporation-Condensation Mechanism or vaporization pressure for the Cavitation Mechanism, Ansys Fluent will take the latent heat values directly from the tabular data. Otherwise, it is calculated as:

(26–3)

Here, and are saturation enthalpies of phase and phase at the saturation temperature, respectively. They are calculated as:

(26–4)

(26–5)

where,
	and = formation enthalpies of phase and phase , respectively
	and = specific heats of phase and phase , respectively
	and = reference temperatures of phase and phase as specified in the Create/Edit Materials dialog box, respectively.
	= saturation temperature

Sensible Enthalpy Definition

For mass transfer cases, Ansys Fluent by default uses the following definition of sensible enthalpy:

(26–6)

where,
	= sensible enthalpy of phase
	= formation enthalpy of phase
	= specific heat of phase
	= temperature of phase
	= reference temperature of phase as specified in the Create/Edit Materials dialog box

The alternative treatment considers the definition of sensible enthalpy that excludes formation enthalpy. Sensible enthalpy for each phase is expressed as:

(26–7)

with =298.15 K.

Heat Flux Reporting Strategies

When you use the alternative formulation, the following additional variable become available for postprocessing under the Phase Interaction... category:

Due to the explicit nature of the alternative formulation, the latent heat source appears as the heat imbalance in heat flux reporting.

If you want to know the heat imbalance due to the latent heat source, you should create a custom-field function for the mass transfer rate multiplied by latent heat, and then report it as a volume integral. Ansys Fluent will report the following value:

(26–8)

where,
	= heat imbalance
	= number of mass transfer mechanisms that you defined
	= mass transfer rate of th mechanism
	= Latent heat of th mechanism
	= volume

When including mass transfer effects in a multiphase simulation, you can choose from the following mechanisms for each phase pair that undergoes mass transfer:

 

26.2.10.2.4. Cavitation Mechanism

The cavitation mechanism allows you to select a cavitation model. For a cavitating flow, it is recommended that you select liquid as the primary phase and vapor as the secondary phase.

The cavitation models are available when using mixture, VOF, and Eulerian multiphase models. You are provided with two model options: Schnerr-Sauer and Zwart-Gerber-Belamri. To open the Cavitation Model dialog box, select cavitation from the Mechanism drop-down list. For information about the cavitation models, refer to Cavitation Models in the Theory Guide.

Figure 26.15: The Cavitation Model Dialog Box

• For the Schnerr-Sauer model, specify the Bubble Number Density ( in Equation 14–588 in the Fluent Theory Guide) under Model Constants. The default value of 1e11 is suitable for most cases.

• For the Zwart-Gerber-Belamri model, specify the Bubble Radius, the Nucleation Site Volume Fraction, the Evaporation Coefficient, and the Condensation Coefficient under Model Constants.

• Under Cavitation Properties, specify the Vaporization Pressure and, if desired, a temperature dependence function. In addition to the methods described in Defining Properties Using Temperature-Dependent Functions (constant, polynomial, piecewise-linear, piecewise-polynomial, or user-defined), you can choose one of the following:

  • rgp-table-sat

    This option allows you to use to define the vaporization pressure using RGP tables as described in Defining Saturation Properties via RGP Tables.

  • taylor-approximation

    The taylor-approximation method models the vaporization pressure as linearly varying with temperature about the free-stream value. This approach can improve numerical stability, but is only appropriate when deviations about the free-stream temperature are sufficiently small that higher-order terms can be neglected. The expression for the vaporization pressure using the taylor-approximation method is:

    (26–9)

    where is the free-stream temperature, is the latent heat, and is a user-modifiable coefficient. In the Taylor Approximation dialog box, you will specify Vaporization Pressure (at the free-stream temperature), Free Stream Temperature, and Thermal Coefficient ().

  • tabular-pt-sat

    This method allows you to specify vaporization pressure using a table that contains data points for saturation temperature and saturation pressure. Saturation pressure will be interpolated based on the static temperature from the solution, which is assumed to be at a saturated state. The table format is described in Reading Files in Tabular Format. Once you select tabular-pt-sat, the Table Input dialog box opens where you can select the appropriate table and the names of the columns from the Saturation Temperature and Saturation Pressure selection lists.

    Figure 26.16: Table Input for Vaporization Pressure

    
    
    

  • tabular-ptl-sat

    (available only with Alternative Modeling of Energy Sources) The method allows you to specify saturation pressure using a table that contains data points for saturation temperature, saturation pressure, and latent heat. Saturation pressure and latent heat will be interpolated based on the static temperature from the solution, which is assumed to be at a saturated state. The table format is described in Reading Files in Tabular Format. Once you select tabular-ptl-sat, the Table Input dialog box opens where you can select the appropriate table and the names of the columns from the Saturation Temperature, Saturation Pressure and Latent Heat selection lists.

  ---

  Note:  If you are using tabular-pt-sat or tabular-ptl-sat to specify vaporization pressure, you must first read an appropriate table following the procedure outlined in Reading Files in Tabular Format. All table data must be in SI units (saturation temperature in Kelvin (K), saturation pressure in Pascal (Pa), and latent heat in Joule/Kg).

  ---

• If you want to include the influence of turbulence on the threshold cavitation pressure, enable Turbulence Factor. If desired, you can adjust the value of the Turbulent Coefficient. For details about the implementation of the Turbulence Factor, see Turbulence Factor in the Fluent Theory Guide.

By default, the minimum vapor pressure limit is set to 1 Pa. The default value for the maximum vapor pressure limit is set to five times the local vapor pressure with consideration of the turbulent and thermal effects for each computational cell and phase. The default and recommended value for the evaporation and condensation coefficients in the Schnerr-Sauer model ( and in Equation 14–592 in the Fluent Theory Guide) are 1 and 0.2, respectively. You can modify these default values using the following expert text commands:

• solve/set/multiphase-numerics/heat-mass-transfer/cavitation/min-vapor-pressure

• solve/set/multiphase-numerics/heat-mass-transfer/cavitation/max-vapor-pressure-ratio

• solve/set/multiphase-numerics/heat-mass-transfer/cavitation/schnerr-cond-coeff

• solve/set/multiphase-numerics/heat-mass-transfer/cavitation/schnerr-evap-coeff

---

Note:

• If you use multiple cavitation mass transfer mechanisms in your simulation, the value you specify for Turbulence Factor will automatically apply to all cavitation mechanisms, thereby overwriting previously existing turbulent coefficients.

• For the Mixture multiphase model, in addition to the Schnerr-Sauer and Zwart-Gerber-Belamri models, the Singhal et al. expert cavitation model can be used. See Using the Singhal et al. Expert Cavitation Model for more information on using this model.

---

Pressure Limiting Method

When calculating the properties of a compressible flow (such as densities and sound speeds), the cavitation model by default limits the absolute pressure to the vapor pressure whenever the absolute pressure drops below the vapor pressure. This default treatment may not predict correct results for a compressible flow because at saturation pressure, the density method behaves as the incompressible-ideal-gas law rather than the ideal-gas law. In such a case, you can apply a special treatment that allows the pressure to drop to the minimum absolute pressure. The treatment correctly predicts shock, which is not possible with the default treatment. To set the pressure limiting method, use the following text command:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/p-limit-method

The available methods are:

• local-pvap-min: Limits the pressure to the local minimum of vapor pressures

• global-pvap-min: Limits the pressure to the global minimum of vapor pressures from all cells

• pabs-min: Limits the pressure to the absolute minimum pressure specified under solution limits specified in the Solution Limits dialog box.

For a cavitating flow, by default, pressure contours are clipped to the pressure specified by the pressure limiting method wherever the pressure drops below the vapor pressure. To see the actual pressure contours, use the following text command:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/display_clipped_pressure?

display clipped pressure in the post-processing [yes]: no

---

Note:  Clipped pressure values are only used in the computation of properties, while the actual pressure, which is used in the calculation of the mass transfer rate, remains unclipped.

---

Turbulent Diffusion Treatment

For turbulent flows, if one of the phases participating in cavitation is primary, then Ansys Fluent automatically enables the generalized turbulent diffusion treatment. The treatment adds a diffusion source in the volume fraction equation by assuming the diffusion coefficient as a function of turbulent viscosity of the respective phase. This helps avoid instantaneous solution instability due to cavitation. For more information about this treatment, see Diffusion in VOF Model in the Fluent Theory Guide.

The generalized turbulent diffusion treatment can be used for simulating flows with two or more phases. By default, for a flow with more than two phases, the turbulent diffusion acts between primary and secondary phases only. The turbulent diffusion between secondary phases is not accounted for.

If you want to use the old turbulent diffusion treatment supported in releases prior to Release 19.2, enter the following text commands:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/turbulent-
diffusion
use generalized treatment of turbulent diffusion [yes] no
use old treatment of turbulent diffusion [yes] yes

Unlike the generalized turbulent diffusion treatment, the old treatment is applicable to only two-phase flows. If used for flows with more than two phases, the old treatment unphysically accounts for each secondary phase interacting with the primary phase, despite the secondary non-vapor phases not participating in cavitation.

If your want to disable the turbulent diffusion treatment for cases where the high turbulent viscosity may be a source of an unstable solution, enter the following text commands:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/turbulent-
diffusion
use generalized treatment of turbulent diffusion [yes] no
use old treatment of turbulent diffusion [yes] no

 

26.2.10.2.5. Evaporation-Condensation Mechanism

The evaporation-condensation mass transfer mechanism enables you to apply the evaporation-condensation model as the mass transfer mechanism. The VOF and Mixture multiphase models use the Lee model (see Lee Model in the Fluent Theory Guide). With the Eulerian multiphase model, you can choose between the Lee model and the Thermal Phase Change model (see Thermal Phase Change Model in the Fluent Theory Guide). When you select evaporation-condensation under Mechanism in the Phase Interaction > Heat, Mass, Reactions > Mass tab of the Multiphase Model dialog box, you will be prompted with the Evaporation-Condensation Model dialog box. Note that this dialog box could also be accessed by clicking Edit... next to the evaporation-condensation mechanism drop-down list.

Figure 26.17: The Evaporation-Condensation Model Dialog Box (Eulerian Multiphase Model)

You need to specify the following settings:

1. (Eulerian multiphase model only) Select the evaporation-condensation Model. The following models are available:

   • Lee

   • Thermal Phase Change

2. Specify the Saturation Temperature for your flow regime. In addition to the methods described in Defining Properties Using Temperature-Dependent Functions (constant, polynomial, piecewise-linear, piecewise-polynomial, or user-defined) you can choose one of the following:

   • rgp-table-sat

     This option allows you to use to define the saturated temperature using RGP tables as described in Defining Saturation Properties via RGP Tables.

   • tabular-pt-sat

     The tabular-pt-sat allows you to specify saturation temperature using a table that contains data points for saturation temperature and saturation pressure. Saturation temperature will be interpolated based on the absolute pressure from the solution, which is assumed to be at a saturated state. The table format is described in Reading Files in Tabular Format. Once you select tabular-pt-sat, the Table Input dialog box opens where you can select the appropriate table and the names of the columns for your simulation from the Saturation Temperature and Saturation Pressure selection lists.

   • tabular-ptl-sat

     (available only with Alternative Modeling of Energy Sources) The method allows you to specify saturation temperature using a table that contains data points for saturation temperature, saturation pressure, and latent heat. Saturation temperature and latent heat will be interpolated based on absolute pressure from the solution, which is assumed to be at a saturated state. The table format is described in Reading Files in Tabular Format. Once you select tabular-ptl-sat, the Table Input dialog box opens where you can select the appropriate table and the names of the columns from the Saturation Temperature, Saturation Pressure and Latent Heat selection lists.

   ---

   Note:

   • If you use tabular-pt-sat or tabular-ptl-sat to specify saturation temperature, you must first read an appropriate table following the procedure outlined in Reading Files in Tabular Format. All table data must be in SI units (saturation temperature in Kelvin (K), saturation pressure in Pascal (Pa), and latent heat in Joule/Kg).

   • If you use the tabular-pt-sat, tabular-ptl-sat, polynomial, piecewise-polynomial, or piecewise-linear option for Saturation Temperature, the pressure-dependency must be specified in terms of absolute pressure.

   ---

3. (Lee model only) Specify the From Phase Frequency and To Phase Frequency model constants. These values correspond to the coefficient (Equation 14–617 in the Theory Guide). The values are 0.1 by default. However, note that the bubble diameter and accommodation coefficient are usually not very well known, so the appropriate values for a given problem can be very different. It is important to tune the values to match experimental data.

4. (Mixture multiphase model only) For certain models and conditions, you can select the Semi-Mechanistic boiling model to model sub-cooled nucleate boiling at low pressure, as described in Including Semi-Mechanistic Boiling.

5. (Thermal Phase Change model only) Specify the following model coefficients:

   • From Phase Scaling Factor: in Equation 14–618 in the Fluent Theory Guide

   • To Phase Scaling Factor: in Equation 14–619 in the Fluent Theory Guide

   If you are using the two-resistance option for heat transfer, these values act as multipliers for the phase heat transfer coefficients determined for each phase and the default value of 1 is usually appropriate. If you are using one of the other heat transfer options, then these parameters correspond to the coefficient (Equation 14–617 in the Theory Guide) and should be tuned based on experimental data.

   ---

   Note:  For a phase pair, only one evaporation-condensation mechanism that uses the Thermal Phase Change model can be defined, and it cannot be combined with other mass transfer mechanisms.

   ---

 

26.2.10.2.6. Species-Mass-Transfer Mechanism

The species-mass-transfer mechanism enables you to model generalized interphase species mass transfer in either the Mixture model or the Eulerian model subject to the following conditions:

• Both phases consist of mixtures with at least two species, and at least one of species is present in both phases.

• The two mixture phases are in contact and separated by an interface.

• Species mass transfer can only occur between the same species from one phase to the other. For example, evaporation/condensation between water liquid and water vapor.

• As in all interphase mass transfer models in Fluent, if a gas mixture is involved in an interphase species mass transfer process, it is always treated as a To Phase and the liquid mixture as a From Phase.

• For the species involved in the mass transfer, the mass fractions in both phases must be determined by solving transport equations. For example, the mass fractions of water liquid and water vapor in an evaporation/condensation case must be solved directly from the governing equations, rather than algebraically or from the physical constraint relations.

When you select species-mass-transfer under Mechanism in the Phase Interaction > Heat, Mass, Reactions > Mass tab of the Multiphase Model dialog box, you will be prompted with the Species Mass Transfer Model dialog box.

---

Note:  If multiple phase pairs have the species-mass-transfer mechanism selected, the same settings in the Species Mass Transfer Model dialog box will be used for all phase pairs.

---

Figure 26.18: The Species Mass Transfer Model Dialog Box

The steps to configure the species mass transfer model are as follows:

1. Under Model Options, choose the sub-model for determining the dynamic equilibrium relations between the same species in a pair of phases.

   Raoult’s Law

   Use Raoult’s Law as described in Raoult’s Law in the Fluent Theory Guide. This model is appropriate for gas-liquid cases in which the liquid phase can be modeled as an ideal liquid mixture. If you use Raoult’s Law, you need to specify the saturation pressure as a constant, polynomial, piecewise-linear, piece-wise polynomial, or as a user-defined function using the DEFINE_PROPERTY macro. You can also specify the saturation pressure using RGP tables as described in Defining Saturation Properties via RGP Tables.

   Henry’s Law

   Use Henry’s Law as described in Henry’s Law in the Fluent Theory Guide. This model is appropriate for cases in which a gas species is dissolved into a liquid mixture phase. If you use Henry’s Law you must specify the method for the Molar Fraction or Molar Concentration. You can choose a constant, vant-hoff (to use the Van’t Hoff correlation), or a user-defined function using the DEFINE_MASS_TRANSFER macro. For the vant-hoff model, you will need to specify Reference Henry Constant ( in Equation 14–658 in the Fluent Theory Guide) and Temperature Dependence () in the Vant Hoff’s Correlation dialog box.

   Equilibrium Ratio

   Use the Equilibrium Ratio method as described in Equilibrium Ratio in the Fluent Theory Guide. This model allows you to specify the equilibrium ratio as a constant, or as a user-defined function. If you use Equilibrium Ratio you must specify a constant or user-defined function using the DEFINE_MASS_TRANSFER macro for Molar Fraction, Molar Concentration, or Mass Fraction.

2. Under Interphase Mass Transfer Coefficient, choose whether you want to specify the mass transfer coefficient on a per-phase basis or on all phases:

   • If you selected Per Phase, you can choose the sub-models for calculating the phase-specific mass transfer coefficients and for the source phase and the destination phase, respectively using Equation 14–647 in the Fluent Theory Guide. The following models are available in Ansys Fluent:

     constant

     Specify a constant value for the mass transfer coefficient.

     sherwood-number

     Specify a constant value for the Sherwood Number. The mass transfer coefficient is calculated from Equation 14–661 in the Fluent Theory Guide.

     ranz-marshall

     Use the Ranz-Marshall model as described in Ranz-Marshall Model in the Fluent Theory Guide. The Ranz-Marshall model is based on boundary layer theory for steady flow past a spherical particle. It is applicable under the following flow conditions:

     

     hughmark

     Use the Hughmark model as described in Hughmark Model in the Fluent Theory Guide. The Hughmark model extends the Ranz-Marshall model for a wider range of relative Reynolds number, .

     higbie

     Use the Higbie model as described in Higbie Model in the Fluent Theory Guide. Note the following when using the Higbie method:

     • The Higbie method is suitable for modeling mass transfer between gas and liquid phases such as in the simulation of oxygen dissolution in mixing tanks.

     • The Higbie correlation is valid only for turbulent flows.

     • The primary phase should be modeled as the liquid phase.

     • When using the Higbie species-mass-transfer mechanism, higbie must be selected for the liquid primary phase, while any available method can be used for the secondary phase.

     zero-resistance

     Specify zero-resistance mass transfer between the bulk phase and interface.

     user-defined

     Use a user-defined function for the mass transfer coefficient defined with the DEFINE_MASS_TRANSFER macro.

     The selection of physically correct mass transfer correlations is highly problem dependent. In the case of mass transfer between a continuous phase and a dispersed phase of approximately spherical particles, the following should be adequate under most situations:

     • ranz-marshall or hughmark for the continuous phase

     • zero-resistance for the dispersed phase

       Using zero-resistance for the dispersed phase implies that the mass transfer occurs very quickly from the interface to the bulk of the dispersed phase. Consequently, the interface concentration and bulk concentration in the dispersed phase are equal. This is usually valid for droplet evaporation or gas absorption/dissolution in bubbles. If there exists significant resistance to the mass transfer on the dispersed phase side, one of the other correlations should be chosen for the dispersed phase.

   • If you select Overall, you can specify the Overall Mass Transfer Coefficient in Equation 14–647 in the Fluent Theory Guide either as a constant or as a user-defined function. These options are the same as those for the Per Phase option. The Overall option is recommended only if the mass transfer coefficient in each phase is unknown.

   For more information about these options, see Mass Transfer Coefficient Models in the Fluent Theory Guide.

 Setup → Boundary Conditions → <boundary-type>  Edit...

The steps you need to perform for each boundary are as follows:

 Setup →   Cell Zone Conditions

Figure 26.25: The Cell Zone Conditions Task Page

The steps for specifying the mixture and individual phase cell zone conditions are listed below:

For more information about inputs for cell zone conditions, see Fluid Conditions.

The boundary conditions you need to specify for the mixture and for the individual phases will depend on which multiphase model you are using.

The steps for copying cell zone and boundary conditions for a multiphase flow are slightly different from those described in Copying Cell Zone and Boundary Conditions for a single-phase flow. The modified steps are listed below:

See Copying Cell Zone and Boundary Conditions for additional information about copying boundary conditions, including limitations.

Once you have initialized the flow (as described in Initializing the Solution), you can define the initial distribution of the phases. For a transient simulation, this distribution will serve as the initial condition at ; for a steady-state simulation, setting an initial distribution can provide added stability in the early stages of the calculation.

You can patch an initial volume fraction for each secondary phase using the Patch Dialog Box.

 Solution → Initialization  Patch...

If the region in which you want to patch the volume fraction is defined as a separate cell zone, you can simply patch the value there. Otherwise, you can create a cell “register” that contains the appropriate cells and patch the value in the register. See Patching Values in Selected Cells for details.

 

26.2.12.1.1. Options for Patching Volume Fraction

You have additional options for how the volume fraction is patched in a user-defined register. A standard patching procedure will initialize all the cells in the register with the specified volume fraction, without any special treatment for cells that are intersected by the fluid-fluid interface.

Patch Reconstructed Interface

This option uses piecewise-linear interface reconstruction to identify the fluid-fluid interface and patches the actual volume fraction field in the cells that intersect the interface.

---

Important:  The Patch Reconstructed Interface algorithm requires that the register coordinates in the Region Register dialog box be well-ordered. That is: X Min < X Max; Y Min < Y Max; Z Min < Z Max. In particular, if you use the Select Points with Mouse feature to specify the coordinates, be sure that this condition is met. If the register coordinates are not well-ordered, the register will still be created/displayed as intended; however, the volume fraction value will not be patched within the register.

The Patch Reconstructed Interface will be applied only on the last register that was defined, even if multiple registers are selected in the Patch dialog box. Therefore, it is recommended that you create and patch registers one at a time.

---

Volumetric Smoothing

This option smooths the volume fraction field on-demand by taking the volumetric average over the cell neighbors. This can help provide better solution stability at startup. After enabling Volumetric Smoothing, you can click Smooth to apply the smoothing. Note that the smoothing is applied to the volume fraction field for all phases in the full domain. The Smoothing Relaxation Factor controls the degree of smoothing applied. You can specify a value between 0 (no smoothing) and 1 (maximum smoothing). For most cases, the default value is recommended. For fine meshes you may choose to try a larger value to aid solution startup. However, excessively large values can have an undesirable effect during the solution as interface sharpening discretization schemes may deteriorate the initial field.

The Smooth command can be used at any time after the solution has been initialized. It can therefore also be used after reading a data file for postprocessing. However, note that the smoothed field will overwrite the original volume fraction field in this case. Also note that you must select a secondary phase variable from the drop-down list in the Patch dialog box to expose the Volumetric Smoothing option.

By default, standard initialization uses domain-averaged values for turbulence variables, which is not ideal for a turbulent flow with multiple phases that have different properties and velocities. Ill-posed initial conditions for turbulence may result in unstable solution, especially at the start of the simulation.

For the VOF and Mixture multiphase models, you can enable the Localized Turbulence Initialization option to obtain a better initial guess for turbulence variables, which will promote better startup and run-time stability.

Once you initialize the flow, all turbulent flow variables relevant to the turbulence model will be initialized based on local velocity and local property in each cell. This type of initialization assumes the turbulent intensity of 5% and the turbulent viscosity ratio of 10. You can adjust these values using the following text commands:

solve/initialize/mp-localized-turb-init/enable

enable localized initialization of turbulent flow variables? [no] yes

solve/initialize/mp-localized-turb-init/turb-init-parameters

turbulent intensity [0.05]

turbulent viscosity ratio [10]

Note that domain-averaged values displayed in the Initial Values group box in the Solution Initialization task page will be overwritten by the variable turbulence field. You can examine this field by displaying contours of Turbulence.

If executing the Patch or Smooth commands leads to a change in initial conditions, initial values of turbulent flow variables will be automatically recalculated.