24.5.2. Defining the 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.

24.5.2.1. 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 Defining the Primary Phase for details.

24.5.2.2. Defining a Non-Granular Secondary Phase

To define a non-granular (that is, liquid or vapor) secondary phase in an Eulerian multiphase calculation, perform the following steps:

  1. Select the phase (for example, phase-2) in the Phases list.

  2. Click Edit... to open the Secondary Phase Dialog Box (Figure 24.38: The Secondary Phase Dialog Box for a Non-Granular Phase).

    Figure 24.38:  The Secondary Phase Dialog Box for a Non-Granular Phase

    The Secondary Phase Dialog Box for a Non-Granular Phase

  3. In the Secondary Phase dialog box, 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 Defining the Primary Phase).

  6. In the Secondary Phase dialog box, 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 Fluent Customization Manual for details about user-defined functions.

  7. Click OK in the Secondary Phase dialog box.

24.5.2.3. Defining a Granular Secondary Phase

To define a granular (that is, particulate) secondary phase in an Eulerian multiphase calculation, perform the following steps:

  1. Select the phase (for example, phase-2) in the Phases list.

  2. Click Edit... to open the Secondary Phase Dialog Box (Figure 24.39: The Secondary Phase Dialog Box for a Granular Phase).

    Figure 24.39:  The Secondary Phase Dialog Box for a Granular Phase

    The Secondary Phase Dialog Box for a Granular Phase

  3. In the Secondary Phase dialog box, 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 Defining the Primary Phase). For a granular phase (which must be placed in the fluid materials category, as mentioned in Steps for Using a Multiphase Model), you need to specify only the density; you can ignore the values for the other properties, since they will not be used.


    Important:  Note that all properties for granular flows can be defined by user-defined functions (UDFs).


    See the Fluent Customization Manual for details about user-defined functions.

  6. Enable the Granular option.

  7. (optional) Enable the Packed Bed option if you want to freeze the velocity field for the granular phase. Note that when you select the packed bed option for a phase, you should also use the fixed velocity option with a value of zero for all velocity components for all interior cell zones for that phase. Using fixed velocity in radial direction as a constant value (other than zero) does not ensure continuity. With the fixed velocity option, both velocity and pressure are fixed in a zone. Since face area in the radial direction is a function of radial distance from the axis, it will result in a mass conservation problem due to flux imbalance.

    Using zero fixed velocity in the radial direction does not cause any problems related to mass conservation.

  8. Specify the Granular Temperature Model. Choose either the default Phase Property option or the Partial Differential Equation option. See Granular Temperature in the Theory Guide for details.

  9. In the Secondary Phase dialog box, specify the following properties of the particles of this phase:

    Diameter

    specifies the diameter of the particles. You can select constant in the drop-down list and specify a constant value, or select user-defined to use a user-defined function. See the Fluent Customization Manual for details about user-defined functions.

    Granular Viscosity

    specifies the method for computing the kinetic () and collisional () components of the granular viscosity (Equation 17–307 in the Fluent Theory Guide). Selecting constant, syamlal-obrien (Equation 17–309), or gidaspow (Equation 17–310) will use these expressions for the kinetic portion of the viscosity and will calculate the collisional portion of the viscosity from Equation 17–308 in the Fluent Theory Guide. Alternatively, you can select user-defined to use a user-defined function. Note that if you select user-defined, your user-defined function must include both the kinetic portion and the collisional portion of the viscosity in the value it returns.

    Granular Bulk Viscosity

    specifies the solids bulk viscosity ( in Equation 17–169 in the Theory Guide). You can select constant (the default) in the drop-down list and specify a constant value, select lun-et-al to compute the value using Equation 17–311 in the Theory Guide, or select user-defined to use a user-defined function.

    Frictional Viscosity

    specifies a shear viscosity based on the viscous-plastic flow ( in Equation 17–307 in the Theory Guide). 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 17–312 in the Theory Guide, or select user-defined to use a user-defined function.

    Angle of Internal Friction

    specifies a constant value for the angle used in Schaeffer’s expression for frictional viscosity (Equation 17–312 in the Theory Guide). This parameter is relevant only if you have selected schaeffer or user-defined for the Frictional Viscosity.

    Frictional Pressure

    specifies the pressure gradient term, , in the granular-phase momentum equation. Choose none to exclude frictional pressure from your calculation, johnson-et-al to apply Equation 17–316 in the Theory Guide, syamlal-obrien to apply Equation 17–228 in the Theory Guide, based-ktgf, where the frictional pressure is defined by the kinetic theory  [26]. The solids pressure tends to a large value near the packing limit, depending on the model selected for the radial distribution function. You must hook a user-defined function when selecting the user-defined option. See the Fluent Customization Manual for information on hooking a UDF.

    Frictional Modulus

    is defined as

    (24–12)

    with , which is the derived option. You can also specify a user-defined function for the frictional modulus.

    Friction Packing Limit

    specifies a threshold volume fraction at which the frictional regime becomes dominant. It is assumed that for a maximum packing limit of 0.6, the frictional regime starts at a volume fraction of about 0.5. This is only a general rule of thumb as there may be other factors involved. The default value is 0.61.

    Granular Conductivity

    specifies the solids granular conductivity ( in Equation 17–319 in the Theory Guide). You can select syamlal-obrien to compute the value using Equation 17–320 in the Theory Guide, select gidaspow to compute the value using Equation 17–321 in the Theory Guide, or select user-defined to use a user-defined function. Note that in the algebraic model, shown in Figure 24.39: The Secondary Phase Dialog Box for a Granular Phase, the granular conductivity is not required in the computation of the granular temperature. This has been obtained by neglecting convection and diffusion in the transport equation, Equation 17–319 in the Theory Guide  [116].

    Granular Temperature

    specifies temperature for the solids phase and is proportional to the kinetic energy of the random motion of the particles. Choose the algebraic, constant, dpm-averaged, or user-defined option.


    Note:  The dpm-averaged method is only available when using the Dense Discrete Phase Model (DDPM).


    Solids Pressure

    specifies the pressure gradient term, , in the granular-phase momentum equation. Choose either the lun-et-al, the syamlal-obrien, the ma-ahmadi, none, or a user-defined option.

    Radial Distribution

    specifies a correction factor that modifies the probability of collisions between grains when the solid granular phase becomes dense. Choose either the lun-et-al, the syamlal-obrien, the ma-ahmadi, the arastoopour, or a user-defined option.

    Elasticity Modulus

    is defined as

    (24–13)

    with .

    Packing Limit

    specifies the maximum volume fraction for the granular phase. For monodispersed spheres, the packing limit is about 0.63, which is the default value in ANSYS 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.

  10. Click OK in the Secondary Phase dialog box.

24.5.2.4. Defining the Interfacial Area Concentration

When using the Eulerian multiphase model, you can choose to solve a transport equation for the interfacial area, which allows for a distribution of secondary phase diameter, or you can use an algebraic model to compute the interfacial area from a specified diameter. To use an algebraic model, refer to Using an Algebraic Interfacial Area Model. To solve the transport equation (Interfacial Area Concentration in the Fluent Theory Guide), perform the following steps:

  1. Select the phase (for example, phase-2) in the Phases list.

  2. Click Edit... to open the Secondary Phase Dialog Box (Figure 24.35: The Secondary Phase Dialog Box Displaying the Interfacial Area Concentration Settings).

  3. In the Secondary Phase dialog box, 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.

  6. Enable the Interfacial Area Concentration option. Make sure the Granular option is disabled for the Interfacial Area Concentration option to be visible in the interface.

  7. In the Secondary Phase dialog box, specify the following properties of the particles of this phase:

    Diameter

    specifies the diameter of the particles or bubbles. You can select constant in the drop-down list and specify a constant value, or select user-defined to use a user-defined function. See the Fluent Customization Manual for details about user-defined functions. The Diameter recommended setting is sauter-mean, allowing for the effects of the interfacial area concentration values to be considered for mass, momentum and heat transfer across the interface between phases.

    Coalescence Kernel and Breakage Kernel

    allows you to specify the coalescence and breakage kernels. You can select none, constant, hibiki-ishii, ishii-kim, yao-morel, or user-defined. The three options, hibiki-ishii, ishii-kim and yao-morel are described in detail in Interfacial Area Concentration in the Theory Guide.

    In addition to specifying the hibiki-ishii, ishii-kim, and yao-morel as the coalescence and breakage kernels, you can also tune the properties of the three models by using the /define/phases/iac-expert/hibiki-ishii-model, /define/phases/iac-expert/ishii-kim-model, and /define/phases/iac-expert/yao-morel-model text commands.

    For each of the three models you can specify the parameters listed in Table 24.13: Parameters for the Coalescence and Breakage Kernels

    Table 24.13:  Parameters for the Coalescence and Breakage Kernels

    Hibiki-Ishii ModelIshii-Kim ModelYao-Morel Model
    Coefficient Gamma_c Coefficient Crc Coefficient K_c1
    Coefficient K_c Coefficient Cwe Coefficient K_c3
    Coefficient Gamma_b Coefficient C Coefficient K_b1
    Coefficient K_b Coefficient Cti alpha_max
    alpha_max alpha_max


    These values are discussed in greater detail in Interfacial Area Concentration in the Theory Guide.

    Nucleation Rate

    is a source term for the interfacial area concentration that models the rate of formation of the dispersed phase. You can choose from constant or user-defined. If the Boiling Model option is enabled, you can also select yao-morel. The yao-morel option is described in Yao-Morel Model in the Theory Guide.

    Critical Weber Number

    will need to be specified if you selected ishii-kim or yao-morel for the Breakage Kernel.

    Dissipation Function

    gives you the option to choose the formula which calculates the dissipation rate used in the hibiki-ishii and ishii-kim models. You can choose amongst constant, wu-ishii-kim, fluent-ke, and user-defined for the dissipation function.

    The wu-ishii-kim option uses a simple algebraic correlation for :

    (24–14)

    where

    and

    where , , , and are the mixture density, mixture velocity, mixture molecular viscosity, and hydraulic diameter of the flow path.

    When you select the wu-ishii-kim model, you will set an additional input for Hydraulic Diameter.

    Hydraulic Diameter

    is the value used in Equation 24–14, should you use the wu-ishii-kim formulation.

    Min/Max Diameter

    allow you to specify the minimum and maximum diameters of the secondary phase to which the interfacial area concentration model is applied, preventing some computing anomalies to spread beyond control.


Note:  When solving a steady-state problem, the preferred setting for the Under-Relaxation Factor is 1.0, as the interfacial area equation for the boiling models is currently under-relaxed using a locally defined pseudo-time step. If you want extra explicit under-relaxation, you may set the value of the Under-Relaxation Factor to less than one, this may be done only in case of serious convergence problems with the interfacial area transport equation. To improve convergence you can switch to a pseudo-time step for the interfacial area concentration only, using the define/phases/iac-expert/iac-pseudo-time-step text command and set the local pseudo-time to less than 1.


24.5.2.5. 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. You can also specify lift forces, wall lubrication forces (for non-granular flows only), turbulent dispersion forces, surface tension effects, and virtual mass force. For granular flows, you will also need to specify the restitution coefficient(s) for particle collisions.

To specify these parameters, click Interaction... to open the Phase Interaction Dialog Box and visit the Drag, Lift, Wall Lubrication, Turbulent Dispersion, Collisions, and Surface Tension tabs.

 Setup → Models → Multiphase → Phases  Edit... → Interaction...

24.5.2.5.1. Specifying the Drag Function

ANSYS Fluent allows you to specify a drag function for each pair of phases. Perform the following steps:

  1. Click the Drag tab.

  2. For each pair of phases, select the appropriate drag function from the corresponding drop-down list.

    • Select ishii to use the fluid-fluid drag function described by Equation 17–417 in the Theory Guide. This option is available when the boiling model is enabled.

    • Select schiller-naumann to use the fluid-fluid drag function described by Equation 17–182 in the Theory Guide. The Schiller and Naumann model is the default method, and it is acceptable for general use in all fluid-fluid multiphase calculations. When using the homogeneous population balance models you can also select schiller-naumann-pb in which case the interfacial area will be calculated directly from the population balance variables.

    • Select morsi-alexander to use the fluid-fluid drag function described by Equation 17–186 in the Theory Guide. 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 17–192 in the Theory Guide. 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. The symmetric drag law is the default method for the Multi-Fluid VOF Model, which is available with Eulerian multiphase model.

    • Select grace to use the fluid-fluid drag function described by Equation 17–197 in the Theory Guide. The Grace model is recommended for gas-liquid flows in which the bubbles can have a range of shapes such as spherical, elliptical, or cap.

    • Select tomiyama to use the fluid-fluid drag function described by Equation 17–203 in the Theory Guide. Like the Grace model, the Tomiyama model is recommended for gas-liquid flows in which the bubbles can have a range of shapes such as spherical, elliptical, or cap.

    • Select anisotropic to use the fluid-fluid drag function described in Multi-Fluid VOF Model in the Theory Guide. The anisotropic drag law is recommended for free surface modeling. It is based on higher drag in the normal direction to the interface and lower drag in the tangential direction to the interface.

    • Select universal-drag for bubble-liquid and/or droplet-gas flow when the characteristic length of the flow domain is much greater than the averaged size of the droplets/bubbles. It is suitable for flows in which the bubbles/droplets may have a range of shapes. The universal drag law is described using Equation 17–207 in the Theory Guide. When universal-drag is selected, you will need to set a value for the surface tension coefficient, under the Surface Tension tab, in the Phase Interaction dialog box. This value will apply to the primary phase and the secondary phase.

    • Select wen-yu to use the fluid-solid drag function described by Equation 17–242 in the Theory Guide. 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. When using the homogeneous population balance models you can also select wen-yu-pb in which case the interfacial area will be calculated directly from the population balance variables.

    • Select gidaspow to use the fluid-solid drag function described by Equation 17–244 in the Theory Guide. The Gidaspow model is recommended for dense fluidized beds.

    • Select syamlal-obrien to use the fluid-solid drag function described by Equation 17–229 in the Theory Guide. The Syamlal-O’Brien model is recommended for use in conjunction with the Syamlal-O’Brien model for granular viscosity.

    • Select syamlal-obrien-para to use the parameterized formulation of the Syamlal-O’Brien model described by Equation 17–239 in the Theory Guide. This model addresses under/over-prediction of bed expansion that can arise with syamlal-obrien. When you first select this model, you will be presented with the Syamlal Obrien Model dialog box.

      There are two inputs:

      Void Fraction

      the volume fraction of the gas phase in the bed at the minimum fluidization condition

      Minimum Fluidization Velocity

      the expected or experimentally-determined nominal minimum fluidization velocity of the gas phase

      Once you have input these values, click Validate/Apply to compute the coefficients c1 and d1 used in Equation 17–240 in the Fluent Theory Guide. A message will also be printed to the text user interface summarizing the fluid and flow properties used in the computation and the resulting values. You should check that these property values are consistent with the properties set elsewhere.


      Important:  If you change property values in the Create/Edit Materials dialog box or diameter in the Secondary Phase dialog box, you must initialize the flow field or run at least one iteration before computing c1 and d1. Otherwise, incorrect properties will be used in the computation.

      Note that the syamlal-obrien-para model is appropriate only for Geldart Group B particles and is only applicable to cases involving a single secondary phase.


    • Select syamlal-obrien-symmetric to use the solid-solid drag function described by Equation 17–250 in the Theory Guide. The symmetric Syamlal-O’Brien model is appropriate for a pair of solid phases.

    • Select huilin-gidaspow to use the fluid-solid drag function described by Equation 17–246 in the Theory Guide. This option provides a better blending function for the Gidaspow model when moving from the dense packing limit to the dilute flow limit.

    • Select gibilaro to use the fluid-solid drag function described by Equation 17–248 in the Theory Guide. This option is used for circulating fluidized beds

    • 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 Fluent Customization Manual for details).

    • If you want to temporarily ignore the interaction between two phases, select none.

24.5.2.5.1.1. Drag Modification

When using the Eulerian or Mixture multiphase models, you can optionally specify a drag modification term for the selected drag law. The drag modification term acts as a multiplier for the drag coefficient computed from the models detailed in Specifying the Drag Function. You can specify the drag modification term individually for each pair of primary-secondary phases. To enable drag modification, perform the following steps:

  1. Check Drag Modification in the Drag tab of the Phase Interaction dialog box.

    An additional drop-down list will appear under Drag Factor for each primary-secondary phase pair.

  2. For each pair of phases, select the Drag Factor to use from the drop-down list.

For additional details on the implementation of the drag modification, see Drag Modification in the Theory Guide.

24.5.2.5.2. Specifying the Restitution Coefficients (Granular Flow Only)

For granular flows, you need to specify the coefficients of restitution for collisions between particles ( in Equation 17–250 and in Equation 17–290 in the Theory Guide). 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.

Perform the following steps:

  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.

24.5.2.5.3. Including the Lift Force

For both granular and non-granular flows, it is possible to include the effect of lift forces ( in Equation 17–255 in the Theory Guide) 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 (for example, if the phases separate quickly), you may want to include this effect.


Important:  Note that the lift force will be more significant for larger particles, but the ANSYS Fluent model assumes that the particle diameter is much smaller than the interparticle spacing. Therefore, the inclusion of lift forces is not appropriate for closely packed particles or for very small particles.


To include the effect of lift forces, perform the following steps:

  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 moraga to use the Moraga lift model (Moraga Lift Force Model in the Theory Guide). The Moraga lift model is applicable to spherical solid particles, drops, and bubbles.

    • Select saffman-mei to use the Saffman-Mei lift model (Saffman-Mei Lift Force Model in the Theory Guide). The Saffman-Mei lift model is applicable to spherical solid particles, and to drops and bubbles that are not significantly distorted.

    • Select legendre-magnaudet to use the Legendre—Magnaudet lift model (Legendre-Magnaudet Lift Force Model in the Theory Guide). The Legendre-Magnaudet model is applicable to small diameter spherical fluid particles, though it can be applied to non-distorted liquid drops and bubbles. It accounts for momentum transfer between the flow around the particle and the inner recirculation flow inside the fluid particle caused by fluid friction/stresses at the fluid interface.

    • Select tomiyama to use the Tomiyama lift model (Tomiyama Lift Force Model in the Theory Guide). The Tomiyama model is applicable to larger-scale deformable bubbles in the ellipsoidal and spherical cap regimes. Its main feature is the prediction of the cross-over point in bubble size at which particle distortion causes a reversal in the sign of the lift force.

    • Select user-defined to use a user-defined function for the lift coefficient (see the Fluent Customization Manual for details).

24.5.2.5.4. Including the Wall Lubrication Force

For liquid-gas bubbly flows using the Eulerian multiphase model, you can include the effect of wall lubrication forces ( in Equation 17–168 in the Theory Guide) on the secondary phase bubbles. These forces tend to push the bubbles away from walls at small wall distances. For details on how wall lubrication is modeled in ANSYS Fluent see Wall Lubrication Force in the Theory Guide.

To include the effect of wall lubrication forces, perform the following steps:

  1. Click the Wall Lubrication tab to display the Wall Lubrication inputs.

  2. For each pair of phases, select the appropriate specification method from the corresponding drop-down list. Note that you will specify the wall lubrication only for pairs consisting of a secondary phase and the primary phase.

24.5.2.5.5. Including the Turbulent Dispersion Force

For turbulent flows using the Eulerian multiphase model, you can include the effects of turbulent dispersion force ( in Equation 17–168 in the Theory Guide). The turbulent dispersion force acts as a turbulent diffusion in dispersed flows. For details on how turbulent dispersion is modeled in ANSYS Fluent see Turbulent Dispersion Force in the Theory Guide.

To include the effects of turbulent dispersion force, perform the following steps:

  1. Click the Turbulent Dispersion tab to display the Turbulent Dispersion inputs.

  2. For each pair of phases, select the appropriate specification method from the corresponding drop-down list. Note that you will specify the turbulent dispersion only for pairs consisting of a secondary phase and the primary phase.

24.5.2.5.6. Including Surface Tension and Wall Adhesion Effects

As discussed in When Surface Tension Effects Are Important in the Theory Guide, the importance of surface tension effects depends on the value of the capillary number, Ca (defined by Equation 17–31 in the Theory Guide), or the Weber number, We (defined by Equation 17–32 in the Theory Guide). Surface tension effects can be neglected if Ca  or We  .


Important:  Note that the calculation of surface tension effects will be more accurate 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. ANSYS Fluent also offers an option to use VOF gradients at the nodes for curvature calculations on meshes when more accuracy is desired. For more information, see Surface Tension and Adhesion in the Theory Guide.


If you want to include the effects of surface tension along the interface between one or more pairs of phases, as described in Surface Tension and Adhesion in the Theory Guide, refer to Including Surface Tension and Adhesion Effects.

24.5.2.5.7. Including the Virtual Mass Force

For both granular and non-granular flows, it is possible to include the “virtual mass force” ( in Equation 17–288 in the Theory Guide) 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 (for example, for a transient bubble column).

To include the effect of the virtual mass force perform the following steps:

  1. Click the Virtual Mass tab to display the Virtual Mass inputs.

  2. Enable Virtual Mass Modeling.

  3. For each phase pair listed under Virtual Mass Coefficient, select the method for specifying the virtual mass coefficient, , in Equation 17–288 in the Fluent Theory Guide. You can choose from the following methods:

    none

    Disable virtual mass modeling for the phase pair.

    constant

    Specify a constant value for the coefficient. The default value of 0.5 is typical.

    user-defined

    Use a user-defined function created with the DEFINE_EXCHANGE_PROPERTY macro. See DEFINE_EXCHANGE_PROPERTY in the Fluent Customization Manual for details.


    Important:  No virtual mass effects will be included unless the Virtual Mass Modeling option is enabled.


  4. If desired, you can enable the Implicit method for virtual mass.

    When using the Implicit method, the Default option uses the complete term in Equation 17–288. You can also choose Option 2 or Option 3, which use locally truncated forms of the virtual mass terms in cells where divergence is detected.

    The Implicit method is recommended for steady-state coupled simulations as it offers improved convergence in such cases. The recommended approach is to begin the simulation using Option 2. Once the solution has converged enough to establish the basic flow field, switch back to Default to include the complete virtual mass term.


Release 18.2 - © ANSYS, Inc. All rights reserved.