The Fluid Pairs tab appears for multiphase simulations and/or when particles are included in the domain. It is used to specify how the fluids interact in a multiphase simulation and how particles interact with the fluids when particles are included.
For details, see Fluid Pairs in the CFX-Solver Modeling Guide.
The top of the Fluid Pair Models tab shows a list of all the phase pairs in the simulation. A phase pair will exist when the morphology of the pair is Continuous Fluid | Continuous Fluid, Continuous Fluid | Dispersed Fluid or Continuous Fluid | Dispersed Solid. If particles have also been included, then a pair will exist for each Continuous Fluid | Particle pair. You should select each pair in turn and set the appropriate options.
The options available will vary considerably depending on your simulation. Many options are not available when the homogeneous multiphase model is used. This is because the interphase transfer rates are assumed to be very large for the homogeneous model and do not require further correlations to model them.
This only applies to Continuous Fluid | Particle pairs. For details, see Particle Fluid Pair Coupling Options in the CFX-Solver Modeling Guide.
You can optionally provide a Surface Tension Coefficient. This should be set in either of the following two cases:
For a Continuous Fluid | Dispersed Fluid pair when you want to model the Drag Force using either the
GraceorIshii Zubermodels. The flow must also be Buoyant to enable these models to be selected. For details, see Interphase Drag for the Particle Model in the CFX-Solver Modeling Guide.When you want to use the surface tension model. This model is only available when
Standardhas been selected as the Free Surface Model on the Fluid Models tab.
You can set a Surface Tension Coefficient in other cases, but it will not be used in your simulation. It does not apply to Continuous Fluid | Particle pairs.
For details, see Surface Tension in the CFX-Solver Modeling Guide.
You can model the surface tension force that exists at a free surface interface. This model applies to all morphology combinations for Eulerian | Eulerian pairs. You must also specify a Surface Tension Coefficient and select the Primary Fluid. For liquid-gas free surface flows, the primary fluid should be the liquid phase.
For details, see Surface Tension in the CFX-Solver Modeling Guide.
This can be selected as one of the following:
This model assumes a continuous phase fluid containing particles of a dispersed phase fluid or solid. It is available when the morphology of the pair is Continuous Fluid | Dispersed Fluid or Continuous Fluid | Dispersed Solid. For details, see The Particle Model in the CFX-Solver Modeling Guide.
This model is only available when the morphology of the pair is Continuous Fluid | Continuous Fluid. An Interface Length Scale is required. It is usually used as a first approximation or combined with a custom interface transfer model. For details, see The Mixture Model in the CFX-Solver Modeling Guide.
This model is available when the free surface model is selected. For details, see The Free Surface Model in the CFX-Solver Modeling Guide. For free surface flow, the particle model is also available if the phase pair is Continuous Fluid | Dispersed Fluid, and the mixture model is also available if the phase pair is Continuous Fluid | Continuous Fluid.
There are a variety of momentum transfer that can be modeled, including the drag force and non-drag forces, which include lift force, virtual mass force, wall lubrication force and turbulent dispersion force.
This option applies to all morphology pair combinations including Continuous Fluid | Particle pairs, but does not apply when the Homogeneous multiphase model is active.
There are many drag force models available in CFX, but most are only applicable to certain morphology combinations. For Continuous Fluid | Particle pairs, the available options are:
The
Schiller-Naumanndrag model.For details, see Interphase Drag in the CFX-Solver Modeling Guide.
The
Drag Coefficient.For details, see Drag Force for Particles in the CFX-Solver Modeling Guide.
The
Ishii Zuberdrag model.For details, see Sparsely Distributed Fluid Particles: Ishii-Zuber Drag Model in the CFX-Solver Modeling Guide and Densely Distributed Fluid Particles: Ishii-Zuber Drag Model in the CFX-Solver Modeling Guide.
The
Gracedrag model.For details, see Sparsely Distributed Fluid Particles: Grace Drag Model in the CFX-Solver Modeling Guide and Densely Distributed Fluid Particles: Grace Drag Model in the CFX-Solver Modeling Guide.
The Particle User Source check box is available when any User Routines of type Particle User Routines exist. For details, see:
The lift force is only applicable to the Particle
Model, which is active for Continuous Fluid |
Dispersed (Fluid, Solid) and Continuous Fluid
| Polydispersed Fluid. For details, see Lift Force in the CFX-Solver Modeling Guide.
This option applies to Continuous Fluid | Dispersed
Fluid pairs using the Particle Model, and to Continuous Fluid | Particle pairs,
but does not apply when the Homogeneous multiphase model is active.
For details, see Virtual Mass Force in the CFX-Solver Modeling Guide.
This option is only applicable to the Particle Model. For details, see Wall Lubrication Force in the CFX-Solver Modeling Guide.
This applies to Continuous Fluid | Dispersed Fluid, Continuous Fluid | Polydispersed Fluid and Continuous Fluid | Dispersed Solid pair combinations for Eulerian | Eulerian pairs, but does not apply when the Homogeneous multiphase model is active. In these cases, the Lopez de Bertodano model is used. For details, see Interphase Turbulent Dispersion Force in the CFX-Solver Modeling Guide.
When particle tracking is used, the turbulent dispersion force also applies to Continuous Fluid | Particle pairs. In these cases, the Particle Dispersion models is used. For details, see Turbulent Dispersion Force in the CFX-Solver Modeling Guide.
This option is only available for Particle Tracking simulations. For details, see Pressure Gradient Force in the CFX-Solver Modeling Guide.
In flows with a dispersed phase, large particles in the dispersed phase tend to increase turbulence in the continuous phase due to the presence of wakes behind the particles. This is known as particle-induced turbulence.
The Enhanced Turbulence Production Model settings can be used to model particle-induced turbulence.
The options are:
NoneSato Enhanced Eddy ViscosityThis option is available for Continuous Fluid | Dispersed Fluid, Continuous Fluid | Polydispersed Fluid and Continuous Fluid | Dispersed Solid pair combinations for Eulerian | Eulerian pairs, but does not apply when the Homogeneous multiphase model is active, and is not available for Continuous Fluid | Particle pairs.
Turbulence Source TermsThis option enables the use of a dissipation timescale model.
For details, see Enhanced Turbulence Production Models in the CFX-Solver Modeling Guide.
This applies to all morphology combinations for Eulerian | Eulerian and Continuous Fluid | Particle pairs, but does not apply when the Homogeneous multiphase model is active.
For details, see Interphase Heat Transfer in the CFX-Solver Modeling Guide for multiphase applications and Interphase Heat Transfer in the CFX-Solver Modeling Guide for particle transport modeling.
Mass transfer can occur in homogeneous and inhomogeneous Eulerian multiphase flows. For such flows, you can set the Mass Transfer option to one of the following:
None
This is an advanced option that allows you to define your own mass transfer sources. For details, see User Specified Mass Transfer in the CFX-Solver Modeling Guide.
This models mass transfer due to phase change, such as condensation, melting or solidification. For details, see Thermal Phase Change Model in the CFX-Solver Modeling Guide.
Note that wall boiling settings are on the Boundary Models tab of the domain. For details, see Boundary Models Tab.
Vapor formation in low pressure regions of a liquid flow (cavitation) can be modeled using the Rayleigh Plesset model or, for advanced users, a user-defined model. For details, see Cavitation Model in the CFX-Solver Modeling Guide.
Additional Variable Pairs details describe the way in which Additional Variables interact between phases. It applies to all morphology combinations for Eulerian | Eulerian pairs, but does not apply when the Homogeneous multiphase model is active.
Only Additional Variable pairs where both are solved using the Transport Equation and have a Kinematic Diffusivity value set can be transferred between phases. These options are set on the fluid-specific tabs for each phase.
For example, consider two phases, Phase A and Phase B, and two Additional Variables, AV1 and AV2.
AV1uses a Transport Equation with diffusion inPhase Aand is unused inPhase B.AV2uses an Algebraic Equation inPhase Aand uses a Transport Equation with diffusion inPhase B.
Additional Variable interphase transfer can only occur between Phase A / AV1 and Phase B / AV2.
For details, see Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide.
You can model transfer of components between phases for Eulerian | Eulerian pairs, when both fluids are multicomponent
mixtures of any type (except fixed composition mixtures). Interphase
species transfer (or component transfer) may be specified between
any two components, A and B, in fluids, 
and 
, respectively,
subject to the following condition:
The mass fractions of A and B must both be determined from transport equations.
It is not possible to specify the species transfer of a component whose mass fraction is determined algebraically, or from the constraint equation.
For more information on implementing component pairs in CFX-Solver, see Component Pairs in the CFX-Solver Modeling Guide.
Mixtures are created in the Material details view, which is described in Material Details View: Variable Composition Mixture. Component transfer enables you to model processes such as evaporation, absorption, and dissolution.
To specify the component transfer model, you should select the component pair from the list on the Fluid Pairs tab and then select the associated toggle. The first component of the component pair corresponds to the first fluid in the fluid pairs list.
Option can be set to Two Resistance or Ranz Marshall. For details, see:
The choice of interfacial equilibrium model depends on the process that you are modeling. For details, see Interfacial Equilibrium Models in the CFX-Solver Modeling Guide.
The Fluid1 and Fluid2 Species
Mass Transfer options are used to choose a correlation
to model the mass transfer coefficient on each side on the interface.
For details, see Species Mass Transfer Coefficients in the CFX-Solver Modeling Guide.
Selecting the toggle enables mass transfer between the two phases.
The options for mass transfer are:
Ranz Marshall. For details, see Ranz Marshall in the CFX-Solver Modeling Guide.Liquid Evaporation Model.For details, see Liquid Evaporation Model in the CFX-Solver Modeling Guide. For oil evaporation, the Light Oil check box should be selected. For details, see Liquid Evaporation Model: Oil Evaporation/Combustion in the CFX-Solver Modeling Guide.None
For details on these options, see:
Particle User Source in the CFX-Solver Modeling Guide.
The drop-down list will contain any User Particle Routines you have created. For details, see Particle User Routines.
Mass transfer between a species in a particle phase and a species in the continuous phase is possible. For example, consider liquid water from a particle evaporating into gaseous H20 in a continuous phase mixture. The particle can be a pure substance or variable composition mixture.
The Particle Breakup models enable you to simulate the breakup of droplets due to external aerodynamic forces. The droplet breakup models are set on a per fluid-pair basis. By default, the Use Liu Dynamic Drag Modification option is activated for the TAB, ETAB and CAB breakup models, whereas the Use Schmehl Dynamic Drag Law option is activated for the Schmehl breakup model. See Particle Breakup Model in the CFX-Solver Modeling Guide for details on the available particle breakup models.
The particle collision model enables you to simulate dense gas-solid
flows with high mass-loading while the particle volume fraction is
still low. Select either Sommerfeld Collision Model or User Defined and specify values for the
particle collision parameters outlined below:
- Sommerfeld Collision Model
Coefficient of Restitution: Enter a numerical quantity or CEL based expression to specify the value of coefficient of restitution for inter-particle collisions. A value of ‘1.0’ means a fully elastic collision, while a value of ‘0.0’ would result in an inelastic collision.Static Friction CoefficientandKinetic Friction Coefficient: Enter a numerical quantity or CEL based expression to specify values of coefficients of friction for inter-particle collisions.See Implementation Theory in the CFX-Solver Theory Guide for more information on setting up
Coefficient of Restitution,Static Friction Coefficient, andKinetic Friction Coefficient.
- User Defined
This option is available only if you have created a particle user routine to set up the model. Specify the name of Particle User Routine and select input arguments and type of particle variables returned to the user routine from the Arguments and Variable List drop-down list, respectively. See Particle User Routines in the CFX-Pre User's Guide for information on setting up a particle user routine.
For additional information, see Particle Collision Model in the CFX-Solver Modeling Guide and the following topics available under Particle Collision Model in the CFX-Solver Theory Guide:
Implementation of a Stochastic Particle-Particle Collision Model in Ansys CFX (includes the discussion on the implementation theory, particle variables, and virtual collision partner)
Particle Collision Coefficients Used for Particle-Particle Collision Model
Limitations of Particle-Particle Collision Model in Ansys CFX