### 12.4.2. Fluid Models Tab

The Fluid Models tab is where models are chosen, which apply to all Eulerian fluids in the simulation. By default, the fluids models must be consistent between all fluid domains in a multidomain simulation, but CFX supports inconsistent physics through the setting of an environment variable. For details, see:

- Using Multiple Domains

- Solid Models Tab.

In a multiphase simulation, the options that are allowed to vary between fluids will appear on the Fluid Specific Models tab instead. For details, see Fluid Specific Models Tab.

Some fluid models can apply to all fluids or can be set on a fluid-specific basis, these models will appear on the Fluid Models section with a `Fluid Dependent` option. If this is selected, then the model appears on the Fluid Specific Models tab.

The options available on the Fluid Specific Models tab depends on the simulation set up (including the type and number of fluids used in the simulation (such as single or multicomponent, single or multiphase, reacting or non-reacting)) and whether Additional Variables have been created.

All details related to Particle Tracking are set on the General Settings tab and the models chosen on the Fluid Models tab do not apply to the particle phase.

Radiation with multiphase is not supported. However, it is allowed for single Eulerian particle tracking cases on the Fluid Specific Models tab.

The available settings depend on the physical models chosen in your simulation.

#### 12.4.2.1. Multiphase Options

These options are only applicable to multiphase simulations.

##### 12.4.2.1.1. Homogeneous Model

Inhomogeneous is the general case of multiphase flow, where each fluid has its own velocity field, turbulence field, and so on. You can select the Homogeneous Model check box to switch to this model, where all fluids share a velocity field, turbulence field, and so on. For details, see The Homogeneous and Inhomogeneous Models in the CFX-Solver Modeling Guide. Both the inhomogeneous and homogeneous models have a Free Surface Model option.

##### 12.4.2.1.2. Free Surface Model

You can select the `Standard` free surface model if you are modeling multiphase flow with a distinct interface between the fluids. For details, see Free Surface Flow in the CFX-Solver Modeling Guide.

##### 12.4.2.1.3. Multiphase Reactions

Multiphase Reactions are available when any reactions have been defined with type Multiphase. For details, see Multiphase: Basic Settings. Any reactions that are to be included in the simulation should be selected from the drop-down list. For details, see Multiphase Reactions in the CFX-Solver Modeling Guide.

#### 12.4.2.2. Heat Transfer

##### 12.4.2.2.1. Homogeneous Model

For details, see Homogeneous Heat Transfer in Multiphase Flow in the CFX-Solver Modeling Guide.

##### 12.4.2.2.2. Heat Transfer: Option

Depending on your simulation, the following heat transfer options are possible. For details, see Heat Transfer in the CFX-Solver Modeling Guide.

- `None`: Not available for compressible fluids, since a temperature is required at which to evaluate the fluid properties.

- `Isothermal`: Not available for reacting fluids.

- `Thermal Energy`: Models the transport of enthalpy through the fluid and is suitable for modeling heat transfer in low-speed flows. For details, see The Thermal Energy Equation in the CFX-Solver Theory Guide.

  The Turbulent Prandtl Number may be customized by selecting the Turbulent Flux Closure check box in the Turbulence settings.

- `Total Energy`: Includes high-speed energy effects. You should include the viscous work term in the energy equation (select Heat Transfer > Incl. Viscous Work Term). For details, see The Total Energy Equation in the CFX-Solver Theory Guide.

  The Turbulent Prandtl Number may be customized by selecting the Turbulent Flux Closure check box in the Turbulence settings.

- `Fluid Dependent`: Is used to set different heat transfer models for each fluid in a multiphase simulation. A heat transfer model is then set for each fluid on the Fluid Specific Models tab. This option cannot be used when Homogeneous Model is selected for the heat transfer model.

Important: If a compressible transient flow is undertaken with only one iteration per time step, then the solution can be incorrect if the Heat Transfer option is not set to Total Energy, or if heat transfer is not included in the simulation. This is due to the CFX-Solver not extrapolating the pressure at the start of the time step in these circumstances. This means that density is not extrapolated, and so the solver cannot calculate an accurate value for the time derivative of density on the first iteration. The workaround for this problem is to either run with at least two iterations per time step, or to use the Total Energy option for Heat Transfer.

#### 12.4.2.3. Turbulence

Advice on which turbulence model is appropriate for your simulation and a description of each model can be reviewed. For details, see:

- Turbulence and Near-Wall Modeling in the CFX-Solver Modeling Guide

- Turbulence Modeling in Multiphase Flow in the CFX-Solver Modeling Guide

- Turbulence Models in the CFX-Solver Theory Guide.

##### 12.4.2.3.1. Homogeneous Model

If you have not selected Homogeneous Model under Multiphase Options, then Homogeneous Model under Turbulence frame will be available.

If selected, this will solve a single turbulence field for an inhomogeneous simulation. There will be no fluid-specific turbulence data to set. For details, see Homogeneous Turbulence in Inhomogeneous Flow in the CFX-Solver Modeling Guide.

If you do not select this check box, then you will usually select `Fluid Dependent` and specify turbulence data on the fluid-specific tabs. Alternatively, the Laminar model can be picked to apply to all fluids (this is not homogeneous turbulence).

Homogeneous multiphase flow always uses homogeneous turbulence; therefore, you only need select the turbulence model to use.

##### 12.4.2.3.2. Turbulence: Option

You can select one of the following turbulence models:

- `None (Laminar)`: Turbulence is not modeled. This should only be used for laminar flow. Of the combustion models, only Finite Rate Chemistry is available for laminar flow. For details, see The Laminar Model in the CFX-Solver Modeling Guide.

- `k-Epsilon`: A standard fluid model that is suitable for a wide range of simulations. For details, see The k-epsilon Model in the CFX-Solver Modeling Guide.

- `Fluid Dependent`: Allows you to set different turbulence models for each fluid in the domain. If this option is selected, the turbulence model for each fluid is set in the Fluid Specific Models tab. This is only available for multiphase simulations when Homogeneous Model is not selected.

- `Shear Stress Transport`: Recommended for accurate boundary layer simulations. For details, see The k-omega and SST Models in the CFX-Solver Modeling Guide.

- `Omega Reynolds Stress / BSL Reynolds Stress`: For details, see Omega-Based Reynolds Stress Models in the CFX-Solver Modeling Guide.

- `QI / SSG / LRR Reynolds Stress`: Provides high accuracy for some complex flows. For details, see Reynolds Stress Turbulence Models in the CFX-Solver Theory Guide.

- `Zero Equation`: Only the Finite Rate Chemistry combustion model is available when using the zero equation turbulence model. For details, see The Zero Equation Model in the CFX-Solver Modeling Guide.

- `RNG k-Epsilon`: A variation of the k-epsilon model.

- `k-Omega / BSL`: The SST model is often preferred to this model.

- `k epsilon EARSM / BSL EARSM`: These models are a simplified version of the Reynolds stress models with application to problems with secondary flows as well as flows with streamline curvature and/or system rotation. For details, see Explicit Algebraic Reynolds Stress Model in the CFX-Solver Theory Guide

- `LES Smagorinsky / LES WALE / LES Dynamic Model`: Available for transient simulation only. For details, see The Large Eddy Simulation Model (LES) in the CFX-Solver Modeling Guide.

- `Detached Eddy Simulation`: Available for transient simulation only. For details, see The Detached Eddy Simulation Model (DES) in the CFX-Solver Modeling Guide.

- `Stress Blended Eddy Simulation`: Available for transient simulation only. This is a refinement of Detached Eddy Simulation. For details, see The Stress-Blended Eddy Simulation (SBES) Model in the CFX-Solver Modeling Guide.

- `SAS SST`: Available for transient simulation only. For details see, The Scale-Adaptive Simulation (SAS) in the CFX-Solver Modeling Guide.

- `Eddy Viscosity Transport Equation`: A one-equation variation of the k-epsilon model. For details, see The Eddy Viscosity Transport Model in the CFX-Solver Theory Guide.

The available Advanced Turbulence Control settings for turbulence modeling depend on the turbulence model. The settings can be used to specify the coefficients for the selected turbulence model. These coefficients are described in Table 12.2: Advanced Turbulence Parameters:

Table 12.2: Advanced Turbulence Parameters

Parameter | Description
SST Reattachment Modification | Available only when Turbulence > Option is set to `Shear Stress Transport`. For details, see The Reattachment Modification (RM) Model in the CFX-Solver Theory Guide.
Eddy Viscosity | Enables you to specify a value that will be picked up by the specified turbulence model; in this case the internal algorithm will not be used.
BC TKI Factor | A factor for turbulence intensity used in turbulence boundary conditions based on “Autocompute Length Scale”, such as “Default Intensity and Autocompute Length Scale” (default = 1000). For more details, see Inlet (Subsonic) in the CFX-Solver Theory Guide.
BetaStar Coefficient | Model coefficient; appears when an omega-based turbulence model is selected (default = 0.09). Can appear in several equations. For example, see Equation 2–36 in the CFX-Solver Theory Guide or Equation 2–51 in the CFX-Solver Theory Guide.
Cmu Coefficient | Model coefficient; appears when an epsilon-based turbulence model is selected (default = 0.09). See Equation 2–22 in the CFX-Solver Theory Guide.
Compressible Production | For details, see The k-epsilon Model in ANSYS CFX in the CFX-Solver Theory Guide.
A1 Coefficient | Model coefficient of the SST turbulence model (default = 0.31). See Equation 2–60 in the CFX-Solver Theory Guide.

Curvature Correction

For details, see:

- Curvature Correction for Two-Equation Models in the CFX-Solver Theory Guide

- Explicit Algebraic Reynolds Stress Model in the CFX-Solver Theory Guide

High Lift Modification | For improved modeling of high-lift devices (for example, airfoils and wings). Leads to stronger flow separation and reduced maximum lift. Available only when Turbulence > Option is set to `Shear Stress Transport`. The `High Lift Correction` option has an adjustable CHL Coefficient, which has a range from 0.5 to 1.0 and a default value of 0.9. For details, see Modifications to SST for High Lift Devices in the CFX-Solver Theory Guide.

K Coefficients

For details, see:

- The k-epsilon Model in ANSYS CFX in the CFX-Solver Theory Guide

- The k-omega Models in ANSYS CFX in the CFX-Solver Theory Guide

k-Omega Regime

For details, see:

- The Baseline (BSL) k-omega Model in the CFX-Solver Theory Guide

- The Shear Stress Transport (SST) Model in the CFX-Solver Theory Guide

k-Epsilon Regime

For details, see:

- The Baseline (BSL) k-omega Model in the CFX-Solver Theory Guide

- The Shear Stress Transport (SST) Model in the CFX-Solver Theory Guide

Epsilon Coefficients | For details, see The k-epsilon Model in ANSYS CFX in the CFX-Solver Theory Guide.
Production Limiter | For details, see Production Limiters in the CFX-Solver Theory Guide.

DES Coefficients

Model parameters for the Detached Eddy Simulation model. For details, see:

- Detached Eddy Simulation Theory in the CFX-Solver Theory Guide

- The Detached Eddy Simulation Model (DES) in the CFX-Solver Modeling Guide

SBES Coefficients

Model parameters for the Stress-Blended Eddy Simulation model. For details, see:

- The Stress-Blended Eddy Simulation (SBES) Model in the CFX-Solver Modeling Guide

- Stress-Blended Eddy Simulation (SBES) in the CFX-Solver Theory Guide

Omega Coefficients | For details, see The k-omega Models in ANSYS CFX in the CFX-Solver Theory Guide.
High Wave Number Damping | Enables you to specify the limiter coefficient () in Equation 2–215 in the CFX-Solver Theory Guide for the SAS SST model (default = 0.11).

##### 12.4.2.3.3. Buoyancy Turbulence

Buoyancy Turbulence is available for two (or more) equation turbulence models. For details, see Buoyancy Turbulence in the CFX-Solver Modeling Guide.

##### 12.4.2.3.4. Wall Function

The wall function is automatically set depending on the turbulence model selected. Therefore, you will not need to change this setting. For multiphase flow, if the fluid dependent turbulence model option is selected, the wall function option appears on the fluid- specific tabs. The Laminar and zero equation turbulence models do not use wall functions. For details, see Modeling Flow Near the Wall in the CFX-Solver Modeling Guide.

##### 12.4.2.3.5. Turbulent Flux Closure for Heat Transfer

Turbulent Flux Closure for Heat Transfer is available for turbulent flow with Thermal Energy or Total Energy heat transfer model. For details, see Heat Transfer in the CFX-Solver Modeling Guide.

#### 12.4.2.4. Reaction or Combustion Model

If the fluid material is defined as Option is `Material Definition` and Composition Option is `Reacting Mixture`, or if a reacting mixture from the material library has been selected as the material for one of the domain fluids, then you can select a combustion model as:

- `Eddy Dissipation`

- `Finite Rate Chemistry`

- `Finite Rate Chemistry and Eddy Dissipation`

- `PDF Flamelet`

- `BVM (Partially Premixed)`

- `Extended Coherent Flame Model`

- `Fluid Dependent` (multiphase only)

Only `Finite Rate Chemistry` is available when `Laminar` or `Zero Equation` turbulence model is used.

In multiphase simulations, when `Fluid Dependent` is selected, a different combustion model can be used for each reacting fluid in the simulation. If the homogeneous multiphase model is used, all fluids must be reacting mixtures that include reactions to enable a combustion to be modeled.

If the fluid material is defined as a reacting mixture from the material library, then the available combustion models are filtered in order to be compatible with the reactions specified in the reacting material.

If the fluid material is defined as Option is `Material Definition` and Composition Option is `Reacting Mixture`, then the complete list of combustion models is presented and the reactions list for the mixture has to be specified. Only those reactions from the material library will be available that are compatible with the selected combustion model.

Depending on the selected combustion model, additional options (such as `Autoignition Model`, `NO Model`, and `Chemistry Post-Processing`) and parameters may be available. For details, see Combustion Modeling in the CFX-Solver Modeling Guide.

##### 12.4.2.4.1. Soot Model

When a combustion model is selected, you can optionally enable the Magnussen soot model to account for the formation of soot. In multiphase simulations, this model appears on the fluid-specific tab for each fluid that uses a combustion model.

A Fuel and Soot Material is required, and the following optional parameters can also be set:

- Fuel Consumption Reaction

- Fuel Carbon Mass Fraction

- Soot Density

- Soot Particle Mean Diameter

For details, see Soot Model in the CFX-Solver Modeling Guide.

#### 12.4.2.5. Thermal Radiation Model

If a heat transfer model other than `None` has been selected, you can model thermal radiation. If a radiation model is selected, you must make sure that the radiation properties for that fluid have been set in the Material details view. For details, see Material Properties Tab. Radiation is not supported for multiphase simulations in CFX.

The four radiation models available in CFX are:

- `Rosseland`

- `P1`

- `Discrete Transfer`

- `Monte Carlo`

A Spectral Model can be selected for all radiation models. If the `Multigray` or `Weighted Sum of Gray Gases` representation is selected for the Spectral Model, then you should create the required number of gray gases.

1. Click Add new item to add a new gray gas. (You can click Delete to delete a highlighted gray gas.)

2. Set the Weight and Absorption Coefficient for each gray gas.

   For details, see Multigray/Weighted Sum of Gray Gases in the CFX-Solver Modeling Guide.

Alternatively, if the Multiband representation is selected, you should create Spectral Bands:

1. Click Add new item to add a new spectral band. (You can click Delete to delete a highlighted spectral band.)

2. Set Option to either `Frequency`, `Wavelength` or `Wavenumber`.

3. Enter upper and lower limits for the option selected.

   This defines the range of the spectral band. For details, see:

   - Multiband in the CFX-Solver Modeling Guide

   - Spectral Model in the CFX-Solver Modeling Guide

   - Radiation Modeling in the CFX-Solver Modeling Guide.

#### 12.4.2.6. Electromagnetic Model

The Electromagnetic Model enables you to define:

Electric Field Model

  Option can be set to `None`, `Electric Potential`, or `User Defined`. For details, see Electric Field in the CFX-Solver Modeling Guide.

Magnetic Field Model

  Option can be set to `None`, `Magnetic Vector Potential`, or `User Defined`.

If a user-defined model is selected, you must make sure that the electromagnetic properties have been set in the Material details view. For details, see Material Properties Tab. Electromagnetic models are supported for multiphase simulations only if homogeneous.

For more information on electromagnetic theory, see Electromagnetic Hydrodynamic Theory in the CFX-Solver Theory Guide.

#### 12.4.2.7. Component Details

If your fluid contains more than one component (that is, you are using a variable composition or reacting mixture, or HCF fuel, created in the Material details view), then Component Details will need to be set on the Fluid Models tab. If using the Algebraic Slip Multiphase model (ASM), the settings are specified in this view as well. For details, see Algebraic Slip Model (ASM) in the CFX-Solver Modeling Guide. When a non-ASM multiphase model is used, the Component Details form appears on the fluid-specific tabs.

- Select each component in turn and set the required option.

- Select the type of equation to solve for this component as `Automatic`, `Transport Equation`, `Constraint`, `Algebraic Equation` or `Algebraic Slip`. A description of the multiphase model is available in:

  - Algebraic Slip Model (ASM) in the CFX-Solver Modeling Guide

  - Component Domain Settings in the CFX-Solver Modeling Guide.

- If you have chosen to solve a transport equation for the component, you can optionally enter a value for Kinematic Diffusivity. If you do not set Kinematic Diffusivity, then the Bulk Viscosity value is used.

- If you have chosen to solve a transport equation or an Algebraic Slip component, you can optionally set a component dependent Turbulent Schmidt Number by enabling the Turbulent Flux Closure check box. If you do not select Turbulent Flux Closure, the value from Turbulence > Turbulent Flux Closure for Heat Transfer will be used.

The Component Details specify the model used to calculate the mass fraction of each component throughout the domain. For details, see Component Domain Settings in the CFX-Solver Modeling Guide.

#### 12.4.2.8. Additional Variable Details

If you have defined any Additional Variables from the Additional Variable details view, then you can choose to include or exclude them here. An Additional Variable is included by selecting it from the Additional Variables Details list and then enabling the check box with the name of the Additional Variable. For details, see Additional Variables.

If an Additional Variable is included, you must select how the Additional Variable level is calculated.

For single phase flows, the CFX-Solver can solve different variations of the conservation equations for the variable including `Transport Equation`, `Diffusive Transport Equation` or `Poisson Equation`.

For multiphase flows, the CFX-Solver can solve different variations of the conservation equations for the variable including `Homogeneous Transport Equation`, `Homogeneous Diffusive Transport Equation`, `Homogeneous Poisson Equation` or `Fluid Dependent`. When the `Fluid Dependent` option is selected, the Additional Variable model details can be set for each fluid on the Fluid Specific Models tab.

If a transport equation is being solved for an Additional Variable, the Turbulent Flux Closure may be optionally specified for turbulent flow. If you do not select Turbulent Flux Closure for the Additional Variable, the default is Option is Eddy Diffusivity and the Turb. Schmidt Num. is set to 0.9.

Alternatively, you can define the variable value algebraically using CEL by selecting the `Algebraic Equation` option. Note that the `Algebraic Equation` option is not available for homogeneous Additional Variables. In addition, only specific Additional Variables are permitted to be homogeneous. For details, see Additional Variables in the CFX-Solver Modeling Guide.

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