allows you to select one of four multiphase models.

allows you to specify the number of phases for the multiphase calculation. You can specify up to 20 phases.

allows you to apply an interface tracking method that couples the level set method with the VOF formulation.

contains parameters related to the VOF and Eulerian model. This section of the dialog box will appear only when Volume of Fluid or Eulerian is the selected Model.

contains options related to the Mixture model.

contains options for modeling flow regime transition. This group box is available only with the Eulerian multiphase model.

contains options related to the Eulerian model.

allows you to specify the number of discrete phases when the Dense Discrete Phase Model option is enabled.

contains an additional option for body force calculations.

contains additional sub-models that can be applied when using the VOF model.

contains additional modeling options.

contains a list of all of the phases in the problem from which you can select the phase you want to define or modify. A phase can be a Primary Phase or a Secondary Phase. You cannot change a phase from primary to secondary, or vice versa. Instead, you can redefine the properties of the primary phase to reflect the new phase designated as primary, and redefine the secondary phases accordingly as well.

adds a new phase in your simulation.

deletes the selected phase.

is a group box where you can define the properties of the selected primary or secondary phase.

displays the ID number of the interaction domain. You will need this number only if you are writing a user-defined function. See the separate Fluent Customization Manual for details about writing user-defined functions for multiphase applications.

tab allows you to specify forces acting between the phases.

tab contains the following tabs:

tab displays the Interfacial Area settings to predict interfacial area between the phases. This tab appears only for the Mixture multiphase model with interphase mass transfer and the Eulerian multiphase model. See Defining the Algebraic Interfacial Area Concentration and Using an Algebraic Interfacial Area Model for information about the available options.

tab allows you to use the diffusive and anti-diffusive discretization procedure across the distinct interfaces.

specifies the number of VOF-to-DPM model transition mechanisms in your simulation. See Setting up the VOF-to-DPM Model Transition for information about the available options.

enables/disables the calculation of energy in the model.

enables/disables the Two-Temperature Model. Only available for the density-based solver.

specifies inviscid flow.

specifies laminar flow.

specifies turbulent flow to be calculated using the Spalart-Allmaras model. (See Spalart-Allmaras Model in the Theory Guide for background about this model. See Setting Up the Spalart-Allmaras Model for details about using this model.)

specifies turbulent flow to be calculated using one of three - models. (See Standard, RNG, and Realizable k-ε Models in the Theory Guide for background about this model. See Setting Up the k-ε Model for details about using this model.)

specifies turbulent flow to be calculated using one of two - models. (See Standard, BSL, and SST k-ω Models in the Theory Guide for background about these models. See Setting Up the k-ω Model for details about using this model.)

specifies turbulent flow to be calculated using the Transition -- model. (See k-kl-ω Transition Model in the Theory Guide for background about this model. See Setting Up the Transition k-kl-ω Model for details about using this model.)

specifies turbulent flow to be calculated using the Transition SST model. (See Transition SST Model in the Theory Guide for background about this model. See Setting Up the Transition SST Model for details about using this model.)

specifies turbulent flow to be calculated using the RSM. (See Reynolds Stress Model (RSM) in the Theory Guide for background about this model. See Setting Up the Reynolds Stress Model for details about using this model.)

specifies turbulent flow to be calculated using the SAS model in combination with the SST - model. (See Scale-Adaptive Simulation (SAS) Model in the Theory Guide for background about this model. See Setting Up Scale-Adaptive Simulation (SAS) Modeling for details about using this model.)

specifies turbulent flow to be calculated using the DES model. (See Detached Eddy Simulation (DES) in the Theory Guide for background about this model. See Setting Up the Detached Eddy Simulation Model for details about using this model.)

(3D only) specifies turbulent flow to be calculated using the LES model. (See Large Eddy Simulation (LES) Model in the Theory Guide for background about this model. See Setting Up the Large Eddy Simulation Model for details about using this model.)

selects the vorticity-based calculation of the deformation tensor (see Equation 4–22 in the Theory Guide).

selects the strain/vorticity-based calculation of the deformation tensor (see Equation 4–24 in the Theory Guide).

selects the standard - model, described in Standard k-ε Model in the Theory Guide and Setting Up the k-ε Model.

selects the RNG - model, described in RNG k-ε Model. in the Theory Guide and Setting Up the k-ε Model.

selects the realizable - model, described in Realizable k-ε Model in the Theory Guide and Setting Up the k-ε Model.

specifies whether or not the low-Reynolds-number RNG modifications to turbulent viscosity should be included. By default, this option is turned off. It is likely to have an effect only when the near-wall regions in the domain are well resolved in terms of mesh density. See Differential Viscosity Modification for details.

specifies whether or not the RNG modification to turbulent viscosity for swirling flows should be included. This option is available only in 3D and 2D axisymmetric swirl solvers, and it can yield improved predictions when solving flows with significant swirl. See Swirl Modification for details.

selects the standard - model, described in Standard k-ω Model in the Theory Guide and Setting Up the k-ω Model.

selects the generalized - model, described in Generalized k-ω  (GEKO) Model in the Theory Guide and Setting up the Generalized k-ω (GEKO) Model.

selects the baseline (BSL) - model, described in Baseline (BSL) k-ω Model in the Theory Guide and Setting Up the k-ω Model.

selects the shear-stress transport (SST) - model, described in Shear-Stress Transport (SST) k-ω Model in the Theory Guide and Setting Up the k-ω Model.

specifies whether corrections that improve the accuracy in predicting low Reynolds number flows should be included. This option is available only for the - models and the stress-omega RSM model. See Low-Re Corrections for details.

specifies whether corrections that improve the accuracy in predicting free shear flows should be included. This option is available only for the standard - model and the stress-omega RSM model. See Shear Flow Corrections for details.

when enabled allows you to specify the Geometric Roughness Height as a constant value.

enables the linear pressure-strain model. See Linear Pressure-Strain Model in the Theory Guide for details.

enables the quadratic pressure-strain model for superior performance in a range of basic shear flows, including plane strain, rotating plane shear, and axisymmetric expansion/contraction. See Quadratic Pressure-Strain Model in the Theory Guide for details. Note that this option cannot be used with the Wall Reflection Effects option or the Enhanced Wall Treatment.

enables a stress-transport model that is based on the omega equations and LRR model [173]. This model is ideal for modeling flows over curved surfaces and swirling flows. See Stress-Omega Model in the Theory Guide for details.

enables a linear model for the pressure-strain term like the Stress-Omega model, but solves the scale equation from the baseline (BSL) - model, and thus removes the free-stream sensitivity observed with the Stress-Omega model. Like the Stress-Omega model, it is recommended for modeling flows over curved surfaces and swirling flows. See Stress-BSL Model in the Theory Guide for details.

enables the explicit setting of boundary conditions for the Reynolds stresses near the walls, using the values computed with Equation 4–260 in the Theory Guide. See Solving the k Equation to Obtain Wall Boundary Conditions for details. This option is on by default.

enables the calculation of the component of the pressure strain term responsible for the redistribution of normal stresses near the wall. See Including the Wall Reflection Term for details. Note that this option is not available if you have enabled the Quadratic Pressure-Strain Model.

enables the Spalart-Allmaras RANS model. See Detached Eddy Simulation (DES) in the Theory Guide for details.

enables the Realizable - RANS model. See Detached Eddy Simulation (DES) in the Theory Guide for details.

enables the SST - RANS Model. See Detached Eddy Simulation (DES) in the Theory Guide for details.

is useful for RANS meshes with high aspect ratios in the boundary layer. This option preserves the RANS model throughout the boundary layer. (See Delayed Detached Eddy Simulation (DDES) for details.)

selects the Smagorinsky-Lilly subgrid-scale model described in Subgrid-Scale Models in the Theory Guide.

selects the Wall-Adapting local Eddy-Viscosity model described in Wall-Adapting Local Eddy-Viscosity (WALE) Model in the Theory Guide.

selects the algebraic Wall-Modeled LES model described in Algebraic Wall-Modeled LES Model (WMLES) in the Theory Guide.

selects the algebraic Wall-Modeled LES - model described in Algebraic WMLES S-Omega Model Formulation in the Theory Guide.

selects the dynamic kinetic energy subgrid-scale model described in Dynamic Kinetic Energy Subgrid-Scale Model in the Theory Guide.

enables the dynamic stress model. It is available for selection when the Smagorinsky-Lilly is selected, and is enabled (and cannot be disabled) when the Kinetic-Energy Transport is selected.

enables the dynamic energy flux model. It is available when the LES model option Dynamic Stress is enabled.

enables the dynamic computation of turbulent Sc ( in Equation 8–5 in the Theory Guide). See Definition of the Mixture Fraction in the Theory Guide for details. It is available when the LES model option Dynamic Stress is enabled.

enables the dynamic mixture fraction variance model. It is available when Non-Premixed Combustion or Partially Premixed Combustion is selected in the Species Model Dialog Box. See The Non-Premixed Model for LES in the Theory Guide for details.

enables the use of standard wall functions (described in Standard Wall Functions in the Theory Guide).

enables the use of scalable wall functions (described in Scalable Wall Functions in the Theory Guide).

enables the use of non-equilibrium wall functions (described in Non-Equilibrium Wall Functions in the Theory Guide).

enables the use of the enhanced wall treatment (described in Enhanced Wall Treatment ε-Equation (EWT-ε) in the Theory Guide). Note that this option will not appear if you have enabled the Quadratic Pressure-Strain Model under Reynolds-Stress Options.

enables the use of the Menter-Lechner near-wall treatment (described in Menter-Lechner ε-Equation (ML-ε) in the Theory Guide). Note that this option is only available when k-epsilon is selected for the Model.

enables you to hook a user-defined function, used to define the Law of the Wall. See User-Defined Wall Functions in the Theory Guide for more information.

enables the effect of pressure gradient.

enables thermal effects in the calculation. This option appears only if the energy equation is enabled.

(if enabled) includes the viscous dissipation terms in the energy equation. This option is recommended when you are solving a compressible flow. Note that this option is always turned on when one of the density-based solvers is used; you will not be able to turn it off.

includes slip boundary conditions for velocity and temperature for modeling fluid flow at very low pressures as in semiconductor fabrication devices. See Slip Boundary Formulation for Low-Pressure Gas Systems in the Theory Guide. This option is available only for laminar flows.

enables the inclusion of buoyancy effects. See Including Buoyancy Effects on Turbulence for details. Only available for non-isothermal flow and when a nonzero gravitational acceleration has been specified in the Operating Conditions Dialog Box.

when enabled, modifies the turbulence production term to sensitize the standard eddy-viscosity models to the effects of streamline curvature and system rotation. This is available for the Spalart-Allmaras, k-epsilon, k-omega, Transition SST, Scale-Adaptive Simulation, and Detached Eddy Simulation with the SST k-omega model.

when enabled, accounts for secondary flows found in rectangular channels, pipes of non-circular cross-section, and wing-body-junction type geometries in the plane normal to the main flow direction into the corner along the bisector.

when enabled, can improve the prediction of free shear layers at high Mach numbers. This is available when the compressible form of the ideal gas law or the real-gas model is activated for k-epsilon, k-omega, Transition k-kl-omega, Reynolds Stress, Scale-Adaptive Simulation, and Detached Eddy Simulation with the Realizable k-epsilon model. For details, see Model Enhancements.

includes the effect of turbulent drift velocity when using the Mixture model. See Modeling Turbulence. Note that this option is only available when using the Mixture model with Slip Velocity enabled in the Multiphase Model dialog box. See Including Mixture Drift Force.

when enabled, the Kato-Launder modification for the production term limits the production term in the turbulence equation. For details see, Production Limiters for Two-Equation Models in the Fluent Theory Guide.

when enabled, limits the production term in the turbulence equation. For details, see Production Limiters for Two-Equation Models in the Fluent Theory Guide.

selects the transition model. You can enable the gamma-transport-eqn model (also known as the Intermittency Transition model). For details, see Intermittency Transition Model in the Theory Guide.

includes the effects of crossflow instability. For details, see Transport Equations for the Intermittency Transition Model in the Theory Guide.

specifies the (default) mixture turbulence model.

specifies the dispersed turbulence model.

specifies the calculation of a set of turbulence equations for each phase.

Selects the wall distance free version of the GEKO model.

Specifies - parameter to optimize flow separation from smooth surfaces.

Specifies - parameter to optimize flow in non-equilibrium near wall regions (such as heat transfer or ).

Specifies - parameter to optimize strength of mixing in free shear flows.

Specifies - parameter to optimize free shear layer mixing (optimize free jets independent of mixing layer).

Specifies the blending function, , which deactivates these parameters inside boundary layers.

(only for the Spalart-Allmaras model) is the constant in Equation 4–19 in the Theory Guide.

(only for the Spalart-Allmaras model) is the constant in Equation 4–15 in the Theory Guide.

(only for the Spalart-Allmaras model) is the constant in Equation 4–17 in the Theory Guide.

(only for the Spalart-Allmaras model) is the constant in Equation 4–28 in the Theory Guide.

(* only for the Spalart-Allmaras model) is the constant in Equation 4–27 in the Theory Guide.

(only for the Spalart-Allmaras model when the Strain/Vorticity-Based Production option is used) is the constant in Equation 4–24 in the Theory Guide.

(only for the standard or RNG - model, the RSM, or the -- Transition model) is the constant that is used to compute .

(only for the standard or RNG - model or the RSM) is the constant used in the transport equation for .

(only for the standard, RNG, or realizable - model or the RSM) is the constant used in the transport equation for .

(only for the dispersed or per-phase - multiphase models) is the constant in Equation 14–412 in the Theory Guide.

(only for the -- Transition model) is the constant in the definition of the effective length,

(only for the -- Transition model) is the constant used in the definition of , where represents the averaged effect of the breakdown of streamwise fluctuations into turbulence during bypass transition

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(**only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the -- Transition model) is the constant

(only for the standard - model and the -- Transition model) is the effective "Prandtl" number for the transport of the specific dissipation rate, .

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the Transition SST model)

(only for the SDES or SBES model) is a constant that serves the same purpose as in the DDES turbulence model (see Equation 4–284 in the Theory Guide).

(only for the SDES or SBES model) is , as described in Shielded Detached Eddy Simulation (SDES) in the Theory Guide.

(only for the WALE subgrid-scale model of the LES or SBES model) is , as described in Wall-Adapting Local Eddy-Viscosity (WALE) Model in the Theory Guide.

(only for the GEKO model) is , as described in Generalized k-ω  (GEKO) Model in the Fluent Theory Guide.

(only for the GEKO model) is , as described in Generalized k-ω  (GEKO) Model in the Fluent Theory Guide.

(only for the GEKO model) is , as described in Generalized k-ω  (GEKO) Model in the Fluent Theory Guide.

(only for the GEKO model) is , as described in Generalized k-ω  (GEKO) Model in the Fluent Theory Guide.

(only for the GEKO model) is , as described in Generalized k-ω  (GEKO) Model in the Fluent Theory Guide.

sets the value of in Equation 4–46 in the Theory Guide. This item appears for the RNG - model when the Swirl Dominated Flow option is turned on.

(only for the standard, BSL, or SST - model, and the Transition SST model) is the constant in Equation 4–75 in the Theory Guide.

(only for the standard, BSL, or SST - model, and the Transition SST model) is the constant in Equation 4–83 in the Theory Guide.

(only for the standard, BSL, or SST - model with the Low-Re Corrections option enabled) is the constant in Equation 4–83 in the Theory Guide.

(only for the standard, BSL, or SST - model, and the Transition SST model) is the constant in Equation 4–88 in the Theory Guide.

(only for the standard - model) is the constant in Equation 4–96 in the Theory Guide.

(only for the standard, BSL, or SST - model) is the constant in Equation 4–88 in the Theory Guide.

(only for the standard, BSL, or SST - model with the Low-Re Corrections option enabled) is the constant in Equation 4–75 in the Theory Guide.

(only for the standard, BSL, or SST - model with the Low-Re Corrections option enabled) is the constant in Equation 4–83 in the Theory Guide.

(only for the standard, BSL, or SST - model when the Compressibility Effects option is enabled) is the constant in Equation 4–87 in the Theory Guide.

(only for the standard, BSL, or SST - model when the Compressibility Effects option is enabled) is the constant in Equation 4–97 in the Theory Guide.

(only for the SST - model, and the Transition SST model) is the constant in Equation 4–118 in the Theory Guide.

(only for the BSL or SST - model, and the Transition SST model) is the constant in Model Constants in the Theory Guide.

(only for the BSL or SST - model, and the Transition SST model) is the constant in Model Constants in the Theory Guide.

is a constant that depends on the turbulence model. For LES, it is the Smagorinsky constant in Equation 4–307 in the Theory Guide. For SAS, it is the high wave number damping coefficient in Equation 4–270 in the Theory Guide.

(only for RSM) is the constant in Equation 4–231 in the Theory Guide.

(only for RSM) is the constant in Equation 4–232 in the Theory Guide.

(only for RSM) is the constant in Equation 4–233 in the Theory Guide.

(only for RSM) is the constant in Equation 4–233 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for RSM with the Quadratic Pressure-Strain Model) is the constant in Equation 4–242 in the Theory Guide.

(only for the Spalart-Allmaras model) is the constant in Equation 4–15 in the Theory Guide.

(only for the standard or realizable - model, the standard - model, the -- Transition model, or the RSM) is the effective "Prandtl" number for transport of turbulence kinetic energy . This effective Prandtl number defines the ratio of the momentum diffusivity to the diffusivity of turbulence kinetic energy via turbulent transport.

(only for the BSL or SST - model, and the Transition SST model) is the effective "Prandtl" number for the transport of turbulence kinetic energy, , inside the near-wall region. See Modeling the Turbulent Viscosity in the Theory Guide for details.

(only for the BSL or SST - model, and the Transition SST model) is the effective "Prandtl" number for the transport of turbulence kinetic energy, , outside the near-wall region. See Modeling the Turbulent Viscosity in the Theory Guide for details.

is the effective "Prandtl" number for transport of the turbulent dissipation rate, , for the standard or realizable - model or the RSM. This effective Prandtl number defines the ratio of the momentum diffusivity to the diffusivity of turbulence dissipation via turbulent transport.

(only for the BSL or SST - model, and the Transition SST model) is the effective "Prandtl" number for the transport of the specific dissipation rate, , inside the near-wall region. See Modeling the Turbulent Viscosity in the Theory Guide for details.

(only for the BSL or SST - model, and the Transition SST model) is the effective "Prandtl" number for the transport of the specific dissipation rate, , outside the near-wall region. See Modeling the Turbulent Viscosity in the Theory Guide for details.

(only for the - multiphase models) is the effective "Prandtl" number for the dispersed phase, . See Turbulence Models in the Theory Guide for details.

(for any turbulence model except the RNG - model) is the turbulent Prandtl number for energy, , in Equation 4–250 in the Theory Guide. (This item will not appear for the LES model if the Dynamic Energy Flux option has been enabled, or for premixed or partially premixed combustion models.) For non-premixed and partially premixed combustion, the energy Prandtl Number is set equal to the PDF Schmidt Number.

(for all turbulence models) is the turbulent Prandtl number at the wall, in Equation 4–343 in the Theory Guide. (This item will not appear for adiabatic premixed combustion or partially premixed combustion models.)

(for turbulent species transport calculations using any turbulence model except the RNG - model) is the turbulent Schmidt number, , in Equation 7–4 in the Theory Guide. (This item will not appear for the LES model if the Dynamic Scalar Flux option has been enabled.)

(for non-premixed or partially premixed combustion calculations using any turbulence model) is the model constant in Equation 8–5 in the Theory Guide.

This coefficient is used by the Production Limiter. For details, see Equation 4–436 in the Fluent Theory Guide.

appears for Spalart Allmaras, -, -, DES, SDES with BSL / SST models, and SBES with BSL / SST. You can select the user-defined functions for turbulent viscosity in the drop-down list.

contains a list of relevant Prandtl and Schmidt numbers for which you can select user-defined functions.

allows you to select a user-defined function for the subgrid-scale turbulent viscosity for the LES model.

allows you to apply SAS in combination with the following -based URANS models: the Standard or BSL - model, the Transition SST model, and the -based Reynolds stress models. For additional information, see Setting Up Scale-Adaptive Simulation (SAS) Modeling.

allows you to apply DES in combination with the BSL - model and Transition SST model. For additional information, see Detached Eddy Simulation (DES).

allows you to apply SBES or SDES in combination with the BSL - model, SST - model, and Transition SST model. See Stress-Blended Eddy Simulation (SBES) and Shielded Detached Eddy Simulation (SDES) in the Theory Guide for details.

specifies that the hybrid RANS-LES model used is either SDES (Shielded DES model), SBES (Stress-Blended Eddy Simulation model), or SBES with User-Defined Function. See Including the SDES or SBES Model with RANS Models for details.

contains options for the subgrid-scale model used in the LES region of your Stress-Blended Eddy Simulation. This portion of the dialog box will appear only if SBES or SBES with User-Defined Function is selected as the Hybrid Model.

Sets the number of time steps between updates of the - part of the SBES model.

disables the calculation of radiation heat transfer.

enables the Rosseland radiation model.

enables the P-1 radiation model.

enables the discrete transfer radiation model (DTRM).

enables the surface-to-surface (S2S) radiation model.

enables the discrete ordinates (DO) radiation model.

enables the Monte Carlo (MC) radiation model.

controls the frequency with which the radiation terms are updated as the continuous phase solution proceeds. The Energy Iterations per Radiation Iteration parameter is set to 10 by default. This implies that the radiation calculation is performed once every 10 iterations of the solution process. Increasing the number can speed the calculation process, but may slow overall convergence.

controls the maximum number of iterations of the radiation calculation during each global iteration. The default setting of 5 means that the radiosity will be updated up to 5 times. The actual number of iterations will be less if the residual convergence criterion is exceeded at any point during these iterations.

This item appears only when Discrete Transfer or Surface to Surface is selected as the Model.

determines when the radiation intensity update is converged. It is defined as the maximum normalized change in the surface intensity from one radiation iteration to the next (see Equation 16–4).

This item appears only when Discrete Transfer or Surface to Surface is selected as the Model.

determines the number of photon histories to be tracked for the Monte Carlo simulation. Too small of a number will produce "speckled" results. Increasing the target number of histories produces a smoother and more accurate solution, but at the expense of higher computation effort.

This item appears only when Monte Carlo is selected.

opens the View Factors and Clustering Dialog Box, in which you can set parameters related to surface clusters and view factors.

allows you to compute the view factors, write the computed view factors to a file, and read the file into Ansys Fluent. When you click Compute/Write/Read..., The Select File Dialog Box will open so that you can specify a name for the file where Ansys Fluent should save the view factors after computing them, and indicate whether the files should be saved in binary format.

opens The Select File Dialog Box, in which you can specify the file from which Ansys Fluent should read view factors.

define the number of control angles used to discretize each octant of the angular space (see Figure 5.3: Angular Coordinate System in the Theory Guide).

are used to control the pixelation that accounts for any control volume overhang (see Figure 5.7: Pixelation of Control Angle in the Theory Guide and the figures and discussion preceding it).

Coarsens the radiation mesh used by the MC model. See Setting Up the MC Model for more information about the use of this parameter.

specifies the number of bands for the non-gray radiation.

contains inputs that define each wavelength band. (It appears only when the Number of Bands is nonzero.) For each band, you can specify a Name, as well as the Start and End wavelength of the band in m. Note that the wavelength bands are specified for vacuum (). Ansys Fluent will automatically account for the refractive index in setting band limits for media with different from unity.

indicates which model is used to calculate radiation effects.

are the components of the sun direction vector.

enables the use of direction vector computed from the solar calculator.

is the amount of energy per unit area due to direct solar irradiation.

is the amount of energy per unit area due to diffuse solar irradiation.

is the fraction of incident solar radiation in the visible part of the solar radiation spectrum. The spectral fraction is not used for DO irradiation since the DO implementation is intended only for a single band. This parameter is available only for Solar Ray Tracing.

specifies the number of time steps that will direct the Ansys Fluent solver to update the solar load data for the specified flow-time intervals in the unsteady solution process.

gives you a choice of forming clusters either manually or automatically.

(available only when the Manual option is enabled) allows you to set the faces per surface cluster (FPSC) value for walls and inlet and outlet boundaries.

(available only when the Automatic option is enabled) allows you to assign different faces per surface cluster (FPSC) values to the walls automatically, based on the distance of the walls from and the FPSC values of the walls that are defined as critical.

specifies how surfaces are defined for the calculation of view factors. See Selecting the Basis for Computing View Factors for more information.

specifies the geometric orientation of surface pairs with respect to each other when using the hemicube method.

specifies the method for computing the view factors. See Selecting the Method for Computing View Factors for information about choosing a method.

contains settings related to the hemicube and ray tracing methods for computing the view factors. All of these inputs are available when Hemicube is selected under Method, whereas only Resolution is available when Ray Tracing is selected. See Selecting the Method for Computing View Factors for information about setting the method parameters.

allows you to define which boundary zones participate in the view factor calculation. See Specifying Boundary Zone Participation for more information.

displays the maximum of the distances between the centroids of critical and all other wall, inlet, and exit zones when the Compute button is clicked. This field is not editable. This is only available when using the Automatic option for clustering.

calculates the distances between the centroids of critical zones and all the other wall, inlet, and exit zones and displays the maximum value in the To All Other Zones field and the To Participating Zones text-entry box. It requires the definition of the critical zone.

displays the maximum of the distances between the centroids of critical and all other wall, inlet, and exit zones when the Compute button is clicked. Unlike the To All Other Zones field, you can edit this text-entry box. You can specify the maximum distance allowed between the centroids of critical zones and all other wall, inlet, or exit zones that participate in the view factor calculation; when you click the Apply button, all of the zones will be marked as either participating or not participating, according to the distance criteria you specified. Note that this field is only available when using the Automatic option for clustering.

marks all of the wall, inlet, and exit zones as either participating or not participating in the view factor calculation, depending on whether the distance from their centroid to the centroid of a critical zone is equal to or less than value entered for To Participating Zones. The Participating Boundary Zones and Non-Participating Boundary Zones lists will be updated accordingly.

specifies the longitude of the desired location in degrees. Values may range from to , where negative values indicate the Western hemisphere and positive values indicate the Eastern hemisphere.

specifies the latitude of the desired location in degrees. Values may range from (South pole) to (North pole) with defined as the equator.

specifies the local time zone of the desired location in hours relative to Greenwich Mean Time (+-GMT). This integer value can range from to .

contains parameters to specify day and month.

contains parameters to specify hour and minutes.

enables theoretically maximum solar irradiation method.

enables fair weather condition solar irradiation method.

allows you to enable or disable the Dual Cell heat exchanger model. When this option is enabled, the corresponding Define... button opens the Dual Cell Heat Exchanger Dialog Box.

allows you to enable or disable the Ungrouped Macro heat exchanger model. When this option is enabled, the corresponding Define... button opens the Ungrouped Macro Heat Exchanger Dialog Box.

allows you to enable or disable the Macro heat exchanger group model. When this option is enabled, the corresponding Define... button opens the Macro Heat Exchanger Group Dialog Box.

specifies the number of passes for the heat exchanger.

allows you to specify the fluid of the primary fluid zone for the heat exchanger.

allows you to specify the fluid for the auxiliary fluid zone, per pass.

allows you to specify how the heat rejection in the heat exchanger is computed.

allows you to specify the heat rejection desired from the heat exchanger (available only when the Fixed Heat Rejection option is enabled).

allows Ansys Fluent to change the temperature of the specified inlet zone in order to match the targeted heat rejection (available only when the Fixed Heat Rejection option is enabled).

controls convergence (available only when the Fixed Heat Rejection option is enabled).

controls divergence (available only when the Fixed Heat Rejection option is enabled).

allows you to choose between using raw performance data or NTU performance data.

contains parameters concerning the heat exchanger’s performance data.

allows you to specify a value for the Core Frontal Area for the primary fluid, or to compute the value from a surface zone using the Compute From drop-down list.

allows you to specify a value for the Core Frontal Area for the auxiliary fluid, or to compute the value from a surface zone using the Compute From drop-down list.

specifies, by default, the mass-weighted average for the temperature of the outlet of Pass 1 to the inlet of Pass 2. Similarly, the mass-weighted-average temperature of the outlet of Pass 2 will be applied at the inlet zone of Pass 3, and so on. (Available only when multiple passes are specified in the Fluid Zones tab.)

allows you to choose one of the following settings:

allows you to specify either the ntu-model or the simple-effectiveness-model for heat transfer. See Choosing a Heat Exchanger Model for information on the differences between these models.

contains a drop-down list of all available core porosity models.

opens the Core Porosity Model Dialog Box.

contains the parameters for heat transfer.

sets the width of the heat exchanger core. The Width is measured in the pass-to-pass direction.

sets the height of the heat exchanger core. The Height is measured in the auxiliary fluid inlet direction.

sets the depth of the heat exchanger core.

specifies the number of passes for the macro grid. (See Figure 16.76: 1x4x3 Macros.)

specify the number of macro rows and columns per pass in the macro grid. (See Figure 16.76: 1x4x3 Macros.)

displays the macro grid. (This button becomes available after you click Apply.) The path of the auxiliary fluid is color-coded in the display: macro is red and macro is blue.

toggles between displaying and not displaying the mesh when the macro mesh is displayed (using the View Passes button). The Mesh Display Dialog Box opens when Draw Mesh is selected.

updates the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction from the plane tool orientation. The Width, Height, and Depth will also be updated. See Using the Plane Tool for information about using the plane tool.

Open the Plane Surface Dialog Box to make the plane tool appear.

specifies the direction in which the auxiliary fluid enters the heat exchanger. See Figure 16.76: 1x4x3 Macros.

specifies the direction in which the auxiliary fluid moves at the end of each pass through the heat exchanger. See Figure 16.76: 1x4x3 Macros.

contains options for specifying auxiliary fluid properties.

specifies the value of in Equation 6–17 in the Theory Guide. This value is specified only if constant-specific-heat is selected.

allows you to specify a user-defined function for the auxiliary fluid enthalpy (see Equation 6–17 in the Theory Guide). This option is available only when user-defined-enthalpy is selected.

sets the flow rate of the auxiliary fluid ( in Equation 6–16 in the Theory Guide).

sets the total heat rejection ( in Equation 6–15 in the Theory Guide). This value is specified only if Fixed Heat Rejection is selected.

sets an initial guess for the inlet temperature ( in Equation 6–11 and Equation 6–16 in the Theory Guide). This value is specified only if Fixed Heat Rejection is selected.

sets the auxiliary fluid initial temperature ( in Equation 6–11 and Equation 6–16 in the Theory Guide). This value is specified only if Fixed Inlet Temperature is selected in the Model Data tab.

sets the auxiliary fluid inlet pressure. This value is specified only if user-defined-enthalpy is selected.

specifies the value of in Equation 6–20 in the Theory Guide. This value is specified only if user-defined-enthalpy is selected.

specifies the value of in Equation 6–21 in the Theory Guide. This value is specified only if user-defined-enthalpy is selected.

sets the value of in Equation 6–2 in the Theory Guide.

sets the value of in Equation 6–2 in the Theory Guide.

sets the value of in Equation 6–2 in the Theory Guide.

sets the value of in Equation 6–2 in the Theory Guide.

sets the value of in Equation 6–2 in the Theory Guide.

sets the value of in Equation 6–3 in the Theory Guide.

sets the value of in Equation 6–3 in the Theory Guide.

gives you a choice of gas flow direction.

allows you to define the upstream and downstream connections.

allows you to select either the simple-effectiveness-model or the ntu-model. See Choosing a Heat Exchanger Model for information on the differences between these models.

specifies whether default values are chosen for the core porosity model.

opens the Core Porosity Model Dialog Box for the definition of a new core porosity model.

contains the parameters for heat transfer.

specifies the width, height and the depth of the heat exchanger.

specifies the number of passes.

specifies the number of rows per pass.

specifies the number of columns per pass.

displays the macro grid. (This button becomes available after you click Set.) The path of the auxiliary fluid is color-coded in the display: macro is red and macro is blue.

toggles between displaying and not displaying the mesh when the macro mesh is displayed (using the View Passes button). The Mesh Display Dialog Box opens when Draw Mesh is selected.

updates the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction from the plane tool orientation. The Width, Height, and Depth will also be updated. See Using the Plane Tool for information about using the plane tool.

specifies the direction in which the auxiliary fluid enters the heat exchanger. See Figure 16.76: 1x4x3 Macros.

specifies the direction in which the auxiliary fluid moves at the end of each pass through the heat exchanger. See Figure 16.76: 1x4x3 Macros.

specifies the method to specify the auxiliary fluid properties. You can choose from constant-specific-heat and user-defined-enthalpy.

sets the specific heat of the auxiliary fluid ( in Equation 6–16 you choose constant-specific-heat.

sets the enthalpy as defined by the user-defined function selected from the drop-down list.

sets the flow rate of the auxiliary fluid ( in Equation 6–16 in the Theory Guide).

sets an initial guess for the inlet temperature ( in Equation 6–11 and Equation 6–16 in the Theory Guide). This value is specified only if Fixed Heat Rejection is selected.

sets the auxiliary fluid inlet pressure. This value is specified only if user-defined-enthalpy is selected.

specifies the value of in Equation 6–20 in the Theory Guide.

specifies the value of in Equation 6–21 in the Theory Guide. This value is specified only if user-defined-enthalpy is selected.

specifies the supplementary fluid flow rate as constant, polynomial or piecewise-linear.

specifies the supplementary fluid temperature as constant, polynomial or piecewise-linear.

specifies the supplementary fluid quality.

disables species calculations.

enables the calculation of multi-species transport (either non-reacting or reacting, depending on the selection for Reactions). See Modeling Species Transport and Finite-Rate Chemistry for details.

enables the calculation of turbulent reacting flow using the non-premixed combustion model. See Modeling Non-Premixed Combustion for details. This option is available only for turbulent flows using the pressure-based solver.

enables the premixed turbulent combustion model. See Modeling Premixed Combustion for details. This option is available only for turbulent flows using the pressure-based solver.

enables the partially premixed turbulent combustion model. See Modeling Partially Premixed Combustion for details. This option is available only for turbulent flows using the pressure-based solver.

enables the composition PDF transport model. See Modeling a Composition PDF Transport Problem for details. This option is available only for turbulent flows using the pressure-based solver.

enables the calculation of reacting flow using the finite-rate formulation. See Volumetric Reactions for details.

enables the calculation of wall surface reactions. See Wall Surface Reactions and Chemical Vapor Deposition for details. This item will appear only if Volumetric is enabled.

enables the calculation of particle reactions. See Particle Reactions for details. This item will appear only if Volumetric is enabled.

enables the calculation of electrochemical reactions. See Electrochemical Reactions for details. This item will appear only if Volumetric is enabled.

is a command button that opens the Integration Parameters Dialog Box. This button appears for the species transport model, when Volumetric is enabled under Reactions and Stiff Chemistry Solver is enabled under Options or when Eddy-Dissipation Concept is enabled under Turbulence-Chemistry Interaction.

(if enabled) includes the heat release due to surface reactions in the energy equation. You must remember to set appropriate formation enthalpies (standard state enthalpies) if you enable this option.

when enabled, includes the effect of surface mass transfer in the continuity equation. This option is always enabled when the density-based solver is used. With the density-based solver, the effect of surface mass transfer in the continuity equation is always included.

is a numerical factor that controls the robustness and the convergence speed. This value ranges between 0 and 1, where 0 is the most robust, but results in the slowest convergence. The default value for the Aggressiveness Factor is 0.5. This parameter appears only when the pressure-based solver is used.

enables efficient integration of stiff chemical kinetics. This item appears only when Finite-Rate/No TCI or Eddy-Dissipation Concept is selected in the Turbulence-Chemistry Interaction group box. See Solution of Stiff Chemistry Systems for details.

enables the integration of chemical kinetics using the Ansys CHEMKIN-CFD Solver, designed for large, stiff chemistry mechanisms. This item appears only when Finite-Rate/No TCI or Eddy-Dissipation Concept is selected in the Turbulence-Chemistry Interaction group box.

enables efficient modeling of chemical kinetics effects based only on equilibrium calculation and assumptions about characteristic timescales for approaching equilibrium. This item is not available for the Eddy Dissipation Concept TCI option. (See The Relaxation to Chemical Equilibrium Model for details.

makes explicit use of chemistry source terms in the species transport equations, without a stiff-chemistry solver (not recommended for stiff or complex chemistry).

(if enabled) includes the effect of enthalpy transport due to species diffusion in the energy equation.

enables the full multicomponent diffusion model. See Full Multicomponent Diffusion in the Fluent Theory Guide for details.

enables the thermal diffusion model. See Thermal Diffusion Coefficients in the Fluent Theory Guide for details.

is used to model liquid reactions. When the Liquid Micro-Mixing model is invoked, Ansys Fluent uses the volume-weighted-mixing-law formula to calculate the density.

(if enabled) includes the ion species migration term in the species transport equation. This item appears only when Electrochemical reactions are enabled.

enables the modeling of laminar flames. This application is typically used as an LES combustion model for turbulent premixed and partially-premixed flames.

enables the calculation of the multi-mode energy equation. This option is available when the composition PDF transport model is selected.

contains a drop-down list of available mixture materials. When you first enable the Species Transport model, you can choose from all of the mixture materials defined in the database, or you can choose a "template" and define your own material. (Click View... to open the Fluent Database Materials Dialog Box and check the properties of the mixture material selected in the list.) See Enabling Species Transport and Reactions and Choosing the Mixture Material for details.

When you use the Non-Premixed Combustion or Partially Premixed Combustion model, this list will be inactive. The mixture material for a non-premixed or partially premixed combustion calculation will be determined from the content of the PDF file generated in Ansys Fluent using the PDF Options parameters.

specifies the number of gas-phase species in the selected Mixture Material. This is an informational display only; you cannot edit this value.

specifies the number of solid species defined in the selected Mixture Material. This is an informational display only; you cannot edit this value. (This list will appear only for Species Transport models involving Wall Surface reactions.)

specifies the number of site species defined in the selected Mixture Material. This is an informational display only; you cannot edit this value. (This list will appear only for Species Transport models involving Wall Surface reactions.)

computes only the Arrhenius rate (see Equation 7–21 in the Theory Guide) and neglects turbulence-chemistry interaction.

(for turbulent flows) computes both the Arrhenius rate and the mixing rate and uses the smaller of the two.

(for turbulent flows) computes only the mixing rate (see Equation 7–39 and Equation 7–40 in the Theory Guide).

(for turbulent flows) models turbulence-chemistry interaction with detailed chemical mechanisms (see Equation 7–39 and Equation 7–40 in the Theory Guide).

opens the Coal Calculator Dialog Box.

opens the Water Chemistry and Corrosion Mechanism dialog box. This item is available only for the Species Transport model with electrochemical reactions. See Procedure for Setting Corrosion Simulations using the Water Corrosion Pre Tool for additional information on using the Water Chemistry and Corrosion Mechanism dialog box.

opens the Select Boundary Species dialog box (see Figure 19.3: The Select Boundary Species Dialog Box).

opens the Select Residual Monitored Species dialog box (see Figure 19.4: The Select Residual Monitored Species).

(Eddy-Dissipation Concept only) contains the following submodels:

(steady-state only) specifies how often Ansys Fluent will update the chemistry during the calculation. Increasing the number can reduce the computational expense of the chemistry calculations. This option is not available when the None - Direct Source option is selected for Chemistry Solver.

(steady-state only) is a numerical factor that controls the robustness and the convergence speed. This value ranges between 0 and 1, where 0 is the most robust, but results in the slowest convergence. The default value for the Aggressiveness Factor is 0.5. This option is available only when Stiff Chemistry Solver or CHEMKIN CFD Solver is selected for Chemistry Solver.

is the threshold for cell temperature below which the chemistry reaction rate in the cell will be set to zero. This may improve the computational time without sacrificing accuracy. The default value is 200 K. This option is available only when Stiff Chemistry Solver or CHEMKIN CFD Solver is selected for Chemistry Solver.

specifies the value of in Equation 7–44 in the Theory Guide. This item appears only for the Constant Coefficients EDC model.

specifies the value of in Equation 7–45 in the Theory Guide. This item appears only for the Constant Coefficients EDC model.

(Partially Stirred Reactor EDC model only) is a group box where you can select how in Equation 7–50 in the Fluent Theory Guide is computed:

allows you to select the efficiency function. You can choose between none, Colin (default), or Charlette. See The Thickened Flame Model in the Fluent Theory Guide for more information about these options.

by default are 8 grid points.

is the representative of the largest eddy sizes, in Equation 7–57 in the Fluent Theory Guide (typically, 1/4 to 1/2 of a characteristics dimension, such as a burner diameter, an inlet diameter, or a size of a bluff body). This item is available only for simulations with the Large Eddy Simulation (LES) turbulence model when Colin is used as the efficiency function.

includes the diffusion flux of species at inlet.

can be enabled to account for cases where substantial pressure changes occur in time and/or space when modeling a non-adiabatic system. See Specifying the Operating Pressure for the System for details.

is used to model liquid reactions. When the Liquid Micro-Mixing model is invoked, Ansys Fluent uses the volume-weighted-mixing-law formula to calculate the density.

is a drop-down list that allows you to choose between the shape of the assumed probability density function (PDF):

This control appears after you generate or read a PDF table into Ansys Fluent.

opens the Coal Calculator Dialog Box.

contains the parameters for the equilibrium chemistry model or the steady diffusion flamelet model.

contains a list of parameter settings.

contains options related to the steady flamelet model.

gives you the option of creating a Premixed Flamelet or a Diffusion Flamelet. This is available when the Flamelet Generated Manifold model is selected.