The Species Model dialog box allows you to set parameters related to the calculation of species transport and combustion. See Enabling Species Transport and Reactions and Choosing the Mixture Material, Manual Inputs for Wall Surface Reactions, User Inputs for Particle Surface Reactions, Using the Premixed Combustion Model, Using the Partially Premixed Combustion Model, and Steps for Using the Composition PDF Transport Model for details about the items below.

Controls
indicates which model, if any, is used to calculate species transport/combustion.
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.
contains options related to the modeling of reacting flow. (This section of the dialog box appears only when Species Transport or Composition PDF Transport is the specified Model.)
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 surface reactions. See Particle Surface 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.
contains additional options for wall surface reactions. This portion of the dialog box appears only if Wall Surface is enabled under Reactions.
(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.
(if enabled) includes the effect of surface mass transfer in the continuity equation.
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.
is a drop-down list in which you can select the solver for the chemically reactive flow simulation. This item appears only for Species Transport and Composition PDF Transport models involving Volumetric reactions.
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).
contains additional options for the Species Transport model and for the Composition PDF Transport. (This section will not appear in the dialog box for the other models.)
includes the diffusion flux of species at inlet.
(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 for details.
enables the thermal diffusion model. See Thermal Diffusion Coefficients 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 controls and information about the mixture being modeled. This section of the dialog box will not appear if Premixed Combustion is the selected under Model.
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.
displays the number of gas-phase species in the selected Mixture Material. This is an informational display only; you cannot edit this value.
displays 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.)
displays 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.)
indicates which model is to be used for turbulence-chemistry interaction when the Species Transport model with Volumetric reactions is used.
computes only the Arrhenius rate (see Equation 7–7 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 7–25 and Equation 7–26 in the Theory Guide).
(for turbulent flows) models turbulence-chemistry interaction with detailed chemical mechanisms (see Equation 7–25 and Equation 7–26 in the Theory Guide).
opens the Coal Calculator Dialog Box.
opens the Select Boundary Species dialog box (see Figure 14.3: The Select Boundary Species Dialog Box).
opens the Select Residual Monitored Species dialog box (see Figure 14.4: The Select Residual Monitored Species).
contains parameters related to the Laminar Finite-Rate or the Eddy-Dissipation Concept model. This section of the dialog box will appear when Laminar Finite-Rate or the Eddy-Dissipation Concept is selected for Turbulence-Chemistry Interaction.
specifies how often ANSYS Fluent will update the chemistry during the calculation. Increasing the number can reduce the computational expense of the chemistry calculations.
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.
specifies the value of in Equation 7–28 in
the Theory Guide.
specifies the value of in Equation 7–29 in the Theory Guide.
by default are 8 grid points.
contains options related for the non-premixed combustion model. (This section will appear only if Non-Premixed Combustion or Partially-Premixed Combustion is the selected Model.)
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.
tab contains the parameters to define problems using the chemistry model. See Setting Up the Equilibrium Chemistry Model for details.
enables the equilibrium chemistry model. See Setting Up the Equilibrium Chemistry Model for details.
enables the steady diffusion flamelet model. See The Diffusion Flamelet Models Theory in the Theory Guide for details.
enables the Eulerian unsteady diffusion flamelet model.
enables the diesel unsteady laminar flamelet model. See Using the Diesel Unsteady Laminar Flamelet Model for details.
enables the flamelet generated manifold (FGM) model. This is available when the Partially Premixed Combustion model is selected. See Partially Premixed Combustion in the Theory Guide for details.
enables adiabatic modeling options for the problem.
enables non-adiabatic modeling options for the problem. See Non-Adiabatic Extensions of the Non-Premixed Model in the Theory Guide for details.
opens the Coal Calculator Dialog Box.
contains the parameters for the equilibrium chemistry model or the steady diffusion flamelet model.
includes the secondary inlet stream in the model.
enables parameters to define fuel stream empirically. This option is available only with the full equilibrium chemistry model.
enables parameters to define secondary stream empirically. This option is available only with the full equilibrium chemistry model.
contains a list of parameter settings.
specifies the system operating pressure used to calculate the density using the ideal gas law. See Specifying the Operating Pressure for the System for details.
specifies the rich flammability limit for fuel stream when the equilibrium chemistry option is used. You will not set these if you have used the empirical definition option for fuel composition. See Enabling the Rich Flammability Limit (RFL) Option for details.
specifies the rich flammability limit for secondary stream when the equilibrium chemistry option is used. You will not set these if you have used the empirical definition option for fuel composition. See Enabling the Rich Flammability Limit (RFL) Option for details.
specifies the lower calorific value of fuel stream.
specifies the specific heat value of fuel stream.
specifies the molecular weight of the fuel stream.
specifies the lower calorific value of secondary stream.
specifies the specific heat value of secondary stream.
specifies the molecular weight of the secondary stream.
contains options related to the steady flamelet model.
enables the Import CHEMKIN Mechanism... button that opens the CHEMKIN Mechanism Import Dialog Box where you can import the CHEMKIN mechanism and thermodynamic data, to create a flamelet file. This option is available for the steady flamelet model. See Setting Up the Steady and Unsteady Diffusion Flamelet Models for details.
enables the Import Flamelet File... button that opens The Select File Dialog Box where you can select the existing flamelet in ANSYS Fluent. You can also set the file type parameters to import the existing flamelet in ANSYS Fluent. See Setting Up the Steady and Unsteady Diffusion Flamelet Models for details. This option is available for 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.
contains the toggle buttons for two flamelet file types.
enables the import of an ASCII format standard flamelet file.
enables the import of an ASCII format CFX-RIF flamelet file.
opens The Select File Dialog Box in which you can save the existing flamelet in ANSYS Fluent to use when running an existing case.
specifies a path for the thermodynamic database file to be read.
tab contains the list of boundary species and related parameters. This is available only for equilibrium chemistry model. See Defining the Stream Compositions for details.
contains the list of the species used in the problem.
specifies the fuel species.
specifies the oxidizing species.
specifies the secondary species.
allows you to specify the species you want to add or remove from the model. You can type the species chemical formula in the field below it.
adds the species in the model.
removes the species from the model.
prints a list of all species in the thermodynamic
database file (thermo.db) in the console
window.
specifies the temperature of different streams that you have defined.
is the temperature of the fuel inlet in the model.
is the temperature of the oxidizer inlet in the model.
is the temperature of the secondary stream inlet in the model.
allows you to define the unit of species concentration.
allows you to specify the species in terms of mass fraction.
allows you to specify the species in terms of mole fraction.
tab contains the parameters for exclusion and inclusion of equilibrium species. This is available only for equilibrium chemistry model. See Forcing the Exclusion and Inclusion of Equilibrium Species for details.
lists the species excluded from equilibrium calculation.
lists the slow-forming species that are zeroed in the initial flamelet profile.
allows you to add equilibrium species.
allows you to remove equilibrium species.
prints a list of all species in the thermodynamic database file in the console window.
allows you to adjust the controls for the flamelet solution. Note that the Create Flamelet option in the Chemistry tab must be selected for the Steady Diffusion Flamelet or Flamelet Generated Manifold models for these controls to be available.
sets the first time step for the solution.
increases the time step at subsequent times. Every time step after the first is multiplied by this value.
specifies the local error controls during numerical integration.
specifies the maximum absolute change in species fraction or temperature at any discrete mixture-fraction.
specifies the maximum total elapsed time for flamelet calculation. ANSYS Fluent will stop the flamelet calculation after the total elapsed time has exceeded this value.
tab allows you to adjust the controls for the flamelet solution. See Defining the Flamelet Controls for details.
consist of the controls for the flamelet solution.
Note: The parameters may vary slightly if you selected the Flamelet Generated Manifold model (see Flamelet Generated Manifold for those specific parameters).
specifies the number of mixture fraction grid points
distributed between the oxidizer () and the fuel (
).
specifies the maximum number of laminar flamelet profiles to be calculated.
is the scalar dissipation of the first flamelet in the library.
specifies the interval between scalar dissipation
values (in )
for which multiple flamelets will be calculated.
enables you to hook a user-defined function for scalar dissipation and mean mixture fraction (or progress variable) grid discretization
determines whether the equilibrium assumption is used to compute the progress variable (Equation 9–2 in the Fluent Theory Guide). By default, this option is selected. If you turn off this option, ANSYS Fluent will compute the progress variable using the solution of flamelet generated with initial scalar dissipation as a denominator in Equation 9–2 in the Fluent Theory Guide.
consist of the controls for the unsteady flamelet solution.
specifies the number of mixture fraction grid points
distributed between the oxidizer () and the fuel (
).
is the limit at which the unsteady flamelet model temporally convects and diffuses a marker probability equation through a steady-state ANSYS Fluent flow-field.
is where flamelets extinguish at large scalar dissipation (mixing) rates.
is the number at which ANSYS Fluent automatically selects the time step for the probability equation based on this convective Courant number.
specifies the number of unsteady laminar flamelets that ANSYS Fluent will automatically generate during the simulation.
begins the laminar flamelet calculation.
opens the Flamelet 3D Surfaces Dialog Box from which you can display 2D plots and 3D surfaces showing the variation of species fraction or temperature with the mean mixture fraction or scalar dissipation.
initializes the unsteady flamelet and its probability marker equation.
opens the Flamelet 2D Curves Dialog Box from which you can display 2D plots of the different variables.
tab contains parameters to create the look-up table. See Calculating the Look-Up Tables for details of the items listed below.
Note: If you selected the Flamelet Generated Manifold model, the parameters will be different. See Calculating the Look-Up Tables for those specific parameters.
consists of the controls for the lookup table. A different set of parameters for you to enter will be displayed if Automated Grid Refinement is enabled or disabled.
specifies the number of grid points for the resolution of the mean mixture fraction, mixture fraction variance, and mean enthalpy (for non-adiabatic systems).
specifies the maximum number of grid points used for tabulation. The grid refinement procedure will stop inserting the points when either the change in value and slope between successive points is within tolerance or the maximum number of grid points are generated.
specifies the maximum allowable change in value of table variables between successive grid points as specified by Equation 8–27 in the Theory Guide.
specifies the maximum change in the slope of table variables between successive grid points as specified by Equation 8–28 in the Theory Guide.
is the maximum number of species stored in the lookup tables.
specifies the minimum temperature in the lookup tables.
is the number of discrete values of at which the look-up tables will
be computed.
is the number of discrete values of at which the look-up tables will be computed. This
option is available only when a secondary stream has been defined.
is the number of discrete values of at which the look-up
tables will be computed. This option is available only when no secondary
stream has been defined.
is the maximum number of species that will be included in the look-up tables.
is the number of discrete values of enthalpy at which the three-dimensional look-up tables will be computed. This input is required only if you are modeling a non-adiabatic system.
is used to determine the lowest temperature for which the look-up tables are generated (see Figure 8.10: Visual Representation of a Look-Up Table for the Scalar as a Function of Mean Mixture Fraction and Mixture Fraction Variance and Normalized Heat Loss/Gain in Non-Adiabatic Single-Mixture-Fraction Systems in the Theory Guide). This option is available only if you are modeling a non-adiabatic system.
is an adaptive algorithm that inserts grid points in all table dimensions so that changes in the values of tabulated variables (such as mean temperature, density and species mass fractions) between successive grid points, as well as changes in their slopes, are less than a user specified tolerance.
specifies that an equilibrium flamelet (that is, )
will be generated in ANSYS Fluent and appended to the flamelet library
before the PDF table is calculated. This option is available only
when you are generating more than one laminar flamelet.
opens the Select Transported Scalars Dialog Box.
generates the look-up table.
opens the PDF Table Dialog Box where you can display 2D plots and 3D surfaces showing the variation of species mole fraction, density, or temperature with the mean mixture fraction, mixture fraction variance, or enthalpy.
tab contains parameters needed to modify the piecewise-linear points. See Modifying the Unburnt Mixture Property Polynomials for the details.
contains the list of properties that you can modify. Edit... opens the Quadratic Mixture Fraction dialog box where you can modify the values of the polynomial coefficients.
For each polynomial function of under Partially Premixed Mixture
Properties you can click Edit... and
specify values for Coefficient 1, Coefficient
2, Coefficient 3, and Coefficient
4 in the appropriate Quadratic of Mixture Fraction dialog box.
when enabled includes the non-adiabatic effects on the laminar flame speed by tabulating the laminar speeds in the PDF table. See Laminar Flame Speed in the Theory Guide.
will calculate the partially premixed properties.
tab contains the options and the parameters for the Turbulent Flame Speed Model, the Variance Settings, and the Turbulence-Chemistry Interaction.
contains the Flame Speed Model drop-down list, which allows you to choose between the zimont or the peters model constants for the Zimont premixed combustion model. (This section will appear only if Premixed Combustion or Partially Premixed Combustion is the selected Model and if the C Equation or G Equation premixed model is chosen.)
specifies the value of in Equation 9–11 in the Theory Guide.
specifies the value of in Equation 9–9 in the Theory Guide.
specifies the value of in Equation 9–16 in the Theory Guide.
specifies the value of in Equation 9–1 in the Theory Guide.
specifies the value of in Equation 9–19.
is enabled by default and described in Peters Flame Speed Model.
allows you to select either the transport equation or algebraic option for the calculation of the flame distance variance. Consult Peters Flame Speed Model in the Theory guide for the variance transport and algebraic equation expressions (Equation 9–6 and Equation 9–7).
includes the curvature source term in the G-Equation, which is the last term in Equation 9–4.
is available if you select Flamelet Generated Manifold for the partially premixed combustion model. The three available options (Finite-Rate, Turbulent Flame Speed, and Finite-Rate/Turbulent Flame Speed) are discussed in FGM Turbulent Closure in the Theory Guide.
is available for the G Equation and C Equation. (This section will appear only if Premixed Combustion or Partially Premixed Combustion is the selected Model.)
contains a drop-down list of the available two options: transport equation and algebraic. Consult Peters Flame Speed Model in the Theory Guide for the variance transport and algebraic equation expressions (Equation 9–6 and Equation 9–7). It is recommended that you use the transport equation option for RANS and the algebraic option for LES.
contains options for the premixed combustion model. (This section will appear only if Premixed Combustion is the selected Model.)
enables the adiabatic premixed combustion model, which calculates temperature using Equation 9–65 in the Theory Guide.
enables the non-adiabatic premixed combustion model, which calculates temperature using Equation 9–66 in the Theory Guide.
contains options for choosing a premixed model.
allows you to choose the C equation as described in C-Equation Model Theory.
allows you to choose the Extended Coherent Flamelet model as described in Extended Coherent Flamelet Model Theory.
allows you to choose the G equation as described in G-Equation Model Theory.
contains model constants for the Extended Coherent Flame Model. (This section will appear only if Premixed Combustion or Partially Premixed Combustion is the selected Model and if the Extended Coherent Flame Model flame speed model is chosen.) See Modifying the Constants for the ECFM Flame Speed Closure for details.
contains a drop-down list of the available ITNFS treatments: constant-delta, meneveau, blint, poinsot, and constant.
sets the flame thickness (Equation 9–29 in the Theory Guide).
set the turbulent Schmidt number ().
set the wall flux coefficient.
contains options for the Composition PDF Transport combustion model. (This section will appear only if Composition PDF Transport is the selected Model.)
solves the composition PDF transport equation by stochastically tracking Lagrangian particles through the domain.
assumes a shape for the PDF, allowing Eulerian transport equations to be derived.
tab contains the mixing models.
contains options to specify the method for modeling molecular diffusion. (This section will appear only if Composition PDF Transport is the selected Model.) See Particle Mixing in the Theory Guide for details.
enables the modified curl model for molecular diffusion.
enables the IEM model for molecular diffusion.
enables the EMST mixing model for molecular diffusion.
specifies the value of the mixing constant in Equation 11–6 and Equation 11–8 in the Theory Guide.
tab allows you to define the fuel and oxidizer compositions. This is only available if you select Eulerian as the PDF Transport Option.
consists of the fuel species and the oxidizer.
is the mole or mass fraction of the fuel stream. The sum of mass or mole fractions of all species in the fuel stream should be 1.
is the mole or mass fraction of the oxidizer stream. The sum of mass or mole fractions of all species in the fuel oxidizer stream should be 1.
specifies the species as a Mass Fraction or Mole Fraction.
tab contains Lagrangian PDF transport parameters.
allows you to set the Particles Per Cell.
sets the number of PDF particles per cell. Higher values of this parameter will reduce statistical error, but increase computational time.
toggles the calculation of local time steps. If this option is disabled, then you will need to specify the Time Step directly (see Equation 11–4 in the Theory Guide). This option is available for steady-state simulations.
specifies the particle convection number (see in Equation 11–4 in the Theory Guide).
specifies the particle diffusion number (see in Equation 11–4
in the Theory Guide).
specifies the particle mixing number (see in Equation 11–4 in the Theory Guide).