The problem setup for species transport and volumetric reactions begins in the Species Model dialog box (Figure 14.1: The Species Model Dialog Box). For cases that involve multiphase species transport and reactions, refer to Modeling Species Transport in Multiphase Flows in the Theory Guide.
Setup → Models → Species
Edit...
Under Model, select Species Transport.
Under Reactions, select Volumetric.
In the Mixture Material drop-down
list under Mixture Properties, select which
mixture material you want to use in your problem or, if you want to
create your own mixture material, retain the default selection of mixture-template consisting of ,
, and
. The drop-down list includes all
of the mixtures that are currently defined in the database. If there
is a mixture material listed that is similar to your desired mixture,
you may choose that material and modify it following the steps provided
in Defining Properties for the Mixture and Its Constituent Species.
The number of species in the selected mixture material is displayed in the Number of Volumetric Species field and, if applicable, in the Number of Solid Species and Number of Site Species fields. To review the mixture composition and reactions of the selected Fluent database mixture material, click the button to the right of Mixture Material. This opens the Fluent Database Materials dialog box. Clicking, in turn, the View... buttons next to Mixture Species and Reaction opens the corresponding dialog boxes allowing you to examine the constituent species and reactions data. Note, that the mixture properties cannot be edited before the mixture material is copied to your Fluent problem. For this reason, all related controls are dimmed while viewing the mixture properties.
When you enable the species transport model by clicking either or Apply, ANSYS Fluent performs the following:
The selected Fluent database mixture material including all constituent fluid materials (species) and properties are automatically copied to your case and appear under Mixture in the tree and the Materials task page.
If any properties for the selected mixture material (or the constituent fluid materials) are missing, the solver prints to the console a notice of the required data.
When the mixture material is copied, the Mixture Material drop-down list in the Species Model dialog box changes to contain only the mixtures defined for your Fluent problem.
The View... button is replaced by the Edit... button giving you an option to access the Edit Material dialog box (Edit Material Dialog Box) from the Species Model dialog box.
The Create/Edit Materials dialog box lists mixture in the Material Type drop-down list allowing you to access the Fluent mixture material database. If you want to check or modify any properties of the mixture material, use the Create/Edit Materials Dialog Box, as described in Defining Properties for the Mixture and Its Constituent Species.
You can add more mixture materials to your case by copying them from the database, as described in Copying Materials from the ANSYS Fluent Database, or by creating a new mixture, as described in Creating a New Material and Defining Properties for the Mixture and Its Constituent Species.
Select the Turbulence-Chemistry Interaction (TCI) modeling option. The following options are available:
computes only the Arrhenius rate (see Equation 7–7 in the Theory Guide) and neglects turbulence-chemistry interaction. This model is recommended for laminar or turbulent flows using complex chemistry where either the turbulence time-scales are expected to be fast relative to the chemistry time scales or where the chemistry is sufficiently complex that the chemistry timescales of importance are highly disparate throughout the simulation. You can specify the following inputs:
Increasing the number reduces the computational expense of the chemistry calculations. By default, ANSYS Fluent will update the chemistry once per flow iteration. This option is not available when the None - Explicit Source option is selected for Chemistry Solver.
This 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 not available when the None - Explicit Source option is selected for Chemistry Solver.
computes both the Arrhenius rate and the mixing rate and uses the smaller of the two.
computes only the mixing rate (see Equation 7–25 and Equation 7–26 in the Theory Guide).
models turbulence-chemistry interaction with detailed chemical mechanisms (see Equation 7–7 and Equation 7–30 in the Theory Guide). When using this model, you can modify the following:
Increasing the number reduces the computational expense of the chemistry calculations. By default, ANSYS Fluent will update the chemistry once per flow iteration.
This 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.
in Equation 7–28 and
in Equation 7–29 in the Theory Guide. The default
values are recommended.
From the Chemistry Solver drop-down list, select the solver for your simulation (note that the solvers available in the drop-down list are dependant on the selected Turbulence-Chemistry Interaction model):
If you want the stiff chemistry to relax to chemical equilibrium without solving reactions, select Relax to Chemical Equilibrium. This option is not available for Eddy Dissipation Concept. For information about the Relaxation to Chemical Equilibrium model, refer to The Relaxation to Chemical Equilibrium Model in the Theory Guide
Important: The Relax to Chemical Equilibrium chemistry solver requires thermodynamic data of all species to calculate chemical equilibrium. You can supply your own database using the CHEMKIN Mechanism Import dialog box (opened by clicking Import CHEMKIN mechanism...) (see Importing a Volumetric Kinetic Mechanism in CHEMKIN Format and Importing a Surface Kinetic Mechanism in CHEMKIN Format for details). A sample database is also contained in the file .../fluentx.x/cpropep/data/thermo.db. If you define your own species in ANSYS Fluent, as determined by the Chemical Formula in the Create/Edit Materials dialog box, and this species name is not in the thermo.db file, ANSYS Fluent will report an error. To overcome this error, you must manually enter all the unknown species in the thermo file.
If you want to solve finite-rate chemistry, select either Stiff Chemistry Solver or CHEMKIN-CFD Solver. These two solvers are available when using the Finite-Rate/No TCI or Eddy-Dissipation Concept TCI option.
Selecting CHEMKIN-CFD Solver will enable you to use the ANSYS CHEMKIN-CFD solution algorithms, which are based on and compatible with the ANSYS Chemkin-Pro technology. Once you click or , you will be prompted to import a CHEMKIN mechanism, if you have not already done so. Refer to the ANSYS Chemkin-Pro Input and Theory manuals on the ANSYS Customer Portal (support.ansys.com/docdownloads) for details on the chemistry formulation options. See Using ANSYS Encrypted Mechanisms for instructions on establishing a CHEMKIN-mechanism based material. In addition, Appendix D: Controlling CHEMKIN-CFD Solver Parameters Using Text Commands includes information about advanced solver settings and diagnostic information for the CHEMKIN-CFD solver.
If you want to make explicit use of chemistry source terms in the species transport equations, without a stiff-chemistry solver, select None - Explicit Source. This default solver is not recommended for stiff or complex chemistry.
(optional) For TCI model options that consider finite-rate chemistry, set the integration parameters using the Integration Parameters dialog box (opened by clicking the button). In the Integration Parameters dialog box, you can select acceleration methods (see Using Chemistry Acceleration for more details):
Dynamic Mechanism Reduction (DMR) (for Stiff Chemistry Solver). See Using Dynamic Mechanism Reduction for details.
Chemistry Agglomeration (CA) (for Stiff Chemistry Solver and Relax to Chemical Equilibrium). See Using Chemistry Agglomeration for details.
ISAT. See Using ISAT for details.
Dynamic Cell Clustering (DCC) (for the CHEMKIN-CFD Solver). See see Using Dynamic Cell Clustering for details.
(optional) Select any Options desired. If you want to model full multicomponent (Stefan-Maxwell) diffusion or thermal (Soret) diffusion, select the Full Multicomponent Diffusion or Thermal Diffusion option, respectively.
See Full Multicomponent Diffusion for details.
Enable the Thickened Flame Model when modeling unsteady laminar flames, or when using an LES model for turbulent premixed and partially-premixed flames. Specify the Number of Grid Points in Flame, which by default are 8 grid points. Consequently, in the Create/Edit Materials dialog box, you will specify the Laminar Flame Speed, for which you have a choice of constant, user-defined, or metghalchi-keck-law, and the Laminar Flame Thickness, for which you have a choice of constant, user-defined, or diffusivity-over-flame-speed.
Note: Since the thickened flame model must capture the correct flame speed, it is imperative that the combination of your chemical mechanism and your molecular transport properties (diffusion coefficients and thermal conductivity) reproduce the correct laminar flame speed. It is recommended that you verify this with a 1D premixed flame simulation using ANSYS Chemkin-Pro, for example.
When the Thickened Flame Model is enabled (Figure 14.2: The Species Model Dialog Box Displaying the Thickened Flame Model), you have the option to hook a UDF in the User-Defined Function Hooks dialog box to customize the Thickened Flame Model parameters. Refer to
DEFINE_THICKENED_FLAME_MODEL
in the Fluent Customization Manual for details.
Important: The Thickened Flame Model is available only for unsteady laminar or turbulent (LES / DES / SAS / SBES / SDES) flows, with Species Transport and Volumetric Reactions enabled.
For information about the theory behind the Thickened Flame Model, refer to The Thickened Flame Model in the Theory Guide.
The Species Model Dialog Box
(optional) Select the species for which you want to specify boundary conditions. Only the species that you have selected will be listed in the relevant boundary condition dialog boxes. This will facilitate the problem setup, especially when a large number of species are used in a gas mixture. Note that the Patch and Hybrid Initialization dialog boxes, as well as the Solution Initialization task page will also display only the selected species.
Click .
By default, all the gas species for which the transport equations are to be applied are set as boundary species and appear in the Selected multiple-selection list of the Select Boundary Species dialog box (see Figure 14.3: The Select Boundary Species Dialog Box).
Modify the boundary species list as follows:
To remove the species from the Selected Species multiple-selection list, select it and click . The species will be moved from the Selected Species list to the Unselected Species list.
To add the species back to the Selected Species list, simply select it in the Unselected Species multiple-selection list and click . The species will be moved from the Unselected Species list to the Selected Species list.
(optional) In a similar manner, click the button and select the species that you want to monitor. Only the residuals for the selected species will be monitored and plotted in the graphics window during the simulation.
By default, all the species for which the species transport equations are to be solved are set as monitored species, and their residual plots will be drawn in the graphics window during the run. For a large number of monitored species, it may be difficult to distinguish the overlapping plot lines. By decreasing the number of monitored species, you can obtain clearer residual plots.
The Fluent solver performs the convergence checks only for the monitored species. To prevent false convergence, make sure to include the species that may have difficulties converging in the monitored species list.
You can modify the list of the monitored species dynamically during a run.