The Reacting Flow Coupling Feature
Use the Reacting Flow () multiphysics coupling to simulate mass transport and reactions in a gas or liquid mixture where the fluid flow can be dependent on the mixture composition. When a Heat Transfer and a Chemistry interface are selected, use this coupling to simulate heat transfer additionally to mass transport and reactions.
The coupling adds the heat source of reaction when a heat transfer interface is selected. No additional heat source needs to be defined to account for it in the heat transfer interface. It also accounts for the multiphysics stabilization terms, for work due to pressure forces and viscous dissipation.
Select a Fluid Flow interface and a Species transport interface to couple fluid flow with mass transport. Chemistry and Heat Transfer are optional. They can be set to None when the coupling is used to simulate isothermal mixtures.
When a Chemistry interface is selected and Heat Transfer is set to None, fluid properties are taken from the Chemistry interface. Set the Temperature to evaluate the fluid properties synchronized with all the physics interfaces at the given temperature.
Select a Chemistry interface and Heat Transfer interface in order to account for the heat of reaction, enthalpy diffusion, viscous heating and mass fluxes contributing to the heat and energy balance.
When Chemistry is set to None and a Heat Transfer interface is selected, the coupling is solved in the same way as when no Heat Transfer interface is selected. Thermodynamic properties are required by the Heat Transfer interface.
The pressure, velocity, and temperature variables of the Reacting Flow coupling node are set to the Common Model Input values of the Default Model Inputs node on the complementary selection, that is, all domains except those from the Selection list. It allows to couple multiple fluid flow or transport of species interfaces with a single heat transfer interface. See Default Model Inputs in the COMSOL Multiphysics Reference Manual for details.
Domain Level Synchronization
The Reacting Flow coupling synchronizes the features from a Chemistry interface, Heat Transfer interface, Single-Phase Flow, or Brinkman Equations, interface and a Transport of Concentrated Species interface. When the Chemistry interface is not selected, the density in the Single-Phase Flow interface is automatically synchronized to the one defined by the Transport of Concentrated Species interface.
The velocity field used by the Transport of Concentrated Species interface and Heat Transfer interface is synchronized to the one computed in the Single-Phase Flow interface.
When a Chemistry interface is selected, the Reacting Flow coupling synchronizes the definition of the thermal conductivity, density, heat capacity, enthalpy, and dynamic viscosity with the other coupled physics interfaces. The reference temperature is taken from the Heat Transfer interface.
The Stefan Velocity
The Reacting Flow coupling feature automatically couples mass transfer on boundaries and applies a corresponding velocity contribution for the flow. Prescribing a net mass boundary flux in the Transport of Concentrated Species interface, either using a Flux or Mass Fraction feature, the Reacting Flow feature computes The Stefan Velocity and applies this in Wall features using the same selection.
Mass Transfer to Other Phases in Porous Media
When coupled to the Brinkman Equations interface, the Reacting Flow node automatically computes the net mass source or sink in a Reactions (when Mass transfer to other phases is enabled) node in the Transport of Concentrated Species interface and adds the corresponding source/sink to the momentum equations of the Fluid and Matrix Properties domains.
Turbulent Mass Transfer
When a turbulence model is used, the Reacting Flow coupling applies turbulence modeling for the mass transport in the following manners:
•
Turbulent heat transfer and mass transport are added, defined from the turbulent viscosity and a turbulent Schmidt number (for more information, see Turbulent Mass Transport Models).
•
Temperature and mass transport wall functions. When a turbulence model using wall functions is used for the fluid flow, the Reacting Flow coupling automatically adds wall functions for the temperature and mass transport on the same boundaries (for more information, see Mass Transport Wall Functions).
Settings
The Label is the default multiphysics coupling feature name.
The Name is used primarily as a scope prefix for variables defined by the coupling node. Refer to such variables in expressions using the pattern <name>.<variable_name>. In order to distinguish between variables belonging to different coupling nodes or physics interfaces, the name string must be unique. Only letters, numbers, and underscores (_) are permitted in the Name field. The first character must be a letter.
The default Name (for the first multiphysics coupling feature in the model) is nirf1.
Domain Selection
The Reacting Flow coupling is automatically defined on the intersection of the selections for the coupled interfaces. When modeling porous media transport a Porous Medium feature, applied on the same domains, is needed in all coupled transport interfaces. Reacting Flow coupling supports porous media transport in Fluid flow and Species transport interfaces.
The Selection list displays the domains where the coupling feature is active.
Coupled Interfaces
This section defines the physics involved in the multiphysics coupling. The Fluid flow, Species transport, Chemistry, Heat Transfer lists include all applicable physics interfaces.
The default values depend on how this coupling node is created.
•
If it is added from the Physics ribbon (Windows users), Physics contextual toolbar (Mac and Linux users), or context menu (all users), then the first physics interface of each type in the component is selected as the default.
•
If it is added automatically when a multiphysics interface is chosen in the Model Wizard or Add Physics window, then the two participating physics interfaces are selected.
You can also select None from a list to uncouple the node from a physics interface.
Click the Go to Source buttons () to move to the main physics interface node for the selected physics interface.
Click the Show or Hide Physics Properties Settings button () to toggle the display of physics properties settings affecting the coupling feature. When a turbulence model is used, turbulent heat and mass transfer is automatically accounted for (see the settings in the Turbulence section below). Using Reacting Flow, the heat and mass transfer treatment at walls follows that applied for the fluid flow. Therefore the Wall treatment setting is also displayed when using a turbulence model. For more information on turbulent mass transfer at walls, see the section Mass Transport Wall Functions in the CFD Module User’s Guide.
If a physics interface is deleted and then added to the model again, then in order to reestablish the coupling, you need to choose the physics interface again from the Fluid flow, Species transport, Chemistry and Heat Transfer lists. This is applicable to all multiphysics coupling nodes that would normally default to the once present interface. See Multiphysics Modeling Workflow in the COMSOL Multiphysics Reference Manual.
Mass transport Turbulence model
When the fluid flow interface uses a turbulence model, select an option from the Mass transport turbulence model list — Kays–Crawford, High Schmidt Number, or User-defined turbulent Schmidt number.
For User-defined turbulent Schmidt number, enter a Turbulent Schmidt number ScT (dimensionless).
The turbulent mass transfer added to the mass fraction equations is defined as
where μT is the turbulent viscosity defined by the flow interface, and the turbulent Schmidt number, ScT, depends on the Mass transport turbulence model used.
Heat Transfer Turbulence Model
This section is available when a Heat Transfer interface is selected and the fluid flow interface uses a turbulence model. When a RANS turbulence model is used, the conductive heat flux is defined as
with the turbulent thermal conductivity defined by the heat transport turbulence model. The turbulent Prandtl number models are available for all RANS turbulence models except for the Elliptic Blending R-ε, while the anisotropic turbulent thermal conductivity models can be used with RANS-RSM turbulence models only, which require the CFD Module. The Turbulence model type used by the fluid flow interface can be displayed by selecting the Show or Hide Physics Property Settings button at the right of the Fluid flow list.
When a RANS-RSM turbulence model (except Elliptic Blending R-ε) is selected in the fluid flow interface, the Heat transport turbulence model can be set to Turbulent Prandtl number (the default) or Anisotropic turbulent thermal conductivity. For RANS-EVM models, this option is not available since only turbulent Prandtl number models can be used. In this case, the subsequent options act as if Turbulent Prandtl number was selected. For Elliptic Blending R-ε, this option is not available either since only anisotropic turbulent thermal conductivity models can be used. In this case, the subsequent options act as if Anisotropic turbulent thermal conductivity was selected.
When Turbulent Prandtl number option is used, the turbulent thermal conductivity is
where μT is defined by the flow interface, and PrT depends on the Turbulent Prandtl number model. Select an option from the Turbulent Prandtl number model list: Kays–Crawford (the default), Extended Kays–Crawford, or User-defined turbulent Prandtl number.
For Extended Kays–Crawford, enter a Reynolds number at infinity Re∞ (dimensionless).
For User-defined turbulent Prandtl number, enter a Turbulent Prandtl number PrT (dimensionless).
When Anisotropic turbulent thermal conductivity option is used, the turbulent thermal conductivity is defined by the selected Anisotropic turbulent thermal conductivity model option: Daly–Harlow (GGDH) (the default), Abe–Suga (High order GGDH), or User-defined turbulent thermal conductivity.
For Daly–Harlow (GGDH), enter the Daly–Harlow model coefficient CG (dimensionless).
For Abe–Suga (High order GGDH), enter the Abe–Suga model coefficient CH (dimensionless).
For User-defined turbulent thermal conductivity, select Isotropic, Diagonal, Symmetric, or Full based on the characteristics of the turbulent thermal conductivity, and enter a value or expression. For Isotropic enter a scalar which will be used to define a diagonal tensor. For the other options, enter values or expressions into the editable fields of the tensor.
The components of the turbulent thermal conductivity κT when given in tensor form are available as ht.kappaTxx, ht.kappaTyy, and so on (using the default name ht).
See Turbulent Conductivity for details.
With CFD Module, this section is also available when either of the LES interfaces RBVMWV or Smagorinsky is used. For these two LES models, additional diffusion terms, corresponding to the ones in the momentum equation, appear in the energy equation. The magnitude of these terms can be controlled by a turbulent Prandtl number.
When the Wall treatment option selected in the fluid flow interface is set either to Wall functions or Automatic, the Thermal wall function can be set to Standard (default) or High viscous dissipation at wall. The Standard option is suitable for most of the configurations. The High viscous dissipation at wall option accounts for viscous dissipation in the boundary layer which is not the case with the Standard option. This is needed for accurate results in case of fast internal flow, especially if paths are narrow or the fluid very viscous.
See Temperature Wall Functions for details.