You are viewing the documentation for an older COMSOL version. The latest version is available here.
Nonisothermal Flow
Use the Nonisothermal Flow () multiphysics coupling to simulate fluid flows where the fluid properties depend on temperature. Models can also include heat transfer in solids or in porous media as well as surface-to-surface radiation and radiation in participating media, with the Heat Transfer Module. The laminar and turbulent (RANS) physics interface supports low Mach numbers (typically less than 0.3). The LES interfaces only support incompressible flow
The Nonisothermal Flow, Laminar Flow interface solves for conservation of energy, mass and momentum in fluids and porous media and for conservation of energy in solids.
It defines p and u variables in order to set the Absolute pressure in the Model Input section and the Velocity field in the Heat Convection section of the Fluid and Porous Medium features in the Heat Transfer interface. In addition it provides all the fluids quantities that may be needed by the Heat Transfer interface (for example, viscosity, turbulence parameters).
In the Fluid Flow interface, it sets the Temperature in the Model Input section and defines the Density in the Fluid Properties section of the Fluid Properties and Fluid and Matrix Properties features.
It synchronizes also the definition of the reference temperature to be used for incompressible flows, and the features from the Heat Transfer and Fluid Flow interfaces when a turbulent flow regime is defined. It also complements the Screen and Interior Fan feature from the flow interface to account for thermal effects.
In addition, it also accounts for the multiphysics stabilization terms, for the heat transfer changes in the turbulent regime (for example, thermal wall functions), for work due to pressure forces and viscous dissipation, and for natural convection, including a Boussinesq approximation
Nonisotermal Flow and Conjugate Heat Transfer trigger pseudo time stepping when Use pseudo time stepping for stationary equation form in the Fluid Flow interface is set to Automatic from physics.
The multiphysics stabilizations (streamline diffusion and crosswind diffusion) are controlled by the Fluid Flow interface. For example, the multiphysics streamline diffusion can be disabled in a Laminar Flow physics node, in the Stabilization section. The stabilization selected in the Heat Transfer physics interface has no effect if the multiphysics coupling stabilization is active, but remains active if not. However, the isotropic diffusion is not a multiphysics stabilization and is controlled by each physics interface. The crosswind diffusion stabilization is turned off for the LES interfaces.
Finally, when one of the physics interfaces or the multiphysics coupling is not solved in a study step, then the stabilization of each solved physics is used instead of the coupled stabilization, and the solver suggestions are uncoupled.
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 nitf1.
Domain Selection
When nodes are added from the context menu, you can select Manual (the default) from the Selection list to choose specific domains to define the nonisothermal flow, or select All domains as needed.
Coupled Interfaces
This section defines the physics involved in the multiphysics coupling. The Fluid flow and 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 either list to uncouple the node from a physics interface. If the physics interface is removed from the Model Builder, for example Heat Transfer in Fluids is deleted, then the Heat transfer list defaults to None as there is nothing to couple to.
Heat Transfer Turbulence Model
This section is available when the fluid flow interface uses a turbulence model. When a RANS turbulence model is used, select an option from the Heat transport turbulence 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 Reinf (dimensionless).
For User-defined turbulent Prandtl number, enter a Turbulent Prandtl number PrT (dimensionless).
When the flow interface uses a RANS turbulence model, the conductive heat flux is defined as
with the turbulent thermal conductivity defined as
where μT is defined by the flow interface, and PrT depends on the Heat transport turbulence model. See Turbulent Conductivity for details.
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.
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.
Material Properties
When the Compressibility setting in the fluid flow interface is set to Incompressible, select the Boussinesq approximation check box in order to use material data evaluated at the reference temperature and reference pressure. If gravity is included in the physics, it is linearized with respect to temperature.
Select an option from the Specify density list — From heat transfer interface (the default), From fluid flow interface, Custom, linearized density or Custom.
For Custom, linearized density, enter the Reference density ρref (SI unit: kg/m3) and the Coefficient of thermal expansion αp (SI unit:1/K), or select From material, or select a variable in the list if available. When Custom, linearized density is selected, regardless how the properties are defined they should be constant. If material properties are not constant you should consider using any of the other options to define the density. Also, if Custom, linearized density is used for incompressible flow, the density ρ is evaluated to ρref. In this case αp is not used unless Boussinesq approximation is selected.
For Custom, enter a Density ρ (SI unit: kg/m3), or select a density in the list if available.
The density definition in the Nonisothermal Flow node ensures that the same definition of the density is used on the fluid flow and heat transfer interfaces. When Include gravity is selected and the Compressibility is set to Incompressible flow in the fluid interface properties, the gravity forces are defined using the coefficient of thermal expansion. Along with the fact that the material properties are evaluated for a constant temperature and pressure, this gravity force definition corresponds to Boussinesq approximation. Unless the density is defined as Custom, linearized density the coefficient of thermal expansion is evaluated from the fluid density.
Select an option from the Specify reference temperature list — From heat transfer interface, From fluid flow interface (the default), or User defined.
For From heat transfer interface, set the Reference temperature Tref (SI unit: K) in the Physical Model section of the interface selected in the Heat transfer list of the Coupled Interfaces section. The Reference temperature input in the Fluid flow interface is synchronized to the same value or expression, and is not editable.
For From fluid flow interface, set the Reference temperature Tref (SI unit: K) in the Physical Model section of the interface selected in the Fluid flow list of the Coupled Interfaces section. The Reference temperature input in the Heat transfer interface is synchronized to the same value or expression, and is not editable.
For User defined, set a value or expression. The Reference temperature inputs in the Physical Model sections of the Heat transfer and Fluid flow interfaces are synchronized to the same value or expression, and are not editable.
Flow Heating
The Include viscous dissipation check box is selected by default to account for the heat source corresponding to viscous heating. Because it may induce an extra computational cost it should be only selected in application where such effect is expected. If no information on this is available, selecting the option ensures that the energy balance for the heat and the flow equation is respected.
When an interface is selected from the Heat transfer list, some of its model inputs are forced with values from the Nonisothermal Flow node. In addition, it defines how the turbulence has to be accounted for, depending on the Fluid flow interface’s turbulence settings. Therefore, each heat transfer or fluid flow interface should be used in at most one Nonisothermal Flow node. In cases where multiple fluid flow interfaces are used, an equal number of heat transfer interfaces and Nonisothermal Flow nodes are needed to define proper multiphysics couplings.
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 or 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.