The available Boundary condition options for an inlet are Velocity, Laminar inflow, Mass flow, and Pressure. After selecting a Boundary Condition from the list, a section with the same or a similar name displays underneath. For example, if Velocity is selected, a Velocity section, where further settings are defined, is displayed.

The Normal inflow velocity is specified as u = −nU0, where n is the boundary normal pointing out of the domain and U0 is the normal inflow speed.

The Velocity field option sets the velocity vector to u = u0. The components of the inlet velocity vector u0 should be defined for this choice.

This option specifies the normal stress, which in most cases is approximately equal to the pressure. If the reference pressure pref, defined at the physics interface level, is equal to 0, the value of the Pressure p0, at the boundary, is the absolute pressure. Otherwise, p0 is the relative pressure at the boundary.

When Include gravity is selected and Use reduced pressure not selected in the interface Physical model section, the Compensate for hydrostatic pressure approximation (named Compensate for hydrostatic pressure for compressible flows) check box is available and selected by default. When it is selected, the hydrostatic pressure is automatically added to the pressure entered in p0 user input.

This boundary condition is applicable when the fluid enters the domain from a long pipe or channel, in which the laminar flow profile is fully developed. The normal stress at the inlet is determined from the flow conditions at the entrance to a fictitious channel of length Lentr appended to the boundary. The inflow can be specified by the Average velocity Uav, the Flow rate V0, or the Entrance pressure pentr.

For the Entrance pressure option, when Include gravity is selected and Use reduced pressure not selected in the interface Physical model section, the Compensate for hydrostatic pressure approximation (named Compensate for hydrostatic pressure for compressible flows) check box is available and selected by default. When it is selected, the hydrostatic pressure is automatically added to the pressure entered in pentr user input.

For the Average velocity and Flow rate options, when Include gravity is selected in the interface Physical model section, Use reduced pressure should also be selected in the interface Physical model section because these two formulations are only valid with reduced pressure.

The mass flow at an inlet can be specified by the Mass flow rate, the Pointwise mass flux, the Standard flow rate, or the Standard flow rate (SCCM).

The Mass flow rate option sets the integrated mass flow across the entire boundary, the Normal mass flow rate to a specific value, m. The mass flow is assumed to be parallel to the boundary normal, and the tangential flow velocity is set to zero.

For 2D components, the Channel thickness dbc is used to define the area across which the mass flow occurs. This setting is not applied to the whole model. Line or surface integrals of the mass flow over the boundary evaluated during postprocessing or used in integration coupling operators do not include this scaling automatically. Such results should be appropriately scaled when comparing them with the specified mass flow.

The Pointwise mass flux sets the mass flow parallel to the boundary normal. The tangential flow velocity is set to zero. The mass flux is a model input, which means that COMSOL Multiphysics can take its value from another physics interface when available. When User defined is selected a value or function Mf should be specified for the Mass flux.

The Standard flow rate Qsv sets a standard volumetric flow rate, according to the SEMI standard E12-0303. The mass flow rate is specified as the volumetric flow rate of a gas at standard density — the Mean molar mass Mn divided by a Standard molar volume Vm (that is, the volume of one mole of a perfect gas at standard pressure and standard temperature). The flow occurs across the whole boundary in the direction of the boundary normal and is computed by a surface (3D) or line (2D) integral. The tangential flow velocity is set to zero.

The standard density can be defined directly, or by specifying a standard pressure and temperature, in which case the ideal gas law is assumed. The options in the Standard flow rate defined by list are:

For 2D components, the Channel thickness dbc is used to define the area across which the mass flow occurs. This setting is not applied to the whole model. Line or surface integrals of the mass flow over the boundary evaluated during postprocessing or used in integration coupling operators do not include this scaling automatically. Such results should be appropriately scaled when comparing them with the specified mass flow.

The Standard flow rate (SCCM) boundary condition is equivalent to the Standard flow rate boundary condition, except that the flow rate is entered directly in SCCMs (standard cubic centimeters per minute) without the requirement to specify units. Here, the dimensionless Number of SCCM units Qsccm should be specified.

For the Turbulent Flow, Spalart-Allmaras interface, a value or expression for the Undamped turbulent kinematic viscosity υ0 should be specified.

For transport-equation turbulence models, apart from the Spalart-Allmaras turbulence model, the following settings are available under the Specify turbulence length scale and intensity option (see Table 3-2 for the default values):

For the v2-f turbulence model, the additional choice between Isotropic_turbulence and Specify turbulence anisotropy appears. For Specify turbulence anisotropy, a value for the turbulent relative fluctuations at the inlet, ζ0, may be specified. When Specify turbulence variables is selected, values or expressions for the dependent turbulence variables should be defined. Availability is based on the physics interface and the boundary condition chosen.

The Turbulent intensity IT and Turbulence length scale LT values are related to the turbulence variables via the following equations, Equation 3-2 for the Inlet and Equation 3-3 for the Open Boundary:

For the Open Boundary and Boundary Stress options, and with any Turbulent Flow interface, inlet conditions for the turbulence variables also need to be specified. These conditions are used on the parts of the boundary where u·n < 0, that is, where flow enters the computational domain.

For the k-ω and SST turbulence models the Turbulent intensity IT and Turbulence length scale LT values are related to the turbulence variables via the following equations, Equation 3-4 for the Inlet and Equation 3-5 for the Open Boundary:

This section is displayed by clicking the Show button () and selecting Advanced Physics Options.