The available Boundary condition options for an inlet are Velocity, Fully developed flow, 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.

The Include synthetic turbulence option is available when the Turbulence Model Type is set to Large Eddy Simulation or Detached Eddy Simulation. It is disabled by default. When it is enabled, the Normal inflow velocity is specified as , and the Velocity field option sets the velocity vector to , where is the fluctuating inlet velocity at time . The section titled Turbulence Conditions controls the parameters that determine the fluctuating velocity.

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 Apply condition on each disjoint selection separately check box is selected per default. When this setting is selected, the mass flow condition is applied separately on each disjoint selection. If this option is not selected, the condition is applied over the whole feature selection. The Apply condition on each disjoint selection separately should be disabled only if the flow conditions are known to be identical on each disjoint boundary.

The Mass flow rate option sets the integrated mass flow over the boundary selection, 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.

The Fully developed flow option adds contributions to the inflow boundary, which force the flow toward the solution for a fully developed channel flow. The channel can be thought of as a virtual extrusion of the inlet cross section. The inlet boundary must hence be flat in order for the fully developed flow condition to work properly. In 2D axisymmetric models, the inlet normal must be parallel to the symmetry axis.

The Apply condition on each disjoint selection separately check box is selected per default. When this setting is selected, the fully developed flow condition is applied separately on each disjoint selection. If this option is not selected, the condition is applied over the whole feature selection. The Apply condition on each disjoint selection separately should be disabled only if the flow conditions are known to be identical on each disjoint boundary.

The fully developed flow condition requires any volume force to be approximately aligned with the normal of the inlet boundary. The exception is gravity when the Include gravity setting is selected in the physics interface settings. Unless Use reduced pressure is also selected, an option to Compensate for hydrostatic pressure or Compensate for hydrostatic pressure approximation becomes available. It is selected per default and should only be deselected if the inlet normal is aligned with the gravity force and you want to specify an average pressure that includes the hydrostatic pressure.

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 3-3 for the default values):

When Include transition modeling is selected in the SST turbulence model, the intermittency, γ, is set to 1. 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.

For the Large Eddy Simulation and Detached Eddy Simulation interfaces, when the Include synthetic turbulence option is selected, the Number of Fourier modes is specified as an integer value greater than or equal to 2 in order to control the number of Fourier modes used in the generation of the fluctuating inlet velocity.

When the Use random seed check box is enabled, one can specify the value of a Random seed, r, which is used in randomly generating various angles that determine the orientation of the fluctuating velocity.

For a detailed formulation of the generation of inlet turbulent fluctuations, see Synthetic Turbulence Inlet Condition section.

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:

For the inlet, IT and LT can be chosen in the lists. There are:

For the Viscoelastic Flow interface, the inlet conditions for the elastic stress components are required. Note, that if several branches are specified in the Fluid Property node, the initial values entered above are applied to all branches.

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