Inlet
This condition should be used on boundaries for which there is a net flow into the domain. To obtain a numerically well-posed problem, it is advisable to also consider the Outlet conditions when specifying an Inlet condition. For example, if the pressure is specified at the outlet, the velocity may be specified at the inlet, and vice versa. Specifying the velocity vector at both the inlet and the outlet may cause convergence difficulties.
Boundary Condition
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.
Velocity
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.
Pressure Conditions
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.
The Suppress backflow option adjusts the inlet pressure locally in order to prevent fluid from exiting the domain through the boundary. If you clear the suppress backflow option, the inlet boundary can become an outlet depending on the pressure field in the rest of the domain.
Flow direction controls in which direction the fluid enters the domain.
-
For Normal flow, it prescribes zero tangential velocity component.
-
For User defined, an Inflow velocity direction du (dimensionless) should be specified. The magnitude of du does not matter, only the direction. du must point into the domain.
Mass Flow
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).
Mass Flow Rate
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.
Pointwise Mass Flux
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.
Standard Flow Rate
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:
Standard density, for which the Standard molar volume Vm should be specified.
Standard pressure and temperature, for which the Standard pressure Pst and the Standard temperature Tst should be defined.
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.
Standard Flow Rate (SCCM)
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.
Turbulent Flow Settings
No additional inlet conditions are required for the algebraic turbulence models: Algebraic yPlus and L-VEL.
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.
 
IT
LT
Uref
k0
ε0
ω0
υ0
About the Turbulent Intensity and Turbulence Length Scale Parameters
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:
(3-2)Inlet
(3-3)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:
(3-4)Inlet
(3-5)Open Boundary
Fully Developed Flow
The Fully developed flow option adds contributions to the inflow boundary, which force the flow towards 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.
Select an option to control the flow rate at the inlet:
Flow rate, V0. Two-dimensional models also require an Entrance thickness, Dz, which is the out-of-plane thickness of the extruded entrance channel.
Average pressure, Pav. Observe that Pav is the average pressure on the inflow 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.
Fully developed inflow can be used in conjunction with the turbulence models. No additional inputs are required for the turbulence variables. They are instead solved for on the inlet boundary to be consistent with the fully developed flow profile.
A fully developed flow boundary cannot be adjacent to any Interior Wall feature.
Constraint Settings
This section is displayed by clicking the Show button () and selecting Advanced Physics Options.
Non-Newtonian Flow (inlet): Application Library path CFD_Module/Single-Phase_Tutorials/non_newtonian_flow