The Velocity Inlet dialog box sets the boundary conditions for a velocity inlet zone. It is opened from the Boundary Conditions Task Page. See Inputs at Velocity Inlet Boundaries for details about defining the items below.

Controls
sets the name of the zone.
displays the name of the phase. This item appears if the VOF, mixture, or Eulerian multiphase model is being used.
allows you to set specific parameters for a particular boundary for open channel wave boundaries. This is available when the volume of fluid multiphase model is selected.
contains the momentum parameters.
sets the method used to define the inflow velocity.
sets the method used to define the direction of flow of the wave. This is available when you enable the Open Channel Wave BC option.
allows specification in terms of a Velocity Magnitude and Flow-Direction.
allows specification in terms of the Cartesian, cylindrical, or local cylindrical velocity components.
allows specification of a Velocity Magnitude normal to the boundary.
specifies relative or absolute velocity inputs. You can choose to enter Absolute velocities or velocities Relative to Adjacent Cell Zone. If you are not using moving reference frames, both options are equivalent, so you need not choose.
is the flow velocity, specified as a constant or a parameter.
specifies whether Cartesian, Cylindrical, or Local Cylindrical velocities will be defined. This item will appear only for 3D cases in which you have selected Magnitude and Direction or Components as the Velocity Specification Method.
set the components of the velocity vector at the inflow boundary. These items will appear for 2D non-axisymmetric models, or for 3D models if you select the Components option as the Velocity Specification Method and Cartesian as the Coordinate System.
set the components of the velocity vector at the inflow boundary. These items will appear for 3D models if you select the Components option as the Velocity Specification Method and Cylindrical or Local Cylindrical as the Coordinate System.
set the components of the velocity vector at the inflow boundary. These items will appear for 2D axisymmetric models.
Important: Swirl-Velocity will appear only for 2D axisymmetric swirl models.
specifies the angular velocity for a 3D flow. This item will appear for a 3D model if you select the
Components option as the Velocity Specification
Method and Cylindrical or Local
Cylindrical as the Coordinate System.
specifies the swirl angular velocity for an axisymmetric swirling flow. This item will appear for an
axisymmetric swirl model if you choose Components as the
Velocity Specification Method.
sets the magnitude of the velocity vector at the inflow boundary. This item will appear if you select the Magnitude and Direction or Magnitude, Normal to Boundary option as the Velocity Specification Method.
set the direction of the velocity vector at the inflow boundary. These items will appear for 2D non-axisymmetric models if you select the Magnitude and Direction option as the Velocity Specification Method, or for 3D models if you select the Magnitude and Direction option as the Velocity Specification Method and Cartesian as the Coordinate System.
set the direction of the velocity vector at the inlet boundary. These items will appear for 3D models if you select the Magnitude and Direction option as the Velocity Specification Method and Cylindrical or Local Cylindrical as the Coordinate System, or for 2D axisymmetric models.
Important: Tangential-Velocity will appear only for 2D axisymmetric swirl models.
sets the X, Y, and Z coordinates of the origin of the local cylindrical coordinate system.
sets the X, Y, and Z components of the direction of the local cylindrical coordinate system.
specifies the pressure to be used as the pressure outlet condition if flow exits the domain at any face on the velocity inlet boundary. (Note that this effect is similar to that of the “velocity far-field” boundary that was available in RAMPANT 3.)
This item appears only for the density-based solvers.
contains the turbulence parameters.
specifies which method will be used to define the turbulence parameters. You can
choose K and Epsilon (-
models and RSM only), K and Omega
(
-
models only), Intensity and Length Scale,
Intensity and Viscosity Ratio, Intensity and Hydraulic
Diameter, Modified Turbulent Viscosity (Spalart-Allmaras
model only), or Turbulent Viscosity Ratio (Spalart-Allmaras model
only). See Determining Turbulence Parameters for information about the inputs for each
of these methods. (This item will appear only for turbulent flow calculations.)
set values for the turbulence kinetic energy and its dissipation rate
. These items will appear if you choose K and
Epsilon as the Specification Method.
set values for the turbulence kinetic energy and its specific dissipation rate
. These items will appear if you choose K and
Omega as the Specification Method.
set values for turbulence intensity and turbulence length scale
. These items will appear if you choose Intensity and Length
Scale as the Specification Method.
set values for turbulence intensity and turbulent viscosity ratio
. These items will appear if you choose Intensity and
Viscosity Ratio as the Specification Method.
set values for turbulence intensity and hydraulic diameter
. These items will appear if you choose Intensity and
Hydraulic Diameter as the Specification Method.
sets the value of the modified turbulent viscosity . This item will appear if you choose Modified Turbulent
Viscosity as the Specification Method.
sets the value of the turbulent viscosity ratio . This item will appear if you choose Turbulent Viscosity
Ratio as the Specification Method.
sets the value of the turbulence intensity for the LES model.
specifies which method will be used to determine the Reynolds stress boundary conditions when the Reynolds stress turbulence model is used. You can choose either K or Turbulent Intensity or Reynolds-Stress Components. If you choose the former, ANSYS Fluent will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Reynolds Stress Model for details. (This item will appear only for RSM turbulent flow calculations.)
specify the Reynolds stress components when Reynolds-Stress Components is chosen as the Reynolds-Stress Specification Method.
contains settings for treatment of acoustic pressure waves at the boundary.
disables special treatment of acoustic pressure waves at the boundary.
enables the general non-reflecting boundary condition treatment described in General Non-Reflecting Boundary Conditions.
enables the impedance boundary condition treatment described in Impedance Boundary Conditions.
enables the transparent flow forcing boundary condition described in Transparent Flow Forcing Boundary Conditions.
contains the parameters for the impedance boundary condition treatment. For details refer to Using the Impedance Boundary Condition.
contains the parameters for the transparent flow forcing boundary condition treatment. For details refer to Using the Transparent Flow Forcing Boundary Condition.
contains the thermal parameters.
specifies the static temperature of the flow.
contains the boundary conditions for the radiation model at the velocity inlet.
set the radiation boundary conditions when you are using the P-1, DTRM, DO, S2S, or MC models for radiation heat transfer. See Defining Boundary Conditions for Radiation for details.
specifies whether or not the velocity inlet participates in solar ray tracing.
specifies a multiplier (ranging from 0 to 1) that is applied to the solar irradiation entering the domain through the velocity inlet.
specifies whether or not the velocity inlet participates in the view factor calculation as part of the S2S radiation model. This parameter is available only if you select the Surface to Surface radiation model.
contains the species parameters.
allows you to specify the species in mole fractions rather than mass fractions.
contains inputs for the mass fractions of defined species. See Defining Cell Zone and Boundary Conditions for Species for details about these inputs. These items will appear only if you are modeling non-reacting multi-species flow or you are using the finite-rate reaction formulation.
set inlet values for the PDF mixture fraction and its variance. These items will appear only if you are using the non-premixed or partially premixed combustion model.
set inlet values for the secondary mixture fraction and its variance. (These items will appear only if you are using the non-premixed or partially premixed combustion model with two mixture fractions.)
sets the value of the progress variable for premixed turbulent combustion. See Setting Boundary Conditions for the Progress Variable for details.
This item will appear only if the premixed or partially premixed combustion model is used.
contains the discrete phase parameters.
sets the way that the discrete phase behaves with respect to the boundary. This item appears when one or more injections have been defined.
rebounds the particle off the boundary with a change in its momentum as defined by the coefficient of restitution. (See Particle Reflection at Wall in the Fluent Theory Guide.)
terminates the trajectory calculations and records the fate of the particle as “trapped”. In the case of evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters the cell adjacent to the boundary. See Figure 23.25: “Trap” Boundary Condition for the Discrete Phase.
reports the particle as having “escaped” when it encounters the boundary. Trajectory calculations are terminated. See Figure 23.26: “Escape” Boundary Condition for the Discrete Phase.
indicates that the direction and velocity of the droplet particles are given by the resulting momentum flux, which is a function of the impingement angle. See Figure 16.6: “Wall Jet” Boundary Condition for the Discrete Phase in the Theory Guide.
specifies a user-defined function to define the discrete phase boundary condition type.
sets the user-defined function from the drop-down list.
contains the multiphase parameters.
specifies the volume fraction of the secondary phase selected in the Boundary Conditions Task Page. This section of the dialog box will appear when one of the multiphase models is being used. See Defining Multiphase Cell Zone and Boundary Conditions for details.
specifies the secondary phase to which the parameters are applied. In case of a three-phase flow, select the corresponding secondary phase from this list.
allows you to choose between Shallow Waves, Shallow/Intermediate Waves or Short Gravity Waves. Information about the two types of waves is available in Open Channel Wave Boundary Conditions in the Theory Guide.
is determined by using the absolute value of height from the free surface to the origin in the direction of gravity and applying the correct sign based on whether the free surface level is above (positive) or below (negative) the origin.
is valid for shallow and intermediate waves. The bottom level is used for calculating the liquid height.
is the direction of wave propagation for a zero wave heading angle.
determines whether to use wave theory or a wave spectrum to model waves in the shallow/intermediate and short gravity wave regimes.
specifies the number of waves you are defining when modeling waves using wave theory.
allows you to choose from First Order Airy (the default), Second Order Stokes, Third Order Stokes, Fourth Order Stokes, and Fifth Order Stokes for shallow/intermediate waves and short gravity waves. For shallow waves, you can choose between Fifth Order Solitary and Fifth Order Cnoidal. Information about the types of wave theory is available in Open Channel Wave Boundary Conditions in the Theory Guide.
is the height difference between a wave crest to the neighboring trough.
Since a solitary wave does not have troughs, the wave height is the distance between a wave crest to mean free surface level.
is the wave length of the shallow wave or short gravity wave.
is the translational distance from the reference point origin in the reference wave propagation direction. This option is used to generate a wave from a location other than the reference frame origin.
is the phase difference between one wave and another.
is the angle between the direction of the wavefront and the reference wave direction, in the plane of the flow surface. In 2D, there are only two possibilities, zero degrees when the wave is in the reference wave direction, and 180 degrees when the wave is in the opposite direction.
specifies the spectrum to use. You can select Pierson-Moskowitz (appropriate for fully-developed seas), Jonswap (appropriate for fetch-limited seas), or TMA (appropriate for fetch-limited, finite-depth seas).
controls the shape and amplitude of the frequency peak in the
Jonswap and TMA formulations. This corresponds to
in Equation 17–100 in the Fluent Theory Guide.
is the mean wave height of the largest 1/3 of waves. This corresponds to
in Equation 17–99 in the Fluent Theory Guide.
is the wave frequency corresponding to the highest wave energy. This corresponds to
in Equation 17–99 and Equation 17–100 in the Fluent Theory Guide.
can be expressed in terms of the peak wave period,
, as
.
specify the frequency range for the spectrum. Note that the Peak Wave Frequency must fall in between Minimum Wave Frequency and .
specifies the number of components into which the frequency spectrum is divided.
specifies the method to use for specifying the directional spreading characteristics. You can choose Unidirectional (for long-crested waves), Frequency Independent Cosine Function (for short-crested waves where the directional component does not depend on frequency), and Frequency Dependant Hyperbolic Function (for short-crested waves where the directional component depends on frequency).
specifies the exponent in the Frequency Independent Cosine Function formulation. This
corresponds to in Equation 17–104 in the Fluent Theory Guide.
specifies the principal wave heading direction.
specifies the deviation from the mean wave direction for calculating the angular range.
specifies the number of components into which the angular range is divided.
displays the boundary conditions for the electric potential field. This tab is available only if you have enabled either the Electric Potential model or the Electrochemical reaction model in the Species Dialog Box.
is a drop-down list of available potential boundary condition types: Specified Flux and Specified Value. For the Specified Flux boundary condition, you will need to specify Current Density at the wall. For the Specified Value boundary condition, you will need to specify Potential at the wall.
contains the UDS parameters.
appears only if user-defined scalars are specified.
specifies whether the scalar is a specified flux or a specified value.
appears only if user-defined scalars are specified.
specifies the value of the scalar.