33.7.18 Velocity Inlet Dialog Box

The Velocity Inlet dialog box sets the boundary conditions for a velocity inlet zone. It is opened from the Boundary Conditions task page. See Section  7.3.4 for details about defining the items below.

Controls

Zone Name   sets the name of the zone.

Phase   displays the name of the phase. This item appears if the VOF, mixture, or Eulerian multiphase model is being used.

Open Channel Wave BC   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.

Momentum   contains the momentum parameters.

Velocity Specification Method   sets the method used to define the inflow velocity.

Wave Velocity Specification Method   sets the method used to define the wave velocity. This is available when you enable the Open Channel Wave BC option.

Magnitude and Direction   allows specification in terms of a Velocity Magnitude and Flow-Direction.

Components   allows specification in terms of the Cartesian, cylindrical, or local cylindrical velocity components.

Magnitude, Normal to Boundary   allows specification of a Velocity Magnitude normal to the boundary.

Reference Frame   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.

Uniform Wave Velocity Magnitude   

Coordinate System   specifies whether Cartesian, Cylindrical, or Local Cylindrical velocities will be input. This item will appear only for 3D cases in which you have selected Magnitude and Direction or Components as the Velocity Specification Method.

X,Y,Z-Velocity   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.

Radial, Tangential, Axial-Velocity   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.

Axial, Radial, Swirl-Velocity   set the components of the velocity vector at the inflow boundary. These items will appear for 2D axisymmetric models.

Swirl-Velocity will appear only for 2D axisymmetric swirl models.

Angular Velocity   specifies the angular velocity $\Omega$ 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.

Swirl Angular Velocity   specifies the swirl angular velocity $\Omega$ for an axisymmetric swirling flow. This item will appear for an axisymmetric swirl model if you choose Components as the Velocity Specification Method.

Velocity Magnitude   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.

X,Y,Z-Component of Flow-Direction   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.

Radial, Tangential, Axial-Component of Flow Direction   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.

Tangential-Velocity will appear only for 2D axisymmetric swirl models.

X,Y,Z-Component of Axis Direction   sets the direction of the axis. These items will appear if the selected Coordinate System is Local Cylindrical.

X,Y,Z-Coordinate of Axis Origin   sets the location of the axis origin. These items will appear if the selected Coordinate System is Local Cylindrical.

Outflow Gauge Pressure   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.

Turbulence   contains the turbulence parameters.

Specification Method   specifies which method will be used to input the turbulence parameters. You can choose K and Epsilon ( $k$- $\epsilon$ models and RSM only), K and Omega ( $k$- $\omega$ models only), Intensity and Length Scale, Intensity and Viscosity Ratio, Intensity and Hydraulic Diameter, or Turbulent Viscosity Ratio (Spalart-Allmaras model only). See Section  7.3.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Turbulent Kinetic Energy, Turbulent Dissipation Rate   set values for the turbulence kinetic energy $k$ and its dissipation rate $\epsilon$. These items will appear if you choose K and Epsilon as the Specification Method.

Turbulent Kinetic Energy, Specific Dissipation Rate   set values for the turbulence kinetic energy $k$ and its specific dissipation rate $\omega$. These items will appear if you choose K and Omega as the Specification Method.

Turbulent Intensity, Turbulent Length Scale   set values for turbulence intensity $I$ and turbulence length scale $\ell$. These items will appear if you choose Intensity and Length Scale as the Specification Method.

Turbulent Intensity, Turbulent Viscosity Ratio   set values for turbulence intensity $I$ and turbulent viscosity ratio $\mu_t/\mu$. These items will appear if you choose Intensity and Viscosity Ratio as the Specification Method.

Turbulent Intensity, Hydraulic Diameter   set values for turbulence intensity $I$ and hydraulic diameter $L$. These items will appear if you choose Intensity and Hydraulic Diameter as the Specification Method.

Turbulent Viscosity Ratio   sets the value of the turbulent viscosity ratio $\mu_t/\mu$. This item will appear if you choose Turbulent Viscosity Ratio as the Specification Method.

Turbulent Intensity   sets the value of the turbulence intensity $I$ for the LES model.

Reynolds-Stress Specification Method   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 Turbulence 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 Section  12.14.3 for details. (This item will appear only for RSM turbulent flow calculations.)

UU,VV,WW,UV,VW,UW Reynolds Stresses   specify the Reynolds stress components when Reynolds-Stress Components is chosen as the Reynolds-Stress Specification Method.

Thermal   contains the thermal parameters.

Temperature   specifies the static temperature of the flow.

Radiation   contains the radiation parameters.

Participates in Solar Ray Tracing   specifies whether or not velocity inlet participate in solar ray tracing.

External Black Body Temperature Method, Internal Emissivity   set the radiation boundary conditions when you are using the P-1 model, the DTRM, the discrete ordinates model, or the S2S model for radiation heat transfer. See Section  13.3.6 for details.

Species   contains the species parameters.

Specify Species in Mole Fractions   allows you to specify the species in mole fractions rather than mass fractions.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  15.1.5 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.

Mean Mixture Fraction, Mixture Fraction Variance   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.

Secondary Mean Mixture Fraction, Secondary Mixture Fraction Variance   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.)

Progress Variable   sets the value of the progress variable for premixed turbulent combustion. See Section  17.3.3 for details.

This item will appear only if the premixed or partially premixed combustion model is used.

DPM   contains the discrete phase parameters.

Discrete Phase BC Type   sets the way that the discrete phase behaves with respect to the boundary. This item appears when one or more injections have been defined.

reflect   rebounds the particle off the boundary with a change in its momentum as defined by the coefficient of restitution. (See Figure  23.4.1.)

trap   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  23.4.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  23.4.3.

wall-jet   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  15.6.1TH-dpm-disp-bound-walljet in the separate Theory Guide.

wall-film   consists of four regimes: stick, rebound, spread, and splash, which are based on the impact energy and wall temperature. Detailed information on the wall-film model can be found in this section in the separate Theory Guide. The Number Of Splashed Drops must be specified.

user-defined   specifies a user-defined function to define the discrete phase boundary condition type.

Discrete Phase BC Function   sets the user-defined function from the drop-down list.

Multiphase   contains the multiphase parameters.

Volume Fraction   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 Section  24.2.9 for details.

Wave BC Options   allows you to choose between Shallow Waves or Short Gravity Waves. Information about the two types of waves is available in this section in the separate Theory Guide.

Secondary Phase for Inlet   is where the specified parameters are valid only for one secondary phase. In case of a three-phase flow, select the corresponding secondary phase from this list.

Wave Amplitude   is the amplitude of the shallow wave or short gravity wave.

Wave Length   is the wave length of the shallow wave or short gravity wave.

Free Surface Level   can be determined using the absolute value of height from the free surface to the origin in the direction of gravity, or by applying the correct sign based on whether the free surface level is above or below the origin.

Bottom Level   is valid only for shallow waves. The bottom level is used for calculating the liquid height.

Wave Heading Angle   

Phase Difference   is the phase difference between one wave and another.

UDS   contains the UDS parameters.

User-Defined Scalar Boundary Condition   appears only if user defines scalars are specified.

User Scalar-n   specifies the whether the scalar is a specified flux or a specified value.

User-Defined Scalar Boundary Value   appears only if user defines scalars are specified.

User Scalar-n   specifies the value of the scalar.