37.8.5. Inlet Vent Dialog Box

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

Controls

Zone Name

sets the name of the zone.

Momentum

contains the momentum parameters.

Reference Frame

specifies the reference frame for the inlet vent. If the cell zone adjacent to the inlet vent is moving, you can choose to specify relative or absolute velocities by selecting Relative to Adjacent Cell Zone or Absolute in the Reference Frame drop-down list.

Gauge Total Pressure

sets the gauge total (or stagnation) pressure of the inflow stream. If you are using moving reference frames, see Defining Total Pressure and Temperature for information about relative and absolute total pressure.

Supersonic/Initial Gauge Pressure

sets the static pressure on the boundary when the flow becomes (locally) supersonic. It is also used to compute initial values for pressure, temperature, and velocity if the inlet vent boundary condition is selected for computing initial values (see Initializing the Entire Flow Field Using Standard Initialization).

Direction Specification Method

specifies the method you will use to define the flow direction. If you choose Direction Vector, you will define the flow direction components, and if you choose Normal to Boundary no inputs are required. See Defining the Flow Direction for information on specifying flow direction.

Coordinate System

specifies whether Cartesian, Cylindrical, Local Cylindrical, Local Cylindrical Swirl vector components will be specified. This item will appear only for 3D cases in which you have selected Direction Vector as the Direction Specification Method.

X,Y,Z-Component of Flow Direction

set the direction of the flow at the inlet boundary. These items will appear if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

Radial, Tangential, Axial Component of Flow Direction

set the direction of the flow at the inlet boundary. These items will appear for 2D axisymmetric cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

Axis Origin

sets the X, Y, and Z coordinates of the origin of the local cylindrical coordinate system.

Axis Direction

sets the X, Y, and Z components of the direction of the local cylindrical coordinate system.

Loss-Coefficient

sets the non-dimensional loss coefficient used to compute the pressure drop. See Specifying the Loss Coefficient for details.

Turbulence

lists the turbulence parameters.

Specification Method

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.)

Turbulent Kinetic Energy, Turbulent Dissipation Rate

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.

Turbulent Kinetic Energy, Specific Dissipation Rate

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.

Turbulence Intensity, Turbulence Length Scale

set values for turbulence intensity and turbulence length scale . These items will appear if you choose Intensity and Length Scale as the Specification Method.

Turbulence Intensity, Turbulent Viscosity Ratio

set values for turbulence intensity and turbulent viscosity ratio . These items will appear if you choose Intensity and Viscosity Ratio as the Specification Method.

Turbulence Intensity, Hydraulic Diameter

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

Modified Turbulent Viscosity

sets the value of the modified turbulent viscosity . This item will appear if you choose Modified Turbulent Viscosity as the Specification Method.

Turbulent Viscosity Ratio

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

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 Reynolds Stress Model 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.

Total Temperature

sets the total temperature of the inflow stream. If you are using moving reference frames, see Defining Total Pressure and Temperature for information about relative and absolute total temperature.

Radiation

contains the radiation parameters.

External Black Body Temperature Method, Internal Emissivity

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.

Participates in Solar Ray Tracing

specifies whether or not the inlet vent participates in solar ray tracing.

Solar Transmissivity Factor

specifies a multiplier (ranging from 0 to 1) that is applied to the solar irradiation entering the domain through the inlet vent.

Participates in View Factor Calculation

specifies whether or not the inlet vent 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.

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 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.)

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 Setting Boundary Conditions for the Progress Variable 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 Particle Reflection at Wall in the Fluent Theory Guide.)

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 23.25: “Trap” Boundary Condition for the Discrete Phase.

escape

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.

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 16.6: “Wall Jet” Boundary Condition for the Discrete Phase in the Theory Guide.

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.

Granular Temperature

specifies temperature for the solids phase and is proportional to the kinetic energy of the random motion of the particles.

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 Defining Multiphase Cell Zone and Boundary Conditions for details.

Open Channel

is available when the VOF model with open channel flow is enabled.

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. This appears when Open Channel is enabled.

Flow Specification Method

allows you to select the type of flow. You can choose Free Surface Level and Velocity, Total Height and Velocity, or Free Surface Level and Total Height. This appears when Open Channel is enabled.

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.

Total Height

is used as an option for describing the flow. It is given by Equation 24–4.

Bottom Level

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

Velocity Magnitude

sets the magnitude of the velocity vector at the inflow boundary.

Level-Set Function Flux

appears if the Level Set option is enabled for the VOF model.

Potential

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.

Potential Boundary Condition

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.

UDS

contains the UDS parameters.

User-Defined Scalar Boundary Condition

appears only if user-defined scalars are specified.

User Scalar n

specifies whether the scalar is a specified flux or a specified value.

User-Defined Scalar Boundary Value

appears only if user-defined scalars are specified.

User Scalar n

specifies the value of the scalar.


Release 18.2 - © ANSYS, Inc. All rights reserved.