37.8.3. Exhaust Fan Dialog Box

The Exhaust Fan dialog box sets the boundary conditions for an exhaust fan zone. It is opened from the Boundary Conditions Task Page. See Inputs at Exhaust Fan Boundaries for details about defining the items below.

Controls

Zone Name

sets the name of the zone.

Phase

displays the name of the phase. It appears only for multiphase flows.

Momentum

contains the momentum parameters.

Backflow Reference Frame

specify whether backflow temperature, pressure, and flow directions are in the Absolute or Relative to the Adjacent Cell Zone reference frame.

Gauge Pressure

sets the gauge pressure at the outlet boundary.

Backflow Direction Specification Method

sets the direction of the inflow stream should the flow reverse direction. You can choose Direction Vector, Normal to Boundary,or From Neighboring Cell.

Coordinate System

contains a drop-down list for selecting the coordinate system. You can choose Cartesian, Cylindrical, or Local Cylindrical. This option is available only when Direction Vector is selected from the Backflow Direction Specification Method drop-down list.

X-, Y-, Z-Component of Flow Direction

allows you to specify the velocity components in x, y, and z directions respectively. This option is available when Cartesian is selected for the Coordinate System.

Radial-, Tangential-, Axial-Component of Flow Direction

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

Backflow Pressure Specification

specifies how the pressure is calculated under backflow conditions. If you select Static Pressure, the Gauge Pressure is directly imposed as the boundary face pressure; if you select Total Pressure, the Gauge Pressure will be combined with a dynamic contribution that is based on the velocity in the adjacent cell zone.

Pressure Jump

specifies the rise in pressure across the fan. See Specifying the Pressure Jump for details.

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.

Turbulence

displays 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.)

Backflow Turbulent Kinetic Energy, Backflow 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.

Backflow Turbulent Kinetic Energy, Backflow Specification 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.

Backflow Turbulent Intensity, Backflow Turbulent 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.

Backflow Turbulent Intensity, Backflow 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.

Backflow Turbulent Intensity, Backflow 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.

Backflow Modified Turbulent Viscosity

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

Backflow Turbulent Viscosity Ratio

sets the value of the backflow 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 backflow 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.)

Backflow UU, VV, WW, UV, VW, UW Reynolds Stresses

specify the backflow Reynolds stress components when Reynolds-Stress Components is chosen as the Reynolds-Stress Specification Method.

Thermal

contains the thermal parameters. This parameter is available only when the energy equation is turned on.

Backflow Total Temperature

sets the total temperature of the inflow stream should the flow reverse direction.

Radiation

contains the boundary conditions for the radiation model at the exhaust fan.

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 fan 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 fan.

Participates in View Factor Calculation

specifies whether or not the fan 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.

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.)

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.

Backflow 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. This tab is available only if you have defined at least one injection.

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.

Backflow Granular Temperature

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

Volume Fraction Specification Method

sets the method used to specify 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.

Backflow Volume Fraction

specifies the volume fraction of the secondary phase as a constant, profile, of UDF function.

From Neighboring Cell

calculates the volume fraction from the neighboring cells.

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.