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

sets the gauge pressure at the outlet boundary.

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

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.

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.

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.

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.

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

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.

displays the turbulence parameters.

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

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 fan 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 fan.

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.

allows you to specify the species in mole fractions rather than mass fractions.

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.)

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.

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.

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

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

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.

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

sets the fan flow direction relative to the zone direction. If Zone Average Direction is pointing in the direction you want the fan to blow, do not select Reverse Flow; if it is pointing in the opposite direction, select Reverse Flow.

displays the (face-averaged) direction vector for the zone as an aid in determining whether or not you want to select Reverse Flow.

enables the use of a boundary profile or user-defined function for the pressure jump specification. See Profiles or the Fluent Customization Manual for details. When this option is enabled, Pressure Jump Profile will appear in the dialog box and the next four items below it will not.

contains a drop-down list from which you can select a boundary profile or a user-defined function for the pressure jump definition. This item will appear if you enable Profile Specification of Pressure-Jump.

specifies the pressure-jump as a constant value or as a polynomial, piecewise-linear, or piecewise-polynomial function of velocity. See Defining the Pressure Jump for details.

limits the minimum and maximum velocity magnitudes used to calculate the pressure jump when it is defined as a function of velocity.

specify the minimum and maximum values to which the velocity magnitude is limited (when the Limit Polynomial Velocity Range option is enabled).

enables the option to use the mass-averaged velocity normal to the fan to determine a single pressure-jump value for all faces in the fan zone.

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

sets the user-defined function from the drop-down list.

enables the specification of a swirl velocity for the fan.

sets the direction vector for the fan’s axis of rotation.

sets the origin in the global coordinate system through which the fan rotation axis passes.

set the radius of the hub. The default is 1e-6 to avoid division by zero in the polynomial.

enables the use of a boundary profile or user-defined function for the tangential velocity specification. See Profiles or the Fluent Customization Manual for details. When this option is enabled, Tangential Velocity Profile will appear in the dialog box and Tangential-Velocity Polynomial Coefficients will not.

contains a drop-down list from which you can select a boundary profile or a user-defined function for the definition of the tangential velocity. This item will appear if you enable Profile Specification of Tangential Velocity.

sets the coefficients for the tangential velocity polynomial. Separate the coefficients by spaces.

enables the use of a boundary profile or user-defined function for the radial velocity specification. See Profiles or the Fluent Customization Manual for details. When this option is enabled, Radial Velocity Profile will appear in the dialog box and Radial-Velocity Polynomial Coefficients will not.

contains a drop-down list from which you can select a boundary profile or a user-defined function for the definition of the radial velocity. This item will appear if you enable Profile Specification of Radial Velocity.

sets the coefficients for the radial velocity polynomial. Separate the coefficients by spaces.

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.

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.

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).

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.

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.

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.

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.

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.

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

lists the turbulence parameters.

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.

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 inlet vent 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 inlet vent.

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.

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.

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

sets the user-defined function from the drop-down list.

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

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.

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

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.

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.

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.

is used as an option for describing the flow. It is given by Equation 26–12.

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

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

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

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

specifies the reference frame for the intake fan. If the cell zone adjacent to the intake fan 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.

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.

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 intake fan boundary condition is selected for computing initial values (see Initializing the Entire Flow Field Using Standard Initialization).

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.

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

set the direction of the flow at the inlet boundary. For compressible flow, if the inflow becomes supersonic, the velocity is not reoriented. These items will appear if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

set the direction of the flow at the inlet boundary. For compressible flow, if the inflow becomes supersonic, the velocity is not reoriented. These items will appear for 2D axisymmetric cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

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

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.

consists of the turbulence parameters.

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.

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 intake fan 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 intake fan.

specifies whether or not the intake 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.

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.

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

sets the user-defined function from the drop-down list.

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

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.

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

specifies the reference frame for the mass flow. If the cell zone adjacent to the mass-flow inlet 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.

specifies whether you are defining Mass Flow Rate, Mass Flux, or Mass Flux with Average Mass Flux.

sets the prescribed mass flow rate for the zone. This flow rate is converted internally to a prescribed uniform mass flux over the zone by dividing the flow rate by the flow direction area projection of the zone. This item will appear if you selected Mass Flow Rate in the Mass Flow Specification Method list.

sets the prescribed mass flux for the zone. This item will appear if you selected Mass Flux or Mass Flux with Average Mass Flux in the Mass Flow Specification Method list.

sets the average mass flux through the zone. See More About Mass Flux and Average Mass Flux for details. This item will appear if you selected Mass Flux with Average Mass Flux in the Mass Flow Specification Method list.

sets the static pressure that will be used to initialize the flow field if the mass-flow inlet boundary condition is selected for initializing flow properties (see Initializing the Entire Flow Field Using Standard Initialization).

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.

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

set the velocity-direction vector of the inflow stream. This vector does not need to be normalized (for example, you can specify the vector (1 1 1) rather than (0.577 0.577 0.577)). These items will appear if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

set the velocity-direction vector of the inflow stream. These items will appear for 2D axisymmetric cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

appear for a 3D Local Cylindrical Swirl coordinate system.

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

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

contains the turbulence parameters.

contains settings for treatment of acoustic pressure waves at the boundary.

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.

sets the total temperature of the inflow stream.

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 mass-flow 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 mass-flow inlet.

specifies whether or not the mass-flow 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.

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.

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.

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.)

(partially-premixed combustion FGM model only) allows you to specify the scalar species mass fractions for the transported scalars that you selected in the Select Transported Scalars dialog box.

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

sets the user-defined function from the drop-down list.

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

specifies the reference frame for the mass flow when the cell zone adjacent to the mass-flow outlet is moving. The only available option is Relative to Adjacent Cell Zone, so you must define the mass flow relative to the adjacent cell zone.

specifies whether you are defining a Mass Flow Rate, Mass Flux, Mass Flux with Average Mass Flux, or (if the density of the material is defined either as an ideal gas or using a real gas model) Exit Corrected Mass Flow Rate.

sets the prescribed mass flow rate for the zone. This flow rate is converted internally to a prescribed uniform mass flux over the zone by dividing the flow rate by the flow direction area projection of the zone. This item will appear if you selected Mass Flow Rate from the Mass Flow Specification Method drop-down list.

sets the prescribed mass flux for the zone. This item will appear if you selected Mass Flux or Mass Flux with Average Mass Flux from the Mass Flow Specification Method drop-down list.

sets the average mass flux through the zone. For details, see Defining the Mass Flow Rate or Mass Flux. This item will appear if you selected Mass Flux with Average Mass Flux from the Mass Flow Specification Method drop-down list.

sets the value for an exit corrected mass flow rate that is maintained by adjusting the mass flow rate to the total conditions at the outlet. The resulting mass flow rate will be proportional to the exit total pressure and inversely proportional to the square root of the exit total temperature (or equivalently, inversely proportional to the stagnation speed of sound). For details, see Exit Corrected Mass Flow Rate. This item will appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow Specification Method drop-down list.

sets the reference temperature for the exit corrected mass flow rate; for details, see Exit Corrected Mass Flow Rate. Typically, it is set to be the same as the inflow total temperature. This item will appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow Specification Method drop-down list.

sets the reference gauge pressure for the exit corrected mass flow rate; for details, see Exit Corrected Mass Flow Rate. Typically, it is set to be the same as the inflow total pressure. This item will appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow Specification Method drop-down list.

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

set the velocity-direction vector of the outflow stream. This vector does not need to be normalized (for example, you can specify the vector (1 1 1) rather than (0.577 0.577 0.577)). These items will appear if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

set the velocity-direction vector of the outflow stream. These items will appear for 2D axisymmetric cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

appear for a 3D Local Cylindrical Swirl coordinate system.

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

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

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 mass-flow outlet 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 mass-flow outlet.

specifies whether or not the mass-flow outlet 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.

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

sets the user-defined function from the drop-down list.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

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

reports the particle as having "escaped" when it encounters the boundary. Trajectory calculations are terminated. See Figure 24.41: “Escape” Boundary Condition for the Discrete Phase.

reintroduces the particle into the domain when it reaches a certain domain boundary (for example, outlet). This item appears when one or more injections have been defined and Unsteady Particle Tracking is enabled in the Discrete Phase Model dialog box. See The reinject Boundary Condition for details.

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 12.6: "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.

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

sets the gauge pressure at the outlet boundary.

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 or From Neighboring Cell no inputs are required. See Defining the Flow Direction for information on specifying flow direction.

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.

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.

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.

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.

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

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.

contains the turbulence parameters.

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

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 outlet vent 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 outlet vent.

specifies whether or not the outlet 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.

allows you to specify the species in mole fractions rather than mass fractions.

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.)

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.

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.

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

sets the user-defined function from the drop-down list.

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

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.

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

constrains the contact angle at the porous jump, When this option is disabled then the forced two-sided adhesion treatment is in effect. See Jump Adhesion for more information.

is the contact angle at the porous jump.

allows the particles to pass through the boundary.

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

reports the particle as having "escaped" when it encounters the boundary. Trajectory calculations are terminated. See Figure 24.41: “Escape” Boundary Condition for the Discrete Phase.

reintroduces the particle into the domain when it reaches a certain domain boundary (for example, outlet). This item appears when one or more injections have been defined and Unsteady Particle Tracking is enabled in the Discrete Phase Model dialog box. See The reinject Boundary Condition for details.

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 12.6: "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.

specifies whether or not the porous jump participates in solar ray tracing.

contains the settings that define the absorptivity of the porous jump.

contains the settings that define the transmissivity of the porous jump.

sets the far-field gauge static pressure.

sets the far-field Mach number. The Mach number can be subsonic, sonic, or supersonic.

allows you to select a Cartesian, Cylindrical, or Local Cylindrical coordinate system. This option is available only for 3D geometry.

set the far-field flow direction. These items will appear if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

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

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.

contains the turbulence parameters.

sets the far-field static temperature.

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 pressure far-field zone 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 pressure far-field zone.

specifies whether or not the pressure far-field zone 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.

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.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

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

sets the user-defined function from the drop-down list.

specifies the reference frame for the pressure inlet. If the cell zone adjacent to the pressure inlet is moving, you can choose to specify the total temperature, total pressure, and velocity components as Relative to Adjacent CellZone or Absolute in the Reference Frame drop-down list.

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.

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 pressure inlet boundary condition is selected for computing initial values (see Initializing the Entire Flow Field Using Standard Initialization).

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. You also have the option to enable Prevent Reverse Flow. See Defining the Flow Direction for information on specifying flow direction.

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

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.

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.

appear for a 3D Local Cylindrical Swirl coordinate system.

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

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

Enables Fluent to erect artificial walls on the boundary mesh faces to prevent flow out of the domain. The artificial walls are removed when the flow is no longer leaving the domain and when a favorable pressure gradient is recovered at the boundary mesh faces.

contains parameters for Inlet Boundary Conditions for Scale Resolving Simulations (only available for transient cases where scale-resolving turbulence models such as SAS, DES, and LES are enabled).

contains the turbulence parameters.

contains settings for treatment of acoustic pressure waves at the boundary.

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.

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.

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 pressure 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 pressure inlet.

specifies whether or not the pressure 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.

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.

(partially-premixed combustion FGM model only) allows you to specify the scalar species mass fractions for the transported scalars that you selected in the Select Transported Scalars dialog box.

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

sets the user-defined function from the drop-down list.

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

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.

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

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

sets the gauge pressure at the outflow boundary.

sets a factor by which the Gauge Pressure is multiplied. This is provided mainly for cases where a non-uniform distribution of the static pressure at the pressure outlet boundary is specified by means of a profile file or a user-defined function.

sets the direction of the inflow stream should the flow reverse direction. If you choose Direction Vector, you will define the flow direction components, and if you choose Normal to Boundary or From Neighboring Cell, no inputs are required. You also have the option to enable Prevent Reverse Flow. See Inputs at Pressure Outlet Boundaries for information on specifying flow direction.

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.

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.

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.

specifies how the pressure is calculated under backflow conditions. When the NRBC option is not enabled, 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. For NRBCs, if you select Static Pressure, the Gauge Pressure is directly imposed as the pressure at infinity; if you select Total Pressure, the pressure at infinity is a calculated value that is based on the Gauge Pressure.

enables the radial equilibrium pressure distribution. See Defining Static Pressure for details.

This item appears only for 3D and axisymmetric swirl solvers.

allows the pressure along the outlet boundary to vary, but maintain an average equivalent to the specified value in the Gauge Pressure input field. In this boundary implementation, the pressure variation provides a low level of non-reflectivity. For more details, see Calculation Procedure at Pressure Outlet Boundaries.

allows you to set mass flow rate as a boundary condition at the outlet.

allows you to specify the flow as either a constant value or a user-defined function.

specifies the range of the pressure limits, which have different pressure variations on different boundaries. The upper and lower pressure limits can be specified as a constant or a profile.

contains the turbulence parameters.

contains settings for treatment of acoustic pressure waves at the boundary.

contains settings for the non-reflecting boundary condition treatment.

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.

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

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 pressure outlet 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 pressure outlet.

specifies whether or not the pressure outlet 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.

allows you to specify the species in mole fractions rather than mass fractions.

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.)

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.

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.

(partially-premixed combustion FGM model only) allows you to specify the scalar species mass fractions for the transported scalars that you selected in the Select Transported Scalars dialog box.

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

sets the user-defined function from the drop-down list.

specifies temperature for the solids phase and is proportional to the kinetic energy of the random motion of the particles. This option is available only for a granular phase with the Mixture and Eulerian multiphase models.

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. This control is not available for the open channel VOF submodel.

(VOF model only) enables the open-channel flow boundary condition. See Modeling Open Channel Flows for more information. This option is available only when the Open Channel VOF submodel is selected in the Multiphase Model dialog box. Once you select this option, you can specify the following conditions:

is a drop-down list of available potential boundary condition types for the potential generated by electron current: 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.

is a drop-down list of available boundary condition types for the potential generated by ionic current. This item is similar to the Potential Boundary Condition drop-down list described above and is available only for the Electrolysis and H2 Pump model.

appears only if user-defined scalars are specified.

appears only if user-defined scalars are specified.

allows the particles to pass through the boundary.

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

reports the particle as having "escaped" when it encounters the boundary. Trajectory calculations are terminated. See Figure 24.41: “Escape” Boundary Condition for the Discrete Phase.

reintroduces the particle into the domain when it reaches a certain domain boundary (for example, outlet). This item appears when one or more injections have been defined and Unsteady Particle Tracking is enabled in the Discrete Phase Model dialog box. See The reinject Boundary Condition for details.

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 12.6: "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 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.

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.

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.

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 parameters for Inlet Boundary Conditions for Scale Resolving Simulations (only available for transient cases where scale-resolving turbulence models such as SAS, DES, and LES are enabled).

contains the turbulence parameters.