[Fluent Inc. Logo] return to home search
next up previous contents index

32.3.18 Define/Boundary Conditions...

The Define/Boundary Conditions... menu item opens the Boundary Conditions panel.



Boundary Conditions Panel


The Boundary Conditions panel allows you to set the type of a zone and display other panels to set the boundary condition parameters for each zone. See Section  here for information about using it.

figure

Controls

Zone   contains a selectable list of zones from which you can select the zone of interest. You can check a zone type by using the mouse probe (see Section  28.3) on the displayed physical grid. This feature is particularly handy if you are setting up a problem for the first time, or if you have two or more zones of the same type and you want to determine the zone IDs. To do this you must first display the grid with the Grid Display panel. Then click the boundary zone with the right (select) mouse button. FLUENT will print the zone ID and type of that boundary zone in the console window.

Type   contains a selectable list of boundary condition types for the selected zone. The list contains all possible types to which the zone can be changed. When you select a boundary condition type in Type, Set... is automatically invoked.

figure   

Note that you cannot use this method to change zone types to or from the periodic type, since additional restrictions exist for this boundary type. Section  6.8.4 explains how to create and uncouple periodic zones.

Phase   specifies the phase for which conditions at the selected boundary Zone are being set. This item appears if the VOF, mixture, or Eulerian multiphase model is being used. See Section  23.9.8 for details.

ID   displays the zone ID number of the selected zone. (This is for informational purposes only; you cannot edit this number.)

Set...   opens the appropriate panel for setting the boundary conditions for that particular boundary type.

Copy...   opens the Copy BCs panel, which allows you to copy boundary conditions from one zone to other zones of the same type. See Section  7.1.5 for details.



Copy BCs Panel


The Copy BCs panel allows you to copy boundary conditions from one zone to other zones of the same type. It is opened from the Boundary Conditions panel. See Section  7.1.5 for details.

figure

Controls

From Zone   specifies the zone that has the conditions you want to copy.

To Zones   specifies the zone or zones to which you want to copy the conditions.

Phase   specifies the phase for which boundary conditions are being copied. This item appears if the VOF, mixture, or Eulerian multiphase model is being used. See Section  23.9.8 for details.

Copy   copies the boundary conditions, setting all of the boundary conditions for the zones selected in the To Zones list to be the same as the conditions for the zone selected in the From Zone list.



Axis Panel


The Axis panel can be used to modify the name of an axis zone; there are no conditions to be set. It is opened from the Boundary Conditions panel. See Section  7.16 for information about axis boundaries.

figure

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.



Exhaust Fan Panel


The Exhaust Fan panel sets the boundary conditions for an exhaust fan zone. It is opened from the Boundary Conditions panel. See Section  7.12.1 for details about defining the items below.

figure

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.

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 for Direction Vector.

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 for cartesian coordinate system.

Radial Equilibrium Pressure Distribution   enables the radial equilibrium pressure distribution. See Section  7.8.1 for details.

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

Pressure Jump   specifies the rise in pressure across the fan. See Section  7.12.1 for details.

Target Mass Flow Rate   allows you to set mass flow rate as a boundary condition at the outlet.

Turbulence   displays 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  7.2.2 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 $k$ and its dissipation rate $\epsilon$. 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 $k$ and its specific dissipation rate $\omega$. These items will appear if you choose K and Omega as the Specification Method.

Backflow Turbulence Intensity, Backflow Turbulence 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulent Viscosity Ratio   sets the value of the backflow turbulent viscosity ratio $\mu_t/\mu$. 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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Participates in S2S Radiation   specifies whether or not fan participate in S2S radiation. This parameter is available only if you select Surface to Surface radiation model.

Participates in Solar Ray Tracing   specifies whether or not fan 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  13.3.15 for details.

Species   contains the species parameters.

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 Section  14.1.5 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.

Backflow Progress Variable   sets the value of the progress variable for premixed turbulent combustion. See Section  16.3.5 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 atleast 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 Figure  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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

Backflow Volume Fraction   specifies the volume fraction of the secondary phase selected in the Boundary Conditions panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.


Fan Panel

The Fan panel sets the boundary conditions for a fan zone. It is opened from the Boundary Conditions panel. See Section  7.20.2 for details about the items below.

figure

Controls

Zone Name   sets the name of the zone.

Pressure-Jump Specification   contains inputs that define the pressure jump across the fan.

Reverse Fan Direction   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.

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

Profile Specification of Pressure-Jump   enables the use of a boundary profile or user-defined function for the pressure jump specification. See Section  7.26 or the separate UDF Manual for details. When this option is enabled, Pressure Jump Profile will appear in the panel and the next four items below it will not.

Pressure Jump Profile   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.

Pressure-Jump   specifies the pressure-jump as a constant value or as a polynomial, piecewise-linear, or piecewise-polynomial function of velocity. See Section  7.20.2 for details.

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

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

Calculate Pressure-Jump from Average Conditions   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.

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  22.13.1.)

trap   terminates the trajectory calculations and records the fate of the particle a s "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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

Swirl-Velocity Specification   contains inputs for the specification of fan swirl velocity. This section of the panel appears only for 3D models.

Swirl-Velocity Specification   enables the specification of a swirl velocity for the fan.

Fan Axis   sets the direction vector for the fan's axis of rotation.

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

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

Profile Specification of Tangential Velocity   enables the use of a boundary profile or user-defined function for the tangential velocity specification. See Section  7.26 or the separate UDF Manual for details. When this option is enabled, Tangential Velocity Profile will appear in the panel and Tangential-Velocity Polynomial Coefficients will not.

Tangential Velocity Profile   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.

Tangential-Velocity Polynomial Coefficients   sets the coefficients for the tangential velocity polynomial. Separate the coefficients by spaces.

Profile Specification of Radial Velocity   enables the use of a boundary profile or user-defined function for the radial velocity specification. See Section  7.26 or the separate UDF Manual for details. When this option is enabled, Radial Velocity Profile will appear in the panel and Radial-Velocity Polynomial Coefficients will not.

Radial Velocity Profile   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.

Radial-Velocity Polynomial Coefficients   sets the coefficients for the radial velocity polynomial. Separate the coefficients by spaces.



Fluid Panel


The Fluid panel sets the conditions for a fluid cell zone. It is opened from the Boundary Conditions panel. See Sections  7.17.1 and 7.19.6 for details about the items below.

figure

Controls

Zone Name   sets the name of the zone.

Material Name   sets the fluid material. The drop-down list contains the names of all materials that have been loaded into the solver. Materials are defined with the Materials panel.

figure   

If you are modeling species transport or multiphase flow, the Material Name list will not appear in the Fluid panel. For species calculations, the mixture material for all fluid zones will be the material you specified in the Species Model panel. For multiphase flows, the materials are specified when you define the phases, as described in Section  23.10.3.

Porous Zone   indicates that the zone is a porous medium. Additional items will appear in the panel when this option is enabled. See Section  7.19.6 for details.

Laminar Zone   disables the calculation of turbulence production

in the fluid zone (appears only for turbulent flow calculations using the Spalart-Allmaras model or one of the $k$- $\epsilon$ or $k$- $\omega$ models). See Section  7.17.1 for details.

Source Terms   enables the specification of volumetric sources of mass, momentum, energy, etc. When you turn on this option, the Source Terms tab will be enabled to allow you to input the values for the desired sources. See Section  7.28 for details.

Fixed Values   enables the fixing of the value of one or more variables in the fluid zone, rather than computing them during the calculation. See Section  7.27 for details.

figure   

You can fix values for velocity components, temperature, and species mass fractions only if you are using the pressure-based solver.

Participates In Radiation   specifies whether or not the fluid zone participates in radiation. This option appears when you are using the DO model for radiation.

Reaction   enables/disables reactions in the porous zone.

Motion   lists the parameters associated to the fluid motion.

Rotation-Axis Origin   specifies the origin for the fluid zone's axis of rotation. See Section  7.17.1 for details. This item will appear only for 3D and 2D non-axisymmetric models.

Rotation-Axis Direction   specifies the direction vector for the fluid zone's axis of rotation. See Section  7.17.1 for details. This item will appear only for 3D.

Motion Type   specifies zone motion for a rotating or translating reference frame or for a sliding zone in a sliding mesh problem. The default selection of Stationary indicates that the zone is not moving. To define the motion of a moving reference frame for the zone, select Moving Reference Frame and specify the items below in the expanded portion of the panel. See Section  10.7, 10.10.1, or 10.10.2 for details. To define zone motion for a moving (sliding) mesh, select Moving Mesh and set the appropriate parameters below. See Section  11.4.2 for details.

Rotational Velocity   contains an input field for the rotational Speed of the zone. This item will appear if you select Moving Reference Frame or Moving Mesh in the Motion Type list.

Translational Velocity   contains inputs for the X, Y, and Z velocities of the zone. This item will appear if you select Moving Reference Frame or Moving Mesh in the Motion Type list.

Porous Zone   lists the parameters associated to porous zone.

Conical   enables the specification of a conical (or cylindrical) porous medium. This item will appear only when the Porous Zone option is enabled for a 3D case.

Cone Half Angle   specifies the angle between the cone's axis and its surface (see Figure  7.19.2). Set this to 0 to define the porous region using a cylindrical coordinate system. This item will appear only when the Porous Zone and Conical options are enabled.

Snap to Zone   aligns the plane (or line, in 2D) tool with the zone selected in the drop-down list. The tool is centered at the centroid of the zone, with the tool's axis normal to the zone. If this axis is not the desired cone axis, reposition the tool (as described in Section  27.6.1). When you are satisfied with the axis, click on the Update From Plane Tool (or Update From Line Tool) button to update the Cone Axis Vector fields.

This item will appear only when the Porous Zone and Conical options are enabled.

Update From Plane Tool   ( Update From Line Tool in 2D) updates the Direction-1 Vector and (in 3D) the Direction-2 Vector from the plane tool orientation. If the Conical option is enabled, this button will update the Cone Axis Vector and the Point on Cone Axis. See Section  7.19.6 for details. This item will appear only when the Porous Zone option is enabled.

Direction-1 Vector, Direction-2 Vector   indicate the directions for which the resistance coefficients are defined. See Section  7.19.6 for details. These items will appear only when the Porous Zone option is enabled, but the Conical option is not. (In 2D, only Direction-1 Vector will appear.)

Cone Axis Vector   specifies the X,Y,Z vector for the cone's axis.

This item will appear only when the Porous Zone and Conical options are enabled.

Point on Cone Axis   specifies a point on the cone's axis. This point will be used by FLUENT to transform the resistances to the Cartesian coordinate system.

This item will appear only when the Porous Zone and Conical options are enabled.

Viscous Resistance, Inertial Resistance   contain inputs for the viscous resistance coefficient $1/\alpha$ and the inertial resistance coefficient $C2$ in each direction. See Section  7.19.6 for details. These items will appear only when the Porous Zone option is enabled.

If you have enabled the Conical option, Direction-1 is the cone axis direction, Direction-2 is the normal to the cone surface (radial ( $r$) direction for a cylinder), and Direction-3 is the circumferential ( $\theta$) direction.

Power Law Model   contains inputs for the C0 and C1 coefficients in the power law model for porous media. See Section  7.19.6 for details.

Fluid Porosity   contains additional inputs for the porous medium. See Section  7.19.6 for details.

Porosity   sets the volume fraction of fluid within the porous region.

Solid Material Name   specifies the solid material in the porous region.

Reaction   lists the parameters for reactions in the porous zone.

Reaction Mechanism   allows you to specify a defined group, or mechanism, of available reactions. See Section  14.1.4 for details about defining reaction mechanisms.

Surface-to-Volume Ratio   specifies the surface area of the pore walls per unit volume ( $\frac{A}{V}$), and can be thought of as a measure of catalyst loading. With this value, FLUENT can calculate the total surface area on which the reaction takes place in each cell by multiplying $\frac{A}{V}$ by the volume of the cell.

Fixed Values   lists the fixed parameters of the fluid zone.
Local Coordinate System For Fixed Velocities   enables the specification of fixed cylindrical velocity components instead of Cartesian components. The local coordinate system is defined by the Rotation-Axis Origin and Rotation-Axis Direction.

This item is available only in 3D, and only when the Fixed Values option is on.



Inlet Vent Panel


The Inlet Vent panel sets the boundary conditions for an inlet vent zone. It is opened from the Boundary Conditions panel. See Section  7.6.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Total Pressure   sets the gauge total (or stagnation) pressure of the inflow stream. If you are using moving reference frames, see Section  7.3.1 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 Section  25.14.1).

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 Section  7.3.1 for information on specifying flow direction.

Coordinate System   specifies whether Cartesian, Cylindrical, or Local Cylindrical vector components will be input. 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.

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.

Loss-Coefficient   sets the nondimensional loss coefficient used to compute the pressure drop. See Section  7.6.1 for details.

Tubulence   lists 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  7.2.2 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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.

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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Total Temperature   sets the total temperature of the inflow stream. If you are using moving reference frames, see Section  7.3.1 for information about relative and absolute total temperature.

Radiation   contains the radiation parameters.

Participates in Solar Ray Tracing   specifies whether or not inlet vent 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  13.3.15 for details.

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.
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 panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.


Intake Fan Panel

The Intake Fan panel sets the boundary conditions for an intake fan zone. It is opened from the Boundary Conditions panel. See Section  7.7.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Total Pressure   sets the gauge total (or stagnation) pressure of the inflow stream. If you are using moving reference frames, see Section  7.3.1 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 intake fan boundary condition is selected for computing initial values (see Section  25.14.1).

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 Section  7.3.1 for information on specifying flow direction.

Coordinate System   specifies whether Cartesian, Cylindrical, or Local Cylindrical vector components will be input. 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. 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.

Radial, Tangential, Axial Component of Flow Direction   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.

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.

Pressure-Jump   specifies the rise in pressure across the fan. See Section  7.7.1 for details.

Turbulence   consists of 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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Turbulence Kinetic Energy, Turbulence 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.

Turbulence 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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.

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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Total Temperature   sets the total temperature of the inflow stream. If you are using moving reference frames, see Section  7.3.1 for information about relative and absolute total temperature.

Radiation   contains the radiation parameters.

Participates in Solar Ray Tracing   specifies whether or not intake-fan 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  13.3.15 for details.

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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 panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.



interface Panel


The interface panel can be used to modify the name of an interface zone; there are no conditions to be set. It is opened from the Boundary Conditions panel. Interface zones are used for multiple reference frame and sliding mesh calculations, and for non-conformal grids. See Section  10.3.1, 11.2, and 6.4 for details.

figure

Controls

Zone Name   sets the name of the zone.

Phase   displays the name of the phase. This item appears only for multiphase flows.



interior Panel


The interior panel can be used to modify the name of an interior zone; there are no conditions to be set. It is opened from the Boundary Conditions panel.

figure

Controls

Zone Name   sets the name of the zone.

Phase   displays the name of the phase. This item appears only for multiphase flows.



Mass-Flow Inlet Panel


The Mass-Flow Inlet panel sets the boundary conditions for a mass-flow inlet zone. It is opened from the Boundary Conditions panel. See Section  7.5.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   displays the momentum boundary conditions.

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

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 in the Mass Flow Specification Method list.

figure   

Note that for axisymmetric problems, this mass flow rate is the flow rate through the entire ( $2\pi$-radian) domain, not through a 1-radian slice.

Mass Flux   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.

figure   

Note that for axisymmetric problems, this mass flux is the flux through a 1-radian slice of the domain.

Average Mass Flux   sets the average mass flux through the zone. See Section  7.5.1 for details. This item will appear if you selected Mass Flux with Average Mass Flux in the Mass Flow Specification Method list.

figure   

Note that for axisymmetric problems, this mass flux is the flux through a 1-radian slice of the domain.

Supersonic/Initialization Gauge Pressure   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 Section  25.14.1).

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 Section  7.3.1 for information on specifying flow direction.

Reference Frame   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.

Coordinate System   specifies whether Cartesian, Cylindrical, or Local Cylindrical vector components will be input. 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 velocity-direction vector of the inflow stream. This vector does not need to be normalized (e.g., 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.

Radial, Tangential, Axial Component of Flow Direction   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.

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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Turbulence Kinetic Energy, Turbulence 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.

Turbulence 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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.

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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Total Temperature   sets the total temperature of the inflow stream.

Radiation   contains the radiation parameters.
Participates in Solar Ray Tracing   specifies whether or not mass-flow 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  13.3.15 for details.

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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.

Progress Variable   sets the value of the progress variable for premixed turbulent combustion. See Section  16.3.5 for details.

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

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.)

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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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.



Outflow Panel


The Outflow panel sets the boundary conditions for an outflow zone. It is opened from the Boundary Conditions panel. See Section  7.10.2 for details about using outflow boundaries.

figure

Controls

Zone Name   sets the name of the zone.

Flow Rate Weighting   specifies the portion of the outflow that is going through the boundary. See Section  7.10.3 for details.

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  13.3.15 for details.

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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. The Number Of Splashed Drops must be specified.

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

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

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



Outlet Vent Panel


The Outlet Vent panel sets the boundary conditions for an outlet vent zone. It is opened from the Boundary Conditions panel. See Section  7.11.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Pressure   sets the gauge pressure at the outlet boundary.

Radial Equilibrium Pressure Distribution   enables the radial equilibrium pressure distribution. See Section  7.8.1 for details.

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

Backflow 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 or From Neighboring Cell no inputs are required. See Section  7.3.1 for information on specifying flow direction.

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

Loss-Coefficient   sets the nondimensional loss coefficient used to compute the pressure drop. See Section  7.11.1 for details.

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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Backflow Turbulence Kinetic Energy, Backflow Turbulence 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.

Backflow Turbulence Kinetic Energy, Backflow 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.

Backflow Turbulence Intensity, Backflow Turbulence 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulent Viscosity Ratio   sets the value of the backflow turbulent viscosity ratio $\mu_t/\mu$. 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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Backflow Total Temperature   sets the total temperature of the inflow stream should the flow reverse direction

Radiation   contains the radiation parameters.

Participates in Solar Ray Tracing   specifies whether or not outlet vent 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  13.3.15 for details.

Species   contains the species parameters.

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 Section  14.1.5 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.

Backflow Progress Variable   sets the value of the progress variable for premixed turbulent combustion. See Section  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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

Backflow Volume Fraction   specifies the volume fraction of the secondary phase selected in the Boundary Conditions panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.



Periodic Panel


The Periodic panel sets the boundary conditions for a periodic zone. It is opened from the Boundary Conditions panel. See Section  7.15.2 for details about the items below. See Section  9.4 for information about fully-developed periodic flow.

figure

Controls

Zone Name   sets the name of the zone.

Periodic Type   indicates whether the periodicity of the domain is Translational or Rotational.

Periodic Pressure Jump   sets the pressure increase/decrease across the periodic boundary. (This item will not appear if the pressure-based (default) solver is used; it is relevant only for the density-based solvers.)



Porous Jump Panel


The Porous Jump panel sets the boundary conditions for a porous-jump zone. It is opened from the Boundary Conditions panel. See Section  7.22 for details about the items below.

figure

Controls

Zone Name   sets the name of the zone.

Face Permeability   sets the face permeability coefficient ( $\alpha$ in Equation  7.22-1).

Porous Medium Thickness   sets the thickness of the porous medium ( $\Delta m$).

Pressure-Jump Coefficient   sets the pressure-jump coefficient ( $C_2$).

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.

interior   allows the particles to pass through the boundary.

reflect   rebounds the particle off the boundary with a change in its momentum as defined by the coefficient of restitution. (See Figure  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.



Pressure Far-Field Panel


The Pressure Far-Field panel sets the boundary conditions for a pressure far-field zone. It is opened from the Boundary Conditions panel. See Section  7.9.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Pressure   sets the far-field gauge static pressure.

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

X,Y,Z-Component of Flow-Direction   set the far-field flow direction. 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 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.

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  7.2.2 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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 Turbulence 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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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   sets the far-field static 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 model, the DTRM, the discrete ordinates model, or the S2S model for radiation heat transfer. See Section  13.3.15 for details.

Participates in Solar Ray Tracing   specifies whether or not pressure far-field participate in solar ray tracing.

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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  16.3.5 for details.

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

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.

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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.



Pressure Inlet Panel


The Pressure Inlet panel sets the boundary conditions for a pressure inlet zone. It is opened from the Boundary Conditions panel. See Section  7.3.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Total Pressure   sets the gauge total (or stagnation) pressure of the inflow stream. If you are using moving reference frames, see Section  7.3.1 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 pressure inlet boundary condition is selected for computing initial values (see Section  25.14.1).

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 Section  7.3.1 for information on specifying flow direction.

Coordinate System   specifies whether Cartesian, Cylindrical, or Local Cylindrical vector components will be input. 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.

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.

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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Turbulence Kinetic Energy, Turbulence 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.

Turbulence 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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.

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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Total Temperature   sets the total temperature of the inflow stream. If you are using moving reference frames, see Section  7.3.1 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 model, the DTRM, the discrete ordinates model, or the S2S model for radiation heat transfer. See Section  13.3.15 for details.

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

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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 panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.



Pressure Outlet Panel


The Pressure Outlet panel sets the boundary conditions for a pressure outlet zone. It is opened from the Boundary Conditions panel. See Section  7.8.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.

Gauge Pressure   sets the gauge pressure at the outflow boundary.

Radial Equilibrium Pressure Distribution   enables the radial equilibrium pressure distribution. See Section  7.8.1 for details.

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

Backflow Direction Specification Method   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. See Section  7.8.1 for information on specifying flow direction.

Target Mass Flow Rate   allows you to set mass flow rate as a boundary condition at the outlet.

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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Backflow Turbulence Kinetic Energy, Backflow Turbulence 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.

Backflow Turbulence Kinetic Energy, Backflow 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.

Backflow Turbulence Intensity, Backflow Turbulence 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulence Intensity, Backflow 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.

Backflow Turbulent Viscosity Ratio   sets the value of the backflow turbulent viscosity ratio $\mu_t/\mu$. 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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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.

Backflow Total Temperature   sets the total temperature of the inflow stream should the flow reverse direction

Radiation   contains the radiation parameters.

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  13.3.15 for details.

Participates in Solar Ray Tracing   specifies whether or not pressure outlet participate in solar ray tracing.

Species   contains the species parameters.

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 Section  14.1.5 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.

Backflow Progress Variable   sets the value of the progress variable for premixed turbulent combustion. See Section  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.

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

Backflow Volume Fraction   specifies the volume fraction of the secondary phase selected in the Boundary Conditions panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.



Radiator Panel


The Radiator panel sets the boundary conditions for a radiator model zone. It is opened from the Boundary Conditions panel. See Section  7.21.2 for details about the items below.

figure

Controls

Zone Name   sets the name of the zone.

Loss Coefficient   specifies the loss coefficient as a constant value or as a polynomial, piecewise-linear, or piecewise-polynomial function of velocity. See Section  7.21.2 for details.

Heat Transfer Coefficient   specifies the heat-transfer coefficient as a constant value or as a polynomial, piecewise-linear, or piecewise-polynomial function of velocity. See Section  7.21.2 for details.

Temperature   sets the temperature used to compute heat flux from the radiator using the Heat-Transfer-Coefficient. If Temperature is zero, the Heat Flux condition is used instead.

Heat Flux   sets the heat flux at the radiator surface (used only when Temperature is zero).

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.

interior   allows the particles to pass through the boundary.

reflect   rebounds the particle off the boundary with a change in its momentum as defined by the coefficient of restitution. (See Figure  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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.



Solid Panel


The Solid panel sets the boundary conditions for a solid cell zone. It is opened from the Boundary Conditions panel. See Section  7.18.1 for details about the items below.

figure

Controls

Zone Name   sets the name of the zone.

Material Name   selects the material type of the solid. Materials are defined with the Materials panel.

Source Terms   enables the specification of a volumetric source of energy. When you turn on this option, the Source Term tab will allow you to input the value for the energy source. See Section  7.28 for details.

Fixed Values   enables the fixing of the value of temperature in the solid zone, rather than computing it during the calculation. See Section  7.27 for details.

figure   

You can fix the value of temperature only if you are using the pressure-based solver.

Participates In Radiation   specifies whether or not the solid zone participates in radiation. This option appears when you are using the DO model for radiation.

Motion   lists the parameters that define motion.

Rotation-Axis Origin   specifies the origin for the axis of rotation of solid zone. See Section  7.18.1 for details. This item will appear only for 3D and 2D non-axisymmetric models.

Rotation-Axis Direction   specifies the direction vector for the solid zone's axis of rotation. See Section  7.18.1 for details. This item will appear only for 3D models.

Motion Type   specifies zone motion for a rotating or translating reference frame or for a sliding zone in a sliding mesh problem. The default selection of Stationary indicates that the zone is not moving. To define the motion of a moving reference frame for the zone, select Moving Reference Frame and specify the items below in the expanded portion of the panel. See Section  10.7 10.10.1, or 10.10.2 for details. To define zone motion for a moving (sliding) mesh, select Moving Mesh and set the appropriate parameters below. See Section  11.4.2 for details.

Rotational Velocity   contains an input field for the rotational Speed of the zone. This item will appear if you select Moving Reference Frame or Moving Mesh in the Motion Type list.

Translational Velocity   contains inputs for the X, Y, and Z velocities of the zone. This item will appear if you select Moving Reference Frame or Moving Mesh in the Motion Type list.

Source Term   lists the parameters for volumetric source of energy.

Energy   displays the total number of energy sources used.

User Scalar n   displays the total number of scalars used.

Fixed Values   lists the parameters that can be declared as fixed during the calculation.

Temperature   specifies the fixed value for temperature.

User Scalar n   specifies the fixed value for user scalar.



Symmetry Panel


The Symmetry panel can be used to modify the name of a symmetry zone; there are no conditions to be set. It is opened from the Boundary Conditions panel. See Section  7.14 for information about symmetry boundaries.

figure

Controls

Zone Name   sets the name of the zone.

Phase   displays the name of the phase. This item is available only for multiphase flows.



Velocity Inlet Panel


The Velocity Inlet panel sets the boundary conditions for a velocity inlet zone. It is opened from the Boundary Conditions panel. See Section  7.4.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Momentum   contains the momentum parameters.
Velocity Specification Method   sets the method used to define the inflow velocity.

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.

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.

figure   

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.

figure   

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  7.2.2 for information about the inputs for each of these methods. (This item will appear only for turbulent flow calculations.)

Turbulence Kinetic Energy, Turbulence 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.

Turbulence 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.

Turbulence Intensity, Turbulence 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.

Turbulence 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.

Turbulence 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.

Turbulence 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, FLUENT will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Section  12.20.3 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  13.3.15 for details.

Species   contains the species parameters.

Species Mass Fractions   contains inputs for the mass fractions of defined species. See Section  14.1.5 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  16.3.5 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  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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  22.13.4.

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 Section  22.4. 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 panel. This section of the panel will appear when one of the multiphase models is being used. See Section  23.9.8 for details.

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.



Wall Panel


The Wall panel sets the boundary conditions for a wall zone. It is opened from the Boundary Conditions panel. See Section  7.13.1 for details about defining the items below.

figure

Controls

Zone Name   sets the name of the zone.

Adjacent Cell Zone   shows the name of the cell zone adjacent to the wall. (This is for informational use only; you cannot edit this field.)

Momentum   displays the momentum boundary conditions.

Wall Motion   contains options for specifying whether or not the wall is moving.

Stationary Wall   specifies that the wall is not moving relative to the adjacent cell zone.

Moving Wall   enables specification of the tangential wall motion. Tangential wall motion is applicable only to viscous flows. Since the inviscid slip condition decouples the tangential wall velocity from the governing equations, tangential wall motion has no effect on inviscid flow.

Motion   contains inputs related to wall motion. See Section  7.13.1 for details.

Relative to Adjacent Cell Zone   enables the specification of a wall velocity relative to the velocity of the adjacent cell zone. (If the adjacent cell zone is not moving, this is equivalent to Absolute.)

Absolute   enables the specification of an absolute wall velocity,

Translational   enables the specification of a translational wall velocity.

Rotational   enables the specification of a rotational wall velocity.

Components   enables the specification of wall velocity components.

Speed   sets the translational or rotational speed of the wall (depending on whether you selected Translational or Rotational).

Direction   sets the direction vector of the translational velocity. (This item will appear if you have chosen the Translational option.)

Rotation-Axis Origin   sets the coordinates of the origin of the axis of rotation, thereby determining the location of the axis. (This item will appear if you have chosen the Rotational option for a non-axisymmetric case.)

Rotation-Axis Direction   sets the direction vector for the axis of rotation. (This item will appear if you have chosen the Rotational option for a non-axisymmetric case.)

Velocity Components   sets the X, Y, and Z-Velocity components of the wall motion. (This item will appear if you have chosen the Components option.)

Shear Condition   contains options for specifying the shear conditions at the wall.

No Slip   specifies a no-slip condition at the wall. No further inputs are required.

Specified Shear   enables specification of zero or non-zero shear. See Section  7.13.1 for details. This option is not available for moving walls.

Marangoni Stress   enables the specification of shear stress caused by the variation of surface tension due to temperature. This option is not available for moving walls.

Shear Stress   contains inputs related to wall shear. These items will appear when Specified Shear is selected as the Shear Condition. See Section  7.13.1 for details.

X-Component, Y-Component, Z-Component, Swirl Component   specify the $x$, $y$, and $z$ or swirl components of shear for a slip wall. Swirl Component is available only for axisymmetric swirl cases.

Marangoni Stress   contains inputs related to Marangoni stress. This item will appear when Marangoni Stress is selected as the Shear Condition. See Section  7.13.1 for details.

Surface Tension Gradient   specifies the surface tension gradient with respect to temperature ( $d \sigma/dT$ in Equation  7.13-1).

Wall Roughness   contains inputs for defining wall roughness in turbulent calculations. See Section  7.13.1 for details.

Roughness Height   sets the roughness height $K_s$ (see Section  7.13.1 for details).

Roughness Constant   sets the roughness constant $C_{K_s}$ (see Section  7.13.1 for details).

Wall Adhesion   contains inputs related to wall adhesion. This section of the panel will appear if you are using the VOF model and have enabled wall adhesion in the Phase Interaction panel.

Contact Angles   specifies the contact angle at the wall for each pair of phases ( $\theta_w$ in Figure  23.3.3). See Section  23.9.8 for details.

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

Thermal Conditions   contains radio buttons for selecting the thermal boundary condition type. See Section  7.13.1 for details about these inputs:
Heat Flux   selects a specified heat flux condition.

Temperature   selects a specified wall temperature condition.

Convection   selects a convective heat transfer boundary condition model.

Radiation   selects an external radiation boundary condition.

Mixed   selects a combined convection/external radiation boundary condition.

Coupled   selects a coupled heat transfer condition. It is applicable only to walls that form the interface between two regions (such as the fluid/solid interface for a conjugate heat transfer problem).

Once a condition type has been selected, the appropriate conditions can be specified.

Heat Flux   sets the wall heat flux to be used for the Heat Flux condition. A specification of zero Heat Flux is simply the adiabatic condition (no heat transfer). A positive value of heat flux implies that heat is input into the domain.

Temperature   sets the wall temperature to be used for the Temperature condition.

Heat Transfer Coefficient   sets the convective heat transfer coefficient to be used for the Convection condition ( $h_{\rm eff}$ in Equation  7.13-12).

Free Stream Temperature   sets the reference or free stream temperature to be used for the Convection condition ( $T_{\rm ext}$ in Equation  7.13-12).

External Emissivity   sets the emissivity of the external wall to be used for the Radiation condition ( $\epsilon_{\rm ext}$ in Equation  7.13-13).

External Radiation Temperature   sets the temperature of the external radiation source/sink to be used for the Radiation condition ( $T_\infty$ in Equation  7.13-13).

Internal Emissivity   sets the internal emissivity of the wall. This item will appear only if you are using the P-1 model, the DTRM, the discrete ordinates model, or the S2S model for radiation heat transfer. (Note that it will not appear if you are using the non-gray discrete ordinates model. In this case, you will enter the Internal Emissivity for each band under Radiation.)

Wall Thickness   sets the thickness of the wall for calculation of thin-wall thermal resistance. (See Section  7.13.1 for details.)

Heat Generation Rate   sets the rate of heat generation in the wall.

Contact Resistance   sets the contact resistance ( $R_c$ in Equation  24.2-16) at the wall. See Section  24.3 for details. This item appears only when the solidification/melting model is used.

Material Name   sets the material type of the wall. The conductivity of the material is used for the calculation of thin-wall thermal resistance. (See Section  7.13.1 for details.) Material is used only when Wall Thickness is non-zero. Materials are defined with the Materials panel.

Shell Conduction   enables shell conduction for the wall. See Section  7.13.1 for details.

Radiation   displays the boundary conditions for the DO radiation model at the wall. This tab is available only if you are using the discrete ordinates radiation model. See Section  13.3.15 for details.

BC Type   contains a drop-down list of available radiation boundary condition types. The available options are opaque and semi-transparent.

Internal Emissivity   specifies the internal emissivity of the wall in each wavelength band. This item will appear only if you are using the non-gray discrete ordinates radiation model and you have selected opaque as the BC Type.

Diffuse Fraction   specifies the fraction of the irradiation that is to be treated as diffuse. By default, the Diffuse Fraction is set to 1, indicating that all of the irradiation is diffuse. If the non-gray DO model is being used, the Diffuse Fraction can be specified for each band.

Beam Width   specifies the beam width for an external semi-transparent wall in terms of the Theta and Phi extents. This item will appear only if you are using the discrete ordinates radiation model and you have selected semi-transparent as the BC Type.

Beam Direction   specifies the beam direction as an X,Y,Z vector. This item will appear only if you are using the discrete ordinates radiation model and you have selected semi-transparent as the BC Type.

Irradiation   specifies the value of the irradiation flux. If the non-gray DO model is being used, a constant Irradiation can be specified for each band.

This item will appear only if you are using the discrete ordinates radiation model and you have selected semi-transparent as the BC Type.

Species   contains the species parameters. This tab is available only if you have enabled the Species Transport model in the Species Model panel.

Reaction   activates reactions at the wall. This item will appear only if you have enabled any of the reactions in the Species Model panel.

Reaction Mechanisms   allows you to specify a defined group, or mechanism, of available reactions. This item will appear only if the Reaction option has been turned on. See Section  14.1.4 for details about defining reaction mechanisms.

Species Boundary Condition   contains options for the specification of species boundary conditions. See Section  7.13.1 for details.

Zero Diffusive Flux   indicates a zero-flux condition for a species. This is the default condition.

Specified Mass Fraction   indicates that the species mass fraction will be specified.

Species Mass Fractions   contains inputs for the species mass fractions of any species for which you have selected Species Mass Fraction as the Species Boundary Condition.

DPM   contains the discrete phase parameters. This tab is available only if you have defined at least one injection.

Discrete Phase Model Conditions   contains inputs for setting the fate of particle trajectories at the wall. These options will appear when one or more injections have been defined. See Section  22.13 for details.

Boundary Cond. Type   sets the way that the discrete phase behaves with respect to the boundary.

reflect   rebounds the particle off the boundary with a change in its momentum as defined by the coefficients of restitution. (See Figure  22.13.1.)

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  22.13.2.

escape   reports the particle as having "escaped'' when it encounters the boundary. Trajectory calculations are terminated. See Figure  22.13.3.

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

Boundary Cond. Function   sets the user-defined function from the drop-down list.

Discrete Phase Reflection Coefficients   determine the behavior of reflecting particles. This item appears when reflect is chosen as the Boundary Cond. Type. See Section  22.13.1 for details on setting the following items.

Normal   sets the type of function for the normal coefficient of restitution. This function can be constant, piecewise-linear, piecewise-polynomial, or polynomial.

Tangent   sets the type of function for the tangential coefficient of restitution. This function can be constant, piecewise-linear, piecewise-polynomial, or polynomial.

Erosion Model   contains inputs for erosion calculations. See Section  22.13.1 for details about these items.

Impact Angle Function   specifies the value of $f(\alpha)$ in Equation  22.5-1.

Diameter Function   specifies the value of $C(d_p)$ in Equation  22.5-1.

Velocity Exponent Function   specifies the value of $b(v)$ in Equation  22.5-1.

UDS   displays the boundary conditions for user-defined scalars (UDSs) at the wall. This tab is available only if you have specified a non-zero number of user-defined scalars in the User-Defined Scalars panel.

User Defined Scalar Boundary Condition   contains options for the specification of UDS boundary conditions. See the separate UDF Manual for details.

Specified Flux   indicates that the flux of the UDS at the wall will be specified.

Specified Value   indicates that the value for the UDS at the wall will be specified.

User Defined Scalar Boundary Value   contains inputs for the value of the flux of the UDS, or the value of the UDS itself, depending on your selection for that UDS under User Defined Scalar Boundary Condition.


next up previous contents index Previous: 32.3.17 Define/Operating Conditions...
Up: 32.3 Define Menu
Next: 32.3.19 Define/Periodic Conditions...
© Fluent Inc. 2006-09-20