The Pressure Outlet dialog box sets the boundary conditions for a pressure outlet zone. It is opened from the Boundary Conditions Task Page. See Inputs at Pressure Outlet Boundaries for details about defining the items below.

Controls
sets the name of the zone.
contains the momentum parameters.
specify whether backflow temperature, pressure, and flow directions are in the Absolute or Relative to the Adjacent Cell Zone reference frame.
sets the gauge pressure at the outflow boundary.
sets a factor by which the Gauge Pressure is multiplied. This is provided mainly for cases where a non-uniform distribution of the static pressure at the pressure outlet boundary is specified by means of a profile file or a user-defined function.
sets the direction of the inflow stream should the flow reverse direction. If you choose Direction Vector, you will define the flow direction components, and if you choose Normal to Boundary or From Neighboring Cell, no inputs are required. See Inputs at Pressure Outlet Boundaries for information on specifying flow direction.
contains a drop-down list for selecting the coordinate system. You can choose Cartesian, Cylindrical, or Local Cylindrical. This option is available only when Direction Vector is selected from the Backflow Direction Specification Method drop-down list.
allows you to specify the velocity components in x, y, and z directions respectively. This option is available when Cartesian is selected for the Coordinate System.
set the direction of the flow at the boundary. These items will appear for 2D axisymmetric cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.
specifies how the pressure is calculated under backflow conditions. When the NRBC option is not enabled, if you select Static Pressure, the Gauge Pressure is directly imposed as the boundary face pressure; if you select Total Pressure, the Gauge Pressure will be combined with a dynamic contribution that is based on the velocity in the adjacent cell zone. For NRBCs, if you select Static Pressure, the Gauge Pressure is directly imposed as the pressure at infinity; if you select Total Pressure, the pressure at infinity is a calculated value that is based on the Gauge Pressure.
enables the radial equilibrium pressure distribution. See Defining Static Pressure for details.
This item appears only for 3D and axisymmetric swirl solvers.
allows the pressure along the outlet boundary to vary, but maintain an average equivalent to the specified value in the Gauge Pressure input field. In this boundary implementation, the pressure variation provides a low level of non-reflectivity. For more details, see Calculation Procedure at Pressure Outlet Boundaries.
Note: The Average Pressure Specification option is not available if the Radial Equilibrium Pressure Distribution option is enabled.
allows you to set mass flow rate as a boundary condition at the outlet.
allows you to specify the flow as either a constant value or a user-defined function.
specifies the range of the pressure limits, which have different pressure variations on different boundaries. The upper and lower pressure limits can be specified as a constant or a profile.
contains the turbulence parameters.
specifies which method will be used to define the turbulence parameters. You can
choose K and Epsilon (-
models and RSM only), K and Omega
(
-
models only), Intensity and Length Scale,
Intensity and Viscosity Ratio, Intensity and Hydraulic
Diameter, Modified Turbulent Viscosity (Spalart-Allmaras
model only), or Turbulent Viscosity Ratio (Spalart-Allmaras model
only). See Determining Turbulence Parameters for information about the inputs for each
of these methods. (This item will appear only for turbulent flow calculations.)
set values for the turbulence kinetic energy and its dissipation rate
. These items will appear if you choose K and
Epsilon as the Specification Method.
set values for the turbulence kinetic energy and its specific dissipation rate
. These items will appear if you choose K and
Omega as the Specification Method.
set values for turbulence intensity and turbulence length scale
. These items will appear if you choose Intensity and Length
Scale as the Specification Method.
set values for turbulence intensity and turbulent viscosity ratio
. These items will appear if you choose Intensity and
Viscosity Ratio as the Specification Method.
set values for turbulence intensity and hydraulic diameter
. These items will appear if you choose Intensity and
Hydraulic Diameter as the Specification Method.
sets the value of the backflow modified turbulent viscosity . This item will appear if you choose Modified Turbulent
Viscosity as the Specification Method.
sets the value of the backflow turbulent viscosity ratio . This item will appear if you choose Turbulent Viscosity
Ratio as the 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 Turbulent Intensity or Reynolds-Stress Components. If you choose the former, ANSYS Fluent will compute the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses yourself. See Reynolds Stress Model for details. (This item will appear only for RSM turbulent flow calculations.)
specify the backflow Reynolds stress components when Reynolds-Stress Components is chosen as the Reynolds-Stress Specification Method.
contains settings for treatment of acoustic pressure waves at the boundary.
disables special treatment of acoustic pressure waves at the boundary.
enables the general non-reflecting boundary condition treatment described in General Non-Reflecting Boundary Conditions.
enables the impedance boundary condition treatment described in Impedance Boundary Conditions.
enables the transparent flow forcing boundary condition described in Transparent Flow Forcing Boundary Conditions.
contains settings for the non-reflecting boundary condition treatment.
defines how the pressure is calculated. For Pressure at Infinity, the pressure at the boundary relaxes toward the Gauge Pressure at infinity; for Average Boundary Pressure, an effort is made to force the average pressure on the boundary to approach the Gauge Pressure value.
contains the parameters for the impedance boundary condition treatment. For details refer to Using the Impedance Boundary Condition.
contains the parameters for the transparent flow forcing boundary condition treatment. For details refer to Using the Transparent Flow Forcing Boundary Condition.
contains the thermal parameters.
sets the total temperature of the inflow stream should the flow reverse direction
contains the boundary conditions for the radiation model at the pressure outlet.
set the radiation boundary conditions when you are using the P-1, DTRM, DO, S2S, or MC models for radiation heat transfer. See Defining Boundary Conditions for Radiation for details.
specifies whether or not the pressure outlet participates in solar ray tracing.
specifies a multiplier (ranging from 0 to 1) that is applied to the solar irradiation entering the domain through the pressure outlet.
specifies whether or not the pressure outlet participates in the view factor calculation as part of the S2S radiation model. This parameter is available only if you select the Surface to Surface radiation model.
contains the species parameters.
allows you to specify the species in mole fractions rather than mass fractions.
set inlet values for the PDF mixture fraction and its variance. (These items will appear only if you are using the non-premixed or partially premixed combustion model.)
set inlet values for the secondary mixture fraction and its variance. (These items will appear only if you are using the non-premixed or partially premixed combustion model with two mixture fractions.)
contains inputs for the mass fractions of defined species. See Defining Cell Zone and Boundary Conditions for Species for details about these inputs. These items will appear only if you are modeling non-reacting multi-species flow or you are using the finite-rate reaction formulation.
sets the value of the progress variable for premixed turbulent combustion. See Setting Boundary Conditions for the Progress Variable for details.
This item will appear only if the premixed or partially premixed combustion model is used.
contains the discrete phase parameters.
sets the way that the discrete phase behaves with respect to the boundary. This item appears when one or more injections have been defined.
rebounds the particle off the boundary with a change in its momentum as defined by the coefficient of restitution. (See Particle Reflection at Wall in the Fluent Theory Guide.)
terminates the trajectory calculations and records the fate of the particle as “trapped”. In the case of evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters the cell adjacent to the boundary. See Figure 23.25: “Trap” Boundary Condition for the Discrete Phase.
reports the particle as having “escaped” when it encounters the boundary. Trajectory calculations are terminated. See Figure 23.26: “Escape” Boundary Condition for the Discrete Phase.
indicates that the direction and velocity of the droplet particles are given by the resulting momentum flux, which is a function of the impingement angle. See Figure 16.6: “Wall Jet” Boundary Condition for the Discrete Phase in the Theory Guide.
specifies a user-defined function to define the discrete phase boundary condition type.
sets the user-defined function from the drop-down list.
contains the multiphase parameters.
specifies temperature for the solids phase and is proportional to the kinetic energy of the random motion of the particles. This option is available only for a granular phase with the Mixture and Eulerian multiphase models.
sets the method used to specify the volume fraction of the secondary phase selected in the Boundary Conditions Task Page. This section of the dialog box will appear when one of the multiphase models is being used. See Defining Multiphase Cell Zone and Boundary Conditions for details. This control is not available for the open channel VOF submodel.
specifies the volume fraction of the secondary phase as a constant, profile, of UDF function.
calculates the volume fraction from the neighboring cells.
(VOF model only) enables the open-channel flow boundary condition. See Modeling Open Channel Flows for more information. This option is available only when the Open Channel VOF submodel is selected in the Multiphase Model dialog box. Once you select this option, you can specify the following conditions:
is used to identify the different outlets that are part of the same outlet group. See Setting the Outlet Group for details.
specifies which method will be used to define the boundary conditions at the open-channel pressure outlet. You can choose from the following options:
Free Surface Level
From Neighboring Cell
Gauge Pressure
Refer to Pressure Outlet in the Fluent Theory Guide for more details.
allows you to choose the desired secondary phase. This control is available only for flow applications with more than two phases.
can be determined by using the absolute value of height from the free surface to the origin in the direction of gravity and applying the correct sign based on whether the free surface level is above (positive) or below (negative) the origin. See Determining the Free Surface Level for details.
is used for calculating the liquid height. It can be determined as described in Determining the Bottom Level.
allows you to specify whether the mixture density used in the hydrostatic profile will be interpolated using the From Neighboring Cell, From Free Surface Level, or Hybrid method. See Choosing the Density Interpolation Method for more information. This drop-down list is available for sub-critical two-phase flow applications.
displays the boundary conditions for the electric potential field. This tab is available only if you have enabled either the Electric Potential model or the Electrochemical reaction model in the Species Dialog Box.
is a drop-down list of available potential boundary condition types: Specified Flux and Specified Value. For the Specified Flux boundary condition, you will need to specify Current Density at the wall. For the Specified Value boundary condition, you will need to specify Potential at the wall.
contains the UDS parameters.
appears only if user-defined scalars are specified.
specifies whether the scalar is a specified flux or a specified value.
appears only if user-defined scalars are specified.
specifies the value of the scalar.