6.3.9. Pressure Outlet Boundary Conditions

Pressure outlet boundary conditions require the specification of a static (gauge) pressure at the outlet boundary. The value of the specified static pressure is used only while the flow is subsonic. Should the flow become locally supersonic, the specified pressure will no longer be used; pressure will be extrapolated from the flow in the interior. All other flow quantities are extrapolated from the interior.

A set of “backflow” conditions is also specified should the flow reverse direction at the pressure outlet boundary during the solution process. Convergence difficulties will be minimized if you specify realistic values for the backflow quantities.

Several options in ANSYS Fluent exist, where a radial equilibrium outlet boundary condition can be used (see Defining Static Pressure and a target mass flow rate for pressure outlets (see Target Mass Flow Rate Option for details) can be specified.

For an overview of flow boundaries, see Flow Inlet and Exit Boundary Conditions.

6.3.9.1. Inputs at Pressure Outlet Boundaries

6.3.9.1.1. Summary

You will enter or select the following information for a pressure outlet boundary:

  • static pressure

  • pressure profile multiplier

  • backflow conditions

    • total (stagnation) temperature (for energy calculations)

    • backflow pressure specification

    • backflow direction specification method

    • turbulence parameters (for turbulent calculations)

    • chemical species mass or mole fractions (for species calculations)

    • mixture fraction and variance (for non-premixed or partially premixed combustion calculations)

    • progress variable (for premixed or partially premixed combustion calculations)

    • multiphase boundary conditions (for general multiphase calculations)

    • type of backflow reference frame (not available for multiphase flows or with the acoustic wave model)

  • radiation parameters (for calculations using the P-1, DTRM, DO, surface-to-surface, or MC models)

  • discrete phase boundary conditions (for discrete phase calculations)

  • open channel flow parameters (for open channel flow calculations using the VOF multiphase model)

  • radial equilibrium pressure distribution

  • average pressure specification (not available for multiphase flows)

  • target mass flow rate (not available for multiphase flows)

  • acoustic wave model settings

All values are entered in the Pressure Outlet Dialog Box (Figure 6.27: The Pressure Outlet Dialog Box), which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and Boundary Conditions). Note that open channel boundary condition inputs are described in Modeling Open Channel Flows, and acoustic wave model settings are described in Boundary Acoustic Wave Models.

Figure 6.27:  The Pressure Outlet Dialog Box

The Pressure Outlet Dialog Box

6.3.9.1.2. Defining Static Pressure

To set the static pressure at the pressure outlet boundary, enter the appropriate value for Gauge Pressure in the Pressure Outlet dialog box. This value will be used when the flow is locally subsonic. Should the flow become locally supersonic, the pressure will be extrapolated from the upstream conditions. By default the subsonic and supersonic local flow condition at the boundary is determined based on the local normal velocity component.

Remember that the static pressure value you enter is relative to the operating pressure set in the Operating Conditions Dialog Box. Refer to Pressure Inputs and Hydrostatic Head regarding hydrostatic pressure.

ANSYS Fluent also provides an option to use a radial equilibrium outlet boundary condition. This option is used to model the exit flow in turbomachinery flow problems. To turn on this option, enable Radial Equilibrium Pressure Distribution. When this feature is active, the specified gauge pressure applies only to the position of minimum radius (relative to the axis of rotation) at the boundary. The static pressure on the rest of the zone is calculated from the assumption that radial velocity is negligible, so that the pressure gradient is given by

(6–90)

where is the distance from the axis of rotation and is the tangential velocity. Note that this boundary condition can be used even if the rotational velocity is zero. For example, it could be applied to the calculation of the flow through an annulus containing guide vanes.


Important:  Note that the radial equilibrium outlet condition is available only for 3D and axisymmetric swirl calculations.


ANSYS Fluent also provides an option to use an Average Pressure Specification method at the pressure outlet boundary. This option allows the pressure along the outlet boundary to vary, but maintain an average equivalent to the specified value in the Gauge Pressure input field. The pressure variation allowed in this boundary implementation slightly diminishes the reflectivity of the boundary as compared with the default uniform pressure specification. In the density-based solver two averaging methods are available, Strong Averaging and Weak Averaging. The average pressure specification in the pressure-based solver is the same as the strong pressure averaging in the density-based solver. For more details, see Calculation Procedure at Pressure Outlet Boundaries.

The Pressure Profile Multiplier allows you to specify a constant 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. The scaling of an outlet profile with a multiplier can be convenient, for example, when computing a performance map for a turbomachine at different mass flow rates. The option will also work for a constant Gauge Pressure simply by scaling its value by a factor. This scaled pressure value will be used consistently when additional options are enabled in the Pressure Outlet dialog box; for example, when the Radial Equilibrium Pressure Distribution option is enabled, the scaled gauge pressure will be applied to the position of minimum radius (relative to the axis of rotation) at the boundary.

6.3.9.1.3. Defining Backflow Conditions

Backflow properties consistent with the models you are using will appear in the Pressure Outlet dialog box. The specified values will be used only if flow is pulled in through the outlet.

  • The Backflow Total Temperature (in the Thermal tab) should be set for problems involving energy calculation.

  • When the direction of the backflow re-entering the computational domain is known, and deemed to be relevant to the flow field solution, you can specify it choosing one of the options available in the Backflow Direction Specification Method drop-down list. The default value for this field is Normal to Boundary, and requires no further input. If you choose Direction Vector, the dialog box will expand to show the inputs for the components of the direction vector for the backflow, and if you are running the 3D version of ANSYS Fluent, the dialog box will display a Coordinate System drop-down list. If you choose From Neighboring Cell, ANSYS Fluent will determine the direction of the backflow using the direction of the flow in the cell layer adjacent to the pressure outlet.

  • For turbulent calculations, there are several ways in which you can define the turbulence parameters. Instructions for deciding which method to use in determining appropriate values for these inputs are provided in Determining Turbulence Parameters. Turbulence modeling in general is described in Modeling Turbulence.

  • If you are modeling species transport, you will set the backflow species mass or mole fractions under Species Mass Fractions or Species Mole Fractions. For details, see Defining Cell Zone and Boundary Conditions for Species.

  • If you are modeling combustion using the non-premixed or partially premixed combustion model, you will set the backflow mixture fraction and variance values. See Defining Non-Premixed Boundary Conditions for details.

  • If you are modeling combustion using the premixed or partially premixed combustion model, you will set the backflow Progress Variable value. See Setting Boundary Conditions for the Progress Variable for details.

  • If you are using the VOF, mixture, or Eulerian model for multiphase flow, you will need to specify volume fractions for secondary phases and (for some models) additional parameters. See Defining Multiphase Cell Zone and Boundary Conditions for details.

  • If backflow occurs,

    1. The pressure you specified as the Gauge Pressure will be used to determine the total pressure or the static pressure (based on your selection from the Backflow Pressure Specification drop-down list), so you need not specify a backflow pressure value explicitly. When Total Pressure is selected for Backflow Pressure Specification, boundary face pressure values are calculated by combining the Gauge Pressure with a dynamic contribution that is based on the velocity in the adjacent cell zone; when Static Pressure is selected for Backflow Pressure Specification, the specified Gauge Pressure value is directly imposed as the boundary face pressure.

    2. The flow direction will be based on your selection from the Backflow Direction Specification Method drop-down list.

    3. The total temperature, total pressure, and flow directions are in absolute or relative to the adjacent cell zone reference frames, based on the Backflow Reference Frame setting specified in the Pressure Outlet dialog box.

    If the cell zone adjacent to the pressure outlet is moving (that is, if you are using a moving reference frame, multiple reference frames, mixing planes, or sliding meshes) and you are using the pressure-based solver, the velocity in the dynamic contribution to total pressure (see Equation 6–74) will be absolute or relative to the motion of the cell zone, depending on whether or not the Absolute velocity formulation is selected in the General task page. For the density-based solver, the velocity in Equation 6–74 (or the Mach number in Equation 6–75) is always in the absolute frame.


Important:  Even if no backflow is expected in the converged solution, you should always set realistic values to minimize convergence difficulties in the event that backflow does occur during the calculation.

The Backflow Reference Frame option is not available for all multiphase models or non-reflecting boundary condition options.


6.3.9.1.4. Defining Radiation Parameters

If you are using the P-1, DTRM, DO, surface-to-surface, or MC models, you will set the Internal Emissivity and (optional) External Black Body Temperature Method. See Defining Boundary Conditions for Radiation for details. (The Rosseland radiation model does not require any boundary condition inputs.)

6.3.9.1.5. Defining Discrete Phase Boundary Conditions

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the pressure outlet. See Setting Boundary Conditions for the Discrete Phase for details.

6.3.9.1.6. Defining Open Channel Boundary Conditions

If you are using the VOF model for multiphase flow and modeling open channel flows, you will need to specify the Free Surface Level, Bottom Level, and additional parameters. See Modeling Open Channel Flows for details.

6.3.9.2. Default Settings at Pressure Outlet Boundaries

Default settings (in SI) for pressure outlet boundary conditions are as follows:

Gauge Pressure 0
Pressure Profile Multiplier 1
Backflow Total Temperature 300
Backflow Turbulent Intensity 5%
Backflow Turbulent Viscosity Ratio 10

6.3.9.3. Calculation Procedure at Pressure Outlet Boundaries

At pressure outlets, if the flow exiting the boundary is subsonic, then ANSYS Fluent uses the pressure specified in the Pressure Outlet dialog box as the static pressure of the fluid at the outlet plane, , and extrapolates all other conditions from the interior of the domain. However, if the flow exiting the boundary becomes supersonic, then the face pressure values are extrapolated from the interior cell pressure.

6.3.9.3.1. Average Pressure Specification

When this option is selected, the exit pressure is not kept constant over the pressure outlet boundary, but instead is allowed to vary across the boundary while maintaining an average boundary pressure close to the specified static exit pressure. This option can be used for pressure specified as a constant or as a profile (for example, in turbomachinery cases with radial, axial, or radial equilibrium pressure distributions).

There are two implementations of the Average Pressure Specification. These are Strong Averaging and Weak Averaging. The strong averaging approach is available in both the density-based and the pressure-based solver. The weak averaging approach is available only in the density-based solver.


Note:
  • The Average Pressure Specification option is not available with multiphase flows.

  • When using the density-based solver, Strong Averaging is the recommended method and is used by default. The weak averaging method is maintained primarily for legacy cases.

  • When one of the Acoustic Wave Models is active, the Average Pressure Specification option is not offered because the pressure will be obtained based on the Acoustic Wave Model chosen.

  • Using the Average Pressure Specification option in unsteady simulations can result in nonphysical pressure feedback and is not recommended.


6.3.9.3.1.1. Strong Averaging

In the Strong Averaging approach, the face pressure value for subsonic exit flow is computed using the following expression:

(6–91)

where

= interior cell pressure at neighboring exit face, f

 

= averaged interior cell pressure at a boundary

 

= specified exit pressure

= pressure blending factor; recovers the fully averaged pressure, recovers the specified pressure.

When the strong averaging option is used with a profile specification method (radial, axial, or radial equilibrium pressure distribution) then the outlet boundary will be subdivided into radial or axial containers called “bins”, and the above averaging procedure is applied to each bin.

You can use the following TUI command to change the blending factor and the number of bins:

/define/boundary-conditions/bc-settings/pressure-outlet

6.3.9.3.1.2. Weak Averaging

When the weak averaging method is used and the flow is subsonic, the pressure at the faces of the outlet boundary is computed using a weighted average of the left and right state of the face boundary. This weighting is a blend of fifth-order polynomials based on the exit face normal Mach number [61]. Therefore, the face pressure is a function of (, , ), where is the interior cell pressure neighboring the exit face f, is the specified exit pressure, and is the face normal Mach number.

Figure 6.28:  Pressures at the Face of a Pressure Outlet Boundary

Pressures at the Face of a Pressure Outlet Boundary

For incompressible flows, the face pressure is computed as an average between the specified pressure and the interior pressure.

(6–92)

In this boundary implementation, the exit pressure is not constant along the pressure outlet boundary. However, upon flow convergence, the average boundary pressure will be close to the specified static exit pressure.

6.3.9.4. Other Optional Inputs at Pressure Outlet Boundaries

6.3.9.4.1. Non-Reflecting Boundary Conditions Option

One of the options that may be used at pressure outlets is non-reflecting boundary conditions (NRBC). This option is used when waves are made to pass through the boundaries while avoiding false reflections. Details of non-reflecting boundary conditions can be found in General Non-Reflecting Boundary Conditions.

6.3.9.4.2. Target Mass Flow Rate Option

The simple Bernoulli's equation is used to adjust the pressure at every iteration on a pressure outlet zone in order to meet the desired mass flow rate. The change in pressure, based on Bernoulli’s equation is given by the following equation:

(6–93)

where is the change in pressure, is the current computed mass flow rate at the pressure-outlet boundary, is the required mass flow rate, is the computed average density at the pressure-outlet boundary, and is the area of the pressure-outlet boundary.

Limitations
  • The target mass flow rate option is not available with multiphase flows or when any of the non-reflecting boundary conditions models are used.

  • If the pressure-outlet zone is used in the mixing-plane model, the target mass flow rate option will not be available for that particular zone.

  • The pressure outlet will not achieve the target mass flow rate if the flow becomes choked (that is, the Mach number of the fluid in the pressure-outlet zone becomes equal to 1).

  • The pressure outlet may not achieve the target mass flow rate if porous zones are present in the flow domain causing a large pressure drop.

Target Mass Flow Rate Settings

To use the target mass flow rate option

  1. Enable Target Mass Flow Rate in the Pressure Outlet dialog box.

  2. Specify the Target Mass Flow as either a constant value or hook a UDF to set the target mass flow rate.

    The settings for the target mass flow rate option can be accessed from the target-mass-flow-rate-settings text command:

    define → boundary-conditions → target-mass-flow-rate-settings

    You will be prompted to

    1. Set the under-relaxation factor (the default setting is 0.05).

    2. Enable the targeted mass flow rate verbosity (the default is no). If enabled, it prints to the console window the required mass flow rate, computed mass flow rate, mean pressure, the new pressure imposed on the outlet, and the change in pressure in SI units.

  3. In the Pressure Outlet dialog box, specify the Upper Limit of Absolute Pressure and Lower Limit of Absolute Pressure. Specifying the range of the pressure limits improves convergence in cases with a large number of outlet boundaries, which have different pressure variations on different boundaries. You can also use the define/boundary-conditions/pressure-outlet text command to specify these limits.

Figure 6.29:  The Pressure Outlet Dialog Box with the Target Mass Flow Rate Option Enabled

The Pressure Outlet Dialog Box with the Target Mass Flow Rate Option Enabled

Solution Strategies When Using the Target Mass Flow Rate Option

If convergence difficulties are encountered or if the solution is not converging at the desired mass flow rate, then try to lower the under-relaxation factor from the default value. Otherwise, you can use the alternate method to converge at the required mass flow rate.

In some cases, you may want to switch off the target mass flow rate option initially, then guess an exit pressure that will bring the solution closer to the target mass flow rate. After the solution stabilizes, you can turn on the target mass flow rate option and iterate to convergence. For many complex flow problems, this strategy is usually very successful.

The use of Full Multigrid Initialization is also very helpful in obtaining a good starting solution and in general will reduce the time required to get a converged solution on a target mass flow rate. For further information on Full Multigrid Initialization, see Full Multigrid (FMG) Initialization.

Setting Target Mass Flow Rates Using UDFs

For some unsteady problems it is desirable that the target mass flow rate be a function of the physical flow time. This enforcement of boundary condition can be done by attaching a UDF with DEFINE_PROFILE functions to the target mass flow rate field.


Important:  Note that the mass flow rate profile is a function of time and only one constant value should be applied to all zone faces at a given time.


An example of a simple UDF using a DEFINE_PROFILE that will adjust the mass flow rate can be found in DEFINE_PROFILE in the Fluent Customization Manual.


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