7.3.8 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 Section  7.3.8 for details), and a target mass flow rate for pressure outlets (see Section  7.3.8 for details) can be specified.

For an overview of flow boundaries, see Section  7.3.1.

Inputs at Pressure Outlet Boundaries

Summary

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

• static pressure

• backflow conditions
  • total (stagnation) temperature (for energy calculations)

  • 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)

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

• discrete phase boundary conditions (for discrete phase calculations)

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

• non-reflecting boundary (for compressible density-based solver, see Section  7.4.2 for details)

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

All values are entered in the Pressure Outlet dialog box (Figure  7.3.7), which is opened from the Boundary Conditions task page (as described in Section  7.1.4). Note that open channel boundary condition inputs are described in Section  24.3.1.

Figure 7.3.7: The Pressure Outlet Dialog Box

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 for subsonic flow only. Should the flow become locally supersonic, the pressure will be extrapolated from the upstream conditions.

Remember that the static pressure value you enter is relative to the operating pressure set in the Operating Conditions dialog box. Refer to Section  7.3.3 regarding hydrostatic pressure.

ANSYS FLUENT also provides an option to use a radial equilibrium outlet boundary condition. To enable this option, turn on 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

where $r$ is the distance from the axis of rotation and $v_\theta$ 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.

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

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 Section  7.3.2. Turbulence modeling in general is described in Chapter  12.

• 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 Section  15.1.5.

• 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 Section  16.8 for details.

• If you are modeling combustion using the premixed or partially premixed combustion model, you will set the backflow Progress Variable value. See Section  17.3.3 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 Section  24.2.9 for details.

• If backflow occurs, the pressure you specified as the Gauge Pressure will be used as total pressure, so you need not specify a backflow pressure value explicitly. The flow direction will be based on your specification of the direction vector.

  If the cell zone adjacent to the pressure outlet is moving (i.e., if you are using a rotating 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  7.3-17) will be absolute or relative to the motion of the cell zone, depending on whether or not the Absolute velocity formulation is enabled in the General task page. For the density-based solver, the velocity in Equation  7.3-17 (or the Mach number in Equation  7.3-18) is always in the absolute frame.

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.

Defining Radiation Parameters

If you are using the P-1 radiation model, the DTRM, the DO model, or the surface-to-surface model, you will set the Internal Emissivity and (optional) External Black Body Temperature Method. See Section  13.3.6 for details. (The Rosseland radiation model does not require any boundary condition inputs.)

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 Section  23.4 for details.

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 Section  24.3.1 for details.

Default Settings at Pressure Outlet Boundaries

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

Gauge Pressure	0
Backflow Total Temperature	300
Backflow Turbulent Kinetic Energy	1
Backflow Turbulent Dissipation Rate	1

Calculation Procedure at Pressure Outlet Boundaries

At pressure outlets, ANSYS FLUENT uses the boundary condition pressure you input as the static pressure of the fluid at the outlet plane, $p_s$, and extrapolates all other conditions from the interior of the domain.

Density-Based Solver Implementation

In the density-based solver, there are three pressure specification methods available:

1.   Weak enforcement of average pressure (default)

2.   Strong enforcement of average pressure

3.   Direct pressure specification

The specification methods can be changed from the text user interface:

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

In the direct pressure specifications, the face pressure at the boundary is same as the value specified in the Pressure Outlet dialog box. The implementation is similar to that in the pressure-based solver. However, the default specification method in the density-based solver is the weak enforcement of average pressure. In this implementation for subsonic flow, 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 [ 44]. Therefore, the face pressure $P_f$ is a function of ( $P_c$, $P_e$, $M_n$), where $P_c$ is the interior cell pressure neighboring the exit face f, $P_e$ is the specified exit pressure, and $M_n$ is the face normal Mach number.

Figure 7.3.8: 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.

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.

In general the weak average pressure enforcement works well in most flow situations. However, for cases where the computed average pressure value does not match the specified pressure value at the boundary (typically this happen when we have a coarse mesh and stretched cells near the pressure-outlet boundary) then the strong average pressure enforcement can be used to guarantee the specified pressure equal to the boundary average pressure. The strong enforcement is achieved by adding locally the difference in pressure value between the latest average pressure for the boundary and the face pressure obtained from weak enforcement. The strong enforcement is applicable when the flow is fully subsonic throughout the boundary.

For all of the three pressure specification methods, if the flow becomes locally supersonic, then the face pressure values $P_f$ are extrapolated from the interior cell pressure.

When one of the NRBC models is used, or when you enable the turbo-specific NRBC model, none of the above specification methods are relevant since face pressure will be obtained from special NRBC proceedures.

If you are specifying a profile rather than a constant value for exit pressure, then you should not use this weak or strong enforcement of average pressure boundary. Instead, you should use the direct pressure specification method.

Other Optional Inputs at Pressure Outlet Boundaries

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 only available when the density-based solver and ideal gas law are used. The NRBC 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 Section  7.4.2 of this chapter.

Target Mass Flow Rate Option

Two methods (Method 1 and Method 2) are available for adjusting the pressure at a pressure-outlet zone in order to meet the desired mass flow rate. Both methods are based on the simple Bernoulli's equation. However, they differ in the internal iteration strategy for obtaining the change in pressure on a pressure-outlet zone. In general, the target mass flow rate is achieved by adjusting the pressure value at the pressure-outlet zone up and down at every iteration. This is done in accordance with one of the two available methods until the desired target mass flow rate is obtained.

The change in pressure based on Bernoulli's equation is given by the following equation:

where $dP$ is the change in pressure, $\dot{m}$ is the current computed mass flow rate at the pressure-outlet boundary, $\dot{m}_{req}$ is the required mass flow rate, $\rho_{ave}$ is the computed average density at the pressure-outlet boundary, and $A$ is the area of the pressure-outlet boundary.

The default method, Method 1, should suffice in obtaining a converged solution on the targeted mass flow rate. However, if convergence difficulties are encountered while using the default method, then you may want to select the alternate method, Method 2. There are other solution strategies that may be used if convergence difficulties are encountered, which will be discussed at the end of this section.

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 (i.e., the Mach number of the fluid in the pressure-outlet zone becomes equal to 1).

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 $\rightarrow$ boundary-conditions $\rightarrow$ target-mass-flow-rate-settings

There are two options under this menu:

(a)   The set-method option allows you to:

i.   Select Method 1 or 2 (the default setting is Method 2).

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

(b)   The verbosity? option, if enabled, 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 7.3.9: 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 Section  26.10.

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.

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 this section in the separate UDF Manual.