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
You will enter the following information for a pressure outlet boundary:
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.
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 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.
| 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.
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:
|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, , 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:
The specification methods can be changed from the text user interface:
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 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.
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 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 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.
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.
Target Mass Flow Rate Settings
To use the target mass flow rate option
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
There are two options under this menu:
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.