### 2.5.1. Mass and Momentum

Information on the mathematical treatment of mass and momentum for an outlet boundary condition is available in the Mass and Momentum subsection of Outlet (Subsonic) in the CFX-Solver Theory Guide.

#### 2.5.1.1. Static Pressure

The Relative Pressure is maintained at a fixed specified value over the outlet boundary. The flow direction is an implicit result of the computation.

#### 2.5.1.2. Normal Speed

Specify the magnitude of the flow velocity at the outlet. The direction of the flow is taken to be locally normal to the outlet boundary surface.

#### 2.5.1.3. Cartesian Velocity Components

The boundary velocity components are specified. Care should be taken to ensure that a non-zero resultant is directed out of the domain.

#### 2.5.1.4. Cylindrical Velocity Components

The components and axis are specified in the same way as for an inlet. For details, see Cylindrical Velocity Components. The resultant flow must be directed out of the domain.

Note: The last three options can cause severe robustness problems if the problem set-up causes a significant departure from the specified velocity distribution anywhere the flow is approaching the outlet. In this case, you may have no choice but to use one of the other options.

#### 2.5.1.5. Average Static Pressure

When this option is selected, the static pressure is allowed to locally vary on the outlet boundary such that the average pressure is constrained in a specified manner. In all cases, the flow direction at the outlet is an implicit result of the computation. For details, see Boundary Conditions in the CFX-Solver Theory Guide.

The following averaging options are available:

##### 2.5.1.5.1. Average Over Whole Outlet

This is the most commonly used option. The average constraint is applied by comparing the area weighted pressure average over the entire outlet to the user-specified value. The pressure profile at the outlet is shifted by this difference such that the new area weighted pressure average will be equal to the user-specified value. The flow direction is an implicit result of the computation.

Note that the specified average pressure may be a pressure profile. If it is, the pressure profile will be averaged and it is this profile average which will be enforced.

##### 2.5.1.5.2. Average Above Specified Radius

The area weighted average of pressure above the specified radius is used as the comparison to the user-specified value (instead of the area weighted average over the entire outlet). The pressure profile is then shifted by the difference between these two values. The radius is calculated as the distance from the local axis of rotation (specified on the boundary for stationary domains) or the domain rotation axis for rotating domains.

The area weighted average of pressure at the outlet in the desired region may not be identical to the specified average static pressure, but it should be quite close. If the flow solver has built artificial walls on the boundary condition the actual average may differ more from the specified value than when no artificial walls are built.

##### 2.5.1.5.3. Average Below Specified Radius

This is the same as Average Above Specified Radius, except that the region below the specified radius is used to obtain the area weighted average.

##### 2.5.1.5.4. Circumferential

In this case, the average pressure is constrained within circumferential bands defined by either a local rotation axis or the domain rotation axis. The circumferential bands are either radial or axial depending on the geometry. The average pressure profile can be set as a constant, CEL analytic expression, profile function or user-defined function.

There is no restriction on how the pressure profile can spatially vary. The number of bands is automatically determined by the flow solver using the maximum number of bands that the underlying CFD mesh on the outlet will enable. Every band contains enough mesh to calculate a circumferential average. The flow solver will print a diagnostic telling you how many bands it is using. It is possible to use fewer bands than the value determined by the flow solver, but not more. You can modify the Maximum Number of Circumferential Bands setting.

The value of Pres. Profile Blend is used to blend between the specified pressure profile and a floating pressure profile where only the average is constrained. For a value of zero, the specified pressure is used only to enforce the average pressure. This allows a transverse pressure profile to develop according to upstream influences, which is much less reflective than specifying the pressure profile itself. For some flows, setting only the average pressure does not constrain the flow enough; in this case, a small amount of blending, the default value of 0.05, or 5%, may be appropriate.

##### 2.5.1.5.5. Radial Equilibrium

In the case of Radial Equilibrium, the averaged static pressure is constrained within radial circumferential bands defined by either a local rotation axis or the domain rotation axis. The band-averaged pressure satisfies radial equilibrium between the radial pressure gradient and the centrifugal force calculated using the band-averaged density and circumferential velocity. Integrating this relationship gives pressure values for each band and requires a user-specified static pressure at a radial reference position as a starting point for the integration. Three different options are available for specifying the radial reference position:

- Option = Specified Radius (you must specify the Specified Radius parameter)

- Option = Minimum Radius (the radius is automatically calculated by the solver)

- Option = Maximum Radius (the radius is automatically calculated by the solver).

The solver generates the circumferential bands the same way as for the circumferential averaged pressure option (see Circumferential Pressure Averaging), except that, in this case, bands are allowed to be oriented only in the radial direction. As for all pressure averaging options, pressure profile blending can be applied to this boundary condition.

#### 2.5.1.6. Mass Flow Rate (Bulk Mass Flow Rate for Multiphase)

When Mass and Momentum > Option is set to `Mass Flow Rate`, you must set Mass and Momentum > Mass Flow Rate. A positive value represents mass flow through the boundary in the specified flow direction. For details, see Flow Direction.

Note: The local velocity across the outlet boundary is part of the solution.

You must also choose one of two settings for Mass Flow Rate Area:

- `As Specified`

  Mass Flow Rate corresponds to the modeled sector, and is applied directly to the boundary. This setting is selected by default.

- `Total for All Sectors`

  This setting is available only for single phase cases that have rotational periodicity and that have a rotational periodic interface. If no rotational periodic interface is present, `Total for All Sectors` is identical to `As Specified`. For details on interface models with rotational periodicity, see Interface Models.

  Mass Flow Rate corresponds to the full geometry. The pair of rotational periodic interfaces (or, in the case of multiple pairs existing in the domain, one such pair) is used to calculate the sector angle (the angle that the modeled sector spans in the full geometry). Mass Flow Rate is multiplied by the ratio between the sector angle and 360° before being applied to the boundary.

  Note: Only one sector angle is calculated per domain. If you have defined multiple pairs of rotational periodic interfaces in the same domain, and they spanned different sector angles, you should check the CFX-Solver out file to see which sector angle was used.

The `Mass Flow Outlet Constraint` option should be chosen from one of three methods depending on the type of flow at the outlet. For details, see Mass Flow Outlet Constraint.

Information on the mathematical treatment of mass flow rate for an outlet boundary condition is available in Mass Flow Rate: Scale Mass Flows, Mass Flow Rate: Shift Pressure with or without Pressure Profile and Mass Flow Rate: Shift Pressure with Circumferential Pressure Averaging in Outlet (Subsonic) in the CFX-Solver Theory Guide.

#### 2.5.1.7. Exit Corrected Mass Flow Rate

The `Exit Corrected Mass Flow Rate` outlet boundary option adjusts the mass flow rate to total conditions at the outlet, maintaining a constant exit corrected mass flow rate. The main application of this boundary option is rotating machinery. The `Exit Corrected Mass Flow Rate` boundary option enables you to sweep through the complete machine operational range, including machine operating points from choked flow to stall conditions.

This outlet boundary option allows you to specify the equivalent mass flow, based on similar criteria, corrected to a specified reference temperature and pressure. By default, the reference pressure and reference temperature are set to Standard Atmosphere Sea Level Static conditions of 15 [°C] and 1 [atm] respectively. Information on the mathematical treatment of exit corrected mass flow rate as an outlet boundary condition is available in Exit Corrected Mass Flow Rate in the CFX-Solver Theory Guide.

For this outlet boundary condition you are required to specify:

- Exit Corrected Mass Flow Rate

  For an ideal gas, the exit corrected mass flow rate is calculated as:

  | (2–3)

  where, and are mass averaged values of total pressure and temperature in the stationary frame at the outlet. and are the reference conditions, which are constants in the equation. It should be noted that the numerical behavior of the boundary condition is not affected by the choice of reference conditions. Rather, the reference conditions simply provide a dimensional meaning to the otherwise non-dimensional mass flow rate.

Because the specified corrected mass flow and reference conditions are constant, you can observe that the resulting mass flow rate must be proportional to the exit total pressure and inversely proportional to the square root of the exit total temperature (or equivalently, inversely proportional to the stagnation speed of sound) in order to maintain a constant exit corrected mass flow. This allows the boundary condition to adapt dynamically to varying operating conditions, while remaining stable as the flow develops from the initial guess.

Currently, the `Exit Corrected Mass Flow Rate` outlet boundary condition is only available for ideal gas materials with the thermal energy or total energy options enabled. For more details on using the Exit Corrected Mass Flow Rate boundary condition, see Computing Speedlines for a Machine in the CFX Reference Guide.

Along with Mass Flow Rate, you can set Mass Flow Rate Area. Because cases that use `Exit Corrected Mass Flow Rate` usually feature rotational periodicity, the default Mass Flow Rate Area option for new cases is `Total for All Sectors`. For details on Mass Flow Rate Area options, see Mass Flow Rate (Bulk Mass Flow Rate for Multiphase).

The `Mass Flow Outlet Constraint` option should be chosen from one of three methods depending on the type of flow at the outlet. For details, see Mass Flow Outlet Constraint.

#### 2.5.1.8. Mass Flow Outlet Constraint

For the Mass Flow Rate and Exit Corrected Mass Flow Rate options you can specify one of three `Mass Flow Outlet Constraint` methods, depending on the type of flow:

##### 2.5.1.8.1. Pressure Shape Unconstrained

This is the default option in ANSYS CFX. The mass flow distribution is a function of the mass flow just upstream of the outlet boundary, and the specified mass flow is enforced at each timestep. The pressure distribution which results is an implicit part of the simulation and is not constrained by the boundary condition.

##### 2.5.1.8.2. Uniform Mass Flux

This specifies a constant mass flow distribution ( U normal is the same across the entire outflow boundary). This option is most useful when the flow is highly tangential relative to the outlet. Under these circumstances, it is difficult to determine the mass flow distribution when the `Pressure Shape Unconstrained` or `Pressure Shape Constrained` options are used. This is because the mass distribution just upstream of and normal to the outlet is a small component relative to the tangential component of the mass flow. Conversely, the `Uniform Mass Flux` option should not be used if the mass flow at the outlet is not highly tangential. This would adversely affect the flow upstream of the boundary where the mass flow distribution is not uniform.

##### 2.5.1.8.3. Pressure Shape Constrained

This option allows you to constrain the pressure profile over the entire boundary. Like `Pressure Shape Unconstrained`, the mass flow distribution is a function of the mass flow just upstream of the outlet boundary, and the specified mass flow is enforced at each timestep. However, the solver also computes the pressure shift between your specified profile and the implicit (floating) profile that enforces the specified mass flow rate.

The `Pressure Shape Constrained` option is generally useful if:

- The pressure profile at the outlet is known.

- The pressure shape is not known, but the implicit pressure profile shape computed using the `Pressure Shape Unconstrained` option is not acceptable.

- The model converges poorly using other Mass Flow Outlet Constraint methods.

If you do not constrain the profile, then the static pressure profile floats and becomes an implicit result of the solution. The shift value works out to the average pressure that enforces the specified mass flow rate. The solver still computes the necessary pressure shift, but otherwise behaves as if the Mass Flow Outlet Constraint setting is `Pressure Shape Unconstrained`.

To use `Pressure Shape Constrained`, you must set the following values:

Pres. Profile Shape

  This is a value or expression that describes the pressure profile at the outlet and is entered in units of pressure. Because the pressure level at the outlet is part of the solution, only the relative variation in the profile is relevant. For example, specifying a constant pressure profile of 0 Pa is the same as specifying a constant pressure profile of 101325 Pa.

Pres. Profile Blend

  This is a measure of enforcement of the specified pressure profile to the outlet boundary. For any blend value, between 0 and 1, the pressure is equal to:

  | (2–4)

  where P profile is the pressure value calculated from the user-specified profile and P floating is derived from the value just upstream of the outflow boundary.

  By default Pres. Profile Blend is set to 0.05. A blend value of 0.0 specifies no enforcement of the pressure profile. In this case, the behavior of the `Pressure Shape Unconstrained` method is recovered. A blend value of 1.0 fully imposes the pressure profile shape (but not the level) as well as the mass flow leaving the domain.

###### 2.5.1.8.3.1. Circumferential Pressure Averaging

For cases that use the `Pressure Shape Constrained` option, a circumferential pressure averaging option is available. This option creates a meridional pressure profile shape based on any specified spatially varying pressure values, and then allows the local relative static pressure distribution to vary within circumferential bands (as done for average pressure outlets) based on that meridional pressure profile shape. This also makes it easy to switch between including or not including circumferential averaging. Note that with circumferential pressure averaging, there is no restriction on circumferential pressure variations in a given band (that is, only the average for a given band is constrained based on the specified pressure profile shape).

#### 2.5.1.9. Degassing Condition (Multiphase only)

Degassing boundary conditions are used to model a free surface from which dispersed bubbles are permitted to escape, but the liquid phase is not. They are useful for modeling flow in bubble columns.

When Degassing Boundary Condition is selected as the Flow Specification of an outlet, the continuous phase and any dispersed solid phases that may be present see this boundary as a free-slip wall and do not leave the domain. Dispersed fluid phases and Lagrange particles see this boundary as an outlet. However, the outlet pressure is not specified. Instead, a pressure distribution is computed on this fixed-position boundary, and can be interpreted as representing the weight of the surface height variations in the real flow.

Because the Degassing Boundary Condition does not specify a pressure value, a fixed pressure reference point will be set automatically for a domain with an incompressible flow with degassing boundaries, but no pressure boundaries.

#### 2.5.1.10. Fluid Velocity (Multiphase only)

This option is only available for an inhomogeneous multiphase simulation. When this option is selected, the Mass and Momentum information is set on a per fluid basis using `Cartesian` or `Cylindrical Velocity Components`.

#### 2.5.1.11. Supercritical (Multiphase only)

Supercritical free surface flow means that the liquid velocity exceeds the local wave velocity, and nothing needs to be set at the outlet (analogous to the supersonic condition for compressible flow). However, for stability purposes, Relative Pres. in Gas (that is, Relative Pressure in Gas: the pressure in the gas phase above the free surface interface) must be set. Note that transcritical free surface flows often have two solutions: one subcritical at the outlet and the other supercritical. Because of this, you may sometimes need to start with a `Static Pressure` or `Average Static Pressure` outlet condition based on a hydrostatic condition which forces the elevation into the supercritical regime.

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