7.3.5 Mass Flow Inlet Boundary Conditions

Mass flow boundary conditions can be used in ANSYS FLUENT to provide a prescribed mass flow rate or mass flux distribution at an inlet. As with a velocity inlet, specifying the mass flux permits the total pressure to vary in response to the interior solution. This is in contrast to the pressure inlet boundary condition (see Section  7.3.3), where the total pressure is fixed while the mass flux varies. However, unlike a velocity inlet, the mass flow inlet is equally applicable to incompressible and compressible flows.

A mass flow inlet is often used when it is more important to match a prescribed mass flow rate than to match the total pressure of the inflow stream. An example is the case of a small cooling jet that is bled into the main flow at a fixed mass flow rate, while the velocity of the main flow is governed primarily by a (different) pressure inlet/outlet boundary condition pair. A mass flow inlet boundary condition can also be used as an outflow by specifying the flow direction away from the solution domain.

Limitations and Special Considerations

• The adjustment of inlet total pressure might result in a slower convergence, so if both the pressure inlet boundary condition and the mass flow inlet boundary condition are acceptable choices, you should choose the former.

• It is not necessary to use mass flow inlets in incompressible flows because when density is constant, velocity inlet boundary conditions will fix the mass flow.

• Mass flow inlet boundary conditions cannot be applied to any of the multiphase models if all phases are incompressible.

• A mass flow boundary operating as an outflow has the following limitations:
  • It is available for single-phase flow only.

  • It is not available with the VOF, mixture, and Eulerian multiphase models in the pressure-based solver.

  • It is not available with the Wet Steam model in the density-based solver.

For an overview of flow boundaries, see Section  7.3.1.

Inputs at Mass Flow Inlet Boundaries

Summary

You will enter the following information for a mass flow inlet boundary:

• type of reference frame

• mass flow rate, mass flux, or (primarily for the mixing plane model) mass flux with average mass flux

• total (stagnation) temperature

• static pressure

• flow direction

• turbulence parameters (for turbulent calculations)

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

• 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)

• discrete phase boundary conditions (for discrete phase calculations)

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

All values are entered in the Mass-Flow Inlet dialog box (Figure  7.3.4), 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 7.3.4: The Mass-Flow Inlet Dialog Box

Selecting the Reference Frame

You will have the option to specify the mass flow boundary conditions either in the absolute or relative reference frame, when the cell zone adjacent to the mass flow inlet is moving. For such a case, choose Absolute (the default) or Relative to Adjacent Cell Zone in the Reference Frame drop-down list. If the cell zone adjacent to the mass flow inlet is not moving, both formulations are equivalent.

Defining the Mass Flow Rate or Mass Flux

You can specify the mass flow rate through the inlet zone and have ANSYS FLUENT convert this value to mass flux, or specify the mass flux directly. For cases where the mass flux varies across the boundary, you can also specify an average mass flux; see below for more information about this specification method.

You can define the mass flux or mass flow rate using a profile or a user-defined function.

The inputs for mass flow rate or flux are as follows:

1.   Specify the mass flow by selecting Mass Flow Rate, Mass Flux, or Mass Flux with Average Mass Flux in the Mass Flow Specification Method drop-down list.

2.   If you selected Mass Flow Rate (the default), set the prescribed mass flow rate in the Mass Flow Rate field when constant is selected from the drop-down list. Otherwise, select your hooked UDF or transient profile.

The hooked UDF or transient profile can only be used to provide time-varying specification of mass flow rate. Therefore, the transient solver must be used to run the simulation. Note that the variation of profile with position in space is not applicable with this hookup.

See this section in the separate UDF Manual for an example of a mass flow inlet UDF.

Note that for axisymmetric problems, this mass flow rate is the flow rate through the entire ( $2\pi$-radian) domain, not through a 1-radian slice.

3.   If you selected Mass Flux, set the prescribed mass flux in the Mass Flux field, or select your hooked UDF or profile.

4.   If you selected Mass Flux with Average Mass Flux, set the prescribed mass flux and average mass flux in the Mass Flux and Average Mass Flux fields.

More About Mass Flux and Average Mass Flux

As noted above, you can specify an average mass flux with the mass flux. If, for example, you specify a mass flux profile such that the average mass flux integrated over the zone area is 4.7, but you actually want to have a total mass flux of 5, you can keep the profile unchanged, and specify an average mass flux of 5. ANSYS FLUENT will maintain the profile shape but adjust the values so that the resulting mass flux across the boundary is 5.

The mass flux with average mass flux specification method is also used by the mixing plane model described in Section  10.3.2. If the mass flow inlet boundary is going to represent one of the mixing planes, then you do not need to specify the mass flux or flow rate; you can keep the default Mass Flow Rate of 1. When you create the mixing plane later on in the problem setup, ANSYS FLUENT will automatically select the Mass Flux with Average Mass Flux method in the Mass-Flow Inlet dialog box and set the Average Mass Flux to the value obtained by integrating the mass flux profile for the upstream zone. This will ensure that mass is conserved between the upstream zone and the downstream (mass flow inlet) zone.

Defining the Total Temperature

Enter the value for the total (stagnation) temperature of the inflow stream in the Total Temperature field in the Thermal tab.

The total temperature is specified either in the absolute reference frame or relative to the adjacent cell zone, depending on your setting for the Reference Frame.

For the Eulerian multiphase model, the total temperature, and mass flux components need to be specified for the individual phases. The Reference Frame ( Relative to Adjacent Cell Zone or Absolute) for each of the phases is the same as the reference frame selected for the mixture phase.

Note that you can only set the reference frame for the mixture, however, the total temperature can only be set for the individual phases.

If the flow is incompressible, then the temperature assigned in the Mass-Flow Inlet dialog box is considered to be the static temperature. For the mixture multiphase model, if a boundary allows a combination of compressible and incompressible phases to enter the domain, then the temperature assigned in the Mass-Flow Inlet dialog box is considered to be the static temperature at that boundary. If a boundary allows only a compressible phase to enter the domain, then the temperature assigned in the Mass-Flow Inlet dialog box is the total temperature (relative/absolute) at that boundary. The total temperature depends on the Reference Frame option selected in the Mass-Flow Inlet dialog box. For the VOF multiphase model, if a boundary allows a compressible phase to enter the domain, then the temperature assigned in the Mass-Flow Inlet dialog box is considered to be the total temperature at that boundary. The total temperature (relative/absolute) depends on the Reference Frame option chosen in the dialog box. Otherwise, the temperature assigned to the boundary is considered to be the static temperature at the boundary. For the Eulerian multiphase model, if a boundary allows a mixture of compressible and incompressible phases in the domain, then the temperature of each of the phases is the total or static temperature, depending on whether the phase is compressible or incompressible. Total temperature (relative/absolute) depends on the Reference Frame option chosen in the Mass-Flow Inlet dialog box.

Defining Static Pressure

The static pressure (termed the Supersonic/Initial Gauge Pressure) must be specified if the inlet flow is supersonic or if you plan to initialize the solution based on the pressure inlet boundary conditions. Solution initialization is discussed in Section  26.9.

The Supersonic/Initial Gauge Pressure is ignored by ANSYS FLUENT whenever the flow is subsonic. If you choose to initialize the flow based on the mass flow inlet conditions, the Supersonic/Initial Gauge Pressure will be used in conjunction with the specified stagnation quantities to compute initial values according to isentropic relations.

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

Defining the Flow Direction

You can define the flow direction at a mass flow inlet explicitly, or you can define the flow to be normal to the boundary.

The procedure for defining the flow direction is as follows, referring to Figure  7.3.4:

1.   Specify the flow direction by selecting Direction Vector, Normal to Boundary, or Outward Normals in the Direction Specification Method drop-down list.

2.   If you selected Direction Vector and your geometry is 2D, go to the next step. If your geometry is 3D, choose Cartesian (X, Y, Z), Cylindrical (Radial, Tangential, Axial), Local Cylindrical (Radial, Tangential, Axial), or Local Cylindrical Swirl in the Coordinate System drop-down list. See Section  7.3.3 for information about Cartesian, cylindrical, local cylindrical, and local cylindrical swirl coordinate systems.

3.   If you selected Direction Vector, set the vector components as follows:

• If your geometry is 2D non-axisymmetric, or you chose to use a 3D Cartesian coordinate system, enter appropriate values for the X, Y, and (in 3D) Z-Component of Flow Direction.

• If your geometry is 2D axisymmetric, or you chose to use a 3D Cylindrical coordinate system, enter appropriate values for the Axial, Radial, and (if you are modeling swirl or using cylindrical coordinates) Tangential-Component of Flow Direction.

• If you chose to use a 3D Local Cylindrical coordinate system, enter appropriate values for the Axial, Radial, and Tangential-Component of Flow Direction, and then specify the X, Y, and Z components of Axis Origin and the Axis Direction.

• If you chose to use a 3D Local Cylindrical Swirl coordinate system, enter appropriate values for the Axial and Radial-Component of Flow Direction in the axial and radial planes, and the Tangential-Velocity. Specify the X, Y, and Z components of the Axis Origin and the Axis Direction.

  Local Cylindrical Swirl should not be used for open channel boundary conditions and on the mixing plane boundaries, while using the mixing plane model.

4.   If you selected Normal to Boundary, there are no additional inputs for flow direction.

Note that if you are modeling axisymmetric swirl, the flow direction will be normal to the boundary; i.e., there will be no swirl component at the boundary for axisymmetric swirl.

5.   If Outward Normals is selected, then the mass flow boundary will operate as an outflow, pumping flow out of the domain with the rate specified in the Mass Flow Specification Method. If the mass flow rate is specified, then by default, the fluxes on the boundary will be allowed to vary to preserve the flow profile out of the domain. At convergence, the total mass flow rate should match the specified value. If constant mass flux is needed rather than the default variable fluxes to preserve the profiles, then you can do so via the text command define /boundary-conditions/bc-settings/mass-flow. Answer no when asked to preserve profile while flow leaves.

The mass flow boundary can also operate as an outflow using the Direction Vector flow specification method if the flow components are pointing away from the boundary.

Defining Turbulence Parameters

For turbulent calculations, there are several ways in which you can define the turbulence parameters. Instructions for deciding which method to use and determining appropriate values for these inputs are provided in Section  7.3.2. Turbulence modeling is described in Chapter  12.

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 (optionally) External Black Body Temperature. See Section  13.3.6 for details. (The Rosseland radiation model does not require any boundary condition inputs.)

Defining Species Mass or Mole Fractions

If you are modeling species transport, you will set the species mass or mole fractions under Species Mole Fractions or Species Mass Fractions. For details, see Section  15.1.5.

Defining Non-Premixed Combustion Parameters

If you are using the non-premixed or partially premixed combustion model, you will set the Mean Mixture Fraction and Mixture Fraction Variance (and the Secondary Mean Mixture Fraction and Secondary Mixture Fraction Variance, if you are using two mixture fractions), as described in Section  16.8.

Defining Premixed Combustion Boundary Conditions

If you are using the premixed or partially premixed combustion model, you will set the Progress Variable, as described in Section  17.3.3.

Defining Discrete Phase Boundary Conditions

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the mass flow inlet. 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 Mass Flow Inlet Boundaries

Default settings (in SI) for mass flow inlet boundary conditions are as follows:

Mass Flow-Rate	1
Total Temperature	300
Supersonic/Initial Gauge Pressure	0
X-Component of Flow Direction	1
Y-Component of Flow Direction	0
Z-Component of Flow Direction	0
Turbulent Kinetic Energy	1
Turbulent Dissipation Rate	1

Calculation Procedure at Mass Flow Inlet Boundaries

When mass flow boundary conditions are used for an inlet zone, a velocity is computed for each face in that zone, and this velocity is used to compute the fluxes of all relevant solution variables into the domain. With each iteration, the computed velocity is adjusted so that the correct mass flow value is maintained.

To compute this velocity, your inputs for mass flow rate, flow direction, static pressure, and total temperature are used.

There are two ways to specify the mass flow rate. The first is to specify the total mass flow rate, $\dot{m}$, for the inlet. The second is to specify the mass flux, $\rho v_n$ (mass flow rate per unit area). If a total mass flow rate is specified, ANSYS FLUENT converts it internally to a uniform mass flux by dividing the mass flow rate by the total inlet area:

If the direct mass flux specification option is used, the mass flux can be varied over the boundary by using profile files or user-defined functions. If the average mass flux is also specified (either explicitly by you or automatically by ANSYS FLUENT), it is used to correct the specified mass flux profile, as described earlier in this section.

Once the value of $\rho v_n$ at a given face has been determined, the density, $\rho$, at the face must be determined in order to find the normal velocity, $v_n$. The manner in which the density is obtained depends upon whether the fluid is modeled as an ideal gas or not. Each of these cases is examined below.

Flow Calculations at Mass Flow Boundaries for Ideal Gases

If the fluid is an ideal gas, the static temperature and static pressure are required to compute the density:

If the inlet is supersonic, the static pressure used is the value that has been set as a boundary condition. If the inlet is subsonic, the static pressure is extrapolated from the cells inside the inlet face.

The static temperature at the inlet is computed from the total enthalpy, which is determined from the total temperature that has been set as a boundary condition. The total enthalpy is given by

where the velocity magnitude is related to the mass flow rate given by Equation  7.3-27 and the known user-specified flow direction vector. Using Equation  7.3-28 to relate density to the (known) static pressure and (unknown) temperature, Equation  7.3-29 can be solved to obtain the static temperature.

When the mass flow is used as an outflow with the profile preserving feature, a scaling factor of the specified mass flow rate over the computed mass flow rate at the boundary is used to scale the normal face velocities at the boundary. The other velocity components will be extrapolated from the interior. Flow variables such as pressure, temperature, species, or other scalar quantities will be also extrapolated from adjacent cell centers.

Flow Calculations at Mass Flow Boundaries for Incompressible Flows

When you are modeling incompressible flows, the static temperature is equal to the total temperature. The density at the inlet is either constant or readily computed as a function of the temperature and (optionally) the species mass or mole fractions. The velocity is then computed using Equation  7.3-27.

Flux Calculations at Mass Flow Boundaries

To compute the fluxes of all variables at the inlet, the flux velocity, $v_n$, is used along with the inlet value of the variable in question. For example, the flux of mass is $\rho v_n$, and the flux of turbulence kinetic energy is $\rho k v_n$. These fluxes are used as boundary conditions for the corresponding conservation equations during the course of the solution.