6.3.5. 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 Pressure Inlet Boundary Conditions), where the total pressure is fixed while the mass flux varies. The mass-flow inlet is applicable to incompressible and compressible flows.


Important:  Use caution when specifying the mass-flow inlet boundary condition for a compressible fluid in internal flow modeling. If the flow path is completely choked with no secondary flow path for relief, the mass-flow inlet boundary condition is not recommended, as it can cause numerical instabilities. In this case, you should switch to the pressure inlet boundary condition or refrain from reaching operating conditions that choke the internal flow. The choking condition can happen in high speed supersonic and transonic flow.


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.

6.3.5.1. 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.

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

6.3.5.2. Inputs at Mass-Flow Inlet Boundaries

6.3.5.2.1. 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, DTRM, DO, surface-to-surface, or MC models)

  • 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)

  • acoustic wave model settings

All values are entered in the Mass-Flow Inlet Dialog Box (Figure 6.23: The Mass-Flow Inlet 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 6.23:  The Mass-Flow Inlet Dialog Box

The Mass-Flow Inlet Dialog Box

6.3.5.2.2. 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.

6.3.5.2.3. 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. Make a selection in the Mass Flow Specification Method drop-down list to specify whether you will define a Mass Flow Rate, Mass Flux, or Mass Flux with Average Mass Flux.

  2. If you selected Mass Flow Rate (the default), enter the prescribed Mass Flow Rate when constant is selected from the drop-down list. Otherwise, select your hooked user-defined function (UDF) or transient profile.


    Important:  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 DEFINE_PROFILE in the Fluent Customization Manual for an example of a mass-flow inlet UDF.


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


  3. If you selected Mass Flux, enter the prescribed Mass Flux, or select your hooked UDF or profile.

  4. If you selected Mass Flux with Average Mass Flux, enter the prescribed Mass Flux and Average Mass Flux.


Important:  Note that for axisymmetric problems, the Mass Flux and Average Mass Flux is the flux through a 1-radian slice of the domain.


6.3.5.2.4. More About Mass Flux and Average Mass Flux

As noted previously, 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 The Mixing Plane Model. 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.

6.3.5.2.5. 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.


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



Important:
  • 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.


6.3.5.2.6. 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 Initializing the Solution.

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 Pressure Inputs and Hydrostatic Head regarding hydrostatic pressure.

6.3.5.2.7. 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 6.23: The Mass-Flow Inlet Dialog Box:

  1. Specify the flow direction by selecting Direction Vector or Normal to Boundary 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 Defining the Flow Direction 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.


      Important:   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.


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


6.3.5.2.8. 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 Determining Turbulence Parameters. Turbulence modeling is described in Modeling Turbulence.

6.3.5.2.9. 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 (optionally) External Black Body Temperature. See Defining Boundary Conditions for Radiation for details. (The Rosseland radiation model does not require any boundary condition inputs.)

6.3.5.2.10. 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 Defining Cell Zone and Boundary Conditions for Species.

6.3.5.2.11. 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 Defining Non-Premixed Boundary Conditions.

6.3.5.2.12. 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 Setting Boundary Conditions for the Progress Variable.

6.3.5.2.13. 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 Setting Boundary Conditions for the Discrete Phase for details.

6.3.5.2.14. 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.

6.3.5.3. 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 Intensity 5%
Turbulent Viscosity Ratio 10

6.3.5.4. 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, , for the inlet. The second is to specify the mass flux, (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:

(6–84)

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 at a given face has been determined, the density, , at the face must be determined in order to find the normal velocity, . 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.

6.3.5.4.1. 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:

(6–85)

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

(6–86)

where the velocity magnitude is related to the mass flow rate given by Equation 6–84 and the known user-specified flow direction vector. Using Equation 6–85 to relate density to the (known) static pressure and (unknown) temperature, Equation 6–86 can be solved to obtain the static temperature.

6.3.5.4.2. 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 6–84.

6.3.5.4.3. Flux Calculations at Mass Flow Boundaries

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


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