7.3.4 Velocity Inlet Boundary Conditions

Velocity inlet boundary conditions are used to define the flow velocity, along with all relevant scalar properties of the flow, at flow inlets. In this case, the total (or stagnation) pressure is not fixed but will rise (in response to the computed static pressure) to whatever value is necessary to provide the prescribed velocity distribution.

This boundary condition is intended for incompressible flows, and its use in compressible flows will lead to a nonphysical result because it allows stagnation conditions to float to any level. You should also be careful not to place a velocity inlet too close to a solid obstruction, since this could cause the inflow stagnation properties to become highly non-uniform.

In special instances, a velocity inlet may be used in ANSYS FLUENT to define the flow velocity at flow exits. (The scalar inputs are not used in such cases.) In such cases you must ensure that overall continuity is maintained in the domain.

For an overview of flow boundaries, see Section  7.3.1.

Inputs at Velocity Inlet Boundaries

Summary

You will enter the following information for a velocity inlet boundary:

• type of reference frame

• velocity magnitude and direction or velocity components

• swirl velocity (for 2D axisymmetric problems with swirl)

• temperature (for energy calculations)

• outflow gauge pressure (for calculations with the density-based solver)

• 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)

• multiphase boundary conditions (for general multiphase calculations)

All values are entered in the Velocity Inlet dialog box (Figure  7.3.3), which is opened from the Boundary Conditions task page (as described in Section  7.1.4).

Figure 7.3.3: The Velocity Inlet Dialog Box

Defining the Velocity

You can define the inflow velocity by specifying the velocity magnitude and direction, the velocity components, or the velocity magnitude normal to the boundary. If the cell zone adjacent to the velocity inlet is moving (i.e., if you are using a rotating reference frame, multiple reference frames, or sliding meshes), you can specify either relative or absolute velocities. For axisymmetric problems with swirl in ANSYS FLUENT, you will also specify the swirl velocity.

The procedure for defining the inflow velocity is as follows:

1.   Specify the flow direction by selecting Magnitude and Direction, Components, or Magnitude, Normal to Boundary in the Velocity Specification Method drop-down list.

2.   If the cell zone adjacent to the velocity inlet is moving, you can choose to specify relative or absolute velocities by selecting Relative to Adjacent Cell Zone or Absolute in the Reference Frame drop-down list. If the adjacent cell zone is not moving, Absolute and Relative to Adjacent Cell Zone will be equivalent, so you need not visit the list.

3.   If you are going to set the velocity magnitude and direction or the velocity components, and your geometry is 3D, choose Cartesian (X, Y, Z), Cylindrical (Radial, Tangential, Axial), or Local Cylindrical (Radial, Tangential, Axial) from the Coordinate System drop-down list. See Section  7.3.3 for information about Cartesian, cylindrical, and local cylindrical coordinate systems.

4.   Set the appropriate velocity parameters, as described below for each specification method.

Setting the Velocity Magnitude and Direction

If you selected Magnitude and Direction as the Velocity Specification Method in step 1 above, you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity Magnitude) and the direction of the vector:

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

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

• If you chose in step 3 to use a 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 the Axis Origin and the Axis Direction.

Figure  7.3.2 shows the vector components for these different coordinate systems.

Setting the Velocity Magnitude Normal to the Boundary

If you selected Magnitude, Normal to Boundary as the Velocity Specification Method in step 1 above, you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity Magnitude).

Setting the Velocity Components

If you selected Components as the Velocity Specification Method in step 1 above, you will enter the components of the velocity vector at the inflow boundary as follows:

• If your geometry is 2D non-axisymmetric, or you chose in step 3 to use the Cartesian coordinate system, you will define the X, Y, and (in 3D) Z-Velocity.

• If your geometry is 2D axisymmetric without swirl, you will set the Radial and Axial-Velocity.

• If your model is 2D axisymmetric with swirl, you will set the Axial, Radial, and Swirl-Velocity, and (optionally) the Angular Velocity, as described below.

• If you chose in step 3 to use a Cylindrical coordinate system, you will set the Radial, Tangential, and Axial-Velocity, and (optionally) the Angular Velocity, as described below.

• If you chose in step 3 to use a Local Cylindrical coordinate system, you will set the Radial, Tangential, and Axial-Velocity, and (optionally) the Angular Velocity, as described below, and then specify the X, Y, and Z component of the Axis Origin and the Axis Direction.

Remember that positive values for $x$, $y$, and $z$ velocities indicate flow in the positive $x$, $y$, and $z$ directions. If flow enters the domain in the negative $x$ direction, for example, you will need to specify a negative value for the $x$ velocity. The same holds true for the radial, tangential, and axial velocities. Positive radial velocities point radially out from the axis, positive axial velocities are in the direction of the axis vector, and positive tangential velocities are based on the right-hand rule using the positive axis.

Setting the Angular Velocity

If you chose Components as the Velocity Specification Method in step 1 above, and you are modeling axisymmetric swirl, you can specify the inlet Angular Velocity $\Omega$ in addition to the Swirl-Velocity. Similarly, if you chose Components as the Velocity Specification Method and you chose in step 3 to use a Cylindrical or Local Cylindrical coordinate system, you can specify the inlet Angular Velocity $\Omega$ in addition to the Tangential-Velocity.

If you specify $\Omega$, $v_\theta$ is computed for each face as $\Omega r$, where $r$ is the radial coordinate in the coordinate system defined by the rotation axis and origin. If you specify both the Swirl-Velocity and the Angular Velocity, or the Tangential-Velocity and the Angular Velocity, ANSYS FLUENT will add $v_\theta$ and $\Omega r$ to get the swirl or tangential velocity at each face.

Defining the Temperature

For calculations in which the energy equation is being solved, you will set the static temperature of the flow at the velocity inlet boundary in the Thermal tab in the Temperature field.

Defining Outflow Gauge Pressure

If you are using the density-based solver, you can specify an Outflow Gauge Pressure for a velocity inlet boundary. If the flow exits the domain at any face on the boundary, that face will be treated as a pressure outlet with the pressure prescribed in the Outflow Gauge Pressure field.

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 in general 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 velocity inlet. See Section  23.4 for details.

Defining Multiphase Boundary Conditions

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.

Default Settings at Velocity Inlet Boundaries

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

Temperature	300
Velocity Magnitude	0
X-Component of Flow Direction	1
Y-Component of Flow Direction	0
Z-Component of Flow Direction	0
X-Velocity	0
Y-Velocity	0
Z-Velocity	0
Turbulent Kinetic Energy	1
Turbulent Dissipation Rate	1
Outflow Gauge Pressure	0

Calculation Procedure at Velocity Inlet Boundaries

ANSYS FLUENT uses your boundary condition inputs at velocity inlets to compute the mass flow into the domain through the inlet and to compute the fluxes of momentum, energy, and species through the inlet. This section describes these calculations for the case of flow entering the domain through the velocity inlet boundary and for the less common case of flow exiting the domain through the velocity inlet boundary.

Treatment of Velocity Inlet Conditions at Flow Inlets

When your velocity inlet boundary condition defines flow entering the physical domain of the model, ANSYS FLUENT uses both the velocity components and the scalar quantities that you defined as boundary conditions to compute the inlet mass flow rate, momentum fluxes, and fluxes of energy and chemical species.

The mass flow rate entering a fluid cell adjacent to a velocity inlet boundary is computed as

Note that only the velocity component normal to the control volume face contributes to the inlet mass flow rate.

Treatment of Velocity Inlet Conditions at Flow Exits

Sometimes a velocity inlet boundary is used where flow exits the physical domain. This approach might be used, for example, when the flow rate through one exit of the domain is known or is to be imposed on the model.

In such cases you must ensure that overall continuity is maintained in the domain.

In the pressure-based solver, when flow exits the domain through a velocity inlet boundary ANSYS FLUENT uses the boundary condition value for the velocity component normal to the exit flow area. It does not use any other boundary conditions that you have input. Instead, all flow conditions except the normal velocity component are assumed to be those of the upstream cell.

In the density-based solver, if the flow exits the domain at any face on the boundary, that face will be treated as a pressure outlet with the pressure prescribed in the Outflow Gauge Pressure field.

Density Calculation

Density at the inlet plane is either constant or calculated as a function of temperature, pressure, and/or species mass/mole fractions, where the mass or mole fractions are the values you entered as an inlet condition.