## 7.3.1 Inputs at Pressure Inlet Boundaries

Summary

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

• total (stagnation) pressure

• total (stagnation) temperature

• flow direction

• static pressure

• 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 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)

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

All values are entered in the Pressure Inlet panel (Figure  7.3.1), which is opened from the Boundary Conditions panel (as described in Section  7.1.4). Note that open channel boundary condition inputs are described in Section  23.10.2.

The pressure field ( ) and your pressure inputs ( or ) include the hydrostatic head , . That is, the pressure in FLUENT is defined as

 (7.3-1)

or

 (7.3-2)

This definition allows the hydrostatic head to be taken into the body force term, , and excluded from the pressure calculation when the density is uniform. Thus your inputs of pressure should not include hydrostatic pressure differences, and reports of pressure ( ) will not show any influence of the hydrostatic pressure. See Section  13.2.5 for information about buoyancy-driven (natural-convection) flows.

Defining Total Pressure and Temperature

Enter the value for total pressure in the Gauge Total Pressure field in the Pressure Inlet panel. Total temperature is set in the Total Temperature field.

Remember that the total pressure value is the gauge pressure with respect to the operating pressure defined in the Operating Conditions panel. Total pressure for an incompressible fluid is defined as

 (7.3-3)

and for a compressible fluid of constant as

 (7.3-4)

 where = total pressure = static pressure M = Mach number = ratio of specific heats

If you are modeling axisymmetric swirl, in Equation  7.3-3 will include the swirl component.

If the adjacent cell zone is moving (i.e., if you are using a rotating reference frame, multiple reference frames, a mixing plane, or sliding meshes) and you are using the pressure-based solver, the velocity in Equation  7.3-3 (or the Mach number in Equation  7.3-4) will be absolute or relative to the grid velocity, depending on whether or not the Absolute velocity formulation is enabled in the Solver panel. For the density-based solvers, the velocity in Equation  7.3-3 (or the Mach number in Equation  7.3-4) is always in the absolute frame.

Defining the Flow Direction

You can define the flow direction at a pressure inlet explicitly, or you can define the flow to be normal to the boundary. If you choose to specify the direction vector, you can set either the (Cartesian) , , and components, or the (cylindrical) radial, tangential, and axial components.

For moving zone problems calculated using the pressure-based solver, the flow direction will be absolute or relative to the grid velocity, depending on whether or not the Absolute velocity formulation is enabled in the Solver panel. For the density-based solvers, the flow direction will always be in the absolute frame.

The procedure for defining the flow direction is as follows, referring to Figure  7.3.1:

1.   Choose which method you will use to specify the flow direction by selecting Direction Vector or Normal to Boundary in the Direction Specification Method drop-down list.

2.   If you selected Normal to Boundary in step 1 and you are modeling axisymmetric swirl, enter the appropriate value for the Tangential-Component of Flow Direction. If you chose Normal to Boundary and your geometry is 3D or 2D without axisymmetric swirl, there are no additional inputs for flow direction.

3.   If you chose in step 1 to specify the direction vector, and your geometry is 3D, you will next choose the coordinate system in which you will define the vector components. Choose Cartesian (X, Y, Z), Cylindrical (Radial, Tangential, Axial), or Local Cylindrical (Radial, Tangential, Axial) in the Coordinate System drop-down list.

• The Cartesian coordinate system is based on the Cartesian coordinate system used by the geometry.

• The Cylindrical coordinate system uses the axial, radial, and tangential components based on the following coordinate systems:

• For problems involving a single cell zone, the coordinate system is defined by the rotation axis and origin specified in the Fluid panel.

• For problems involving multiple zones (e.g., multiple reference frames or sliding meshes), the coordinate system is defined by the rotation axis specified in the Fluid (or Solid) panel for the fluid (or solid) zone that is adjacent to the inlet.

For all of the above definitions of the cylindrical coordinate system, positive radial velocities point radially out from the rotation axis, positive axial velocities are in the direction of the rotation axis vector, and positive tangential velocities are based on the right-hand rule using the positive rotation axis (see Figure  7.3.2).

• The Local Cylindrical coordinate system allows you to define a coordinate system specifically for the inlet. When you use the local cylindrical option, you will define the coordinate system right here in the Pressure Inlet panel. The local cylindrical coordinate system is useful if you have several inlets with different rotation axes.

4.   If you chose in step 1 to specify the direction vector, define the vector components as follows:

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

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

• If you are using Local Cylindrical coordinates, enter the appropriate values for Axial, Radial, and Tangential-Component of Flow Direction, and then specify the X, Y, and Z-Component of Axis Direction and the X, Y, and Z-Coordinate of Axis Origin.

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

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  25.14.

Remember that the static pressure value you enter is relative to the operating pressure set in the Operating Conditions panel. Note the comments in Section  7.3.1 regarding hydrostatic pressure.

The Supersonic/Initial Gauge Pressure is ignored by FLUENT whenever the flow is subsonic, in which case it is calculated from the specified stagnation quantities. If you choose to initialize the solution based on the pressure-inlet conditions, the Supersonic/Initial Gauge Pressure will be used in conjunction with the specified stagnation pressure to compute initial values according to the isentropic relations (for compressible flow) or Bernoulli's equation (for incompressible flow). Therefore, for a sub-sonic inlet it should generally be set based on a reasonable estimate of the inlet Mach number (for compressible flow) or inlet velocity (for incompressible flow).

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  7.2.2. Turbulence modeling in general is described in Chapter  12.

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) Black Body Temperature. See Section  13.3.15 for details. (The Rosseland radiation model does not require any boundary condition inputs.)

Defining Species Mass Fractions

If you are modeling species transport, you will set the species mass fractions under Species Mass Fractions. For details, see Section  14.1.5.

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  15.13.

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  16.3.5.

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 inlet. See Section  22.13 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  23.9.8 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  23.10.2 for details.

Previous: 7.3 Pressure Inlet Boundary
Up: 7.3 Pressure Inlet Boundary
Next: 7.3.2 Default Settings at