
Summary
You will enter the following information for a pressure inlet boundary:
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.
Pressure Inputs and Hydrostatic Head
The pressure field ( ) and your pressure inputs ( or ) include the hydrostatic head , . That is, the pressure in FLUENT is defined as
or
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 buoyancydriven (naturalconvection) 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
and for a compressible fluid of constant as
where  =  total pressure  
=  static pressure  
M  =  Mach number  
=  ratio of specific heats 
If you are modeling axisymmetric swirl, in Equation 7.33 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 pressurebased solver, the velocity in Equation 7.33 (or the Mach number in Equation 7.34) 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 densitybased solvers, the velocity in Equation 7.33 (or the Mach number in Equation 7.34) 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 pressurebased 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 densitybased 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:
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 righthand rule using the positive rotation axis (see Figure 7.3.2).
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 pressureinlet 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 subsonic 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.
Defining Radiation Parameters
If you are using the P1 radiation model, the DTRM, the DO model, or the surfacetosurface 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 NonPremixed Combustion Parameters
If you are using the nonpremixed 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.