ANSYS FLUENT 12.0 User's Guide - 7.3.3 Pressure Inlet Boundary Conditions

7.3.3 Pressure Inlet Boundary Conditions

Pressure inlet boundary conditions are used to define the fluid pressure at flow inlets, along with all other scalar properties of the flow. They are suitable for both incompressible and compressible flow calculations. Pressure inlet boundary conditions can be used when the inlet pressure is known but the flow rate and/or velocity is not known. This situation may arise in many practical situations, including buoyancy-driven flows . Pressure inlet boundary conditions can also be used to define a "free'' boundary in an external or unconfined flow.

For an overview of flow boundaries, see Section 7.3.1.

Inputs at Pressure Inlet Boundaries

Summary

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

type of reference frame
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 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)
open channel flow parameters (for open channel flow calculations using the VOF multiphase model)

All values are entered in the Pressure Inlet dialog box (Figure 7.3.1), 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 7.3.1:** The **Pressure Inlet** Dialog Box

Pressure Inputs and Hydrostatic Head

When gravitational acceleration is activated in the Operating Conditions dialog box (accessed from the Boundary Conditions task page), the pressure field (including all pressure inputs) will include the hydrostatic head. This is accomplished by redefining the pressure in terms of a modified pressure which includes the hydrostatic head (denoted ) as follows:

$p' = p + \rho_0{\vec g}\cdot{\vec r}$

(7.3-12)

where $\rho_0$ is a constant reference density, $\vec g$ is the gravity vector (also a constant), and

${\vec r} = x{\hat i} + y{\hat j} + z{\hat k}$

(7.3-13)

is the position vector. Noting that

$\nabla(\rho_{0}{\vec g}\cdot{\vec r}) = \rho_{0}{\vec g}$

(7.3-14)

it follows that

$\nabla p'= \nabla(p + \rho_0{\vec g}\cdot{\vec r})=\nabla p - \rho_0{\vec g}$

(7.3-15)

The substitution of this relation in the momentum equation gives pressure gradient and gravitational body force terms of the form

$\nabla p' + (\rho - \rho_0){\vec g}$

(7.3-16)

where $\rho$ is the fluid density. Therefore, if the fluid density is constant, we can set the reference density $\rho_0$ equal to the fluid density, thereby eliminating the body force term. If the fluid density is not constant (for example, density is given by the ideal gas law), then the reference density should be chosen to be representative of the average or mean density in the fluid domain, so that the body force term is small.

An important consequence of this treatment of the gravitational body force is that your inputs of pressure (now defined as ) should not include hydrostatic pressure differences. Moreover, reports of static and total pressure will not show any influence of the hydrostatic pressure. See Section 13.2.4 for additional information.

Defining Total Pressure and Temperature

Enter the value for total pressure in the Gauge Total Pressure field in the Pressure Inlet dialog box. Total temperature is set in the Thermal tab, 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 dialog box. Total pressure for an incompressible fluid is defined as

$p_0 = p_s + \frac{1}{2} \rho \vert\vec v \vert^2$

(7.3-17)

and for a compressible fluid of constant as

${p_0} = p_s \left (1 + \frac{\gamma - 1}{2} {\rm M}^2 \right )^{\gamma/(\gamma-1)}$

(7.3-18)

where		=	total pressure
		=	static pressure
	M	=	Mach number
	$\gamma$	=	ratio of specific heats $(c_p/c_{\rm v})$

If you are modeling axisymmetric swirl, ${\vec v}$ in Equation 7.3-17 will include the swirl component.

If the cell zone adjacent to a pressure inlet is defined as a moving reference frame zone, and you are using the pressure-based solver, the velocity in Equation 7.3-17 (or the Mach number in Equation 7.3-18) will be absolute or relative to the mesh velocity, depending on whether or not the Absolute velocity formulation is enabled in the General task page. For the density-based solver, the Absolute velocity formulation is always used; hence, the velocity in Equation 7.3-17 (or the Mach number in Equation 7.3-18) is always the Absolute velocity.

If Reference Frame is set to Absolute in the Pressure Inlet dialog box, then the total temperature, total pressure, and flow direction are also in the absolute reference frame, and therefore, the ANSYS FLUENT solver will convert it to the relative reference frame.
If Reference Frame is set to Relative to Adjacent Cell Zone in the Pressure Inlet dialog box, then the total temperature, total pressure, and velocity components are also relative to the adjacent cell zone and no change is needed.

For the Eulerian multiphase model, the total temperature, and velocity 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 the total pressure values need to be specified in the mixture phase.

If the flow is incompressible, then the temperature assigned in the Pressure Inlet dialog box will be considered 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 Pressure Inlet dialog box will be considered the static temperature at that boundary. If a boundary allows only a compressible phase to enter the domain, then the temperature assigned in the Pressure Inlet dialog box will be taken as the total temperature (relative/absolute) at that boundary. The total temperature will depend on the Reference Frame option selected in the Pressure 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 Pressure Inlet dialog box will be considered the total temperature at that boundary. The total temperature (relative/absolute) will depend on the Reference Frame option chosen in the dialog box. Otherwise, the temperature assigned to the boundary will be considered 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 will be the total or static temperature, depending on whether the phase is compressible or incompressible.

Total temperature (relative/absolute) will depend on the Reference Frame option chosen in the Pressure Inlet dialog box.

Defining the Flow Direction

The flow direction is defined as a unit vector ( $\vec d$ ) which is aligned with the local velocity vector, $\vec v$ . This can be expressed simply as

$\vec d = \frac{\vec v}{\vert\vec v\vert}$

(7.3-19)

For the inputs in ANSYS FLUENT, the flow direction $\vec d$ need not be a unit vector, as it will be automatically normalized before it is applied.

For a rotating reference frame, the relative flow direction $\vec d_{r}$ is defined in terms of the relative velocity, $\vec v_{r}$ . Thus,

$\vec d_{r} = \frac{\vec v_r}{\vert\vec v_r\vert}$ (7.3-20)

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 mesh velocity, depending on whether or not the Absolute velocity formulation is enabled in the General task page. For the density-based solver, the flow direction will always be in the absolute frame.

The procedure for defining the flow direction is as follows (refer to Figure 7.3.1):

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 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 selected Direction Vector in step 1, and your geometry is 3D, choose Cartesian (X, Y, Z), Cylindrical (Radial, Tangential, Axial), Local Cylindrical (Radial, Tangential, Axial), or Local Cylindrical Swirl from the Coordinate System drop-down list. Some notes on these selections are provided below:

The Cartesian coordinate option is based on the Cartesian coordinate system used by the geometry. Enter appropriate values for the X, Y, and Z-Component of Flow Direction.

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 dialog box.

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) dialog box 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 outward 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).

Figure 7.3.2: Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains

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 dialog box. The local cylindrical coordinate system is useful if you have several inlets with different rotation axes. 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 Axis Direction.

The Local Cylindrical Swirl coordinate system option allows you to define a coordinate system specifically for the inlet where the total pressure, swirl velocity, and the components of the velocity in the axial and radial planes are specified. Enter appropriate values for the Axial and Radial-Component of Flow Direction, and the Tangential-Velocity. Specify the X, Y, and Z components of the Axis Origin and Axis Direction. It is recommended that you start your simulation with a smaller swirl velocity and then progressively increase the velocity to obtain a stable solution.

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 Direction Vector in step 1, and your geometry is 2D, define the vector components as follows:

For a 2D planar geometry, enter appropriate values for the X, Y, and Z-Component of Flow Direction.

For a 2D axisymmetric geometry, enter appropriate values for the Axial, Radial-Component of Flow Direction.

For a 2D axisymmetric swirl geometry, enter appropriate values for the Axial, Radial, and Tangential-Component of Flow Direction.

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 26.9.

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.

The Supersonic/Initial Gauge Pressure is ignored by ANSYS 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 7.3.2. 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 pressure 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.

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 Pressure Inlet Boundaries

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

Gauge Total Pressure	0
Supersonic/Initial Gauge Pressure	0
Total Temperature	300
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 Pressure Inlet Boundaries

The treatment of pressure inlet boundary conditions by ANSYS FLUENT can be described as a loss-free transition from stagnation conditions to the inlet conditions. For incompressible flows, this is accomplished by application of the Bernoulli equation at the inlet boundary. In compressible flows, the equivalent isentropic flow relations for an ideal gas are used.

Incompressible Flow Calculations at Pressure Inlet Boundaries

When flow enters through a pressure inlet boundary, ANSYS FLUENT uses the boundary condition pressure you input as the total pressure of the fluid at the inlet plane, . In incompressible flow , the inlet total pressure and the static pressure, , are related to the inlet velocity via Bernoulli's equation:

$p_0= p_s + \frac{1}{2} \rho v^2$

(7.3-21)

With the resulting velocity magnitude and the flow direction vector you assigned at the inlet, the velocity components can be computed. The inlet mass flow rate and fluxes of momentum, energy, and species can then be computed as outlined in Section 7.3.4.

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

If flow exits through a pressure inlet, the total pressure specified is used as the static pressure. For incompressible flows, total temperature is equal to static temperature.

Compressible Flow Calculations at Pressure Inlet Boundaries

In compressible flows , isentropic relations for an ideal gas are applied to relate total pressure, static pressure, and velocity at a pressure inlet boundary. Your input of total pressure, , at the inlet and the static pressure, , in the adjacent fluid cell are thus related as

$\frac{p'_0 + p_{\rm op}}{p'_s + p_{\rm op}} = \left (1 + \frac{\gamma - 1}{2} {\rm M}^2 \right )^{\gamma / (\gamma - 1)}$

(7.3-22)

where

${\rm M} \equiv \frac{v}{c} = \frac{v}{\sqrt{\gamma R T_s}}$

(7.3-23)

= the speed of sound, and $\gamma = c_p/c_{\rm v}$ . Note that the operating pressure, $p_{\rm op}$ , appears in Equation 7.3-22 because your boundary condition inputs are in terms of pressure relative to the operating pressure. Given $p'_{0}$ and $p'_{s}$ , Equations 7.3-22 and 7.3-23 are used to compute the velocity magnitude of the fluid at the inlet plane. Individual velocity components at the inlet are then derived using the direction vector components.

For compressible flow, the density at the inlet plane is defined by the ideal gas law in the form

$\rho = \frac{p_s' + p_{\rm op}}{RT_s}$

(7.3-24)

For multi-species gas mixtures, the specific gas constant, , is computed from the species mass or mole fractions, that you defined as boundary conditions at the pressure inlet boundary. The static temperature at the inlet, , is computed from your input of total temperature, , as

$\frac{T_0}{T_s} = 1 + \frac{\gamma - 1}{2} {\rm M}^2$

(7.3-25)

Previous: 7.3.2 Using Flow Boundary
Up: 7.3 Boundary Conditions
Next: 7.3.4 Velocity Inlet Boundary