If it is important to accurately represent a boundary layer or fully-developed turbulent flow at the inlet, you should ideally set the turbulence quantities by creating a profile file (see Profiles) from experimental data or empirical formulas. If you have an analytical description of the profile, rather than data points, you can either use this analytical description to create a profile file, or create a user-defined function to provide the inlet boundary information. (See the Fluent Customization Manual for information on user-defined functions.)

Once you have created the profile function, you can use it as described below:

In some situations, it is appropriate to specify a uniform value of the turbulence quantity at the boundary where inflow occurs. Examples are fluid entering a duct, far-field boundaries, or even fully-developed duct flows where accurate profiles of turbulence quantities are unknown.

In most turbulent flows, higher levels of turbulence are generated within shear layers than enter the domain at flow boundaries, making the result of the calculation relatively insensitive to the inflow boundary values. Nevertheless, caution must be used to ensure that boundary values are not so unphysical as to contaminate your solution or impede convergence. This is particularly true of external flows where unphysically large values of effective viscosity in the free stream can “swamp” the boundary layers.

You can use the turbulence specification methods described above to enter uniform constant values instead of profiles. Alternatively, you can specify the turbulence quantities in terms of more convenient quantities such as turbulence intensity, turbulent viscosity ratio, hydraulic diameter, and turbulence length scale. The default Turbulence Specification Method is set to Turbulent Viscosity Ratio (for the Spalart-Allmaras model) or Intensity and Viscosity Ratio (for the -  models, the -  models, or the RSM). These quantities are discussed further in the following sections.

The turbulence intensity, , is defined as the ratio of the root-mean-square of the velocity fluctuations, , to the mean flow velocity, .

A turbulence intensity of 1% or less is generally considered low and turbulence intensities greater than 10% are considered high. Ideally, you will have a good estimate of the turbulence intensity at the inlet boundary from external, measured data. For example, if you are simulating a wind-tunnel experiment, the turbulence intensity in the free stream is usually available from the tunnel characteristics. In modern low-turbulence wind tunnels, the free-stream turbulence intensity may be as low as 0.05%.

For internal flows, the turbulence intensity at the inlets is totally dependent on the upstream history of the flow. If the flow upstream is under-developed and undisturbed, you can use a low turbulence intensity. If the flow is fully developed, the turbulence intensity may be as high as a few percent. The turbulence intensity at the core of a fully-developed duct flow can be derived from an empirical correlation by Blasius for pipe flows (see Chapter 20 Equations (20-4) and (20-5) in [137]), using the additional estimation of the RMS velocity fluctuation at the pipe core :

(7–72)

At a Reynolds number of 50,000, for example, the turbulence intensity will be 4%, according to this formula.

The default value for turbulence intensity is 5% (medium intensity).

The turbulence length scale, , is a physical quantity related to the size of the large eddies that contain the energy in turbulent flows.

In fully-developed duct flows, is restricted by the size of the duct, since the turbulent eddies cannot be larger than the duct. An approximate relationship between and the physical size of the duct is

(7–73)

where is the relevant dimension of the duct and ensures consistency with the definition of the turbulent length scales for one- and two-equation turbulence models. The factor of 0.07 is based on the maximum value of the mixing length in fully-developed turbulent pipe flow, where is the diameter of the pipe. In a channel of non-circular cross-section, you can base on the hydraulic diameter.

If the turbulence derives its characteristic length from an obstacle in the flow, such as a perforated plate, it is more appropriate to base the turbulence length scale on the characteristic length of the obstacle rather than on the duct size.

It should be noted that the relationship of Equation 7–73, which relates a physical dimension () to the turbulence length scale (), is not necessarily applicable to all situations. For most cases, however, it is a suitable approximation.

Guidelines for choosing the characteristic length or the turbulence length scale for selected flow types are listed below:

The turbulent viscosity ratio, , is directly proportional to the turbulent Reynolds number (). is large (on the order of 100 to 1000) in high-Reynolds-number boundary layers, shear layers, and fully-developed duct flows. However, at the free-stream boundaries of most external flows, is fairly small. Typically, the turbulence parameters are set so that . For internal flows values up to 100 are sensible for the turbulent viscosity ratio, . The default value for the turbulent viscosity ratio is set to 10.

To specify quantities in terms of the turbulent viscosity ratio, you can choose Turbulent Viscosity Ratio (for the Spalart-Allmaras model) or Intensity and Viscosity Ratio (for the -  models, the -  models, or the RSM). The default value for the turbulence intensity is set to 5% (medium intensity) and the turbulent viscosity ratio, , has a default value of 10.

To obtain the values of transported turbulence quantities from more convenient quantities such as , , or , you must typically resort to an empirical relations in addition to the formal definitions of these quantities. Several formal definitions and useful empirical relations, most of which are used within Ansys Fluent, are presented below.

To obtain the modified turbulent viscosity, , for the Spalart-Allmaras model from the turbulence intensity, , and length scale, , the following equation can be used. Note that this equation assumes that there is no viscous damping, that is, (see Modeling the Turbulent Viscosity in the Theory Guide).

(7–74)

This formula is also used in Ansys Fluent if you select the Intensity and Hydraulic Diameter specification method with the Spalart-Allmaras model. In this case, is obtained from Equation 7–73. ensures consistency with the definition of the eddy viscosity for - and - turbulence models. The value of is 0.09.

When using a moving reference frame, be aware of the order of the conversion operations applied to the inlet velocity and to the turbulence quantities, which is explained in the next section. It concerns the values of in Equation 7–74.

The relationship between the turbulent kinetic energy, , and turbulence intensity, , is

(7–75)

where is the magnitude of the mean flow velocity.

This relationship is used in Ansys Fluent whenever the Intensity and Hydraulic Diameter, Intensity and Length Scale, or Intensity and Viscosity Ratio method is used instead of specifying explicit values for and or .

If you know the turbulence length scale, , you can determine from the relationship

(7–76)

The determination of was discussed previously.

This relationship is used in Ansys Fluent whenever the Intensity and Hydraulic Diameter or Intensity and Length Scale method is used instead of specifying explicit values for and .

The value of can be obtained from the turbulent viscosity ratio and using the following relationship:

(7–77)

where is an empirical constant specified in the turbulence model.

This relationship is used in Ansys Fluent whenever the Intensity and Viscosity Ratio method is used instead of specifying explicit values for and .

If you are simulating a wind-tunnel situation in which the model is mounted in the test section downstream of a mesh and/or wire mesh screens, you can choose a value of such that

(7–78)

where is the approximate decay of you want to have across the flow domain (say, 10% of the inlet value of ), is the free-stream velocity, and is the streamwise length of the flow domain. Equation 7–78 is a linear approximation to the power-law decay observed in high-Reynolds-number isotropic turbulence. Its basis is the exact equation for in decaying turbulence, .

If you use this method to estimate , you should also check the resulting turbulent viscosity ratio to make sure that it is not too large, using Equation 7–77.

Although this method is not used internally by Ansys Fluent, you can use it to derive a constant free-stream value of that you can then specify directly by choosing K and Epsilon in the Turbulence Specification Method drop-down list. In this situation, you will typically determine from using Equation 7–75.

If you know the turbulence length scale, , you can determine from the relationship

(7–79)

where is an empirical constant specified in the turbulence model. The determination of was discussed previously.

This relationship is used in Ansys Fluent whenever the Intensity and Hydraulic Diameter or Intensity and Length Scale method is used instead of specifying explicit values for and .

The value of can be obtained from the turbulent viscosity ratio and using the following relationship:

(7–80)

This relationship is used in Ansys Fluent whenever the Intensity and Viscosity Ratio method is used instead of specifying explicit values for and .

When the RSM is used, if you do not specify the values of the Reynolds stresses explicitly at the inlet using the Reynolds-Stress Components option in the Reynolds-Stress Specification Method drop-down list, they are approximately determined from the specified values of . The turbulence is assumed to be isotropic such that

(7–81)

and

(7–82)

(no summation over the index ).

Ansys Fluent will use this method if you select K or Turbulence Intensity in the Reynolds-Stress Specification Method drop-down list.

When using Scale Resolving Simulations (SAS, DES, SDES, SBES, and LES models), it is possible to specify unsteady Fluctuating Velocity at velocity and pressure inlets to generate realistic turbulent content. Therefore, additional input is required for velocity and pressure inlets such as the choice of Fluctuating Velocity Algorithm and corresponding parameters (as shown in Figure 7.34: Specifying Inlet Turbulence for Scale Resolving Simulation). The available methods along with their options are described in Inlet Boundary Conditions for Scale Resolving Simulations in the Fluent Theory Guide. Note that even though some LES models do not require specification of the Turbulence parameters at the boundary, it is required when a Fluctuating Velocity Algorithm is selected. Additional parameters available for the Fluctuating Velocity Algorithm are listed in Pressure Inlet Dialog Box and Velocity Inlet Dialog Box.

Figure 7.34: Specifying Inlet Turbulence for Scale Resolving Simulation

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

All values are entered in the Pressure Inlet Dialog Box (Figure 7.35: The Pressure 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 7.35: The Pressure Inlet Dialog Box

 

7.4.3.1.1.1. 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 that includes the hydrostatic head (denoted ) as follows:

(7–83)

where is a constant operating density, is the gravity vector (also a constant), and

(7–84)

is the position vector. Noting that

(7–85)

it follows that

(7–86)

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

(7–87)

where is the fluid density. Therefore, if the fluid density is constant, we can set the operating density 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 operating 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 Buoyancy-Driven Flows and Natural Convection for additional information.

 

7.4.3.1.1.2. 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

(7–88)

and for a compressible fluid of constant as

(7–89)

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

If you are modeling axisymmetric swirl, in Equation 7–88 will include the swirl component.

The Total Temperature, Gauge Total Pressure, and flow directions are in absolute or relative to the adjacent cell zone reference frames, based on the Reference Frame setting in the Pressure Inlet dialog box.

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 7–88 (or the Mach number in Equation 7–89) 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 7–88 (or the Mach number in Equation 7–89) is always the Absolute velocity.

For the Eulerian multiphase model, the total temperature, and velocity components must 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 must be specified in the mixture phase.

---

Important:

• 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.

---

 

7.4.3.1.1.3. Defining the Flow Direction

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

(7–90)

---

Important:  For the inputs in Ansys Fluent, the flow direction need not be a unit vector, as it will be automatically normalized before it is applied.

---

---

Important:  For a moving reference frame, the relative flow direction is defined in terms of the relative velocity, . Thus,

(7–91)

---

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 selected 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 7.35: The Pressure 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 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 (for example, 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 7.36: Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains).

     Figure 7.36: 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.

     ---

     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 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 7.36: Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains shows the vector components for these different coordinate systems.

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:

(7–92)

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 Calculation Procedure at Velocity Inlet Boundaries.

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.

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 therefore related as

(7–93)

where

(7–94)

= the speed of sound, and . Note that the operating pressure, , appears in Equation 7–93 because your boundary condition inputs are in terms of pressure relative to the operating pressure. Given and , Equation 7–93 and  Equation 7–94 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

(7–95)

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

(7–96)

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

All values are entered in the Velocity Inlet Dialog Box (Figure 7.37: The Velocity Inlet Dialog Box), which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and Boundary Conditions ). Note that acoustic wave model settings are described in Boundary Acoustic Wave Models.

Figure 7.37: The Velocity Inlet Dialog Box

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 (that is, if you are using a moving 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:

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:

Figure 7.36: Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains shows the vector components for these different coordinate systems.

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).

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 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 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 in addition to the Tangential-Velocity.

If you specify , is computed for each face as , where 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 and to get the swirl or tangential velocity at each face.

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 velocity 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 velocity 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

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.

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.

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 in general is described in Modeling Turbulence.

The options available depend on which radiation model is active. For details, see Defining Boundary Conditions for Radiation.

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.

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.

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.

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the velocity inlet. See Setting Boundary Conditions for the Discrete Phase for details.

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 Defining Multiphase Cell Zone and Boundary Conditions for details.

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

(7–97)

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

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 the pressure-based solver, when flow exits the domain through a velocity inlet boundary condition, Ansys Fluent uses the boundary velocity to compute the flow flux through the exit flow area and the viscous term in the momentum equation. The convection term in all equations including momentum uses upwind discretization and takes the values of the upstream cells.

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 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.

You will enter the following information for a mass-flow inlet boundary:

All values are entered in the Mass-Flow Inlet Dialog Box (Figure 7.38: 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 7.38: The Mass-Flow Inlet Dialog Box

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.

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:

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 Legacy 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.

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.

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.

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 7.38: The Mass-Flow Inlet Dialog Box:

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.

The options available depend on which radiation model is active. For details, see Defining Boundary Conditions for Radiation.

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.

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.

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.

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.

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.

If the fluid is an ideal gas, the static temperature and static pressure are required to compute the density:

(7–99)

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

(7–100)

where the velocity magnitude is related to the mass flow rate given by Equation 7–98 and the known user-specified flow direction vector. Using Equation 7–99 to relate density to the (known) static pressure and (unknown) temperature, Equation 7–100 can be solved to obtain the static temperature.

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 7–98.

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.

You will enter the following information for a mass-flow outlet boundary:

All values are entered in the Mass-Flow Outlet Dialog Box (Figure 7.39: The Mass-Flow Outlet Dialog Box), which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and Boundary Conditions).

Figure 7.39: The Mass-Flow Outlet Dialog Box

Mass-flow outlets only support the Relative to Adjacent Cell Zone specification for the Reference Frame.

You can specify the mass flow rate through the outlet 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 specify an average mass flux. For compressible problems, you can specify that the mass flow rate is adjusted to total conditions at the outlet, thus maintaining a constant exit corrected mass flow rate.

You can define the mass flow or mass flux rate using a profile or a user-defined function (UDF). For an example of a mass-flow outlet UDF, see DEFINE_PROFILE in the Fluent Customization Manual.

The inputs for mass flow rate or flux are as follows:

The mass flow boundary will be pumping flow out of the domain normal to the boundary at the prescribed rate or flux. If the mass flow rate is specified, then by default, the fluxes on the boundary will be allowed to vary to preserve the flow profile out of the domain. At convergence, the total mass flow rate should match the specified value.

The options available depend on which radiation model is active. For details, see Defining Boundary Conditions for Radiation.

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the mass-flow outlet. See Setting Boundary Conditions for the Discrete Phase for details.

The Exit Corrected Mass Flow Rate specification method adjusts the mass flow rate to the total conditions at the outlet, maintaining a constant exit corrected mass flow rate. This boundary option is mainly intended for turbomachinery applications. This method allows you to sweep through the complete machine operational range, including machine operating points from choked flow to stall conditions. When using the Exit Corrected Mass Flow Rate specification method, the boundary operates like a mass-flow outlet on the left side of the speedline curve away from the best efficiency point, and more like a pressure outlet boundary to the right of the best efficiency point all the way beyond the choke point. This method allows you to specify the equivalent mass flow, based on similar criteria, corrected to a specified reference temperature and pressure.

For compressible flows, the exit corrected mass flow rate () is calculated as:

(7–102)

where and are mass-averaged values of total pressure and temperature in the absolute frame at the outlet. and are the reference conditions, which are constants in the equation. It should be noted that the numerical behavior of the boundary condition is not affected by the choice of reference conditions; rather, the reference conditions simply provide a dimensional meaning to the otherwise non-dimensional mass flow rate. It is typical to specify these reference conditions to be the same as the inflow total pressure and temperature.

In order to maintain a constant exit corrected mass flow, you can observe that the resulting mass flow rate must be proportional to the exit total pressure and inversely proportional to the square root of the exit total temperature (or equivalently, inversely proportional to the stagnation speed of sound). This allows the boundary condition to adapt dynamically to varying operating conditions, while remaining stable as the flow develops from the initial guess.

Note that the Exit Corrected Mass Flow Rate specification method is only available for ideal gas and real gas materials.

You can obtain an initial exit corrected mass flow rate value () from a previously converged case that uses standard inlet and outlet boundaries (for example, a pressure inlet and a pressure outlet). Use the converged solution to obtain the mass-flow-averaged value of and at the outlet boundary, as well as the mass flow rate (). These values can then be applied to Equation 7–102 along with and (which are usually taken as the inflow total temperature and pressure). After you have calculated the exit corrected mass flow rate, you can adjust this value up or down in order to traverse the speed line from choke to stall.

An inlet vent is considered to be infinitely thin, and the pressure drop through the vent is assumed to be proportional to the dynamic head of the fluid, with an empirically determined loss coefficient that you supply. That is, the pressure drop, , varies with the normal component of velocity through the vent, , as follows:

(7–103)

where is the fluid density, and is the non-dimensional loss coefficient.

You can define the Loss-Coefficient across the vent as a constant, polynomial, piecewise-linear, or piecewise-polynomial function of the normal velocity. The dialog boxes for defining these functions are the same as those used for defining temperature-dependent properties. See Defining Properties Using Temperature-Dependent Functions for details.

An intake fan is considered to be infinitely thin, and the discontinuous pressure rise across it is specified as a function of the velocity through the fan. In the case of reversed flow, the fan is treated like an outlet vent with a loss coefficient of unity.

You can define the Pressure-Jump across the fan as a constant, polynomial, piecewise-linear, or piecewise-polynomial function of the normal velocity. The dialog boxes for defining these functions are the same as those used for defining temperature-dependent properties. See Defining Properties Using Temperature-Dependent Functions for details.

You will enter or select the following information for a pressure outlet boundary:

All values are entered in the Pressure Outlet Dialog Box (Figure 7.42: The Pressure Outlet 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 7.42: The Pressure Outlet Dialog Box

To set the static pressure at the pressure outlet boundary, enter the appropriate value for Gauge Pressure in the Pressure Outlet dialog box. This value will be used when the flow is locally subsonic. Should the flow become locally supersonic, the pressure will be extrapolated from the upstream conditions. By default the subsonic and supersonic local flow condition at the boundary is determined based on the local normal velocity component.

Remember that the static pressure value you enter is relative to the operating pressure set in the Operating Conditions Dialog Box. Refer to Pressure Inputs and Hydrostatic Head regarding hydrostatic pressure.

Ansys Fluent also provides an option to use a radial equilibrium outlet boundary condition. This option is used to model the exit flow in turbomachinery flow problems. To turn on this option, enable Radial Equilibrium Pressure Distribution. When this feature is active, the specified gauge pressure applies only to the position of minimum radius (relative to the axis of rotation) at the boundary. The static pressure on the rest of the zone is calculated from the assumption that radial velocity is negligible, so that the pressure gradient is given by

(7–104)

where is the distance from the axis of rotation and is the tangential velocity. Note that this boundary condition can be used even if the rotational velocity is zero. For example, it could be applied to the calculation of the flow through an annulus containing guide vanes.

Ansys Fluent also provides an option to use an Average Pressure Specification method at the pressure outlet boundary. This option allows the pressure along the outlet boundary to vary, but maintain an average equivalent to the specified value in the Gauge Pressure input field. The pressure variation allowed in this boundary implementation slightly diminishes the reflectivity of the boundary as compared with the default uniform pressure specification. In the density-based solver two averaging methods are available, Strong Averaging and Weak Averaging. The average pressure specification in the pressure-based solver is the same as the strong pressure averaging in the density-based solver. For more details, see Calculation Procedure at Pressure Outlet Boundaries.

The Pressure Profile Multiplier allows you to specify a constant factor by which the Gauge Pressure is multiplied. This is provided mainly for cases where a non-uniform distribution of the static pressure at the pressure outlet boundary is specified by means of a profile file or a user-defined function. The scaling of an outlet profile with a multiplier can be convenient, for example, when computing a performance map for a turbomachine at different mass flow rates. The option will also work for a constant Gauge Pressure simply by scaling its value by a factor. This scaled pressure value will be used consistently when additional options are enabled in the Pressure Outlet dialog box; for example, when the Radial Equilibrium Pressure Distribution option is enabled, the scaled gauge pressure will be applied to the position of minimum radius (relative to the axis of rotation) at the boundary.

Backflow properties consistent with the models you are using will appear in the Pressure Outlet dialog box. The specified values will be used only if flow is pulled in through the outlet.

The options available depend on which radiation model is active. For details, see Defining Boundary Conditions for Radiation.

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the pressure outlet. See Setting Boundary Conditions for the Discrete Phase for details.

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.

When this option is selected, the exit pressure is not kept constant over the pressure outlet boundary, but instead is allowed to vary across the boundary while maintaining an average boundary pressure close to the specified static exit pressure. This option can be used for pressure specified as a constant or as a profile (for example, in turbomachinery cases with radial, axial, or radial equilibrium pressure distributions).

There are two implementations of the Average Pressure Specification. These are Strong Averaging and Weak Averaging. The strong averaging approach is available in both the density-based and the pressure-based solver. The weak averaging approach is available only in the density-based solver.

 

7.4.9.3.1.1. Strong Averaging

In the Strong Averaging approach, the face pressure value for subsonic exit flow is computed using the following expression:

(7–105)

where	= interior cell pressure at neighboring exit face, f
	= averaged interior cell pressure at a boundary
	= specified exit pressure
	= pressure blending factor; recovers the fully averaged pressure, recovers the specified pressure.

When the strong averaging option is used with a profile specification method (radial, axial, or radial equilibrium pressure distribution) then the outlet boundary will be subdivided into radial or axial containers called “bins”, and the above averaging procedure is applied to each bin.

You can use the following TUI command to change the blending factor and the number of bins:

/define/boundary-conditions/bc-settings/pressure-outlet

 

7.4.9.3.1.2. Weak Averaging

When the weak averaging method is used and the flow is subsonic, the pressure at the faces of the outlet boundary is computed using a weighted average of the left and right state of the face boundary. This weighting is a blend of fifth-order polynomials based on the exit face normal Mach number [91]. Therefore, the face pressure is a function of (, , ), where is the interior cell pressure neighboring the exit face f, is the specified exit pressure, and is the face normal Mach number.

Figure 7.43: Pressures at the Face of a Pressure Outlet Boundary

For incompressible flows, the face pressure is computed as an average between the specified pressure and the interior pressure.

(7–106)

In this boundary implementation, the exit pressure is not constant along the pressure outlet boundary. However, upon flow convergence, the average boundary pressure will be close to the specified static exit pressure.

One of the options that may be used at pressure outlets is non-reflecting boundary conditions (NRBC). This option is used when waves are made to pass through the boundaries while avoiding false reflections. Details of non-reflecting boundary conditions can be found in General Non-Reflecting Boundary Conditions.

The simple Bernoulli's equation is used to adjust the pressure at every iteration on a pressure outlet zone in order to meet the desired mass flow rate. The change in pressure, based on Bernoulli’s equation is given by the following equation:

(7–107)

where is the change in pressure, is the current computed mass flow rate at the pressure-outlet boundary, is the required mass flow rate, is the computed average density at the pressure-outlet boundary, and is the area of the pressure-outlet boundary.

Limitations

Target Mass Flow Rate Settings

To use the target mass flow rate option

Figure 7.44: The Pressure Outlet Dialog Box with the Target Mass Flow Rate Option Enabled

Solution Strategies When Using the Target Mass Flow Rate Option

If convergence difficulties are encountered or if the solution is not converging at the desired mass flow rate, then try to lower the under-relaxation factor from the default value. Otherwise, you can use the alternate method to converge at the required mass flow rate.

In some cases, you may want to switch off the target mass flow rate option initially, then guess an exit pressure that will bring the solution closer to the target mass flow rate. After the solution stabilizes, you can turn on the target mass flow rate option and iterate to convergence. For many complex flow problems, this strategy is usually very successful.

The use of Full Multigrid Initialization is also very helpful in obtaining a good starting solution and in general will reduce the time required to get a converged solution on a target mass flow rate. For further information on Full Multigrid Initialization, see Full Multigrid (FMG) Initialization.

Setting Target Mass Flow Rates Using UDFs

For some unsteady problems it is desirable that the target mass flow rate be a function of the physical flow time. This enforcement of boundary condition can be done by attaching a UDF with DEFINE_PROFILE functions to the target mass flow rate field.

An example of a simple UDF using a DEFINE_PROFILE that will adjust the mass flow rate can be found in DEFINE_PROFILE in the Fluent Customization Manual.

You will enter the following information for a pressure far-field boundary:

All values are entered in the Pressure Far-Field Dialog Box (Figure 7.45: The Pressure Far-Field Dialog Box), which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and Boundary Conditions).

Figure 7.45: The Pressure Far-Field Dialog Box

To set the static pressure and temperature at the far-field boundary in the Pressure Far-Field dialog box, enter the appropriate values for Gauge Pressure and Mach Number in the Momentum tab. The Mach number can be subsonic, sonic, or supersonic. Set the Temperature in the Thermal tab.

You can define the flow direction at a pressure far-field boundary by setting the components of the direction vector. If your geometry is 2D non-axisymmetric enter appropriate values for X and Y in the Pressure Far-Field dialog box (Figure 7.45: The Pressure Far-Field Dialog Box). If your geometry is 2D axisymmetric, enter the appropriate values for Axial, Radial, and (if you are modeling axisymmetric swirl) Tangential-Component of Flow Direction.

If your geometry is 3D, you can choose a Coordinate System that is Cartesian, Cylindrical, or Local Cylindrical. In the Cartesian coordinate system, enter the appropriate values for X, Y, and Z-Component of Flow Direction. If the direction cosine data on the boundary is available, then use the cylindrical or local cylindrical coordinate system and specify the Axial, Radial, Tangential-Component of Flow Direction. For Cylindrical, axis parameters need to be specified on the adjacent cell zone of the boundary face. For Local Cylindrical Swirl, specify the Axis Origin and Axis Direction.

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.

The options available depend on which radiation model is active. For details, see Defining Boundary Conditions for Radiation.

If you are modeling species transport, you will set the species mass or mole fractions under Species Mass Fractions or Species Mole Fractions. See Defining Cell Zone and Boundary Conditions for Species for details.

In general, there are no boundary conditions for you to set at an outflow boundary. If, however, 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 Method in the Outflow dialog box. These parameters are described in Defining Boundary Conditions for Radiation. The default value for Internal Emissivity is 1 and the default value for Black Body Temperature is 300.

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the outflow boundary. See Setting Boundary Conditions for the Discrete Phase for details.

An outlet vent is considered to be infinitely thin, and the pressure drop through the vent is assumed to be proportional to the dynamic head of the fluid, with an empirically determined loss coefficient that you supply. That is, the pressure drop, , varies with the normal component of velocity through the vent, , as follows:

(7–113)

where is the fluid density, and is the nondimensional loss coefficient.

You can define a constant, polynomial, piecewise-linear, or piecewise-polynomial function for the Loss Coefficient across the vent. The dialog boxes for defining these functions are the same as those used for defining temperature-dependent properties. See Defining Properties Using Temperature-Dependent Functions for details.

An exhaust fan is considered to be infinitely thin, and the discontinuous pressure rise across it is specified as a function of the local fluid velocity normal to the fan. You can define a constant, polynomial, piecewise-linear, or piecewise-polynomial function for the Pressure Jump across the fan. The dialog boxes for defining these functions are the same as those used for defining temperature-dependent properties. See Defining Properties Using Temperature-Dependent Functions for details.

Figure 7.49: The Exhaust Fan Dialog Box

You will enter the following information for a wall boundary:

The roughness parameters are in the Momentum tab of the Wall Dialog Box (see Figure 7.54: The Wall Dialog Box for Marangoni Stress), which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions).

To model the wall roughness effects, you must specify two roughness parameters: the Roughness Height, , and the Roughness Constant, . The default roughness height () is zero, which corresponds to smooth walls. For the roughness to take effect, you must specify a nonzero value for . For a uniform sand-grain roughness, the height of the sand-grain can simply be taken for . For a non-uniform sand-grain, however, the mean diameter () would be a more meaningful roughness height. For other types of roughness, an “equivalent” sand-grain roughness height could be used for . The above approaches are only relevant if the height is considered constant per surface. However, if the roughness constant or roughness height is not constant, then you can specify a profile (see Profiles). Similarly, user-defined functions may be used to define a wall roughness height that is not constant. For details on the format of user-defined functions, refer to the Fluent Customization Manual.

Choosing a proper roughness constant () is dictated mainly by the type of the given roughness. The default roughness constant () was determined so that, when used with - turbulence models, it reproduces Nikuradse’s resistance data for pipes roughened with tightly-packed, uniform sand-grain roughness. You may need to adjust the roughness constant when the roughness you want to model departs much from uniform sand-grain. For instance, there is some experimental evidence that, for non-uniform sand-grains, ribs, and wire-mesh roughness, a higher value () is more appropriate. Unfortunately, a clear guideline for choosing for arbitrary types of roughness is not available.

Additional roughness models are available if you have selected the Spalart-Allmaras or the SST k-ω model in the Viscous Model dialog box. See the Steps in Using a Turbulence Model for more information. With one of these viscous models active, the additional roughness models will be available on the Wall boundary condition panel on the Momentum tab under Wall Roughness → Roughness Models → High Roughness (Icing). A discussion of the treatment of the turbulence models with the High Roughness (Icing) enabled is given in Treatment of the Spalart-Allmaras Model for Icing Simulations and Treatment of the SST Model for Icing Simulations. These models are primarily designed and tested for simulations of icing applications, however they may also be useful for other applications in which the boundary layer is fully resolved and there is surface roughness that is large relative to the near-wall mesh.

Note that the High Roughness (Icing) models are only valid for low-Re number turbulence, or need fine near-wall meshes (mesh should fully resolve the boundary layer).

Figure 7.50: The Wall Dialog Box for High Roughness (Icing) Models

You have the following options:

 

7.4.15.3.2.2. NASA Correlation

If the NASA Correlation option is selected, the surface sand-grain roughness height is computed with an empirical NASA correlation for icing in air flows [141]. The sand-grain roughness height is computed from the product of the following coefficients:

(7–114)

(7–115)

(7–116)

Where is the Free Stream Velocity, is the Free Stream Temperature, LC is the Liquid Content (in most cases water for ice accretion), c is the Characteristic Length, and .

The sand-grain roughness height is then obtained from the formulation:

(7–117)

 

7.4.15.3.2.3. Shin-et-al

If the Shin-et-al option is selected the empirical correlation for the surface sand-grain roughness is computed with the Shin and Bond formulation [141], which modifies the NASA correlation (see the NASA Correlation for a description of variables) with the following factor:

(7–118)

where MVD is the droplet mean diameter (Droplet Diameter). The corresponding value of the sand-grain roughness height is obtained from:

(7–119)

If you want to include tangential motion of the wall in your calculation, you need to define the translational or rotational velocity, or the velocity components. Select the Moving Wall option under Wall Motion. The Wall dialog box will expand, as shown in Figure 7.51: The Wall Dialog Box for a Moving Wall, to show the wall velocity conditions.

Note that you cannot use the moving wall condition to model problems where the wall motion with respect to the adjacent cell zone has a component that is normal to the wall itself. For such problems, consider using a Sliding or Dynamic Mesh approach as discussed in Modeling Flows Using Sliding and Dynamic Meshes. Ansys Fluent will neglect any normal component of wall motion that you specify using the methods below.

Four types of shear conditions are available:

The no-slip condition is the default, and it indicates that the fluid sticks to the wall and moves with the same velocity as the wall, if it is moving. The specified shear and Marangoni stress boundary conditions are useful in modeling situations in which the shear stress (rather than the motion of the fluid) is known. Examples of such situations are applied shear stress, slip wall (zero shear stress), and free surface conditions (zero shear stress or shear stress dependent on surface tension gradient). The specified shear boundary condition allows you to specify the , , and components of the shear stress as constant values or profiles. The Marangoni stress boundary condition allows you to specify the gradient of the surface tension with respect to the temperature at this surface. The shear stress is calculated based on the surface gradient of the temperature and the specified surface tension gradient. The Marangoni stress option is available only for calculations in which the energy equation is being solved.

The specularity coefficient shear condition is specifically used in multiphase with granular flows. The specularity coefficient is a measure of the fraction of collisions that transfer momentum to the wall and its value ranges between zero and unity. This implementation is based on the Johnson and Jackson [74] boundary conditions for granular flows.

Shear conditions are entered in the Momentum tab of the Wall Dialog Box, which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions ).

You can model a no-slip wall by selecting the No Slip option under Shear Condition. This is the default for all walls in viscous flows.

In addition to the no-slip wall that is the default for viscous flows, you can model a slip wall by specifying zero or nonzero shear. For nonzero shear, the shear to be specified is the shear at the wall by the fluid. To specify the shear, select the Specified Shear option under Shear Condition (see Figure 7.52: The Wall Dialog Box for Specified Shear). You can then enter , , and components of shear under Shear Stress.

Figure 7.52: The Wall Dialog Box for Specified Shear

For multiphase granular flow, you can specify the specularity coefficient such that when the value is zero, this condition is equivalent to zero shear at the wall, but when the value is near unity, there is a significant amount of lateral momentum transfer. To specify the specularity coefficient, select the Specularity Coefficient option under Shear Condition (see Figure 7.53: The Wall Dialog Box for the Specularity Coefficient) and enter the desired value in the text-entry box under Specularity Coefficient.

Figure 7.53: The Wall Dialog Box for the Specularity Coefficient

Ansys Fluent can also model shear stresses caused by the variation of surface tension due to temperature. The shear stress applied at the wall is given by

(7–120)

where is the surface tension gradient with respect to temperature, and is the surface gradient. This shear stress is then applied to the momentum equation.

To model Marangoni stress for the wall, select the Marangoni Stress option under Shear Condition (see Figure 7.54: The Wall Dialog Box for Marangoni Stress). This option is available only for calculations in which the energy equation is being solved. You can then enter the surface tension gradient ( in Equation 7–120) in the Surface Tension Gradient field. Wall functions for turbulence are not used with the Marangoni Stress option.

Figure 7.54: The Wall Dialog Box for Marangoni Stress

Ansys Fluent offers a partial-slip boundary condition for rarefied gases. In the rarefied regime, the finite amount of friction is no longer sufficient to allow the full adhesion of gas particles onto solid walls, see Partial Slip for Rarefied Gases.

For a fixed heat flux condition, choose the Heat Flux option under Thermal Conditions. You will then need to set the appropriate value for the heat flux at the wall surface in the Heat Flux field. You can define an adiabatic wall by setting a zero heat flux condition. This is the default condition for all walls.

To select the fixed temperature condition, choose the Temperature option under Thermal Conditions in the Wall dialog box. You will need to specify the temperature at the wall surface (Temperature). The heat transfer to the wall is computed using Equation 7–123 or Equation 7–124.

For a convective heat transfer wall boundary, select Convection under Thermal Conditions. Your inputs of Heat Transfer Coefficient and Free Stream Temperature will allow Ansys Fluent to compute the heat transfer to the wall using Equation 7–127.

If radiation heat transfer from the exterior of your model is of interest, you can enable the Radiation option in the Wall dialog box and set the External Emissivity and External Radiation Temperature.

You can choose a thermal condition that combines the convection and radiation boundary conditions by selecting the Mixed option. With this thermal condition, you will need to set the Heat Transfer Coefficient, Free Stream Temperature, External Emissivity, and External Radiation Temperature.

When modeling the heat transfer of applications that have perturbed flow and/or disturbed boundary layers, it can be necessary to augment the calculation of the diffusive heat flux with a convective augmentation factor. Such applications include the modeling of underhood and underbody heat loads, as wells as transient heat transfer in fully warmed-up exhaust systems.

The convective augmentation factor represents the ratio of the measured Nusselt number to the Nusselt number of an ideal flow. You can define it by using the following text command:

define → boundary-conditions → wall

You will be prompted to define the Convective Augmentation Factor as either a profile or a single value. Note that a value of 1 (the default value) represents no augmentation of the diffusive heat flux, whereas values greater than 1 initiate augmentation. For further details, see the equation for qid in DEFINE_HEAT_FLUX of the Fluent Customization Manual.

By default, a wall will have a thickness of zero. You can, however, in conjunction with any of the thermal conditions, model a thin layer of material on the wall. For example, you can model the effect of a piece of sheet metal between two fluid zones, a coating on a solid zone, or contact resistance between two solid regions. Ansys Fluent will solve a 1D steady heat conduction equation to compute the thermal resistance offered by the wall and the heat generation in the wall.

To include these effects in the heat transfer calculation you will need to specify the type of material, the thickness of the wall, and the heat generation rate in the wall:

When postprocessing a wall that has a thickness but does not have shell conduction enabled, the Temperature... category provides three options: the temperature of the adjacent fluid / solid cells are stored as Static Temperature; the temperature of the wall surface itself is stored as Wall Temperature; and the temperature of the surface that is separated from the fluid / solid cells by the wall thickness is stored as Wall Temperature (Thin). If a more detailed analysis of the solid zone and surfaces is required, then you should consider creating layers of solid cells in your meshing application.

If the wall zone has a fluid or solid region on each side, it is called a “two-sided wall”. When you read a mesh with this type of wall zone into Ansys Fluent, a “shadow” zone will automatically be created so that each side of the wall is a distinct wall zone. In the Wall dialog box, the shadow zone’s name will be shown in the Shadow Face Zone field. You can choose to specify different thermal conditions on each zone, or to couple the two zones:

 

7.4.15.5.8.1. Orthogonality-Based Secondary Gradient Limiting at Coupled Two-Sided Walls

When cells near coupled two-sided walls have poor face orthogonality with respect to the wall, the tangential component (also known as the secondary gradient) of the discretized diffusive flux for the energy and user-defined scalar equations can become unbounded. This generates instabilities that can lead to solution divergence. When using the pressure-based solver, you have the option of limiting the secondary gradients in order to control the cross-diffusion source term. This control mechanism can improve the robustness of the discretization method while maintaining solution accuracy.

When this secondary gradient limiting is enabled, the diffusive flux approximation (described in Connectivity Macros in the Fluent Customization Manual) at the wall is modified so that a coefficient () controls the diffusion term:

(7–121)

where the diffusion coefficient is a function of face orthogonality—that is, the dot product between (the area vector for the face, normal to the wall) and (the unit vector along the line connecting the cell centroid (0) and face centroid (1)). Note that .

Note the following limitations:

• It is only available with the pressure-based solver.

• It can only be applied to the energy calculation and/or user-defined scalars (UDS) on coupled two-sided walls (that is, wall / wall-shadow pairs with Coupled selected from the Thermal Conditions list in the Thermal tab).

To enable orthogonality-based secondary gradient limiting, use the following text commands:

• For the energy equation:

  solve → set → advanced → secondary-gradient-limiting → energy?

• For user-defined scalars:

  solve → set → advanced → secondary-gradient-limiting → uds?

When you enable secondary gradient limiting, by default it is applied to faces on the coupled two-sided walls using mesh quality limits from 0.7–0.9. You can shift the range if necessary by using the following text command; note that shifting this range closer to 1 will decrease the risk of divergence, but at the cost of accuracy.

solve → set → advanced → secondary-gradient-limiting → mesh-quality-limits

If the wall is not between two cell zones but is adjacent only to a single solid cell zone that involves solid motion with a nonzero translational or rotational velocity, then the Boundary Advection option is available. If the velocity for the solid motion (specified in the Solid Motion tab in the Solid dialog box) is directed into or out of the domain to a significant degree on that wall, then you should consider enabling the Boundary Advection option. This option allows you to account for the advection of thermal energy into or out of the solid domain at a rate that is consistent with the velocity normal to the boundary, the temperature of the material, and the material properties.

As an alternative to setting this option for each individual wall, you can use the following text command to review all the walls and automatically enable the Boundary Advection option where needed. The option is enabled on every appropriate wall for which the average angle of the velocity of the solid is greater than 2 degrees.

define → boundary-conditions → detect-boundary-advection

For details on setting up the solid motion model for a domain, see Defining Zone Motion.

To enable shell conduction for a wall, enable the Shell Conduction option in the Wall boundary condition dialog box. You can then click the Edit... button to open the Shell Conduction Layers dialog box, where you can define the properties of the single or multiple layers of the shell. Note that you must specify a nonzero wall thickness for every layer of the shell. When shell conduction is enabled, Ansys Fluent will compute heat conduction for the wall not only in the normal direction (which is always computed when the energy equation is solved), but also in the planar directions. The Shell Conduction option will appear in the Wall dialog box for all walls when solution of the energy equation is active (except for mapped interfaces). For information about how the thermal conditions are applied on a wall with shell conduction enabled, managing multiple shells, and postprocessing shell conduction walls, see Shell Conduction.

Ansys Fluent cases with shell conduction can be read in serial or parallel. Either a partitioned or an unpartitioned case file can be read in parallel (see Mesh Partitioning and Load Balancing for more information on partitioning). After reading a case file in parallel, shell zones can be created on any wall.

To convert every wall with a finite thickness into a shell with a single action, the TUI command define/boundary-conditions/modify-zones/create-all-shell-threads can be used; each converted shell will have a single layer with the same thickness as the original thin wall (any pre-existing shells will not be modified). To disable shell conduction in every wall with a single action, the TUI command define/boundary-conditions/modify-zones/delete-all-shells can be used. These capabilities are available in both serial and parallel mode.

For more information on shell conduction, see Shell Conduction.

System Coupling allows the input and output of thermal data from Ansys Fluent. When Fluent is coupled with another system in Workbench using System Coupling, you can select the via System Coupling option on the desired wall boundaries to receive thermal data through System Coupling service. Note that this option does not need to be selected to provide thermal data from Fluent.

For more details about setting up a simulation with System Coupling, see the Performing System Coupling Simulations Using Fluent and the System Coupling User's Guide.

When thermal data is transferred into Fluent via System Coupling, the following variables are available:

When thermal data is transferred out of Fluent via System Coupling, the following variables are available:

For each data transfer, you specify the type of data transfer (the variables transferred) during the System Coupling setup.

As part of standard heat transfer boundary condition settings in Ansys Fluent, you can also specify the type of material, the thickness of the wall, and the heat generation rate in the wall. Select the material type in the Material Name drop-down list; if you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box (this dialog box contains just the properties of the selected material, and not the full contents of the standard Create/Edit Materials dialog box). You can specify the thickness in the Wall Thickness number-entry box and the heat generation rate in the Heat Generation Rate number-entry box.

Mapped interfaces provide a robust approach for modeling coupled walls between zones when the interface zones penetrate each other or have gaps between them (see Figure 7.58: 2D Interface with Penetration and Gaps). For the interface wall boundary zones created as part of such interfaces, via Mapped Interface is automatically selected from the Thermal Conditions list in the Thermal tab of the Wall dialog box, in order to interpolate the thermal data.

For more details about mapped interfaces, see The Mapped Option and Using a Non-Conformal Mesh in Ansys Fluent.

Figure 7.58: 2D Interface with Penetration and Gaps

Such boundaries also allow you to specify the standard heat transfer boundary condition settings, such as the type of material, the thickness of the wall, and the heat generation rate in the wall. Select the material type in the Material Name drop-down list; if you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box (this dialog box contains just the properties of the selected material, and not the full contents of the standard Create/Edit Materials dialog box). You can specify the thickness in the Wall Thickness number-entry box and the heat generation rate in the Heat Generation Rate number-entry box. Note that the Shell Conduction option is not available with the via Mapped Interface thermal condition.

In the rarefied regime, the parietal gas temperature may differ from the imposed wall temperature. For details, see Temperature Jump for Rarefied Gases.

In hypersonic flows, the recombination of atoms is usually dominant at the wall. The atoms that diffuse to the wall can either reflect from the wall or recombine into molecules, see Partial Catalytic Boundary Condition for Walls.

If you are using the VOF model and you are modeling wall adhesion, you can specify the contact angle for each pair of phases at the wall in the Momentum tab of the Wall dialog box. See Steps for Setting Boundary Conditions for details.

In a laminar flow, the wall shear stress is defined by the normal gradient of the tangential velocity at the wall:

(7–122)

When there is a steep velocity gradient at the wall, you must be sure that the mesh is sufficiently fine to accurately resolve the boundary layer. Guidelines for the appropriate placement of the near-wall node in laminar flows are provided in Mesh Element Distribution.

Wall treatments for turbulent flows are described in Near-Wall Treatments for Wall-Bounded Turbulent Flows in the Theory Guide.

When a fixed temperature condition is applied at the wall, the heat flux to the wall from a fluid cell is computed as

(7–123)

where
	= fluid-side local heat transfer coefficient
	= wall surface temperature
	= local fluid temperature
	= radiative heat flux

Note that the fluid-side heat transfer coefficient is computed based on the local flow-field conditions (for example, turbulence level, temperature, and velocity profiles), as described by Equation 7–130.

Heat transfer to the wall boundary from a solid cell is computed as

(7–124)

where
	= thermal conductivity of the solid
	= local solid temperature
	= distance between wall surface and the solid cell center

When you define a heat flux boundary condition at a wall, you specify the heat flux at the wall surface. Ansys Fluent uses Equation 7–123 and your input of heat flux to determine the wall surface temperature adjacent to a fluid cell as

(7–125)

where, as noted above, the fluid-side heat transfer coefficient is computed based on the local flow-field conditions. When the wall borders a solid region, the wall surface temperature is computed as

(7–126)

When you specify a convective heat transfer coefficient boundary condition at a wall, Ansys Fluent uses your inputs of the external heat transfer coefficient and external heat sink temperature to compute the heat flux to the wall as

(7–127)

where
	= external heat transfer coefficient defined by you
	= external heat-sink temperature defined by you
	= radiative heat flux

Equation 7–127 assumes a wall of zero-thickness.

When the external radiation boundary condition is used in Ansys Fluent, the heat flux to the wall is computed as

(7–128)

where
	= emissivity of the external wall surface defined by you
	= Stefan-Boltzmann constant
	= surface temperature of the wall
	= temperature of the radiation source or sink on the exterior of the domain, defined by you
	= radiative heat flux to the wall from within the domain

Equation 7–128 assumes a wall of zero-thickness.

When you choose the combined external heat transfer condition, the heat flux to the wall is computed as

(7–129)

where the variables are as defined above. Equation 7–129 assumes a wall of zero-thickness.

In laminar flows, the fluid side heat transfer at walls is computed using Fourier’s law applied at the walls. Ansys Fluent uses its discrete form:

(7–130)

where is the local coordinate normal to the wall.

For turbulent flows, Ansys Fluent uses the law-of-the-wall for temperature derived using the analogy between heat and momentum transfer  [84]. See Standard Wall Functions in the separate Theory Guide for details.