7.3.2 Using Flow Boundary Conditions

This section provides an overview of flow boundaries in ANSYS FLUENT and how to use them.

ANSYS FLUENT provides 10 types of boundary zone types for the specification of flow inlets and exits: velocity inlet, pressure inlet, mass flow inlet, pressure outlet, pressure far-field, outflow, inlet vent, intake fan, outlet vent, and exhaust fan.

The inlet and exit boundary condition options in ANSYS FLUENT are as follows:

• Velocity inlet boundary conditions are used to define the velocity and scalar properties of the flow at inlet boundaries.

• Pressure inlet boundary conditions are used to define the total pressure and other scalar quantities at flow inlets.

• Mass flow inlet boundary conditions are used in compressible flows to prescribe a mass flow rate at an inlet. It is not necessary to use mass flow inlets in incompressible flows because when density is constant, velocity inlet boundary conditions will fix the mass flow. Like pressure and velocity inlets, other inlet scalars are also prescribed.

• Pressure outlet boundary conditions are used to define the static pressure at flow outlets (and also other scalar variables, in case of backflow). The use of a pressure outlet boundary condition instead of an outflow condition often results in a better rate of convergence when backflow occurs during iteration.

• Pressure far-field boundary conditions are used to model a free-stream compressible flow at infinity, with free-stream Mach number and static conditions specified. This boundary type is available only for compressible flows.

• Outflow boundary conditions are used to model flow exits where the details of the flow velocity and pressure are not known prior to solution of the flow problem. They are appropriate where the exit flow is close to a fully developed condition, as the outflow boundary condition assumes a zero streamwise gradient for all flow variables except pressure. They are not appropriate for compressible flow calculations.

• Inlet vent boundary conditions are used to model an inlet vent with a specified loss coefficient, flow direction, and ambient (inlet) total pressure and temperature.

• Intake fan boundary conditions are used to model an external intake fan with a specified pressure jump, flow direction, and ambient (intake) total pressure and temperature.

• Outlet vent boundary conditions are used to model an outlet vent with a specified loss coefficient and ambient (discharge) static pressure and temperature.

• Exhaust fan boundary conditions are used to model an external exhaust fan with a specified pressure jump and ambient (discharge) static pressure.

Determining Turbulence Parameters

When the flow enters the domain at an inlet, outlet, or far-field boundary, ANSYS FLUENT requires specification of transported turbulence quantities. This section describes which quantities are needed for specific turbulence models and how they must be specified. It also provides guidelines for the most appropriate way of determining the inflow boundary values.

Specification of Turbulence Quantities Using Profiles

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 Section  7.6) 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 separate UDF Manual for information on user-defined functions.)

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

• Spalart-Allmaras model: Choose Turbulent Viscosity or Turbulent Viscosity Ratio in the Turbulence Specification Method drop-down list and select the appropriate profile name in the drop-down list next to Turbulent Viscosity or Turbulent Viscosity Ratio. ANSYS FLUENT computes the boundary value for the modified turbulent viscosity, $\tilde{\nu}$, by combining $\mu_t/\mu$ with the appropriate values of density and molecular viscosity.

• $k$- $\epsilon$ models: Choose K and Epsilon in the Turbulence Specification Method drop-down list and select the appropriate profile names in the drop-down lists next to Turbulent Kinetic Energy and Turbulent Dissipation Rate.

• $k$- $\omega$ models: Choose K and Omega in the Turbulence Specification Method drop-down list and select the appropriate profile names in the drop-down lists next to Turbulent Kinetic Energy and Specific Dissipation Rate.

• Reynolds stress model: Choose K and Epsilon in the Turbulence Specification Method drop-down list and select the appropriate profile names in the drop-down lists next to Turbulent Kinetic Energy and Turbulent Dissipation Rate. Choose Reynolds-Stress Components in the Reynolds-Stress Specification Method drop-down list and select the appropriate profile name in the drop-down list next to each of the individual Reynolds-stress components.

Uniform Specification of Turbulence Quantities

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. These quantities are discussed further in the following sections.

Turbulence Intensity

The turbulence intensity, $I$, is defined as the ratio of the root-mean-square of the velocity fluctuations, $u'$, to the mean flow velocity, $u_{\rm avg}$.

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 estimated from the following formula derived from an empirical correlation for pipe flows:

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

Turbulence Length Scale and Hydraulic Diameter

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

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

where $L$ is the relevant dimension of the duct. The factor of 0.07 is based on the maximum value of the mixing length in fully-developed turbulent pipe flow, where $L$ is the diameter of the pipe. In a channel of non-circular cross-section, you can base $L$ 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  7.3-2, which relates a physical dimension ( $L$) to the turbulence length scale ( $\ell$), is not necessarily applicable to all situations. For most cases, however, it is a suitable approximation.

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

• For fully-developed internal flows, choose the Intensity and Hydraulic Diameter specification method and specify the hydraulic diameter $L=D_H$ in the Hydraulic Diameter field.

• For flows downstream of turning vanes, perforated plates, etc., choose the Intensity and Length Scale method and specify the characteristic length of the flow opening for $L$ in the Turbulent Length Scale field.

• For wall-bounded flows in which the inlets involve a turbulent boundary layer, choose the Intensity and Length Scale method and use the boundary-layer thickness, $\delta_{99}$, to compute the turbulence length scale, $\ell$, from $\ell=0.4 \delta_{99}$. Enter this value for $\ell$ in the Turbulence Length Scale field.

Turbulent Viscosity Ratio

The turbulent viscosity ratio, $\mu_t/\mu$, is directly proportional to the turbulent Reynolds number ( ${\rm Re}_t \equiv k^2/(\epsilon \nu)$). ${\rm Re}_t$ 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, $\mu_t/\mu$ is fairly small. Typically, the turbulence parameters are set so that $1 < \mu_t/\mu <10$.

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 $k$- $\epsilon$ models, the $k$- $\omega$ models, or the RSM).

Relationships for Deriving Turbulence Quantities

To obtain the values of transported turbulence quantities from more convenient quantities such as $I$, $L$, or $\mu_t/\mu$, you must typically resort to an empirical relation. Several useful relations, most of which are used within ANSYS FLUENT, are presented below.

Estimating Modified Turbulent Viscosity from Turbulence Intensity and Length Scale

To obtain the modified turbulent viscosity, $\tilde{\nu}$, for the Spalart-Allmaras model from the turbulence intensity, $I$, and length scale, $\ell$, the following equation can be used:

This formula is used in ANSYS FLUENT if you select the Intensity and Hydraulic Diameter specification method with the Spalart-Allmaras model. $\ell$ is obtained from Equation  7.3-2.

Estimating Turbulent Kinetic Energy from Turbulence Intensity

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

where $u_{\rm avg}$ is 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 $k$ and $\epsilon$.

Estimating Turbulent Dissipation Rate from a Length Scale

If you know the turbulence length scale, $\ell$, you can determine $\epsilon$ from the relationship

where $C_{\mu}$ is an empirical constant specified in the turbulence model (approximately 0.09). The determination of $\ell$ 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 $k$ and $\epsilon$.

Estimating Turbulent Dissipation Rate from Turbulent Viscosity Ratio

The value of $\epsilon$ can be obtained from the turbulent viscosity ratio $\mu_t/\mu$ and $k$ using the following relationship:

where $C_{\mu}$ is an empirical constant specified in the turbulence model (approximately 0.09).

This relationship is used in ANSYS FLUENT whenever the Intensity and Viscosity Ratio method is used instead of specifying explicit values for $k$ and $\epsilon$.

Estimating Turbulent Dissipation Rate for Decaying Turbulence

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 $\epsilon$ such that

where $\Delta k$ is the approximate decay of $k$ you wish to have across the flow domain (say, 10% of the inlet value of $k$), $U_\infty$ is the free-stream velocity, and $L_\infty$ is the streamwise length of the flow domain. Equation  7.3-7 is a linear approximation to the power-law decay observed in high-Reynolds-number isotropic turbulence. Its basis is the exact equation for $k$ in decaying turbulence, $U \partial k/\partial x = - \epsilon$.

If you use this method to estimate $\epsilon$, you should also check the resulting turbulent viscosity ratio $\mu_t/\mu$ to make sure that it is not too large, using Equation  7.3-6.

Although this method is not used internally by ANSYS FLUENT, you can use it to derive a constant free-stream value of $\epsilon$ 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 $k$ from $I$ using Equation  7.3-4.

Estimating Specific Dissipation Rate from a Length Scale

If you know the turbulence length scale, $\ell$, you can determine $\omega$ from the relationship

where $C_{\mu}$ is an empirical constant specified in the turbulence model (approximately 0.09). The determination of $\ell$ 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 $k$ and $\omega$.

Estimating Specific Dissipation Rate from Turbulent Viscosity Ratio

The value of $\omega$ can be obtained from the turbulent viscosity ratio $\mu_t/\mu$ and $k$ using the following relationship:

This relationship is used in ANSYS FLUENT whenever the Intensity and Viscosity Ratio method is used instead of specifying explicit values for $k$ and $\omega$.

Estimating Reynolds Stress Components from Turbulent Kinetic Energy

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 $k$. The turbulence is assumed to be isotropic such that

and

(no summation over the index $\alpha$).

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

Specifying Inlet Turbulence for LES

The turbulence intensity value specified at a velocity inlet for LES, as described in Section  12.14.4, is used to randomly perturb the instantaneous velocity field at the inlet. It does not specify a modeled turbulence quantity. Instead, the stochastic components of the flow at the inlet boundary are accounted for by superposing random perturbations on individual velocity components as described in this section in the separate Theory Guide.