ANSYS FLUENT 12.0 Theory Guide - 4.11.4 Inlet Boundary Conditions for the LES Model

This section describes the three algorithms available in ANSYS FLUENT to model the fluctuating velocity at velocity inlet boundaries or pressure inlet boundaries.

The stochastic components of the flow at the velocity-specified inlet boundaries are neglected if the No Perturbations option is used. In such cases, individual instantaneous velocity components are simply set equal to their mean velocity counterparts. This option is suitable only when the level of turbulence at the inflow boundaries is negligible or does not play a major role in the accuracy of the overall solution.

To generate a time-dependent inlet condition, a random 2D vortex method is considered. With this approach, a perturbation is added on a specified mean velocity profile via a fluctuating vorticity field (i.e. two-dimensional in the plane normal to the streamwise direction). The vortex method is based on the Lagrangian form of the 2D evolution equation of the vorticity and the Biot-Savart law. A particle discretization is used to solve this equation. These particles, or "vortex points'' are convected randomly and carry information about the vorticity field. If

is the number of vortex points and

is the area of the inlet section, the amount of vorticity carried by a given particle

is represented by the circulation $\Gamma_i$ and an assumed spatial distribution $\eta$ :

$\displaystyle \Gamma_i(x,y)$	$\textstyle =$	$\displaystyle 4 \sqrt{\frac{\pi A k(x,y)}{3N [2 \ln(3) - 3\ln(2)]}}$	(4.11-31)

$\displaystyle \eta({\vec x})$	$\textstyle =$	$\displaystyle \frac{1}{2\pi \sigma^2} \left(2e^{-\vert x\vert^2/2\sigma^2} -1 \right) 2e^{-\vert x\vert^2/2\sigma^2}$	(4.11-32)

where

is the turbulence kinetic energy. The parameter $\sigma$ provides control over the size of a vortex particle. The resulting discretization for the velocity field is given by

${\vec u}({\vec x}) = \frac{1}{2\pi} \sum_{i=1}^N \Gamma_i \f... ... x}'\vert^2/2\sigma^2} ) }{\vert{\vec x} - {\vec x}'_i\vert^2}$

(4.11-33)

Where $\vec z$ is the unit vector in the streamwise direction. Originally [ 311], the size of the vortex was fixed by an ad hoc value of $\sigma$ . To make the vortex method generally applicable, a local vortex size is specified through a turbulent mixing length hypothesis. $\sigma$ is calculated from a known profile of mean turbulence kinetic energy and mean dissipation rate at the inlet according to the following:

where

. To ensure that the vortex will always belong to resolved scales, the minimum value of $\sigma$ in Equation 4.11-34 is bounded by the local grid size. The sign of the circulation of each vortex is changed randomly each characteristic time scale $\tau$ . In the general implementation of the vortex method, this time scale represents the time necessary for a 2D vortex convected by the bulk velocity in the boundary normal direction to travel along

times its mean characteristic 2D size ( $\sigma_m$ ), where

is fixed equal to 100 from numerical testing. The vortex method considers only velocity fluctuations in the plane normal to the streamwise direction.

In ANSYS FLUENT however, a simplified linear kinematic model (LKM) for the streamwise velocity fluctuations is used [ 219]. It is derived from a linear model that mimics the influence of the two-dimensional vortex in the streamwise mean velocity field. If the mean streamwise velocity

is considered as a passive scalar, the fluctuation

resulting from the transport of

by the planar fluctuating velocity field

is modeled by

where $\vec{g}$ is the unit vector aligned with the mean velocity gradient $\vec{\nabla U}$ . When this mean velocity gradient is equal to zero, a random perturbation can be considered instead.

Since the fluctuations are equally distributed among the velocity components, only the prescribed kinetic energy profile can be fulfilled at the inlet of the domain. Farther downstream, the correct fluctuation distribution is recovered [ 219]. However, if the distribution of the normal fluctuations is known or can be prescribed at the inlet, a rescaling technique can be applied to the synthetic flow field in order to fulfill the normal statistic fluctuations

, and

as given at the inlet.

With the rescaling procedure, the velocity fluctuations are expressed according to:

$u^{'*}_i=u'_i\frac {\sqrt{<u_iu_i>}}{\sqrt{2/3 k}}$

(4.11-36)

This also results in an improved representation of the turbulent flow field downstream of the inlet. This rescaling procedure is used only if the Reynolds-Stress Components is specified as the Reynolds-Stress Specification Method, instead of the default option K or Turbulence Intensity.

Since the vortex method theory is based on the modification of the velocity field normal to the streamwise direction, it is imperative that you create an inlet plane normal (or as close as possible) to the streamwise velocity direction.

The spectral synthesizer provides an alternative method of generating fluctuating velocity components. It is based on the random flow generation technique originally proposed by Kraichnan [ 171] and modified by Smirnov et al. [ 321]. In this method, fluctuating velocity components are computed by synthesizing a divergence-free velocity-vector field from the summation of Fourier harmonics. In ANSYS FLUENT, the number of Fourier harmonics is fixed to 100.

Both the vortex method and the spectral synthesizer are available for velocity inlet and pressure inlet boundary conditions. For the velocity inlet, the fluctuations are added on the mean specified velocity. For the pressure inlet, virtual body forces are employed in the momentum equations to add the reconstructed turbulent fluctuations to the velocity field. These virtual body forces are considered only in the first LES cells close to the inlet.

Both methods are also available for the DES models. However, note that such unsteady boundary conditions are appropriate and effective mainly for external aerodynamic flows. For internal flows, if the inlet is inside a full RANS zone, the fluctuations generated by both methods will be rapidly damped by the RANS turbulent eddy viscosity. Note also that whether the inlet will be fully or partly covered by a RANS zone will depend on the mesh and on the DES model.

Finally it should be noted that both methods require realistic inlet conditions (U,k, $\epsilon$ profiles) which can be obtained from separate RANS simulations. Unrealistic ("flat") turbulent profiles at inlets will generate unrealistic turbulent eddies at inlets.