This section describes the 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 (that is, 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
and an assumed spatial distribution
:
(4–308) |
(4–309) |
where is the turbulence kinetic energy. The parameter
provides control over the size of a vortex particle. The resulting
discretization for the velocity field is given by
(4–310) |
Where is the unit vector in the streamwise direction. Originally [431], the size of the vortex was fixed by an ad hoc value of
. To make the vortex method generally applicable, a local vortex size is
specified through a turbulent mixing length hypothesis.
is calculated from a known profile of mean turbulence kinetic energy and mean
dissipation rate at the inlet according to the following:
(4–311) |
where . To ensure that the vortex will always belong to resolved scales, the minimum
value of
in Equation 4–311 is bounded by the local grid size.
The sign of the circulation of each vortex is changed randomly each characteristic time scale
. 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 (
), 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 [306]. 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
(4–312) |
where is the unit vector aligned with the mean velocity gradient
. 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 [306].
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:
(4–313) |
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.
Important: 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. Problems can arise if the inlet
convective velocity is of the same order or lower than , as this can cause local outflow. For this reason it should be applied with
caution for Tu~1 or smaller).
The vortex method covers the entire boundary for which it is selected with vortices, even in regions, where the incoming turbulence level is low (freestream). For efficiency reasons, it is therefore recommended that you restrict the domain of the VM to the region where you which to generate unsteady turbulence. As an example, assume a thin mixing layer enters through a much larger inlet region. It is then advised to split the inlet boundary into three parts. One below the mixing layer with constant inlet velocity, one where the mixing layer enters the domain using the VM and a third above the mixing layer, again with a constant velocity. Thereby the vortices are concentrated at the domain of interest. Otherwise, a very large number of vortices would have to be generated to ensure a sufficient number of them in the thin mixing layer region.
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 [241] and modified by Smirnov et al. [446]. 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.
Important: 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 SAS, DES, SDES, and SBES models. If unsteadiness inside the domain can be sustained depends on the flow and the grid spacing, especially when using the SAS or the DDES models for wall bounded flows.
Finally it should be noted that both methods require realistic inlet conditions (U,k,
profiles) that can be obtained from separate RANS simulations. Unrealistic
(“flat”) turbulent profiles at inlets will generate unrealistic turbulent eddies at
inlets.