Numerical Simulation of Turbulent Flows using the SST-SAS Model
MAURO GRIONI1,2, SERGIO ELASKAR1,3,4, PASCAL BRUEL5, ANIBAL MIRASSO2
1National Scientific and Technical Research Council (CONICET),
ARGENTINA
2Institute of Structural Mechanics and Seismic Risk,
Research and teaching staff, Faculty of Engineering,
National University of Cuyo,
Mendoza 5500,
ARGENTINA
3Department of Aeronautical, Faculty of Exact, Physical and Natural Sciences,
National University of Córdoba,
Córdoba 5000,
ARGENTINA
4Institute of Advanced Studies in Engineering and Technology (IDIT),
National University of Córdoba,
Córdoba 5000,
ARGENTINA
5CNRS,
University Pau & Pays Adour, LMAP, Inria Cagire Team,
Avenue de l’Université, 64013 Pau,
FRANCE
Abstract: - Turbulent flows play a crucial role in various engineering and scientific applications, and the
accurate prediction of these flows remains a challenging task. This review explores the application of the Shear
Stress Transport Scale-Adaptive Simulation (SST-SAS) turbulence model for solving incompressible turbulent
flows, with a specific focus on unsteady wakes behind bluff bodies. Providing a concise overview of the
model’s formulation and its advantages, this article highlights the efficacy of the SST-SAS model in simulating
the intricate dynamics in different configurations of circular cylinders. The present study affirms that the SST-
SAS model can be considered a highly viable alternative for simulating unsteady flows around bluff bodies due
to the good predictive quality of the resulting simulations.
Key-Words: - SST-SAS turbulence model, unsteady flow, interference effects, wall proximity, tandem circular
cylinders, staggered tube bundle, wall-mounted cylinder.
Received: January 22, 2023. Revised: November 13, 2023. Accepted: December 12, 2023. Published: January 29, 2024.
1 Introduction
It is widely acknowledged that for quite a broad
range of flow configurations, the Reynolds-
Averaged Navier-Stokes (RANS) approach can
yield relatively satisfactory results for mean flow
quantities at a moderate computational cost.
However, in scenarios of flows largely dominated
by large-scale separation, the standard RANS
methodology finds rapidly its limits. Under such
conditions, the intricate nature of turbulent flows
calls for alternative modeling techniques to obtain
more accurate numerical predictions. In the last
decade, significant strides have been made in Large
Eddy Simulation (LES) models but their systematic
application to specific industrial flows at very high
Reynolds and Rayleigh numbers remains quite a
challenge, [1]. The hybridization of LES with
RANS is one possibility that permits to strike a
balance between the results’ accuracy and
computational efficiency, [2]. Revisiting the RANS
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
24
Volume 19, 2024
framework and reevaluating the derivation of its
governing equations was another option followed in
[3], to develop an unsteady RANS (URANS) model
called the scale-adaptive simulation (SAS)
approach. More specifically, the SAS version called
SST-SAS [4], and based on the k–ω SST RANS
model, [5], became quite a popular choice when it
comes to selecting a turbulence model. Indeed, a
search through the literature of the last ten-year
period with the keyword “SST-SAS” in the title or
the abstract returns more than one hundred
references. The diversity of flow configurations
dealt with is quite impressive, a glimpse of it is
given by the references listed below:
Canonical configurations: flows over a
backward-facing step [6]; the periodic hill
[7]; flows past a circular cylinder [8], [9],
[10], [11], [12]; flows past two circular
cylinders [13]; the flow past a prismatic
bluff body [14]; twin impinging jets [15].
Systems of practical interest: the flow
around a high-speed train [16], the flow past
an airfoil [17]; the flow over a wall mounted
array of cubes [11]; the flow in a tube
bundle [18], [19]; flows in centrifugal
pumps [7], [20]; the flow in a pressure wave
exchanger [21]; the filling of a tank [22]; a
ship air wake [23]; flows in Francis turbines
[24], [25], [26].
In the above-listed studies, the SST-SAS
method was employed either with commercial codes
(ANSYS-FLUENT, CFX, STAR-CCM+) or with
the open-source library OpenFOAM or in-house
codes. But, regardless of the kind of numerical set-
up used, the SST-SAS turbulence model is generally
praised for its capability of well-predicting on
relatively coarse meshes the mean flow properties
while being able to resolve a significant portion of
the flow temporal fluctuations. It should be noted
though that in most of these studies, the assessment
of the quality of the model is largely based on visual
comparisons with experimental data and not on the
recourse to objective criteria. Some studies are
performing such a comparison on integral flow
quantities but only two studies are using objective
criteria to compare experimental and numerical data
sets, [14], [18]. The context regarding the use of the
SAS approach being now recalled, the objective of
the present contribution is i) to review published
applications of the SST-SAS model to the
simulation of incompressible unsteady flow over
cylinder(s) and ii) to present new results obtained
for the configuration of the flow over a wall-
mounted cylinder. Such configurations hold
practical relevance in various engineering
applications, including heat exchangers, pipelines
used in fuel storage and distribution chains, and
offshore and ocean structures like subsea pipelines,
marine risers, and platform legs. The paper is
organized as follows: Section 2 describes the
governing equations and the SST-SAS turbulence
model. In Section 3, the reviewed cases are analyzed
and discussed. Section 4 presents recent
experimental and numerical results for the flow
around a wall-mounted cylinder. Finally, Section 5
presents the concluding remarks along with some
axes of future activity.
2 Background
2.1 Flow Model Formulation
The behavior of fluids in motion is comprehensively
described by the Navier-Stokes and continuity
equations. The ensemble averaging of these
equations, considering a constant density,
isothermal, and incompressible body force-free
flow, yields the Unsteady Reynolds-Averaged
Navier-Stokes (URANS) equations. In the Cartesian
coordinate system (O, x1, x2, x3), these equations can
be expressed as follows:
0
i
x
i
u
(1)
''
1
jiuu
i
x
j
u
j
x
i
u
j
x
j
x
p
j
x
j
u
i
u
t
i
u
(2)
where
i
u
is the ensemble average component of
the velocity in the direction
i
x
,
is the density of
the fluid,
p
is the ensemble average pressure,
is
the kinematic viscosity and
'' jiuu
is the Reynolds
stress tensor. To complete this URANS system, the
Reynold stress tensor, representing turbulence
effects through nonlinear terms, is modeled through
a Boussinesq-like relation, namely:
ij
k
ti
j
j
i
ji x
u
x
u
uu
3
2
''
(3)
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
25
Volume 19, 2024
where the turbulent eddy viscosity
t
and the
turbulence kinetic energy k are calculated thanks to
the recourse to the SST-SAS turbulence model.
2.2 SST-SAS Two-Equation Turbulence
Model
Menter and co-authors developed the Scale
Adaptive Simulation (SAS) method [3], [27], [28] to
simulate turbulent flows by using a two-equation
model. When the SAS approach is coupled with the
k-ω SST model [5], it yields the SST-SAS
turbulence model [3], [4], [29], [30]. The resulting
equations for k and ω are given by:
j
x
k
k
j
x
k
k
P
j
x
k
j
u
t
k
*
(4)
SAS
Q
j
x
j
x
k
F
j
x
j
x
k
P
t
j
x
j
u
t
1
2,
2
1
1
2
(5)
where
1
F
is a blending function and
k
P
is the
production term of turbulence kinetic energy given
by
2
S
t
k
P
with
ij
S
ij
SS 2
and
i
x
j
u
j
x
i
u
ij
S2
1
. The constant
*
is taken
equal to 0.09 and
2,
= 1.168 while the turbulent
diffusivities are expressed as
k
t
k
and
t
where the value of
k
and
, just
like
, result from a mix between the constants of
the k–ε and k–ω models. The SST-SAS model
differs from the original SST model by the addition
of the source term (QSAS) in the transport equation
for the turbulence eddy frequency ω. In contrast, the
equation for the turbulence kinetic energy k remains
unchanged. The additional source term (QSAS) is
given as:
]0,
1
,
1
max
2
2
2
2
max[
22
j
x
k
j
x
k
j
x
j
x
k
SAS
C
vK
L
L
SQ
k
SAS
(6)
where the model parameters are given by
51.3
2
3/2
,
2
SAS
C
,
is the von Karman constant.
The turbulence length scale (L) is calculated as:
25.0
c
k
L
(7)
(a)
(b)
Fig. 1: Airflow past two circular cylinders arranged
in tandem (Re = 1.66 x 105) - 2D contours snapshots
of (
/
t
): a) SST-SAS turbulence model and b) k-
ω SST turbulence model
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
26
Volume 19, 2024
(a)
(b)
Fig. 2: Airflow past two circular cylinders arranged
in tandem (Re = 1.66 x 105) - Snapshots of the Q-
criterion iso-surface (Q = 1s-2) applied to the
resolved velocity field: a) SST-SAS turbulence
model and b) k-ω SST turbulence model
The von Karman length-scale
vK
L
acts as a
sensor to detect the flow unsteadiness susceptibility
of the resolved velocity field, which is defined as:
2
2
2
2
i
x
j
x
vK
L
j
i
i
j
j
i
u
u
x
u
x
u
(8)
In flow regions where QSAS is sufficiently large
thanks to large values of
2
vK
L
L
, the turbulent
viscosity
/k
t
experiences a dramatic reduction
driven by the concomitant increase (resp. decrease)
of ω (resp. k). This behavior is illustrated in Figure
1 for the flow past two cylinders in tandem at
non-dimensional distance L/D = 3.7 (see section 3.2
for an in-depth analysis of such a flow
configuration). It can be seen that when compared to
the level obtained with a simulation based on the
use of the sole k-ω model (Figure 1-(b)), an almost
sixfold decrease in the maximum level of the
turbulent eddy viscosity is obtained when using the
SST-SAS model (Figure 1-(a)). The direct
consequence of this reduction is the presence of a
significantly broader range of structures in the
cylinder's wakes when using the SST-SAS model.
This phenomenon can be qualitatively illustrated by
displaying representative iso-surfaces of the Q-
criterion (Q = 1/2(Ω2-S2), where S is the strain rate
and Ω is the vorticity) obtained by processing two
individual snapshots of the resolved flow fields. As
depicted in Figure 2-(a), the presence of small-scale
structures in the flow field is clearly visible in the
snapshot of the resolved field obtained with the
SST-SAS model whereas these small-scale
structures are absent on the snapshot taken from the
simulations with the standard k-ω SST turbulence
model (Figure 2-(b)).
3 Case Analysis and Discussion
Despite the great simplicity of its geometry, the
configuration obtained by uniformly flowing at a
velocity U∞ a fluid of kinematic viscosity υ past a
circular cylinder of diameter D features quite a
fascinating diversity of flow patterns and related
dynamics as suggested by [31]. Since the beginning
of the twentieth century, a great deal of studies
focused on the characterization of the different flow
regimes whose onset proved to be driven by the
value of the Reynolds number defined as Re =
U∞D/υ. Still relevant today, the extensive review
published in 1991 by [32] provided quite a complete
panorama regarding the complexity of such a flow
configuration. As recalled by [33], there exists three
different flow regimes when progressively
increasing Re: the subcritical regime (Re ≤ 1.5-2 x
105), the supercritical regime (4-5 x 105 ≤ Re ≤ 4-5 x
106) and the transcritical regime (Re ≥ 4-5 x 106.
[32], split the subcritical regime into not less than
seven different sub-regimes and thanks to
visualizations they explained the different
underlying and differentiating mechanisms that led
to such a classification of the subcritical regime.
The interested reader is referred to the review by,
[32] and the references therein for further
explanations regarding the mechanisms at work in
this kind of flow configuration. If additional
complexity comes into play such as with the
presence of confinement, [34], or of additional
cylinders, then what was observed for the isolated 1-
cylinder flow configuration has to be revisited to
account for new mechanisms of interference. This is
precisely such kind of situations that call for
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
27
Volume 19, 2024
numerical simulations to help explain and predict
the outcome of such complex interference. Along
these lines, the objective of this section is to
highlight the capability of numerical simulations (in
particular with the SST-SAS turbulence model) to
help investigate three different flow past cylinder(s)
configurations characterized by the specific nature
of the interference to be dealt with, namely: a
circular cylinder in proximity to a plane wall,
circular cylinders in a free stream arranged in
tandem and the flow through a staggered tube
bundle.
3.1 The Flow over a Circular Cylinder in the
Vicinity of a Plane Wall
A notable feature of the flow past a circular cylinder
in the subcritical regime is the unsteadiness of the
cylinder wake. Taking the form of a periodic vortex
shedding, it leads to the continuous application of
fluctuating forces exerted on the cylinder. However,
when the cylinder is positioned close to a plane wall
at a distance of G, the flow dynamics become more
complex. In such a configuration, distinct changes
in aerodynamic drag and lift forces are observed.
There exists a critical gap ratio ((G/D)crit) for which
the suppression of vortices takes place. This
phenomenon is primarily controlled by three key
parameters: the Reynolds number (Re), the
boundary layer thickness (δ), and the gap ratio
(G/D). Various computational fluid dynamics
methods employed to investigate such a flow
configuration are now discussed. Let's start with
[35], who studied the conditions for observing the
suppression of the vortex shedding for a Reynolds
number Re ranging from 80 to 1000. They solved
the 2D Navier–Stokes equations by using a finite
difference method. Their results showed that the
critical gap ratio ((G/D)crit), at which the vortex
shedding was suppressed was a decreasing function
of the Reynolds number. [36], solved also the 2D
Navier–Stokes equations but using a stream-
function/vorticity formulation. For Re = 1200 and
G/D = 0.5 and 1.5, they found the calculated lift and
drag coefficients and the predicted vortex shedding
behavior match well with available experimental
results. [37], employed the 2D Unsteady Reynolds-
Averaged Navier Stokes (URANS) equations with
the standard high Reynolds number k–ε model at Re
ranging from 1 x 104 to 4.8 x 104 with δ/D = 0.14-2.
They reported an under-prediction of hydrodynamic
quantities (Cd, Cl, St, and Cp) and attributed this to
the intrinsic limitations of the k–ε model for such a
flow configuration. In a subsequent study, [38],
investigated near-bed flow mechanisms around a
marine pipeline close to a flat seabed at Re = 3.6 x
106. The predicted hydrodynamic quantities were in
satisfactory agreement with published experimental
data. In their simulations at Re = 2 x 104, [39],
selected the k-ω model. Their results exhibited good
qualitative agreement with published experimental
data. However, detailed comparisons with
experimental results and discussions for G/D < 0.4
were not provided. [40], used both URANS and the
Detached-Eddy Simulation (DES) to simulate the
flow around a circular cylinder positioned near a
moving plane wall at Re = 4 x 104. They found that
DES proved superior to URANS in predicting the
disappearance of vortex shedding as well as the
time-averaged drag coefficients, the separation
angles, and the velocity profiles in the near-wake
region. The SST-SAS turbulence model was
selected by [12], to conduct two-dimensional (2D)
simulations around a circular cylinder positioned
near a plane wall. The simulations considered
factors such as wall proximity, boundary layer
effects, and the variation of Reynolds number.
Furthermore, three-dimensional (3D) simulations
were also carried out to assess the importance of
three-dimensional effects, [10]. Comparative
analyses demonstrated a superior performance of the
3D simulations concerning the prediction of
aerodynamic characteristics, and vortex shedding as
well as the prediction of the critical values of
((G/D)crit) at which the suppression of vortex
shedding occurred. [41], shared a similar
perspective, suggesting that 3D Large Eddy
Simulation (LES) offers distinct advantages over the
widely used 2D Reynolds-Averaged Navier-Stokes
(RANS) k–ε model [42], as well as over 2D LES.
The 3D LES results offer more reliable integrated
forces and better capture flow details for different
values of G/D. Additionally, in [11], the results
obtained with the SST-SAS turbulence model
showed that (G/D)crit decreased as Re was increased
from 8.6 x 104 to 2.77 x 105, a trend similar to that
observed by [38]. However, in [10], the change in
(G/D)crit was associated more with the shift in flow
regimes (from subcritical to critical) than with a
change in the Reynolds number itself. On the other
hand, the critical gap was not overly sensitive to the
incident boundary layer thickness (δ) since for Re =
1.89 x 105, the results showed that (G/D)crit
decreased from 0.3 to 0.2 when δ/D was increased
from 0.1 to 1.1. This trend was echoing the findings
by [43] and [44].
3.2 Circular Cylinders Arranged in Tandem
in a Free Stream
Placing more than one cylinder within the fluid
stream leads to the so-called flow interference
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
28
Volume 19, 2024
regime. The tandem configuration corresponds to
the case of two cylinders arranged in line in a
crossflow. The wake of the upstream cylinder
modifies the incoming flow conditions for the
downstream cylinder, while this second cylinder
interferes with the wake dynamics and vortex
formation region of the upstream cylinder. [45],
described this reciprocal impact as 'wake
interference'. Depending on the distance between
the cylinders, different flow behaviors occur around
both cylinders that have significant effects on the
vortice detachment and the resulting loads on the
cylinders. The distance between the cylinders called
the spacing is expressed as the ratio of the center-to-
center distance L to the cylinder diameter, denoted
as L/D. Particularly crucial is the critical spacing
(L/D)crit associated with the onset of the vortex
shedding from the upstream cylinder.
Many computational studies of tandem cylinders
in steady cross-flow have been undertaken. [46],
used a fractional step method at Re varying from
100 to 200 to analyze the flow around multiple
cylinders. The numerical simulation approach has
been less effective compared to the experimental
data, due to the intricacy of the flow across
cylinders, [47]. [48], considered a laminar flow
regime at Re = 100 for a six-row inline tube bank. A
critical spacing range between 3.0 and 3.6 was
identified at which the mean drag as well as the
RMS (root mean square) lift and drag coefficients
for the last three cylinders reached their maximum
values. In [49], a standard LES with the
Smagorinsky subgrid-scale model was retained to
explore the characteristics of the vortices shed from
the circular tandem cylinders at Re = 2.2 x 104 and
L/D varying from 2 to 5. They found that the critical
spacing was about L/D = 3.25 and the mean drag
and fluctuating lift coefficients of each cylinder
jumped to higher values for this critical spacing.
[50], discussed the flow characteristics across
tandem circular cylinders in the range of subcritical
(Re = 2.4 x 104) and supercritical (Re = 3.0 x 106)
regimes by numerical simulation at L/D ranging
from 2 to 5 by means of improved delayed DES
(IDDES) method. They demonstrated that for both
Reynolds numbers, the vortex shedding occurred
from both upstream and downstream cylinders as
soon as L/D ≥ 3.5. Moreover, the fluctuating lift
coefficients of the upstream cylinder were almost
independent of Re, but those of the downstream
cylinder dropped as Re was increased. In [51],
Delayed Detached Eddy Simulations (DDES) were
used to simulate the flow around tandem circular
cylinders at L/D = 3.7 and Re = 1.66 x 105.
Simulations were performed on a (relatively) coarse
grid containing about 31 million grid points, and on
a fine grid containing about 133 million grid points.
The conclusion drawn was that some of the fine grid
DDES results were not significantly different from
those obtained with the coarse grid DDES. [52],
simulated the flow interference between tandem
cylinders based on the hybrid RANS/LES methods
with non-linear eddy viscosity formulations at Re =
1.66 x 105 for L/D = 1.4, 3, and 3.7. The presence of
a bistable wake between the cylinders and the
subsequent drag inversion on the downstream
cylinder was noted at L/D = 3. Additionally, it was
observed that the bistable wake resulted in an
elevation of the turbulent kinetic energy level within
the gap between the cylinders.
The evaluation of the SST-SAS model's
performance was conducted in the analysis of the
flow around two circular cylinders of identical
diameter arranged in tandem at a high subcritical
Reynolds number (Re = 1.2 x 105) by [13].
Additionally, [53], employed a numerical model that
combines Reynolds-Averaged Navier-Stokes
(RANS) and Large Eddy Simulation (LES) to
simulate the flow around two tandem cylinders at Re
= 1.66 x 105 for L/D = 3.7. In this study, the results
obtained with the SST-SAS model were utilized
only for comparative purposes. In [13], interference
effects for distances L/D varying from 1.1 to 7 were
explored by comparing them with those obtained for
the flow around a single isolated cylinder. The
results under-predicted the mean drag coefficient for
the upstream cylinder, while that for the
downstream cylinder provided they were in
satisfactory agreement with their experimentally
obtained counterparts. A critical spacing value of
(L/D)crit = 3 and the flow patterns associated with
the bistable flow, [54], were also observed.
3.3 Staggered Tube Bundle
The flow through bundles of cylinders has been
mostly investigated in the context of heat exchanger
design and analysis. This configuration exhibits a
vortex shedding behavior quite similar to that
observed for the flow past a single cylinder but with
the added complexity of strong interactions between
the wakes of the tubes. This configuration represents
quite a challenging test case for any existing model
or newly derived model. Indeed, many researchers
have simulated this configuration using a broad
range of approaches, from RANS models to Direct
Numerical Simulation (DNS). For validation
purposes, many of these studies used the
experimental data obtained in [55], [56], [57], for
the configuration of water flowing through a
staggered tube bundle array at Re = 18000.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
29
Volume 19, 2024
[58], examined the turbulent flow through a tube
bundle at a Reynolds number of 9300, both
experimentally and numerically. They closed the
steady RANS equations by using four different
turbulence models: k–ε, k–ω, SST, and the Reynold
Stress Model (RSM). The Reynolds normal stresses
approximated from the k–ω and SST models
demonstrated a closer agreement with experiments
than those obtained from the RSM model. However,
these RANS simulations failed to provide reliable
predictions for this flow due to the poor estimation
of the turbulence kinetic energy behavior. [59],
applied RANS and URANS simulations to predict
the experiments in [55], [56], [57]. URANS
simulations using a Reynolds stress model (RSM)
exhibited better agreement with experimental data
than the 2-equation model, although some
discrepancies persisted, particularly when it came to
reproducing the Reynolds normal stress behavior.
[60] and [61], investigated the same flow
configuration as [59], and reached similar
conclusions when comparing the results of RANS
and URANS simulations. [62], employed LES and a
k–ε model to simulate experiments configuration in
[55], [56], [57]. They reported well-predicted mean
velocity profiles in both cases. However, in the
wake region, the k–ε model provided a poorer
quality of prediction of the Reynolds stresses
compared to LES. [63], utilized LES, coarse LES,
and RSM-based URANS approaches to model the
flow in [55], [56], [57], at a Reynolds number of
9000. They reported that both the LES and RSM-
based URANS approach provided satisfactory
results compared to experiments, with the former
being slightly more consistent with DNS results. A
study by [64], employed Partially Filtered Navier–
Stokes (PANS) and LES, reporting that both
methods predicted the flow with relatively good
agreement with experimental data, although PANS
simulation was conducted on a much coarser grid
than LES. [65], used 3D DNS to predict
experiments in [55], [56], [57], at a lower Reynolds
number (Re = 6000) to limit the computational cost.
The results were in good agreement with the
experiments. Additionally, [66], performed DNS
simulations of the flow through a staggered tube
bundle over the range 1030 ≤ Re ≤ 5572. One of
their objectives was to determine the Reynolds
number value at which transition occurs at the
matrix transition point e.g. the point at which the
second frequency peak becomes prominent in the
spectral signature of the vortex shedding. They
observed that such a transition occurred at Re ≈
3000, a value similar to that observed for the
transition for the single-cylinder flow configuration.
The study by [18], delved into the predictive
capabilities of the SST-SAS turbulence model. They
simulated the flow configuration in [55], [56], [57].
Their results proved to be quite satisfactory when
compared with the experimental data in terms of
both mean velocity components and turbulence
quantities. The study introduced a quantitative
objective scoring criterion, utilizing relevant norms
to compare the SST-SAS results with those obtained
from other models in the literature. The comparison
revealed that the SST-SAS model presented a
remarkable consistency in its predictive capability,
ranking among the top-performing models in
agreement with experimental data. Moreover, in
[18], an in-depth analysis of the Reynolds stress
tensor's behavior was conducted for unsteady
URANS models. The analysis utilized the triple
decomposition of the instantaneous velocity field.
The findings indicated that, in the case of the SST-
SAS model, the contribution of time-resolved
motion to the total velocity correlations was
significantly higher when compared to other
URANS models, reaching levels exceeding 95 %.
4 Wall-mounted Cylinder
“The more available experimental data, the better
for simulation validation” is the motto behind the
choice of building up a new experiment on turbulent
flows over a wall-mounted cylinder to create a
database that will be subsequently made available in
open access. The configuration represents a
distinctive case where the cylinder encounters the
flow passage from only one side. The experimental
and numerical results reported here are restricted to
a low Reynolds subcritical flow at Re = 2300 based
on the diameter of the cylinder D = 0.04 m, the
kinematic viscosity of air υ = 1.53 x 10-5 m2/s, and
the bulk velocity Ubulk = 0.88 m/s.
4.1 Experimental Set-Up and Metrology
The MAVERIC test facility installed on the
premises of LMAP (CNRS/Pau University, France)
for studying effusion cooling flows, [67], [68], was
updated to accommodate a specifically designed test
section housing a removable cylinder of the circular
cross-section. A side view of the test section fitted
with the cylinder is displayed in Figure 3. The rig
consists basically of two 2.5 m-long superimposed
separate channels of identical rectangular cross-
section (width W = 400 mm x height H = 120 mm)
followed by the Plexiglas-made test section. Each
channel is fed in air by a dedicated centrifugal fan
powered by a 1-KW electrical motor regulated in
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
30
Volume 19, 2024
rotation by a Siemens Micro-Master MC420
controller. The test section which accommodates the
plate supporting the removable cylinder in the upper
channel is followed by the exhaust section which
evacuates outside the airflow through the lateral
wall of the laboratory. A two-component planar
particle image velocimetry (PIV) LaVision system
combined with computer-controlled translation
stages permitted to selection the desired image plane
by accurately displacing the Imager Pro X CCD
recording camera (1600 pixels x 1200 pixels,
intensity range over 14 bits, 50 mm lens, f-number =
4). The airflow was seeded with Di-Ethyl-Hexyl-
Sebacat (DEHS) particles of 1 μm of average
diameter. A double-pulse Nd-Yag laser combined
with divergent optics produced a divergent laser
sheet (wavelength = 532 nm, thickness of the sheet
≈ 1 mm) introduced normally in the flow through
the top wall of the test section (Figure 3).
All the measurements were made in the mid-
plane of the channel. Twelve hundred double-frame
recordings featuring a 10-pixel/mm resolution were
acquired for three different streamwise positions of
the camera to cover a flow region extending from 6
D upstream to 6 D downstream of the cylinder. The
number of recordings was chosen to ensure the
convergence of the estimator of the average of the
two velocity components. The recordings were first
pre-processed by i) subtracting the background
images obtained by firing the lasers without seeding
the flow and ii) normalizing the particle intensity.
Then, these pre-processed recordings were
successively processed by a multi-pass cross-
correlation algorithm (LaVision Davis Software
8.4.0) using interrogation windows of decreasing
size from 96 pixels x 96 pixels down to 32 pixels x
32 pixels.
Fig. 3: Wall-mounted cylinder - Side view of the
test section of the MAVERIC rig and some
components of the PIV system
4.2 Numerical Set-Up
The numerical solver used in this research was the
commercial CFD code Ansys Fluent 15, in line with
[69]. This code employs the finite volume cell-
centered method to solve the governing equations
describing fluid motion in a segregated manner.
Spatial discretization of these equations was
performed on three-dimensional structured grids
generated with ICEM CFD. Convection terms were
discretized using a bounded central differencing
scheme, while pressure and turbulent quantities (k
and ω) were evaluated with a second-order scheme.
Further, the equations were discretized in time using
a bounded second-order implicit scheme. The
pressure-velocity coupling was managed using the
SIMPLE (Semi-Implicit Method for Pressure-linked
Linked Equations) algorithm, [70]. Results from
[71], utilizing the SST-SAS turbulence model
demonstrated that SIMPLE exhibits acceptable
performances in resolving unsteady turbulent flow
around a circular cylinder, requiring less
computational time compared to the SIMPLEC [72]
and PISO [73] approaches.
4.2.1 Boundary Condition
Figure 4 depicts a schematic of the computational
domain and of the boundary conditions employed.
Inlet conditions for this investigation are established
using a velocity profile outlined in Eq. (9). The
resulting profile is incorporated as an input
condition through the User-Defined Function (UDF)
provided by the code. At the outlet, a reference zero
pressure condition is applied. For the upper and
lower limits of the domain, a no-slip wall condition
is specified. The same condition of zero velocity on
the wall is applied to the surface of the cylinder.
Lastly, at the lateral limits (normal to the x−y
plane), periodicity conditions are imposed,
considering that we are dealing with a reduced 2D
model corresponding to the length of the cylinder.
(9)
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
31
Volume 19, 2024
Fig. 4: Flow around a wall-mounted circular
cylinder at Re = 2300 - Schematic of the
computational domain and boundary conditions
used for the simulations. The diameter of the
cylinder is D = 40 mm
(a)
(b)
Fig. 5: Flow around a wall-mounted circular
cylinder at Re = 2300 - 2D cutting view of the 3D
structured mesh: a) Overview of the mesh and b)
Detail at the intersection between the supporting
wall and the cylinder surface
4.2.2 Mesh
The three-dimensional mesh is generated by
extending the two-dimensional mesh (Figure 5) in
the z direction, spanning it over a distance equal to
twice the cylinder diameter. Figure 5-(a) provides an
overall view of the mesh which featured refinement
near the cylinder surface and at the level of the
upper and lower limits of the domain. This
refinement was crucial for accurately capturing the
boundary layer on these surfaces, ensuring that the
normal distance to the wall of any wall-adjacent cell
satisfied y+ < 1. Figure 5-(b) illustrates how the
structured mesh was adapted to reproduce
accurately the acute angle formed between the
bottom of the cylinder and the supporting wall.
(a)
(b)
(c)
(d)
(e)
Fig. 6: Flow around a wall-mounted circular
cylinder at Re = 2300 - Contours of the velocity
field (m/s) and average Reynolds stress fields
(m2/s2); (a) streamwise component of the velocity;
(b) normal component of the velocity; (c)
longitudinal Reynolds stress Rxx; (d) normal
Reynolds stress Ryy; (e) shear Reynolds stress Rxy
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
32
Volume 19, 2024
4.3 Illustration of the Average Flow Field
The simulated flow field is initially illustrated by
presenting the time average of the fields of the two
velocity components, Vx (Figure 6-(a)) and Vy
(Figure 6-(b)), along with the fields of three
components of the Reynolds stress tensor (Figure 6-
(c) to 6-(d)).
In both time averages of the resolved fields of
Vx and Vy, a small recirculation zone can be
observed e.g. where the streamlines approaching the
cylinder appear to bifurcate. One part of the flow is
directed towards the upper surface of the cylinder,
while the other part is oriented towards the wall,
hence delimitating a recirculation zone. The flow
bifurcation point and the recirculation zone closely
resemble those obtained by PIV for a cylinder in
contact with a plane wall at Re = 3000 by [74] (refer
to Figure 2 in their study). It is worth stressing that
in [74], was visualized the flow only in the region in
front of and above the cylinder, making a direct
comparison challenging for the recirculation region
generated behind the cylinder. Nevertheless, a
comparison is feasible for the region behind the
cylinder with the PIV data obtained by [75], at Re =
Fig. 7: Flow around a wall-mounted circular cylinder at Re = 2300. Profiles of the time average of the
streamwise velocity component at four vertical cross-sections. Upper left: upstream position at x = -100 mm
(x/D = -2.5). Upper right: downstream position at x=60 mm (x/D = 1.5). Lower left: downstream position at x
= 100 mm (x/D = 2.5). Lower right: downstream position at x = 200 mm (x/D = 5)
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
33
Volume 19, 2024
5000. Although the Reynolds number is slightly
different, it's apparent that the main recirculation
and the recirculation generated just behind the
cylinder and the lower limit (Figure 6-(a) and (b))
are highly similar to those obtained for Re = 5000
(Figure 2 in [75]).
Fig. 8: Flow around a wall-mounted circular cylinder at Re = 2300. Profiles of the time average of the normal
velocity component at four vertical cross-sections. Upper left: upstream position at x = -100 mm (x/D = -2.5).
Upper right: downstream position at x=60 mm (x/D = 1.5). Lower left: downstream position at x = 100 mm
(x/D = 2.5). Lower right: downstream position at x = 200 mm (x/D = 5)
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
34
Volume 19, 2024
4.4 Preliminary Comparison of PIV vs CFD
Results
The normal profiles of the streamwise and the
normal components of the velocity and their
experimentally obtained counterparts are shown in
Figure 7 and Figure 8 at four different abscissas.
The corresponding vertical cross-sections are
materialized by vertical dashed cutting lines in
Figure 6-(a) and (b). The prediction of the velocity
component profiles with SST-SAS proved to be
quite satisfactory when compared to their
experimental counterpart. Indeed, the profiles of the
velocity streamwise component (Vx) are very well
predicted by the SST-SAS calculations for the three
positions at x = 60, 100, and 200 mm which
represent the recirculation zone downstream of the
cylinder. Regarding the normal velocity component
Vy, the comparison is qualitatively good but
features some significant discrepancies indicating
that the predicted and the measured recirculation
zones might have slightly different dimensions. The
use of the triple decomposition of the instantaneous
velocity field, [18], showed that the contribution of
the resolved part of the motion to the total Reynolds
stress was negligible. In simpler terms, the velocity
unsteadiness is dampened, resulting in a fully steady
state for the flow. Consequently, for this flow
configuration, the QSAS term does not play a
determinant role as observed in the preceding cases
indicating that the standard k-ω SST model is
recovered in this case.
5 Conclusion
This review strongly supports the notion that the
SST-SAS model is a highly relevant choice for
simulating unsteady flows around bluff bodies.
From both a qualitative and quantitative points of
view, the predictive capacity of SST-SAS based
simulations proved to be quite superior to those
provided by standard RANS models and to match at
quite an affordable cost those obtained by the most
advanced simulation tools such as the family of LES
based approaches. However the world of turbulence
modeling is far from being frozen as new
“competitors” are continuously emerging. This is
the case of the so-called hybrid temporal LES
(HTLES) advocated by Manceau and his group [76],
[77]. In its version based on the SST-SAS model on
a modification of the k-ω SST model, the HTLES
provides quite a sound alternative to the SST-SAS
approach. Comparing the performances of both
approaches will be one of the topics of our future
activity as well as the enrichment and publication of
the PIV database for the configuration of the flow
past wall-mounted cylinder(s).
Acknowledgement:
The authors express their gratitude to the National
University of Córdoba, the National University of
Cuyo, and the University Pau & Pays Adour for
their valuable support. Additionally, the first author
acknowledges the support of CONICET in
sustaining this research. This work is dedicated to
the memory of Ph.D. Jose Tamagno, is a
distinguished expert in fluid mechanics whose
legacy continues to influence our understanding of
this field.
References:
[1] Hanjalic, K., Launder, B., Eddy-Viscosity
transport modelling: A historical review, in:
50 Years of CFD in Engineering Sciences,
Springer, pp. 295-316, 2020.
[2] Al-Khalidy, N., Building Generated Wind
Shear and Turbulence Prediction Utilising
Computational Fluid Dynamics, WSEAS
Transactions on Fluid Mechanics, Vol.13, pp.
126-135, 2018.
[3] Menter, F.R., Egorov, Y., A Scale Adaptive
Simulation model using two-equation models.
AIAA Paper 2005, Vol. 1905, pp. 1-13, 2005.
[4] Egorov, Y., Menter, F., Development and
application of SST-SAS turbulence model in
the DESIDER project. Notes on Numerical
Fluid Mechanics and Multidisciplinary
Design, Vol.97, pp. 261–270, 2008.
[5] Menter, F.R., Two-equation eddy-viscosity
turbulence models for engineering
applications. AIAA Journal, Vol.32, pp. 1598–
1605, 1994.
[6] Shahi, M., Kok, J.B.W., Pozarlik, A., On
characteristics of a non-reacting and a reacting
turbulent flow over a backwards facing step
(BFS). International Communications in Heat
and Mass Transfer, Vol.61, pp. 16-25, 2015.
[7] Hundshagen, M., Casimir, N., Pesch, A.,
Falsafi, S., Skoda, R., Assessment of scale-
adaptive turbulence models for volume-type
centrifugal pumps at part load operation.
International Journal of Heat and Fluid Flow,
Vol. 85, 108621, 2020.
[8] Menter, F., Elements, and applications of
Scale-Resolving Simulation methods in
industrial CFD. Fröhlich, J., Kuerten, H.,
Geurts, B., Armenio, V. (Eds.), Direct and
Large-Eddy Simulation IX, ERCOFTAC
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
35
Volume 19, 2024
Series, Vol. 20, Springer, Cham, pp. 179-195,
2015.
[9] Zheng, W., Yan, C., Liu, H., Luo, D.,
Comparative assessment of SAS and DES
turbulence modeling for massively separated
flows. Acta Mechanica Sinica, Vol.32, pp. 12
21, 2016.
[10] Grioni, M., Elaskar, S., Mirasso, A., Scale-
Adaptive Simulation of flow around a circular
cylinder near a plane boundary. Journal of
Applied Fluid Mechanics, Vol.11, No.6, pp.
1477-1488, 2018.
[11] ElCheikh, A., ElKhoury, M., Effect of local
grid refinement on performance of scale-
resolving models for simulation of complex
external flows. Aerospace, Vol.6, No.8, 2019.
[12] Grioni, M., Elaskar, S., Mirasso, A.,
Numerical simulation of flow around circular
cylinder near a plane wall: effects of wall
proximity, boundary layer and Reynolds
number. South Florida Journal of
Development, Vol.4, No.5, pp. 2099-2113,
2023.
[13] Grioni, M., Elaskar, S., Mirasso, A., A
numerical study of the flow interference
between two circular cylinders in tandem by
Scale-Adaptive Simulation model. Journal of
Applied Fluid Mechanics, Vol.13, No.1, pp.
169-183, 2020.
[14] Duan, Y., Cooling, C., Ahn, J.S., Jackson, C.,
Flint, A., Eaton, M.D., Bluck, M.J., Using a
Gaussian process regression inspired method
to measure agreement between experiment
and CFD simulations. International Journal of
Heat and Fluid Flow, Vol.80, 108497, 2019.
[15] Taghinia, J., Rahman Mizanur, M., Siikonen,
T., Numerical investigation of twin-jet
impingement with hybrid-type turbulence
modeling. Applied Thermal Engineering,
Vol.73, pp. 650-659, 2014.
[16] Munoz Paniagua, J., García, J., Lehugueur,
B., Evaluation of RANS, SAS and IDDES
models for the simulation of the flow around a
high-speed train subjected to crosswind.
Journal of Wind Engineering and Industrial
Aerodynamics, Vol. 171, pp. 50-66, 2017.
[17] Niu, X.-F., Li, Y., Wang, X.-N, Numerical
study of aerodynamic noise behaviors for a
vertically installed flat strut behind an
asymmetrical airfoil. European Journal of
Mechanics / B Fluids, Vol.88, pp. 17-33,
2021.
[18] Grioni, M., Bruel, P., Elaskar, S., Mirasso, A.,
An application of the scale adapted simulation
to the unsteady flow across a tube bundle.
International Journal of Heat and Fluid Flow,
Vol.96, pp. 109007, 2022.
[19] Zhao, H., gao, P., Tian, R., Li, X., A three-
dimensional refined numerical simulation of
cross-flow induced vibration mechanism in
the tube bundle. Nuclear Engineering and
Design, Vol.405, 112223, 2023.
[20] Si, Q., Yuan, J., Yuan, S., Wang, W., Zhu, L.,
Bois, G., Numerical investigation of pressure
fluctuation in centrifugal pump volute based
on SAS model and experimental validation.
Advances in Mechanical Engineering, Vol.
2014, P72081, 2014.
[21] Kurec, K., Piechna, J., Gumowski, K.,
Investigations on unsteady flow within a
stationary passage of a pressure wave
exchanger, by means of PIV and CFD
calculations. Applied Thermal Engineering,
Vol. 112, pp. 610-620, 2017.
[22] Gonin, R., Horgue, P., Guibert, R., Fabre, D.,
Bourguet, R., Ammouri, F., Vyazmina, E.,
Advanced modeling improves thermal thermal
gradient prediction during compressed
hydrogen tank filling. International Journal of
Hydrogen Energy, Vol. 48, pp. 30057-30068,
2023.
[23] Shukla, S., Singh, S.N., Sinha, S.S.,
Vijayakumar, R., Comparative assessment of
URANS, SAS and DES turbulence modeling
in the predictions of massively separated ship
air wake characteristics. Ocean Engineering,
Vol. 229, 108954, 2021.
[24] Sotoudeh, N., Maddahian, R., Cervantes M.J.,
Investigation of a rotating vortex rope
formation during load variation in a Francis
turbine draft tube. Renewable Energy,
Vol.151, pp. 238-254, 2020.
[25] Salehi, S., Nilsson, H., Lillberg, E., Edh, N.,
An in-depth numerical analysis of transient
flow field in a Francis turbine during
shutdown. Renewable Energy, Vol. 179, pp.
2322-2347, 2021.
[26] Arabnejad, M.H., Nilsson, H., Bensow, R.E.,
Investigation of flow-induced instabilities in a
Francis turbine operating in con-cavitating
and cavitating part-load conditions. Fluids,
Vol.8, No.2, 61, 2023.
[27] Menter, F., Kuntz, M., Bender, R., A Scale-
Adaptive Simulation model for turbulent flow
predictions. AIAA Paper 2003, Vol.0767, pp.
1-11, 2003.
[28] Menter, F., Egorov, Y., Revisiting the
turbulent scale equation, in IUTAM
Symposium on One Hundred Years of
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
36
Volume 19, 2024
Boundary Layer Research, Springer, Vol.129,
2006.
[29] Menter, F., Egorov, Y., The Scale-Adaptive
Simulation method for unsteady turbulent
flow predictions. part 1: theory and model
description. Flow, Turbulence and
Combustion, Vol.85, No.1, pp. 113-138, 2010.
[30] Davidson, L., Evaluation of the SST-SAS
model: channel flow, asymmetric diffuser,
and axi-symmetric hill. in: Proc. of
ECCOMAS 2006, Egmond aan Zee,
Netherlands, pp. 1-20, 2006.
[31] Morkovin, M.V., Flow around circular
cylinder—a kaleidoscope of challenging fluid
phenomena. In Proceedings of the ASME
Symposium on Fully Separated Flows, ASME,
New York, pp. 102-118. 1964.
[32] Coutanceau, M., Defaye, Circular cylinder
wake configurations: a flow visualization
survey. Applied Mechanics Reviews, Vol.44,
No.6, pp. 255-305, 1991.
[33] Farell, C., Blessmann, J., On critical flow
around smooth circular cylinders. Journal of
Fluid Mechanics. Vol.36, pp.375-391, 1983.
[34] Nguyen, Q.D., Lu, W., Chan, L., Ooi, A., Lei,
C., A state-of-the-art review of flows past
confined circular cylinders. Physics of Fluids,
Vol.35, 071301, 2023.
[35] Lei, C., Cheng, L., Armfield, S.W.,
Kavanagh, K., Vortex shedding suppression
for flow over a circular cylinder near a plane
boundary. Ocean Engineering. Vol.27, pp.
1109-1127, 2000.
[36] Dipankar, A. and Sengupta, T. K, Flow past a
circular cylinder in the vicinity of a plane
wall. Journal of Fluids and Structures.
Vol.20, pp. 403- 423, 2005.
[37] Ong, M.C., Utnes, T., Holmedal, L.E.,
Myrhaug, D., Pettersen, B., Numerical
simulation of flow around a marine pipeline
close to the seabed. Coastal Engineering.
Vol.3, pp. 2730-2742, 2008.
[38] Ong, M.C., Utnes, T., Holmedal, L.E.,
Myrhaug, D., Pettersen, B., Numerical
simulation of flow around a circular cylinder
close to a flat seabed at high Reynolds
numbers using a k − ϵ model. Coastal
Engineering. Vol.57, pp. 931-947, 2010.
[39] Zhao, M., Cheng, L., and Teng, B., Numerical
Modeling of Flow and Hydrodynamic Forces
Around a Piggyback Pipeline Near the
Seabed. Journal of Waterway, Port, Coastal,
Ocean Engineering. Vol.133, No.4, pp. 286-
295, 2007.
[40] Nishino, T., Roberts, G.T. and Zhang, X.,
Unsteady RANS and detached-eddy
simulations of flow around a circular cylinder
in ground effect. Journal of Fluids and
Structures. Vol.24, pp. 18-33, 2008.
[41] Abrahamsen Prsic, M., Chen Ong, M.,
Pettersen, B., Myrhaug, D., Large Eddy
Simulations of flow around a circular cylinder
close to a flat seabed. Marine Structures.
Vol.46, pp. 127-148, 2016.
[42] Ong, M.C., Utnes, T., Holmedal, L.E.,
Myrhaug, D., Pettersen, B., Near-bed flow
mechanisms around a circular marine pipeline
close to a flat seabed in the subcritical flow
regime using a k − ϵ model. Offshore Mech
Arct Eng. Vol.134, No.2, pp. 021803, 2012.
[43] Buresti, G. and Lanciotti, A., Mean and
fluctuating forces on a circular cylinder in
cross-flow near a plane surface. Journal of
Wind Engineering and Industrial
Aerodynamics. Vol.41, pp. 639-650, 1992.
[44] Lei, C., Cheng, L., Kavanagh, K,
Reexamination of the effect of a plane
boundary on force and vortex shedding of a
circular cylinder. Journal of Wind
Engineering and Industrial Aerodynamics.
Vol.81, pp. 263-286, 1999.
[45] Zdravkovich, M., The effects of interference
between circular cylinders in cross flow.
Journal of fluids and structures. Vol.1, No.2,
pp. 239-261, 1987.
[46] Meneghini, J.R., Saltara, F., Siqueira, C.,
Ferrari, J.Jr., Numerical simulation of flow
interference between two circular cylinders in
tandem and side-by-side arrangements.
Journal of fluids and structures. Vol.15, No.2,
pp. 327-350, 2001.
[47] Sumner D., Two circular cylinders in cross
flow: a review. Journal of fluids and
structures. Vol.26, pp. 849-899, 2010.
[48] Liang, C., Papadakis, G., Luo, X., Effect of
tube spacing on the vortex shedding
characteristics of laminar flow past an inline
tube array: a numerical study. Computers &
Fluids. Vol.38, No.4, pp. 950-964, 2009.
[49] Kitagawa, T. Ohta, H., Numerical
investigation on flow around circular
cylinders in tandem arrangement at a
subcritical Reynolds number. Journal of
Fluids and Structures. Vol.24, No.5, pp. 680-
699, 2017.
[50] Hu X, Zhang X, You Y., On the flow around
two circular cylinders in tandem arrangement
at high Reynolds numbers. Ocean
Engineering. Vol.189, pp. 106301, 2019.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
37
Volume 19, 2024
[51] Uzun, A., Yousuff Hussaini, M., An
application of delayed detached eddy
simulation to tandem cylinder flow field
prediction. Computers & Fluids. Vol.60, pp.
71-85, 2012.
[52] Gopalan, H., Jaiman, R., Numerical study of
the flow interference between tandem
cylinders employing non-linear hybrid
URANS–LES methods. Journal of Wind
Engineering and Industrial Aerodynamics.
Vol.142, pp. 111-129, 2015.
[53] Weinmann, M., Sandberg, R., Doolan, C.,
Tandem cylinder flow and noise predictions
using a hybrid RANS/LES approach.
International Journal of Heat and Fluid Flow.
Vol.50, pp. 263-278, 2014.
[54] Igarashi, T., Characteristics of the flow
around two circular cylinders arranged in
tandem: 1st report. Bulletin of JSME. Vol.24,
No.188, pp. 232-331, 1981.
[55] Simonin, O., Barcouda, M., Measurements of
fully developed turbulent flow across tube
bundle. in: Proceedings of the Third
International Symposium on Applications of
Laser Anemometry to Fluid Mechanics,
Lisbon, Portugal, 1986.
[56] Simonin, O., Barcouda, M., Measurements
and prediction of turbulent flow entering a
staggered tube bundle. in: Proceedings of the
Fourth International Symposium on
Applications of Laser Anemometry to Fluid
Mechanics, Lisbon, Portugal, 1988.
[57] Simonin, O., Barcouda, M., Flow through
staggered tube bundle – ERCOFTAC Classic
Collection Database, 1986, [Online].
http://cfd.mace.manchester.ac.uk/ercoftac/dok
u.php?id=cases:case078 (Accessed Date:
January 24, 2024).
[58] Paul, S., Ormiston, S., Tachie, M.,
Experimental and numerical investigation of
turbulent crossflow in a staggered tube
bundle. International Journal of Heat and
Fluid Flow. Vol.29, No.2, pp. 387-414, 2008.
[59] Johnson, R.W., Modeling strategies for
unsteady turbulent flows in the lower plenum
of the VHTR. Nuclear Engineering and
Design. Vol.238, No.3, pp. 482-491, 2008.
[60] Ridluan, A., Tokuhiro, A., Benchmark
simulation of turbulent flow through a
staggered tube bundle to support CFD as a
reactor design tool. part I: SRANS CFD
simulation. Journal of Nuclear Science and
Technology. Vol.45, No.12, pp. 1293-1304,
2008.
[61] Ridluan, A., Tokuhiro, A., Benchmark
simulation of turbulent flow through a
staggered tube bundle to support CFD as a
reactor design tool. part II: URANS CFD
simulation. Journal of Nuclear Science and
Technology. Vol.45, No.12, pp. 1305-1315,
2008.
[62] Rollet-Miet, P., Laurence, D., Ferziger, J.,
LES, and RANS of turbulent flow in tube
bundles. International Journal of Heat and
Fluid Flow. Vol.47, No.14-16, pp. 3057-3071,
1999.
[63] Benhamadouche, S., Laurence, D., LES,
coarse LES, and transient RANS comparisons
on the flow across a tube bundle.
International Journal of Heat and Fluid Flow.
Vol.24, pp. 470-479, 2003.
[64] Minelli, G., Krajnovi´c, S., Basara, B., LES,
and PANS of turbulent flow through a
staggered tube bundle. in: Fluids Engineering
Division Summer Meeting, Vol. 58059,
American Society of Mechanical Engineers, p.
V01BT12A009, 2017.
[65] Moulinec, C., Pourquie, M., Boersma, B.,
Buchal, T., Nieuwstadt, F., Direct numerical
simulation on a cartesian mesh of the flow
through a tube bundle. International Journal
of Computational Fluid Dynamics. Vol.18,
No.1, pp. 1-14, 2004.
[66] Linton, D., and Thornber, B., Direct
numerical simulation of transitional flow in a
staggered tube bundle. Physics of Fluids.
Vol.28, No.2, pp. 024111, 2016.
[67] Bruel, P., Florenciano, J.-L., Kousksou, T.,
Lederlin, T., A test facility for assessing
simulations of jets in cross flow
configurations, in Proceedings of the Ninth
International ERCOFTAC Symposium on
Engineering Turbulence Modelling and
Measurements, Thessaloniki, Greece, hal-
00768340, 2012.
[68] Florenciano, J.-L., Study of the response of a
flow with wall mass transfer to acoustic
forcing (Étude de la réponse d’un écoulement
avec transfert pariétal de masse à un forçage
acoustique). Phd thesis (in French), University
of Pau and Pays Adour, 2013, [Online].
https://www.theses.fr/2013PAUU3013
(Accessed Date: January 24, 2024).
[69] Teixeira, G.S., De Campos, M.D., Best
Practice Guidelines on the Ansys in Building
Wind Action Applications. WSEAS
Transactions on Fluid Mechanics, Vol.18, pp.
114-122, 2023,
https://doi.org/10.37394/232013.2023.18.12.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
38
Volume 19, 2024
[70] Patankar, S.V., Spalding, D.B., A calculation
procedure for heat, mass and momentum
transfer in three-dimensional parabolic flows.
International Journal of Heat and Mass
Transfer, Vol.15, pp. 1787-1806, 1972.
[71] Grioni, M., Elaskar, S., Bruel, P., Mirasso, A.,
Comparison of velocity-pressure coupling
algorithms for unsteady flow problems around
a circular cylinder (Comparación de
algoritmos de acoplamiento velocidad-presión
para problemas no estacionarios del flujo
alrededor de un cilindro circular). 2022 IEEE
Biennial Congress of Argentina
(ARGENCON), Published in IEEE Xplore, pp.
1-8, 2022.
[72] Van Doormaal, J., Raithby, G., Enhancements
of the simple method for predicting
incompressible fluid flows. Numerical Heat
Transfer, Vol.7, No.2, pp. 147-163, 1984.
[73] Issa, R. I., Solution of the implicitly
discretized fluid flow equations by operator
splitting. Journal of Computational Physics,
Vol.62, No.1, pp. 40-65, 1986.
[74] Akoz, M. S., Sahin, B., Akilli, H., Flow
characteristic of the horizontal cylinder placed
on the plane boundary. Flow Measurement
and Instrumentation. Vol.21, No.4, pp. 476-
487, 2010.
[75] Ozdil, N. F. T. y Akilli, H., Flow comparison
around horizontal single and tandem cylinders
at different immersion elevations. Ocean
Engineering, Vol.189, pp. 106352, 2019.
[76] Duffal, V., de Laage de Meux, B., Manceau,
R., Development and validation of a new
formulation of hybrid temporal large-eddy
simulation. Flow, Turbulence and
Combustion, Vol.108, pp. 1-42, 2022.
[77] Mehta, M., Manceau, R., Duffal, V, de Laage
de Meux, B., An active hybrid Reynolds-
Averaged Navier-Stokes/Large Eddy
Simulation approach for grey area mitigation.
Physics of Fluids, Vol. 35, No.12, 125116,
2023.
Contribution of Individual Authors to the
Creation of a Scientific Article (Ghostwriting
Policy)
The authors equally contributed to the present
research, at all stages from the formulation of the
problem to the final findings and solution.
Sources of Funding for Research Presented in a
Scientific Article or Scientific Article Itself
This work has been supported for the Projects
ECOS Sud-MinCyT cofinanced by Ministère de
l’Europe et des Affaires Étrangères (MEAE) and the
Ministère de l’Enseignement Supérieur et de la
Recherche et de l’Innovation (MESRI) on the
French side and by Ministry of Science, Technology
and Innovation on the Argentine side, CONICET-
PUE-IDIT, “Vulnerability of infrastructure and
physical environment associated with fuel
transportation and storage”, FONCyT-PICT-2017
“Study of the structural vulnerability of fuel storage
tanks and pipes due to loads generated by wind and
explosions”, CONICET-PIP-GI “Effects of wind,
explosions, and fire in fuel storage tanks”, the
National University of Córdoba “Development and
application of theoretical, numerical, experimental
and computational codes in fluid mechanics and
chaotic intermittency” and the National University
of Cuyo Project 06/B050-T1, “Numerical models
for the wind action on the layout of circular
cylindrical structures with different diameters”.
Conflict of Interest
The authors have no conflicts of interest to declare.
Creative Commons Attribution License 4.0
(Attribution 4.0 International, CC BY 4.0)
This article is published under the terms of the
Creative Commons Attribution License 4.0
https://creativecommons.org/licenses/by/4.0/deed.en
_US
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2024.19.3
Mauro Grioni, Sergio Elaskar, Pascal Bruel, Anibal Mirasso
E-ISSN: 2224-347X
39
Volume 19, 2024
