Content uploaded by Yaseen Aziz
Author content
All content in this area was uploaded by Yaseen Aziz on Mar 03, 2024
Content may be subject to copyright.
ZANCO Journal of Pure and Applied Sciences
The official scientific journal of Salahaddin University-Erbil
ZJPAS (2018) 30(s1)s83-s93
*Corresponding Author:
Email: yaseen90aziz@gmail.com
Numerical Modeling of Flow in Side Channel Spillway Using ANSYS-CFX
Shahin S. Ahmed1 and *Yaseen W. Aziz2
1 Asst. prof. Department of Dams and Water Resources, College of Engineering, University of
Salahaddin, Erbil, Kurdistan Region, Iraq.
2 M.Sc. Department of Dams and Water Resources, College of Engineering, University of Salahaddin,
Erbil, Kurdistan Region, Iraq.
INTRODUCTION
Side channel Spillway (SCS) is one of the
types of spillway that is usually provided at
earth dams in order to release flood discharge
from the reservoir to prevent overtopping and
damage of the dam. Therefore, spillway is an
important structure in the dam.
Thus, great attention should be paid to study
the hydraulic characteristics of the structure.
SCS consists of six parts namely; side weir,
trough channel, control section channel,
transition section channel, chute channel and
stilling basin. Flow in the side channel is very
complex called spatially varied flow (SVF),
resulting from added of water along the length
of the weir (Subramanya, 2009). Computation
fluid dynamics (CFD) is a branch of fluid
A R T I C L E I N F O
A B S T R A C T
Article History:
Received: 14/05/2017
Accepted: 12/04/2018
Published:01/06/2018
Side channel spillway is one of the most common types of
spillways provided at earth dams to release flood discharge
laterally. Flow in side channel is complex due to discharge
changing along its length. Due to rapid advent of computer
technology computational fluid dynamics (CFD) is extensively
used to model and analyze complex issues in engineering problems.
In the present study ANSYS-CFX code has been used to predict
flow characteristics in the side channel spillway. Grid dependence
study provided to select the optimum grid size that can predict free
surface profile accurately with minimum computational time. In
addition, various turbulence models such as k- ε and RNG k- ε
were used. The capability of each turbulence model to predict flow
characteristics in the spillway were tested. The k- ε and RNG k- ε
turbulence models gives good results at most parts of the spillway,
while RNG k- ε turbulence model needs higher computational time.
Furthermore, the ability of the code to predict free surface water
profile for various discharges was validated using results of the
physical model. The comparisons of water surface profile predicted
by ANSYS-CFX with the physical model show good agreement.
Unlikely, at the location of hydraulic jump in the stilling basin for
higher discharges which characterized by strong aeration ANSYS-
CFX with k- ε turbulence model failed to give accurate predicts of
the free surface water profile.
Keywords:
Side Channel Spillway
CFD
ANSYS-CFX
Turbulence models
84 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
mechanics that can simulate real fluid by using
numerical methods to solve the governing
equations. Nowadays CFD is extensively used
by the researchers to model and analyze
complex problems in engineering due to rapid
advent of high performance computers and
parallel computation methods. Investigation of
dynamic pressure fluctuation in stepped three
sided spillway (U shape) using FLOW 3D code
was performed by (Taghizadeh et al, 2012). A
good agreement was found when the results of
the numerical model compared with the
experimental results. Furthermore, (Gellibert et
al, 2016) conducted a study to investigate the
performance of side channel spillway of a
selected dam using ANSYS-CFX code. The
result of water surface profile in the spillway
compared with results of the original study, the
results showed good agreement between them.
Flow characteristics in the hydraulic jump
investigated using ANSYS-CFX code, Flow-
3D and openFOAM by (Castillo et al, 2014),
the k-ω turbulence model in the recirculation
zone displayed a better agreement and more
realistic than k- ε. The flow simulation in front
of rectangular broad crested weir was carried
out by (Zachoval and Rousar, 2015) and
compared their results with experimental
results. The most reliable result was obtained
by using RNG k- ε turbulence model but from
all two layers turbulence models (SST) provide
most reliable results. In the present study the
flow characteristics in SCS were investigated
using ANSYS-CFX 14. The results of the
numerical model were validated against the
physical model data of (Aziz, 2016).
MATERIALS AND METHODS
In the current study ANSYS-CFX code
has been used for flow simulation in the side
channel spillway. The code is based on finite
volume method, which discretizes Naiver
stokes equations at each computational cell. In
turbulent flow, velocity at each point consists
of two components, mean (
and fluctuating
velocities (). The mass and momentum
equations in the time average form for
incompressible flow can be written as:
The Naiver - Stokes equations with time
average velocity called Reynolds averaged
Naiver – Stokes (RANS) equations. This
method eliminates turbulent fluctuations by the
averaging process. The averaging of nonlinear
terms in the Naiver Stokes equations causes
additional unknowns called Reynolds stress.
Most of commercial CFD codes use time
average equations such as RANS equations for
modeling turbulent flow. The term ( is
referred to the Reynolds stresses, in three
dimensional (RANS) equations there are six
unknown terms, they behave like stresses.
The turbulence modeling is a
computational procedure that can close the
governing equations by modeling Reynolds
stresses (Piradeepan, 2002). Numerous
turbulence models are available based on
RANS equations. ANSYS-CFX contains
numerous turbulence models which can be
divided into two groups namely; eddy viscosity
and Reynolds stress models.
The k – ε Turbulence Model
This turbulence model is a semi empirical
model. It is probably the most common type
used than the other types. It gives a good result
in many industrial flows. This model has two
model equations one for k (turbulent kinetic
energy) and other for ε (dissipation rate). In
this model the eddy viscosity is linked to the
85 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
turbulent kinetic energy and dissipation
(ANSYS, 2011a) as:
Where: k is the turbulent kinetic energy, is
the rate of dissipation of turbulent kinetic
energy, is an empirical constant = 0.09.
The separate transport equations solve for
k and at a given time. The transport equations
for k and are as follow (Launder and
Spalding, 1974):
Where:
is Prandtl number connect the diffusivity of
k to the eddy viscosity, typically the value of
1.0 is used, is Prandtl number connect the
diffusivity of to the eddy viscosity, typically
the value of 1.3 is used. The value of and
are 1.44 and 1.92 respectively.
The standard (k -) model equations (4),
(5) have been developed for fully turbulent
flow which cannot be applied to the near wall
that characterized by viscous layer has low
Reynolds number, this leads to erroneous
results (Abo, 2013).
The Renormalized Group (RNG) k -
Turbulence Model
The RNG k - turbulence model is based
on the re-normalization group (RNG) analysis
of Naiver – Stokes equations (ANSYS 2011a).
The RNG method uses statistical mechanics to
extend the k- model. This model
systematically removes the small scales of
motion from the Naiver - Stokes equations by
expressing their effects in terms of large scale
motions and modified viscosity (Versteeg and
Malalasekera, 2007, p.87).
The RNG k-model was first derived by
(Yakhot et al., 1992), the equations are as
follows:
Where:
,
Where:, ,, , , , are
constants
= 0.0845, = =1.39, =
1.42,=1.68,
Geometry and Mesh Generation
For the present study, three dimensional
geometry of the model was created using
AutoCAD 2013. The geometry exported from
AutoCAD as a file (.sat) and then imported to
the ANSYS Design Modeler. To generate mesh
for the fluid domain, ANSYS ICEM CFD was
used that is a powerful tool for mesh generation
which contains numerous techniques. In this
tool different element shapes are available such
as tetrahedral, hexahedral, prism, and pyramid
with different formats such as multi-block,
structured, unstructured, and many others.
Because the geometry of the spillway is
complex, so it is divided into some parts in
order to facilitate controlling mesh type and the
size. Different mesh methods were used, for
sweepable parts such as chute transition and
control channel sweep method was used with
the manual controlling source and target face.
For other parts such as stilling basin where
sweep method cannot be applied multi-zone
86 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
and tetrahedron method was employed. A finer
grid size was selected for those parts were high
flow gradient were observed (Figure 1).
Figure 1 typical view of mesh generation for different
parts of side channel spillway.
Boundary Conditions
Boundary conditions have an important
role in the flow simulation; accurate result can
be obtained by specifying an appropriate initial
and boundary conditions. ANSYS-CFX code
contains several boundary conditions such as
inlet, outlet, opening, wall and symmetry
(Figure 2). Inlet boundary condition specified
at inlet section with the average velocity, water
and air volume fraction. Supercritical outlet
type was specified at the outlet since the flow
is supercritical, opening boundary condition
was specified for the top of the spillway. Sides
and bottom of the domain were specified as no
slip wall boundary condition, the fluid velocity
next to the wall immediately is equal to zero
(ANSYS, 2011b).
Figure 2 Boundary conditions for model of side
channel spillway.
RESULTS AND DISCUSSION
Verification of ANSYS-CFX Results
Because of the numerical models are based
on many assumptions which influence the
results, these models should be verified in
order to assure accuracy of the results. The
most important factors that considered in this
study are meshing size and turbulence models.
. For this purpose the results of water surface
profile obtained from ANSYS-CFX were
compared with the physical model results.
3.1.1. Mesh size
Three models were simulated with three
sets of mesh sizes, coarse, medium and fine
meshes, with a number of grids (1300000,
2500000, and 3750000) for the design
discharge (33.451 l/s). All models were
simulated with the steady state analysis type
with using k- ε turbulence model. Total
computational time for fine, medium and
coarse meshes were (52, 35 and 16) hours
respectively. The free surface profile along the
centerline and right side wall of the trough,
chute channel and stilling basin were taken for
comparing the results of numerical models with
results of physical model (Figure 3). The
percentage error between the physical model
87 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
0
0.02
0.04
0.06
0.08
0.1
0.12
0 0.5 1 1.5 2
Depth of Water (m)
Distance (m)
Centerline
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
0.065
0.07
0.075
0.08
0.085
0.09
0.095
0.1
0 0.5 1 1.5 2
Depth of water (m)
Distance (m)
Right side wall
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
0.02
0.03
0.04
0.05
0.06
0.07
0 0.5 1 1.5 2 2.5 3
Depth of water (m)
Distance (m)
Centerline
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
0.02
0.035
0.05
0.065
0.08
0.095
0 0.5 1 1.5 2 2.5 3
Depth of water (m)
Distance (m)
Right side wall
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
0
0.02
0.04
0.06
0.08
0.1
0.12
0 0.1 0.2 0.3 0.4 0.5 0.6 0.7
Depth of water (m)
Distance (m)
Centerline
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
0
0.02
0.04
0.06
0.08
0.1
0 0.2 0.4 0.6 0.8
Depth of water (m)
Distance (m)
Right side wall
Physical Model
CFX (Grid 3.75 M)
CFX (Grid 2.5 M)
CFX (Grid 1.3 M)
and the ANSYS-CFX was calculated at those
sections were flow depths from the physical
model are measured. Finally, average
percentage of error (APE) computed between
ANSYS-CFX and the physical model for each
part (Table 1).
a) Trough Channel
b) Chute Channel
C) Stilling Basin
Figure 3 Flow depth obtained from for physical
model and numerical models (Grid 3.75 M, Grid 2.5
M and Grid 1.3 M).
Table 1 The APE between physical model and
ANSYS-CFX with different grid number along the
centerline and right side wall at some parts of
spillway
According to the results of tables (1) the
following conclusions were made:
1- The accuracy of ANSYS-CFX using
2500000 grids is almost close to that using
3750000 grids, in spite its computational
time is less.
2- A noticeable deviation between the results
of CFX with the physical model are exist at
the end of stilling basin were strong jump
occurs. This deviation due to the
complexity of the phenomenon rather than
mesh density.
Parts
APE of Grid
3.75 M with
P.M.
APE of Grid
2.5 M with
P.M.
APE of Grid
1.3 M with
P.M.
Trough
Channel
C.L.
4.53
5.23
5.79
R.S.
3.7
3.82
4.3
Chute
Channel
C.L.
3.24
3.43
4.1
R.S.
8.92
9.17
9.59
Stilling
Basin
C.L.
14
15.66
16.9
R.S.
7.4
13.93
19.04
88 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
0
0.02
0.04
0.06
0.08
0.1
0.12
0 0.5 1 1.5 2
Depth of water (m)
Distance (m)
Centerline
Physical Model
RNG k-ε Model
k-ε Model
0.02
0.04
0.06
0.08
0.1
0.12
0 0.5 1 1.5 2
Depth of water (m)
Distance (m)
Right Side Wall
Physical Model
RNG k-ε Model
k-ε Model
0
0.01
0.02
0.03
0.04
0.05
0.06
0.07
0 1 2 3
Depth of water (m)
Distance (m)
Centerline
Physical Model
RNG k-ε Model
k-ε Model
0
0.02
0.04
0.06
0.08
0.1
0 1 2 3
Depth of water (m)
Distance (m)
Right Side Wall
Physical Model
RNG k-ε Model
k-ε Model
0
0.02
0.04
0.06
0.08
0.1
0.12
0 0.1 0.2 0.3 0.4 0.5 0.6 0.7
Depth of water (m)
Distance (m)
Centerline
Physical Model
RNG k-ε Model
k-ε Model
0
0.02
0.04
0.06
0.08
0.1
0 0.1 0.2 0.3 0.4 0.5 0.6 0.7
Depth of water (m)
Distance (m)
Right Side Wall
Physical Model
RNG k-ε Model
k-ε Model
3- For the above reasons the numerical model
with 2500000 grids can be used for flow
simulation in side channel spillway.
Turbulence models
To test the effect of turbulence models on the
numerical results of water surface profile, two
turbulence models were used for flow
simulation in the side channel spillway. The
first one is k- ε and the second is RNG k- ε
turbulence model. Both simulations were
performed for the design discharge (33.451 l/s).
The total time required to finish both
simulations with k- ε and RNG k- ε were 35,
42 hours respectively. The free surface water
profile predicted by ANSYS-CFX using these
two turbulence models compared with the
physical model results at trough channel, chute
channel and stilling basin of the spillway at the
centerline and the right side wall of them
(Figure 4). The APE between physical model
and ANSYS-CFX are shown in Table 2.
a) Trough Channel
b) Chute Channel
c) Stilling Basin
Figure 4 Flow depth obtained from physical model
and numerical model (using k- ε and RNG k- ε).
89 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
Table 2 The APE between physical model and
ANSYS-CFX using (k- ε and RNG k- ε model) at
some parts of spillway.
Parts
APE k- ε model
with physical
model
APE RNG k- ε
model with
physical model
Trough
Channel
C.L.
5.3
5.6
R.S.
3.8
3.6
Chute
Channel
C.L.
3.44
3.4
R.S.
9.2
9.7
Stilling
Basin
C.L.
15.7
16.75
R.S.
13.95
13.4
The overall percentage of error showed
that the k- ε turbulence model can be used for
modeling of turbulent flow in the side channel
spillway which needs less computational time
than RNG k- ε model. Both turbulence models
seem fail to predict water surface profile at the
location of hydraulic jump. Due to high error
percentages at the jump location, it needs an
extra study to test the capability of k- ε
turbulence model at those locations.
Water Surface Profile (WSP)
The results of WSP along the centerline of
the spillway for various discharges predicted
by ANSYS-CFX plotted with the
corresponding WSP of the physical model as
shown in figure 5. There is a good agreement
between predicted WSP by CFX with the
observed WSP from The physical model at
most parts of the spillway. At the chute channel
good agreement was found between CFX and
physical model results especially at the
centerline. While, there is differences between
them at the sides of the chute channel this is
mostly due to cross waves that created in the
chute channel due to sharp alignment of the
transition channel. The water level becomes
rising and falling near boundaries of the chute
channel till the flow reaches its downstream
height of waves reduced (Figure 6). At stilling
basin the results of ANSYS-CFX can be
outlined in the following points:
1- At the beginning of the stilling basin
(before jump occurs) the results of
ANSYS-CFX are well agreed with results
of the physical model.
2- At the jump location which characterized
by high streamline curvature and high air
concentration, especially for higher
discharges there are differences between
the flow depth obtained from CFX and that
obtained from the physical model. This
may be related to:
a) The complexity of the situation and
the turbulence model which cannot
well detect air entrainment
phenomenon. This well agree with
the results obtained by (Zhan et al,
2016) (Numerical investigation of
air-entrainment in skimming flow
over stepped spillway) showing that
RANS with k- ε is not suitable for
simulation of free surface aeration.
Likewise, (Castillo et al, 2014) have
doubts about the suitability of using
k- ε turbulence model to solve
hydraulic jumps.
b) In physical model point gauge is used
for measuring flow depth which is
not a good instrument for measuring
water depth at the location of the
hydraulic jump accurately.
3- Furthermore, as it can be observed from
figures 5b, c, d, for discharges lower than
the design discharge, location of the jump
moves to the upstream. Differences
between the physical model and ANSYS-
CFX results in the stilling basin occurred at
the jump location only. This deviation
diminishes at very low discharges in which
the hydraulic jump is unlikely form or the
weak jump may be formed.
90 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
0
0.1
0.2
0.3
0.4
0.5
0 2 4 6
WSE (m)
Distance (m)
a) 33.451 l/s
Physical Model
ANSYS CFX
0
0.1
0.2
0.3
0.4
0.5
0 2 4 6
WSE (m)
Distance (m)
b) 30.77 l/s
Physical
Model
0
0.1
0.2
0.3
0.4
0.5
0 2 4 6
WSE (m)
Distance (m)
c) 12 l/s
Physical Model
ANSYS CFX
0
0.1
0.2
0.3
0.4
0.5
0 2 4 6
WSE (m)
Distance (m)
d) 5.88 l/s
Physical Model
ANSYS CFX
Figure 5 Comparison of ANSYS CFX and physical
model water surface profile in side channel spillway
for different discharge.
Figure 6 Rising and falling free surface with color-
coded values at side wall of the chute channel
detected by ANSYS-CFX.
3.3. Velocity Profile
Figure 7 shows velocity distribution along
the spillway obtained from CFD code CFX.
The vertical velocity profile was taken at some
section in the trough channel, chute channel
and stilling basin as shown in figure 8, but
from the physical model velocity does not
measured in order to compare it with CFX.
From figure 8a it is clear that the flow is non-
uniform at the beginning of the trough channel.
This is due to the effect of the jet of water from
the crest. At the downstream sections of trough
channel the effect of jet reduced, the uniform
flow is nearly to achieve. In the chute channel
it is clear that the flow is almost uniform, and
velocity increases as flow goes downstream.
Furthermore, maximum vertical velocity can be
observed near the free surface flow (figure 8b).
The results of vertical velocity profile in the
stilling basin indicated that there is no the
recirculation zone at the centerline of the
stilling basin. For X* (X/L (length of the
channel)) = 0.077 the velocity is decreased to
its minimum value as depth of water increased,
then it increased till reached maximum value
when Y* (y/ymax) was equal to 0.75. This is due
to separation of incoming jet of water from
bottom of the basin when spread into the
stilling basin.
91 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
0
0.5
1
1.5
0 0.5 1 1.5
Y*
V*
X*=0.148
0
0.5
1
1.5
0.7 0.8 0.9 1 1.1
Y*
V*
X*=0.296
0
0.5
1
1.5
0.7 0.8 0.9 1 1.1
Y*
V*
X*=0.444
0
0.5
1
1.5
0.5 0.7 0.9 1.1
Y*
V*
X*=0.592
0
0.5
1
1.5
0.5 0.7 0.9 1.1
Y*
V*
X*=0.769
0
0.5
1
1.5
0.5 0.7 0.9 1.1
Y*
V*
X*=0.946
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X*=0.2
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X*=0.4
Figure 7 Velocity distribution with color-coded values
within the spillway predicted by ANSYS-CFX
a) Trough Channel
b) Chute Channel
92 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X*=0.6
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X*=0.8
0
0.5
1
1.5
0 0.5 1 1.5
Y*
V*
X*= 0.077
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X* = 0.38
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X* = 0.69
0
0.5
1
1.5
0.6 0.8 1 1.2
Y*
V*
X* = 1
c) Stilling Basin
Figure 8 Vertical velocity distributions within the
spillway
CONCLUSION
Flow in side channel spillway was simulated
using ANSYS-CFX code which is based on
finite volume method. The results of water
surface profile for different discharges were
compared with the physical model results.
Velocity distribution predicted by CFX and
vertical velocity profile was taken at various
sections within the spillway. The following
conclusion was established.
1. The results of k- ε and RNG k- ε turbulence
models relatively close to each other at
most parts of the spillway compared to the
physical model results.
2. 2. The predicted WSP by ANSYS-CFX at
the center of chute channel is better
agreeing with the physical model compared
at the boundaries due to cross waves.
3. The ANSYS-CFX code with k- ε
turbulence model could well predict the
free surface water profile in the SC
spillway components. Unlikely, it failed to
give accurate predicts of WSP at the
hydraulic jump when strong aeration
occurred.
4. For lower discharges ANSYS-CFX code
gave good predict of WSP in the stilling
basin because the hydraulic jump is
relatively weak.
5. Flow in the chute channel was almost close
to uniform compared with the flow in
trough channel and stilling basin.
93 Ahmad .S .and Aziz .Y / ZJPAS: 2018, 30(s1): s83-s93
REFERENCES
ABO, A. A. (2013) A three dimensional flow model
for different cross section high velocity channels.
PhD thesis, faculty of marine sciences and
engineering, Plymouth University.
ANSYS (2011a). ANSYS CFX Release 14.0 -
Theory Guide. Computer software manual.
ANSYS (2011b). ANSYS CFX Release 14.0 -
Modeling Guide. Computer software manual.
AZIZ, Y. W. (2016) Evaluation of Hydraulic
Performance of Nazanin Dam Side Channel
Spillway. M.Sc thesis, Dams and Water
Resources Department, College of Engineering,
University of Salahaddin.
CASTILLO, L. G., CARRILLO, J. M., GARCIA, J.
T. and VIGUERAS -RODRIGUEZ, A. (2014)
Numerical Simulations and Laboratory
Measurements in Hydraulic Jumps. 11th
International Conference on Hydroinformatics,
HIC 2014. New York City, USA, Paper 345.
http://academicworks.cuny.edu/cc_conf_hic/345
GELLIBERT, A., SAVATIER, J., PEPIN, N. and
FULLY, O. (2016) 3D Computational Modeling
of the Galaube Dam Spillway. In Advances in
Hydroinformatics (p. 361-376). Springer
Singapore.
GENERAL DIRECTORATE OF DAMS AND
RESERVOIRS (2013) Design Report of Nazanin
Dam.
HIRT, C. W. and NICHOLS, B. D. (1981) Volume
of Fluid (VOF) Method for the Dynamics of
Free Boundaries. Journal of Computational
Physics, 39 (1). P. 201-225.
LAUNDER, B. E. and SPALDING, D. B. (1974)
The Numerical Computation of Turbulent Flows.
Computer Methods in Applied Mechanics and
Engineering, 3(2). p. 269-289.
MACHAJSKI, J. and OLEARCZYK, D. (2011)
Model Investigations of Side Channel Spillway
of the Złotniki Storage Reservoir on the Kwisa
River. In Experimental Methods in Hydraulic
Research (p. 189-202). Springer Berlin
Heidelberg.
MILESI G. and CAUSSE, S. (2014) 3D Numerical
Modeling of a Side - Channel Spillway. In
Advances in Hydroinformatics (p. 487–498).
Springer Singapore.
PIRADEEPAN, N. (2002) An Experimental and
Numerical Investigation of a Turbulent Airfoil
Wake in a 90o Curved Duct. PhD thesis,
Department of Mechanical Engineering, Brunel
University.
SUBRAMANYA, K. (2009) Flow in Open
Channels. Third edition, New Delhi,Tata
McGraw-Hill Education.
TAGHIZADEH, H., NEYSHABOUR, S. A.A. S.
and GHASEMZADEH, F. (2012) Dynamic
Pressure Fluctuations in Stepped Three - Side
Spillway. Iranica Journal of Energy &
Environment, 3(1). p.95-104.
VERSTEEG, H. K. and MALALASEKERA, W.
(2007) An introduction to Computational Fluid
Dynamics. Second Edition, Edinburgh Gate,
Harlow, Addison Wesley Longman Ltd.
YAKHOT, V., ORSZAG, S. A., THANGAM, S.,
GATSKI, T. B., and SPEZIALE, C. G. (1992)
Development of Turbulence Models for Shear
Flows by a Double Expansion Technique.
Physics of Fluids A, 4(7). p.1510-1520.
ZACHOVAL, Z. and ROUSAR, L. (2015) Flow
Structure in front of the Broad – Crested Weir.
In EPJ Web of Conferences, 92. p. 02117. EDP
Sciences.
http://dx.doi.org/10.1051/epjconf/20159202117
ZHAN, J., ZHANG, J. and GONG, Y. (2016)
Numerical Investigation of Air-Entrainment in
Skimming Flow over Stepped Spillway.
Theoretical and Applied Mechanics Letters. 6
(3). p. 139-142.
