ArticlePDF Available

CFD Modeling of Simultaneous Flow Over Broad Crested Weir and Through Pipe Culvert using Different Turbulence Models

Authors:
ZANCO Journal of Pure and Applied Sciences
The official scientific journal of Salahaddin University-Erbil
ZJPAS (2018),30 (5); 131-139
http://dx.doi.org/10.21271/ZJPAS.30.5.11
CFD Modeling of Simultaneous Flow Over Broad Crested Weir and Through Pipe
Culvert using Different Turbulence Models
Othman K. Mohammed1, Yaseen W. Aziz2
1- Department of Civil Engineering, College of Engineering, Salahaddin University-Erbil
2- Department of Dams and Water Resources Engineering, College of Engineering, Salahaddin University-Erbil
1. INTRODUCTION
In the case of culvert overtopping with water,
where the culvert cross sectional area is
insufficient to drain the incoming flood, the
ordinary solution is either to replace the old
culvert with a bigger capacity one or to add new
vents to the original one. An alternative solution is
to use a hydraulic structure (broad crested weir with
circular opening). In this case a part of the flow
will go through the culvert vents (circular
openings) and the rest will overtop it. (Mahmoud
S. M. 2002) and (Negm A. M. 2002) conducted
an experimental investigation on simultaneous
flow through box culvert and over contracted
broad crested weir. The flow at the culvert
outlet is considered as submerged flow, a
discharge prediction models have been
developed by means of multiple linear
regression techniques. (Othman K. Mohammed
2010) simulated experimentally the combined
flow through pipe culvert and over broad
crested weirs of different side slopes, he
developed empirical relations between the
discharge coefficient and geometrical
parameters of the combined weir culvert
model. Due to high cost in construction of the
physical models (Kositgittiwong, 2012). . In
addition, because of the difficulties in solving
the high order partial differential equations of
many fluid flow (Aziz, 2016). Nowadays, most
researchers turn to the use of numerical
methods. (Sarker and Rhodes 2004) compared
the free surface profile over a laboratory
rectangular broad crested weir with numerical
CFD model using commercial software
FLUENT applying both slandered k ε model
and (RNG) k ε model, they reported that the
A R T I C L E I N F O
A B S T R A C T
Article History:
Received: 05/04/2018
Accepted: 10/09/2018
Published:28/10/2018
Culverts and broad crested weirs are hydraulic structures that could be used
for measuring the flow rate in open channels. In this research, a simultaneous
flow over broad crested weir and through pipe culvert was simulated using
the numerical software ANSYS CFX. Three turbulence models were used for
the modeling of flow turbulent to determine the best turbulence model for
combined flow simulation. To achieve this purposes, results of simulations
have been compared with data gathered from lab experiments from literature.
The computational results showed a close agreement with obtained
experimental data, but that of the (RNG) k ε model provides more accurate
results compared with other two turbulence models used in this study.
Therefore, it can be concluded that this turbulence model (RNG) k ε model
can be used for simulation of simultaneous flow over broad crested weir and
below through culverts.
Keywords:
Broad Crested Weir
CFD Modeling
Simultaneous Flow
Turbulence Models
ANSYS CFX
Corresponding Author:
Othman K. Mohammed
othman.mohammed@su.edu.krd
132 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
uncertainties in predicting the water levels
above and D/S the crest were higher compared
to the wave-like profile observed in the
laboratory experiments. (Hargreaves D. M.
2007) conducted a serious of CFD simulations
using version 6.2 of FLUENT, for predicting
free surface profiles over broad crested weir,
they used the experimental data of (Hager W.
and Schwalt M. 1994) to verify the validity of
the computational code in prediction the
position of free surface profile, velocity and
pressure distributions for different flow rates.
(Afshar, H. and Hoseini, H. 2013) used CFD
together with laboratory model in order to
simulate the flow over rectangular broad-
crested weir. Simulations were performed
using three turbulence models of the RNG k–ε,
standard k–ε and the large eddy simulation
(LES) to find the water level profile and
streamlines. Their results indicated that RNG
model has lowest error compared with the
other models. (S. Hoseini, S. Jahromi and M.
Vahid 2013) used ANSYS FLUENT V.14
together with laboratory model for determining
the discharge coefficient of the rectangular
broad-crested side weir located on the
trapezoidal channel, they found that both
results of CFD and physical model showed that
Cd coefficient decreases with increasing values
of Fr and Cd coefficient increases with
increasing values of Re. (Hoseini S. H. 2014)
simulated the free surface flow over the
triangular broad-crested weir using FLOW 3D.
The simulation results were found in
reasonable agreement with experimental
observations. (Jalil, Shaker and Qasim, Jihan
2016) used FLOW-3D and HEC-RAS
software’s to predict the free surface profile of
Flow over Single-Step Broad- Crested Weir,
they found that HEC-RAS has limited ability to
produce curved profiles past vertical faces,
while FLOW-3D produced more accurate
results. (Al-Hashimi A. S. 2017) used Fluent
Software to compare four different turbulence
models accuracy in computing free surface
flow over broad crested weir and stepped weir
with rounded corner. Results are compared
with the experimental data and showed that the
predictions provided by the standard k–ε model
are closer to the experimental data, whereas
those obtained from the standard k–ω model
deviate the most. As found from literature
survey that the characteristics of flow over
broad crested weir along with the development
of CFD codes have attracted the attention of
many investigators. In this study, the flow
characteristics through Combined Pipe Culvert
and Broad Crested Weir were investigated
using ANSYS-CFX 14. The results of the
numerical model were compared with the
experimental data of (Othman K. Mohammed
2010).
2. THEORETICAL ANALYSIS
Computational Fluid Dynamics (CFD) involves
the solution of the equations of fluid flow (in a
special form) over a region of interest, with
specified (known) conditions on the boundary
of that region. The set of the governing
equations of fluid flow which are solved by
ANSYS-CFX are the Reynold average Navier-
Stokes equations. The governing equations of
continuity and momentum for incompressible
flow can be written as:










Where:
ρ = fluid density,
= average velocity in x
and y directions, x and y = space dimensions, t
= time, P = the pressure, µ =µo + µt , µo is
dynamic viscosity and µt is turbulence
133 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
viscosity, gi = acceleration due to gravity and

= the body force.
The suffices i and j indicate that the stress
component acts in the j-direction on a surface
normal to the i-direction. (Versteeg H. K. and
Malalasekera W. 2007)
ANSYS-CFX code uses finite volume method
to convert governing equations to algebraic
equation in order to be solved numerically. The
Naiver - Stokes equations with time average
velocity called Reynolds averaged Naiver
Stokes (RANS) equations. since the Navier-
Stokes equations are non-linear, it is difficult to
solve them analytically especially for turbulent
flow. Because the size of the computational
cells should be smaller than the length scale of
the smallest turbulent this is impossible which
cannot be achieved in many cases (Versteeg H.
K. and Malalasekera W. 2007).
Turbulent models have been classified based
on the application of their design and number
of differential equations to create relation
between turbulence stresses and averaged rates
or their gradients. Among these models, two-
equations model for modeling turbulence with
RANS equations have been used, one-layer
model such as k ε and (RNG) k ε and two-
layer model such as shear stress transport
(SST).
2.1. Standard k ε model:
This model expresses the turbulent
viscosity in terms of turbulent kinetic energy
(k) and its dissipation rate (ε). The following
two transport partial differential equations are
solved for the values of k and ε (Launder and
Spalding 1974):














The eddy viscosity µt is written as follows



 



Model constants: C1ε = 1.44, C2ε = 1.92,
=0.09, σk =1.0, and σε =1.3.
2.2. Renormalization Group (RNG) k ε
model (Choudhury D. 1993):
The (RNG) k-ε turbulence model is derived
from the instantaneous Navier-Stokes
equations, from using a mathematical
technique called, “renormalization group"
(RNG) methods. The analytical derivation
results in a RNG model with constants
different from those in the standard k-ε model
and additional terms and functions in the
transport equations for k and ε.





134 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139








 

 

In above Equations, C1ε, C2ε, and are
constants and equal to 1.42, 1.68, and 0.0845,
respectively. ak and aɛ equal to 1.393, ηo equal
to 4.38, µεff equal to 1 and β equal to 0.012.
2.3. Shear Stress Transport (SST) model
(Menter FR, 1994):
Menter (1994) developed the SST turbulence
model to blend effectively the robust and
accurate formulation of the k- ω model in the
near-wall region with the free stream
independence of the k- ω model in the far field.
It is an eddy-viscosity model which includes
two main novelties:
It is combination of a k-ω model (in the
inner boundary layer) and k-ε model (in the
outer region of and outside of the boundary
layer);
A limitation of the shear stress in adverse
pressure gradient regions is introduced.
The transport equations and effective viscosity
are modelled in SST k-ω model, by the
following equations:




















α* damps the turbulent viscosity causing a low
Reynolds number correction
, is the generation of and









F1, F2 are the blending functions
, represent the dissipation of and due
to turbulence
3. EXPERIMENTAL DATA
The experimental data (Table 1) used for the
comparisons were taken from laboratory tests
conducted by (Othman K. Mohammed 2010).
The geometry and dimensions of the combined
broad crested weir and pipe culvert model are
stated in Fig. (1). The experiments were
conducted in a horizontal research flume with a
width of 0.5 m, a height of 0.5 m and a total
length of 12 m. the laboratory model was made
of concrete box shape like of dimensions (50 x
50 x 13.1 cm), containing a plastic pipe 10.6
cm diameter. The notations in this paper are
kept identical to those defined by (Othman K.
Mohammed 2010).
135 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
Table 1, Experimental data.
Run
H/P
Q l/sec
Cd
1
0.180
10.780
0.526
2
0.240
12.360
0.521
3
0.310
15.140
0.542
4
0.400
17.950
0.527
5
0.480
21.620
0.531
6
0.510
22.720
0.535
7
0.560
24.900
0.53
8
0.590
28.270
0.569
9
0.760
37.010
0.566
10
0.930
47.350
0.575
Fig. (1) Geometry of the tested Model D = 10.6 cm,
P = 13. 1cm, L = 50 cm
4. NUMERICAL MODELLING
The numerical model was constructed at the
same dimensions as the physical model. This
allows direct comparison of the predicted
results with physical model results.
4.1. Mesh Design
Meshing is an important step to solve the
hydraulic systems in numerical modelling.
According to earlier studies, the smaller the
mesh size the greater is the accuracy and the
more is the computational time (Aziz, Y. W.
2016). ANSYS ICEM was used for mesh
generation as it contains many methods for
mesh generation. In this study the Multi-zone
method was used with the maximum and
minimum mesh size of 0.05 m and 0.000196 m
respectively such as mesh sizes used by (Aziz,
Y. W. 2016), and the hexahedron mesh type
was provided as shown in Fig. (2).
Fig. (2) Meshing and its Distribution
4.2. Boundary conditions
ANSYS-CFX contains several boundary
conditions including inlet, outlet, opening and
wall. Fig. (3). Inlet boundary condition
imposed at inlet section with the average
velocity, water and air volume fraction. Static
pressure used at the outlet and opening
boundary condition was specified for the top of
the fluid domain. On the walls, the no slip wall
boundary condition was applied; that is the
fluid velocity next to the wall immediately is
equal to zero. Walls were assumed to be
smooth, since the channel sides were made
from glass.
136 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
Fig. (3) Boundary conditions
5. RESULTS AND DISCUSSION
To have access to an appropriate turbulence
model for the simulation, the numerical model
is examined with different models of
turbulence such as standard k ε model, RNG
k ε model and SST model under the same
conditions (boundary condition, material, mesh
and so on). Then the results of these turbulence
models are compared with those provided by
the experimental data
The experimental and numerical results of
discharge through combined broad crested weir
and pipe culvert were plotted as shown in Fig.
(4). The results for all turbulence models with
the experimental data are very close to each
other, but some of them are in closer agreement
to the experimental data as presented in table 1.
Fig. (4) Comparison of QCFD with QExp for Combined
Weir and Culvert
Slight deviations are observed between the
predicted by numerical model and the
measured values from Fig. (4)
Fig. (5) shows the 3D and longitudinal section
at the center line of the simulated velocity
distribution through the culvert and over the
weir predicted by the k- ɛ turbulence model for
discharge flow rate of 28.27 l/s. Since from the
experiment there is no any measurement of
velocity, so the comparion with the CFD
modelling can not be done.
10
20
30
40
50
10 20 30 40 50
Q CFX
l/sec
Q exp
l/sec
k- ɛ
RNG k- ɛ
SST
137 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
Fig. (5) Velocity distribution through combined structure
for discharge 28.27 (l/sec) using k-ε turbulence model.
Table (2) shows that discharge coefficient
results obtained from SST turbulence are
mostly closer than the other models to the
experimental data. Further, it can be observed
that the RNG k- ɛ turbulence model performs
better than k- ɛ model. In addition, k- ɛ has
lesser agreement with the experimental data as
it has higher error percentage.
Table (2) Discharge coefficient and relative error of the
numerical simulations
Exp.
CFX
Standard k- ɛ
RNG k- ɛ
SST
Cd
Cd
Error
%
Cd
Error
%
Cd
Error
%
0.526
0.521
1.018
0.519
1.267
0.521
0.939
0.521
0.514
1.433
0.512
1.742
0.513
1.541
0.542
0.554
2.163
0.552
1.849
0.552
1.934
0.527
0.525
0.391
0.525
0.468
0.525
0.288
0.531
0.542
2.079
0.539
1.468
0.542
2.064
0.535
0.539
0.840
0.535
0.023
0.538
0.564
0.53
0.539
1.658
0.533
0.554
0.535
0.888
0.569
0.565
0.675
0.560
1.536
0.562
1.280
0.566
0.565
0.202
0.565
0.263
0.565
0.188
0.575
0.566
1.625
0.563
2.064
0.566
1.582
Discharge coefficients Resulted from Applying
turbulent models together with experimental
values plotted against relative upstream water
depth (H/P) are shown in Fig. (6). In this figure
H and P stand for the head of water above the
weir and weir height respectively. It can be
seen that, for all cases Cd increased with (H/P)
increasing this is due to increase the ratio of
(Flow cross sectional Area/Contracted
parameter).
Fig. (6) Head-discharge coefficient of the numerical
simulations and Experimental data
In order to determine the accuracy of the
simulation results, the Relative Error percent
(E %) of the experimental and the numerical
discharge results are calculated using the
equation:

  


Table (3) Relative Errors of the average discharge
coefficient
Exp.
CFX
Standard k- ɛ
RNG k- ɛ
SST
Cd
Cd
Error
%
Cd
Error
%
Cd
Error
%
0.542
0.543
1.208
0.540
1.123
0.542
1.127
0.5
0.52
0.54
0.56
0.58
0.1 0.3 0.5 0.7 0.9 1.1
Cd
H/P
exp.
k- ɛ
RNG k- ɛ
SST
138 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
Errors for discharge coefficient Resulting from
applying different turbulent models are shown
in Fig. (7).
Fig. (7) Discharge coefficient and their Relative Errors
from Applying Different Turbulent Models
It can be seen that (Fig 6 and Fig 7) the results
of k- ε turbulence model for discharge
coefficient are greater than those obtained by
experiments, but those of both (RNG) k ε and
SST are lower than experimental results. From
table (3) it is clear that higher percentage error
obtained by using k ε turbulence model,
while using RNG k ε has lower average
percentage error with the experimental data.
These differences can be clearly seen in charts
shown in Fig. (7).
6. CONCLUSIONS
In the present study, flow over broad crested
weir combined with the circular culvert is
simulated using ANSYS CFX. The
sensitivity of the results obtained from CFD
modeling of different turbulence models is
examined, to determine the turbulence model
that gives accurate predict of flow through the
combined structure. The summery of the
results of this study can be defined as follows:
1) SST model perform much better has the
maximum accuracy in comparison with
other turbulence models for most
discharges values, but for average relative
percentage error, (RNG) k- ε has a bit
greater accuracy than SST.
2) The results of k- ε have less accuracy
compared with other turbulence models.
3) The discharge coefficient in all methods
slightly increased with upstream relative
head (H/P) which was (from 0.526 to
0.575) such variation may be considered as
constant, same conclusion indicated by
(Hager W. and Schwalt M. 1994) for broad
crested weir flow.
4) It is also concluded that, such type of
software is useful to study the number of
fluid flow problems without going for
expensive and time consuming
experiments.
REFERENCES
Afshar, H. and Hoseini, H. "Experimental and 3D Numerical
Simulation of Flow over a Rectangular Broad-Crested
Weir". International Journal of Engineering and
Advanced Technology (IJEAT) August 2013, Volume-2,
Issue-6, 214-219.
Al-Hashimi A. S., Madhloom M. H., and Nahi N. T.
"Experimental and Numerical Simulation of Flow Over
Broad Crested Weir and Stepped Weir using Different
Turbulence Models", Journal of Engineering and
Sustainable Development Vol. 21, No. 02, March 2017.
Aziz, Y. W. "Evaluation of Hydraulic Performance of
Nazanin Dam Side Channel Spillway" MSc Thesis,
College of Engineering Salahaddin University Erbil
2016.
Choudhury D., (1993). "Introduction to the Renormalization
Group Method and Turbulence Modeling", Fluent Inc.
Technical Memorandum TM-107.
Duangrudee and Kositgittiwong "Validation of Numerical
Model of the Flow Behavior through Smooth and
Stepped Spillways using Large-scale Physical Model"
PhD Thesis, Faculty of Engineering, King Mongkut’s
University of Technology Thonburi 2012.
Duru, Aysel "Numerical Modelling of Contracted Sharp
Crested Weirs" MSc Thesis, School of Natural and
Applied Sciences of Middle East Technical University,
2014
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
Standard k- ɛ RNG k- ɛ SST
Exp.
CFX
E%
139 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139
Hager W. H. and Schwalt M. "Broad-crested weir", Journal
of Irrigation and Drainage Engineering, Vol. 120, No. 1,
(1994), pp.13-26.
Hargreaves D. M., Morvan H. P. and Wright N. G.
"Validation of the Volume of Fluid Method for Free
Surface Calculation: The Broad-Crested Weir",
Engineering Applications of Computational Fluid
Mechanics Vol. 1, No. 2, pp. 136146 (2007)
Hoseini, S.H. "3D Simulation of Flow over a Triangular
Broad-Crested Weir", Journal of River Engineering,
2(2), 1-7 (2014).
Jalil, Shaker & Qasim, Jihan. (2016). Numerical Modelling
of Flow over Single-Step Broad- Crested Weir Using
FLOW-3D and HEC-RAS. Polytechnic General
Sciences Journal/ Erbil Polytechnic University. 6. 435-
448.
Launder, B. E., and Spalding, D. B. “The numerical
computation of turbulent flows.” computer methods in
applied mechanics and engineering 3 (1974) 269-289.
Mahmoud S. M. "Characteristics and Prediction of
Simultaneous Flow Over Broad-Crested Weirs and
Through Culverts", EJEST, Vol, 6, No.1, January 2002
Menter FR (1994). "Two-equation eddy viscosity turbulence
models for engineering applications". AIAA Journal
32(8):1598-1605.
Negm A. M. Analysis and modeling of simultaneous flow
through box culverts and over contracted broad-crested
weirs Proc. of 5th International Conference on Hydro-
science and Engineering. ICHE2002. Sept. 18- 21.
Warsaw, Poland.
Othman K. Mohammed "Flow Characteristics through Pipe
Culvert Combined with Broad Crested Weir" MSc
Thesis, College of Engineering Salahaddin University
Erbil 2010.
S. Hoseini, S. Jahromi, M. Vahid “Determination of
Discharge Coefficient of Rectangular Broad-Crested
Side Weir in Trapezoidal Channel by CFD” IJHE 2013,
2(4): 64-70
Sarker, M.A and Rhodes, D.G," Calculation of free surface
profile over a rectangular broad-crested weir". Flow
Measurement and Instrumentation, 2004, 15(4) 215-219.
Versteeg H. K. and Malalasekera W. "An Introduction to
Computational Fluid Dynamics" Second Edition,
Pearson Education Limited 2007, pp 14, 66.
Wilcox D. C., "Turbulence Modeling for CFD", DCW
Industries Inc., La Canada, California (1993).
... RNG k-ɛ turbulence models showed the best performance to show the cross waves. Mohammed and Aziz (2018) simulated simultaneous flow over broad-crested weir and through pipe culvert using a numerical software and investigated different turbulence. Computational results indicated that RNG k − ε model has the maximum accuracy. ...
Article
Full-text available
In the present study, both experimental and numerical were conducted on a free surface flow over an obstacle. Numerical simulations were performed using the Renormalization Group (RNG-k-ɛ) based Reynolds-Averaged Navier–Stokes (RANS) turbulence model coupled with the Volume OF Fluid (VOF) method in FLUENT Software to investigate the effect of the channel slope on the flow pattern upstream, above and downstream the obstacle. Respectively, 5%, 7%, 8%, 10%, 20% and 50% channel slopes were considered. Numerical simulation has showed a good agreement compared against experimental results. Effect of the slope on the flow is observed particularly upstream of the obstacle where the flow takes the vertical direction after hitting the upstream wall. The more the slope becomes steeper, the higher the level of the water is. Recirculation zones in the case of a horizontal channel are elongated downstream the weir, whereas in the case of a sloped channel, they are localized just at the foot of the downstream wall.
Article
Introduction. The authors present one of methods for measuring water flows through the intake of a hydroelectric power plant. The new structure has a metal frame and a folding rotary row. The authors analyzed the advantages of the proposed, and mase strength and hydraulic analyses. Computational studies of the stress-strain state, made with account taken of the actual hydrodynamic pressure, allow choosing the optimal position of measurement points, designing a frame structure, and making highly accurate measurements of energy characteristics. Materials and methods. Top international publications, as well as archived materials, were analyzed to select the universal frame structure. The most promising directions were identified; the advantages and disadvantages of the proposed solutions were taken into account. Complex computational studies were performed using ANSYS Mechanical, a universal industrial software package, and ANSYS CFX, a specialized module for modeling flows of liquids and gases with account taken of turbulence. Results. The position of measurement points that ensure the least distortion of the flow and tilt angles of hydraulic turntables were determined during the hydraulic simulation. The flow loads were taken into account when the stress-strain state of the universal frame structure was calculated; optimal design solutions were selected to ensure the strength and reliability of metal elements. Stress concentration zones were identified for monitoring purposes during installation. Conclusions. Given the mathematical modeling data and experimental field studies, a universal frame structure for energy tests was substantiated. The new design ensures a measurement error of ±0.67 %, which corresponds to the leading world standards.
Article
Full-text available
A broad-crested weir has been considered the most hydraulic structures which was used in open channels for flow measurement and to control the water surface levels due to its simplicity. Both experimental and numerical models were conducted on a broad crested weir and stepped weir with a rounded corner. In this study, FLUENT software as a type of Computational Fluid Dynamics (CFD) model, represented as a numerical model in order to simulate flow over weirs that govern by Reynold averaged Navier Stoke equation and their results were compared with experimental results. The structured mesh with high concentration near the wall regions was employed in the numerical model. The volume of fluid (VOF) method with four turbulence models of Standard k-ε, RNG k-ε, Realizable k-ε and Standard k-ω are applied to estimate the free surface profile. The result showed that the flow over weirs is turbulent and the characteristics of free surface were complex and often difficult to be predicted. Also, the comparison of water surface profile between experimental value and numerical results obtained from the turbulent models showed that the standard k-ε model has the best similarity and standard k-ω model has the minimum similarity with experimental value.
Article
en Discharge measurement and control structures are widely employed in hydraulic engineering applications. The objective of this study is to numerically investigate the modelling of two different structures, namely sharp‐crested weirs as Problem 1 and combined weir and gate systems as Problem 2. The research methodology herein is based on the comparison of results of numerical simulations with experimental data for both problems separately. For the purpose of performing numerical simulations, the Reynolds‐averaged Navier–Stokes (RANS) equations are solved by finite volume formulation using commercially available Flow‐3D software. Assessment of empirical data and numerical findings for both problems reveals that discharge rates agree reasonably well. In addition, using the capabilities of numerical modelling, weir and gate discharge coefficients in the combined system are calculated separately which were not easy to obtain in experimental studies. It is seen that gate and weir discharge coefficients of the combined system are different and higher than the corresponding coefficients of the individual systems. © 2020 John Wiley & Sons, Ltd. Résumé fr Les structures de mesure et de contrôle du débit sont largement utilisées dans les applications de génie hydraulique. L'objectif de cette étude est d'étudier numériquement la modélisation de deux structures différentes, à savoir des seuils à crête vive comme problème 1 et des systèmes de seuil et de barrière combinés comme problème 2. La méthodologie de recherche ici est basée sur la comparaison des résultats de simulations numériques avec des données expérimentales pour les deux problèmes séparément. Dans le but d'effectuer des simulations numériques, les équations de Reynolds‐averaged Navier–Stokes (RANS) sont résolues par formulation de volumes finis à l'aide du logiciel Flow‐3D disponible dans le commerce. L'évaluation des données empiriques et des résultats numériques pour les deux problèmes révèle que les taux de rejet concordent assez bien. De plus, en utilisant les capacités de la modélisation numérique, les coefficients de débit de seuil et de vanne dans le système combiné sont calculés séparément, ce qui n'était pas facile à obtenir dans les études expérimentales. On voit que les coefficients de débit de vanne et de seuil du système combiné sont différents et supérieurs aux coefficients correspondants des systèmes individuels. © 2020 John Wiley & Sons, Ltd.
Article
Broad-crested weir is one of the most widely used hydraulic structures in irrigation and drainage systems. On natural streams where it is necessary to measure wide range of discharges, a triangular broad-crested weir has several advantages. Firstly, it provides a large breadth at high flows, so that the backwater effect is not excessive. Secondly, at low flows, the breadth is reduced so that the sensitivity of the weir remains acceptable. In this study, laboratory measurements on triangular broad-crested weir with different geometry were taken to investigate the flow pattern over a triangular broad-crested weir and new approach was undertaken to determine discharge coefficient equation. Results showed that the dimensionless parameters of h 1/L and Froude number have an effect on equation determining the discharge coefficient of the triangular broad-crested weirs. Good agreements between the measured values and the values calculated from the predictive equation are obtained. Therefore, an accurate equation for the discharge coefficient of the triangular broad-crested weirs in over-full condition ([Inline formula]) is introduced and could be used with confidence.
Article
This paper describes the validation of Computational Fluid Dynamics (CFD) for modelling free surface flows over common hydraulic structures. A series of CFD simulations are compared against an existing set of experimental data for the free surface flow over a broad-crested weir. By fixing the upstream and downstream water depths in the CFD model, it was possible to reproduce the experimental free surface profiles, pressure and velocity profiles and discharges over the weir for a range of discharge rates. The sensitivity of the results to the choice of turbulence model is presented. Gaining confidence in a modeling technique in this way, allows for the future modeling of more complex hydraulic structures and the introduction of the more complex physics required for modeling processes such as scour.
Article
Measurements of the free-surface profile over a laboratory-scale, rectangular broad-crested weir were compared with numerical calculations using commercial software. Although the geometry of the weir is simple, the fluid mechanics is complex with regions of separated flow that affect its hydrometric performance. For the given flow rate, the prediction of the upstream water depth was excellent and the rapidly-varied flow profile over the crest was reproduced quite well. In the supercritical flow downstream, a stationary wave profile was observed and reproduced in form by the calculations.