Numerical simulations of turbulent and flow characteristics of complex river reach in Pakistan

Muhammad Usman; Saman Shahid; Shahid Ali; Muhammad Kaleem Ullah

doi:10.4491/eer.2021.369

Environ Eng Res > Volume 28(1); 2023 > Article

Usman, Shahid, Ali, and Ullah: Numerical simulations of turbulent and flow characteristics of complex river reach in Pakistan

Research

Environmental Engineering Research 2023; 28(1): 210369.

Published online: February 20, 2022

DOI: https://doi.org/10.4491/eer.2021.369

Numerical simulations of turbulent and flow characteristics of complex river reach in Pakistan

Muhammad Usman¹, Saman Shahid^2,^†

, Shahid Ali³, Muhammad Kaleem Ullah⁴

¹Department of Civil Engineering, University of Management and Technology (UMT), Lahore, Pakistan

²Department of Sciences & Humanities, National University of Computer & Emerging Sciences (NUCES), Pakistan

³Department of Civil Engineering, National University of Computer & Emerging Sciences (NUCES), Pakistan

⁴Department of Civil Engineering, The University of Lahore, Lahore, Pakistan

^†Corresponding author, E-mail: drshahidsaman@gmail.com, Tel: +0092 42 111 128128, Fax: +0092 42 5165232

Received August 09, 2021 Revised December 16, 2022 Accepted February 16, 2022

(open-access):

This is an Open Access article distributed under the terms of the Creative Commons Attribution Non-Commercial License (http://creativecommons.org/licenses/by-nc/3.0/) which permits unrestricted non-commercial use, distribution, and reproduction in any medium, provided the original work is properly cited.

Abstract

The study included the numerical simulation of a curved open channel flow of Chashma Barrage for different velocities along left & right river banks, and water depths downstream of the river reach. The physical model was constructed in one of the experimental trays at the Irrigation Research Institute. Different trials were carried out at low, medium, and high discharges after the calibration of the physical model. A 2D computational fluid dynamics ANSYS FLUENT software was used to simulate various turbulences and flow properties for various discharges (500,000, 800,000, and 957,289 cusecs) using two different turbulent models: k-epsilon and Reynolds’s stress. The simulation findings were compared to the physical modeling results in terms of velocities and water depths for verification. In both velocity (18–27%) and water depth (18–36%) measurements, the k-model had a lower average percentage error than the RS model. On verification using physical modeling, the total average percentage difference from the k-model for all discharges was less than 25%. Numerical simulations based on computational fluid dynamics can be used to better understand turbulence and flow parameters, as well as to assess and develop barrage engineering.

Keywords: ANSYS FLUENT, Computational Fluid Dynamics, k-epsilon (ɛ) model, Reynolds’s Stress Model, Velocity Magnitude, Water Depth

1. Introduction

The estimation of flow parameters in curved open channels is one of the most important tasks in river engineering and related subjects. There is no practical method to completely comprehend the complicated phenomena of flow-like mean velocity profile, turbulence attributes of flow-like turbulence intensity, turbulence kinetic energy, turbulent viscosity, and Reynolds’ stresses, and others. Laboratory research to determine the flow parameters of curved channels is often time-consuming, costly, and difficult to meet in situ circumstances. When verifying simulation models and calibrating them, laboratory results are frequently unreliable [1]. Computational fluid dynamics (CFD) is an effective simulation-based numerical analysis technique that can cope with a variety of canal boundary conditions to examine fluid flow by solving numerous equations. There is an increased utilization of the CFD simulation model because it is a cost-effective option as compared to physical modeling. However, the quality of the mesh, boundary conditions, and selected models can impact the outcome of CFD models. These models have been developed as RANS (Reynolds-averaged Navier-Stokes) or LES (large eddy simulation) to calculate an accurate flow prediction [2]. RANS is generally thought to be more useful than grid generation and time simulations, both of which are used in engineering exercises. LES, on the other hand, can accurately predict the turbulent flow and coherent structure that arises [3]. The current study was aimed to numerically simulate a curved open channel flow of Chashma Barrage (Pakistan) for different velocities at various points along left & right river banks and water depths at different installed gauges along with the downstream of the river reach. The current study also validated and verified the simulation results in velocity magnitudes and water depths with the results of the physical modeling which was conducted at the Hydraulic Research Station Nandipur, Gujranwala. Two important turbulent models, i.e., the k-ɛ (k-Epsilon) model and RS (Reynolds’s stress) were used to numerically simulate the open channels for various turbulences and flow properties under various discharges through CFD ANSYS FLUENT software. The comparison of flow and turbulence properties like dynamic Pressure, velocities, turbulence kinetic energy (KE), wall shear stress, turbulence intensity, and total pressure using both turbulent models at different design discharges was also conducted. The present research studied the various flow and turbulence properties of the open channel reach about 9.65 km or 6 miles downstream of the Chashma barrage. The Chashma barrage is a barrage on the River Indus in the Mianwali District of Punjab, Pakistan towards 304 km NW of Lahore and 56 km downstream of Jinnah Barrage. Chashma barrage was constructed in 1971 and is designed with a discharging capacity of 950,000 Cs.

Kamel et al. (2014) [4] established an important turbulence model known as the k-epsilon (k-ɛ) model to determine the flow in meandering open channels. Previously, the numerical simulation of flow was observed by Wang et al. (2014) [5] in a compound multistage waterway with vegetation. For simulation, they applied the k-ɛ turbulence model to determine the various turbulence properties. To mimic the flow process through a vegetation patch, Zeng and Li (2014) [6] employed a 3D RANS model with the Spalart–Allmaras turbulence closure. One of the most common turbulence models known as Reynolds’s stress (RS) model has been used to investigate the flow pattern through discontinuous double-layered vegetation patches. A channel regime has been constructed through the GAMBIT (Geometry and Mesh Building Intelligent Toolkit) software. In addition, the channel geometry can be loaded into the ANSYS FLUENT program to determine different flow and turbulence parameters [7]. Anjum et al. (2018) [7] studied various properties like mean velocity, Reynolds’s stresses, and turbulence kinetic energy through simulation, and their contours were obtained after post-processing in ANSYS FLUENT. It was observed after simulations that, Reynolds stresses, turbulent kinetic energy, and turbulence intensity showed a very large variation inside the vegetation zone as compared to the gap regions. Koutrouveli et al. (2014) [8] identified the effect of groyne spacing on the flow characteristics like mean velocity, turbulence dissipation rate, and bed shear stress by utilizing a 3D-RANS solver. The solution of the ruling equations on the finite volume discretization was derived from the computational fluid dynamic codes i.e., via ANSYS-FLUENT. The equations were evaluated via. steady-state mode with required equilibrium conditions. Ghisalberti and Nepf (2004) [9] investigated the influence of shear layers generated by vegetation on mean velocity profiles experimentally and numerically. Yokojima et al. (2015) [10] simulated the flow of open channels by using the LES model considering the cylindrical vegetation structures. Järvelä (2005) [11] performed experiments to analyze the effect of flexible vegetation on the flow structure.

2. Materials and Methods

The methodology adopted in the research work is presented in Fig. S1 (see supplementary information).

2.1. Input Data

The primary input data was collected from the National Engineering Services Pakistan (NESPAK), Lahore. The NESPAK provided the data on the various cross-sections (widths & depths) of the downstream reach of Chashma Barrage.

The reach length that was analyzed is shown in Fig. S2. The plan view or layout of Chashma Barrage downstream reach that was provided through AutoCAD by NESPAK file is shown in Fig. S3.

2.2. Arrangements of the Channel reach to Carry out the Physical Modeling

The physical model was constructed in one of the experimental trays at the Irrigation Research Institute (IRI) Nandipur, Gujranwala. The scale of the physical model had been kept at 1:300 horizontal and 1:50 vertical to layout the Indus River reach of about 6 miles. The other conversion factors regarding the area, velocity, discharge, and time are provided in Table 1.

2.3. Glimpses of the Physical Modeling of the Downstream Reach in Dry Phase

The physical model was constructed based on the information and drawings provided by the NESPAK, which included the topographic survey layout plan, river cross-sections, details of the Chashma barrage, and existing training works. Drawings of the headrace and the tailrace channel of the Chashma powerhouse were also arranged and provided by NESPAK. The setup to perform physical modeling at the research station is shown in Fig. S4(a). The river rating curves at Chashma barrage downstream were also provided by NESPAK for the model operation. The physical modeling was carried out in the dry phase is shown in Fig. S4(b).

2.4. Model Calibration and Hydraulic Testing

To achieve the river morphology, the physical model was first calibrated against historic floods. After satisfactory calibration, the trials were run to observe the behavior of flows within the study reach for achieving the object of the model study. After the model was built, the first objective was to calibrate it against the historic floods of 2010 and 2015. After calibration of the physical model, different trials were carried out at low, medium, and high discharges. Adequate time was given to each trial so that the modeled river reach attained a stable bed configuration and bank formation against that flow. The physical modeling carried out in the wet phase is shown in Fig. S5. Different discharge types and their respective values are given in Table 2.

2.5. Measurements of Water Levels and Velocities at Different Discharges

To determine the water levels within the river geometry, various gauges were installed at different points, which recorded the water levels under different discharges (e.g., 500,000, 800,000, and 957,289 cusecs). For water level measurement, the position of different gauges within the river propagation is shown in Fig. S6(a). Velocity measurements were carried out by using current meters along both (left/right) river banks to observe the scour potential. Fig. S6(b) shows the left and right banks downstream of the river, where velocity had to be measured. Table 3 shows the measurements of water level at various gauges installed within the river geometry. Velocity measurements on the left and right banks of the river are shown in Table 4.

2.6. k-Epsilon (k-ɛ) Model

The best known k-ɛ model is a two-equation turbulence model, which is incorporated in most of the commercial computational fluid dynamic codes. Following five empirical constants are considered in k-ɛ model: C_μ, C_ɛ₁, C_ɛ₂, σ_k, and σ_ɛ. The transport equation is given below Eq. (1) was considered for the dissipation rate [4]:

(1)

\frac{\partial \in}{\partial t} + U_{i} \frac{\partial \in}{\partial x_{i}} = \frac{\in}{k} (C_{\in 1} P - C_{\in 2} \in) + \frac{\partial}{\partial x_{i}} (\frac{v_{t}}{σ_{\in}} \frac{\partial \in}{\partial x_{i}})

Where,

$\frac{\partial ɛ}{\partial t} = R a t e o f C h a n g e o f ɛ$
$U i \frac{\partial ɛ}{\partial x i} = T r a n s p o r t o f ɛ by convection$
$\frac{ɛ}{k} (C ɛ_{1} P - C ɛ_{2} ɛ) = P r o d u c t i o n a n d d i s s i p a t e r a t e o f ɛ$
$\frac{\partial}{\partial x i} (\frac{V t}{σ ɛ} \frac{\partial ɛ}{\partial x i}) = T u r b u l e n t T r a n s p o r t o f ɛ$

2.7. Reynolds Stress (RS) Model

The Reynolds stress (RS) model is an advanced Reynolds-Averaged Navier-Stokes turbulence model. Eq. (2) is a general form for the Reynolds stresses [7].

(2)

\frac{\partial R i j}{\partial t} + C i j = P i j + D i j - ɛ i j + Π i j + Ω i j

Where R_ij = rate of change of Reynolds stresses, C_ij = transport of convection, P_ij = rate of production of Reynolds stresses, D_ij = transport of stresses by diffusion, ɛ_ij = dissipation rate of stresses, Π_ij = stresses transport due to turbulent pressure–strain interactions, and Ωij = transport of stresses due to rotation [7].

2.8. Numerical Simulation

In the coding for a CFD package, there are four basic steps: setting up the experimental channel’s geometry, producing the geometry’s mesh, setting up the Physics, and post-processing [2]. Two important turbulent models, i.e., the k - ɛ (k-Epsilon) model and RS (Reynolds’s stress) were used to simulate open channels for various turbulences and flow properties under various discharges through CFD ANSYS FLUENT software. Open channel is also known as a turbulent channel because the flow in the channel is turbulent and turbulent channels can also be studied numerically by using an isotropic k-ɛ model [12]. The K-ɛ model and RS models are the most important turbulence closure model that is used for the simulation of river flows. CFD is frequently used as a technique to investigate flow structure in developing areas of the flow field for the determination of velocity, pressure, shear stress, the effect of turbulence, and others [13].

2.9. Input Data Used for the Numerical Simulation in ANSYS FLUENT

There was no information available on the bed levels and water levels at the cross-section where the Chashma barrage gates or bays are located. As a result, we gathered all of the essential input data from the barrage section’s nearest point, the G4 point, where bed levels were derived from an AutoCAD file. The inlet point discharges were unknown, but the respective velocities were provided for the 2D simulation by IRI (Irrigation Research Institute, Gujranwala). The reach’s details are provided in Table 5, for the 2D simulation.

2.10. Comparison between Physical Modeling and Numerical Simulations

The simulation results were compared with velocities and water depths with the physical modeling, which was conducted at the Hydraulic Research Station Nandipur, Gujranwala for verification and validation. The percentage errors were calculated between the numerical simulation results from two turbulent models (k - ɛ & RS) with the physical modeling results for the parameters (velocities and water-depths) at various discharges (500,000, 800,000, and 957,289 cusecs).

2.11. Other Flow and Turbulence Properties

The comparison of remaining flow and turbulence properties like dynamic Pressure, velocities, turbulence kinetic energy (KE), wall shear stress, turbulence intensity, and total pressure using both turbulent models at design discharge Q = 800,000 cusecs was also done. Moreover, the determination of Reynolds’s Stresses like normal, shear, and total stresses at various sections of bellas through the RS model at Q = 800,000 cusecs were also evaluated.

3. Results

3.1. Mesh Generation

The meshing of geometry is the most important step in numerical analysis. Subdividing or discretizing the geometry into the elements or cells by which the variables will be calculated numerically is called meshing. Meshing splits into a variety of fixed figures of nodes. Fig. S7(a) shows the updated mesh that was generated in ANSYS FLUENT after several iterations. The refined and zoomed image to show different nodes of the geometry is shown in Fig. S7(b).

3.2. Various Flow and Turbulence Parameters Obtained through ANSYS FLUENT Simulation

The 2D simulation in ANSYS FLUENT was done to compare the velocities at various points along the left and right banks of the river experimentally and by simulation using different turbulence models at the following discharge values:

For 500,000 cusecs (less than design discharge of Chashma Barrage)
For 800,000 cusecs (at design discharge of Chashma Barrage)
For 957,289 cusecs (greater than design discharge of Chashma Barrage)

Velocity contours using k-ɛ model at Q = 500,000 cusecs are shown in Fig. S8(a). On the other way, velocity vectors showing different contours with different colors are shown in Fig. S8(b). Velocity contours using the RS model at Q = 500,000 cusecs are shown in Fig. S9. Velocity contours using k-ɛ model and RS model for discharge values at Q= 800,000 cusecs and Q = 957,289 cusecs are shown in Fig. S13–S16.

2D simulation in ANSYS FLUENT was done to compare the water depth values at various gauge locations within the river propagation geometry experimentally and by simulation using different turbulence models at the following discharge values:

For 50,000 cusecs (less than design discharge of Chashma Barrage)
For 500,000 cusecs (less than design discharge of Chashma Barrage)
For 800,000 cusecs (at design discharge of Chashma Barrage)
For 957,289 cusecs (greater than design discharge of Chashma Barrage)

Static Pressure contours using k-ɛ model at Q = 500,000 cusecs is shown in Fig. S10(a). The static pressure contours using the RS model at Q = 500,000 cusecs are shown in Fig. S10(b). Static Pressure contours using k-ɛ model and RS model for discharge values at Q = 50,000 cusecs, Q = 800,000 cusecs, and Q = 957,289 cusecs are shown in Fig. S17–S19. The other flow and turbulence properties were analyzed only at discharge and inlet velocity of 9.76 ft/s at Q = 800,000 cusecs.

Fig. S11(a) shows the turbulence intensity contours using the k-ɛ model at design discharge. While total pressure stress contours using the RS model at Q = 800,000 cusecs is shown in Fig. S11(b). Remaining flow and turbulence properties like normal stresses, shear stresses, total stresses, dynamic pressure, total pressure, velocity magnitude, turbulence kinetic energy, wall shear stress, and turbulence intensity were analyzed using both turbulent models at design discharge Q = 800,000 cusecs are shown in Fig. S20–S26.

3.3. Comparison of Physical Modeling Results with the Simulation Results in the Magnitudes of Velocities and Water Depths

3.3.1. Velocity comparison

Table 6 shows the velocity comparison between the physical modeling & numerical simulation along the left and right banks at Q = 500,000 cusecs and Q = 800,000 cusecs. However, the velocity comparisons between the physical modeling & numerical simulation along the left and right banks at Q = 957,289 cusecs in tabular form are shown in Table S1.

3.3.2. Water depths comparison

Table 7 shows the water depth comparison between the physical modeling & numerical simulation at various gauges at Q = 500,000 cusecs and Q = 800,000 cusecs. However, the water depths comparison between the physical modeling & numerical simulation at various gauges at Q = 50,000 cusecs and Q = 957,289 cusecs are shown in Tables S3 and S4.

3.3.3. Different flow and turbulence properties at start and endpoints of bellas at Q = 800,000 cusecs

The different flow and turbulence parameters were determined at u/s (upstream) and d/s (downstream) (or at the starting and ending points of bellas) within the river geometry to see the phenomena of erosion and deposition of the sediments on these points. The various sections of bellas within the river geometry at u/s and d/s section are shown in Fig. S12.

3.4. Comparison of % Errors between Physical Modeling and Numerical Simulation (Velocities & Water-Depths)

After getting the results like velocity at various points along the left and right banks of the river, water depths at various gauge locations, various flows and turbulence properties from the physical modeling were compared with the numerical simulations from two different turbulent models (k-ɛ and RS) using ANSYS FLUENT. The comparison is as follows:

3.4.1. Velocities along the left and right banks of the river

3.4.1.1. For Q = 500,000 cusecs (Along with the points on the right bank of the river)

The average percentage error from the results of physical modeling was lower (18.37%) in the k-ɛ model as compared to the RS model (25.16%). However, at one velocity (V3) point, the k-ɛ model reported a higher percentage difference as compared to the RS model (Table 8).

3.4.1.2. For Q = 500,000 cusecs (Along the points on the left bank of the river)

The average percentage error from the results of physical modeling was lower (21.09%) in the k-ɛ model as compared to the RS model (29.49%). However, at one velocity (V11) point, the k-ɛ model reported a higher percentage difference as compared to the RS model (Table 8).

3.4.1.3. For Q = 800,000 cusecs (Along the points on the right bank of the river)

The average percentage error from the results of physical modeling was lower (25.52%) in the k-ɛ model as compared to the RS model (27.93%). However, at two velocity points (V2 and V5), the k-ɛ model reported a higher percentage difference as compared to the RS model (Table 8).

3.4.1.4. For Q = 800,000 cusecs (Along the points on the left bank of the river)

The average percentage error from the results of physical modeling was lower (28.51%) in the k-ɛ model as compared to the RS model (33.27%). However, at two velocity points (V9 and V11), the k-ɛ model reported a higher percentage difference as compared to the RS model (Table 8).

3.4.1.5. For Q = 957,289 cusecs (Along the points on the right bank of the river)

The average percentage error from the results of physical modeling was lower (27.52%) in the k-ɛ model as compared to the RS model (34%) (Table S2).

3.4.1.6. For Q = 957,289 cusecs (Along the points on the left bank of the river)

The average percentage error from the results of physical modeling was lower (27.65%) in the k-ɛ model as compared to the RS model (37.74%) (Table S2).

The verification percentage difference was in closer values between k-ɛ model and the RS model in velocity comparison (on the right side bank) at 800,000 Cu of discharge. Minimum average percentage difference (18%) was observed from the k-ɛ model in velocities of the right side of the river bank at the 500,000 Cu of discharge. Maximum average percentage difference (37.74%) from RS model in velocities of the left side of the river bank at 957,289 Cu of discharge. The overall average percentage different from k-ɛ model for all discharges was less than 25% on verification with the physical modeling. However, the overall average percentage difference was 31% from the RS model for all discharges on verification with the physical modeling. Therefore, overall, concerning the average values, the numerical simulation via. the k-ɛ model gave more accurate results as compared to the RS model in velocities along with the mentioned points at the right/left banks of the river.

3.5. Water Depths at Various Gauge Locations within the River Geometry

3.5.1. For Q = 500,000 cusecs (At different gauge locations within the river geometry)

The average percentage error from the results of physical modeling was lower (18.46%) in the k-ɛ model as compared to the RS model (22%). However, at two points (G-4 and G-5), the k-ɛ model reported a higher percentage difference as compared to the RS model (Table S13).

3.5.2. For Q = 800,000 cusecs (At different gauge locations within the river geometry)

The average percentage error from the results of physical modeling was lower (19%) in the k-ɛ model as compared to the RS model (28.73%). However, at two points (G-5 and G-6), the k-ɛ model reported a higher percentage difference as compared to the RS model (Table S13).

3.5.3. For Q = 957,289 cusecs (At different gauge locations within the river geometry

The average percentage error from the results of physical modeling was lower (36.33%) in the k-ɛ model as compared to the RS model (46.24%). However, at one point (G-4), the k-ɛ model reported a higher percentage difference as compared to RS model Table S5.

The average percentage difference was also in closer value water depth comparisons at 500,000 Cu from for k-ɛ and RS models. In comparison with experimental results, the minimum average percentage difference (18%) was observed from the k-ɛ model with water depth measurements at 500,000 Cu of discharge. Similarly, the maximum average percentage difference (46%) from the RS model with water depth measurements at 957,289 Cu of discharge. The overall average percentage different from k-ɛ model for all discharges was less than 25% on verification with the physical modeling. However, the overall average percentage difference was 32% from the RS model for all discharges on verification with the physical modeling. Therefore, overall, concerning the average values, the numerical simulation via. the k-ɛ model gave more accurate results as compared to the RS model in water-depths at different locations within the river geometry.

3.6. Other Flow and Turbulence Properties Comparison

The comparison of remaining flow and turbulence properties like dynamic pressure, velocity magnitudes, turbulence kinetic energy (KE), wall shear stress, turbulence intensity, and total pressure using both turbulent models at design discharge Q= 800,000 cusecs in tabular form are shown in Tables S6 to S11. Determination of Reynolds’s Stresses like normal, shear, and total stresses at various sections of bellas through RS model at Q = 800,000 cusecs in tabular form are shown in Table S12.

4. Discussion

Numerical simulation as part of computational fluid dynamics (CFD) of an open channel flow is a challenging task. The current study conducted a numerical simulation through two different turbulent models (k-ɛ & RS) of a curved open channel flow of Chashma Barrage at different velocities (along left & right river banks) and water depths (at downstream of the river reach). Because the characteristics of open channel flow are influenced by the interaction of the fluid with a variety of structural components such as walls and channel bed, gravity, turbulence, and friction, the current research primarily focused on flow properties such as the average velocity of flow and depth of water at various points along the river’s path, as well as turbulence properties such as turbulence KE, turbulence intensity, static and dynamic pressures, and so on. Different trials were carried out at low, medium, and high discharges after the calibration of the physical model. A 2D computational fluid dynamics ANSYS FLUENT software was used to simulate various turbulences and flow properties for various discharges (500,000 cusecs, 800,000 cusecs & 957,289 cusecs) using two different turbulent models: k-epsilon and Reynolds’s stress. The simulation findings were compared to the physical modeling results in terms of velocities and water depths for verification. Because flow in an open channel is turbulent and transitory, it is extremely difficult to anticipate. In addition to this irregularity, the curvedness of the channel’s geometry and the variation of the free surface concerning time also affect the prediction. To examine a flow structure, the distribution of velocity, and mass transport in a meandering straight and compound open channel, the outcomes of the non-linear k–ɛ model of turbulence have been introduced. Similar study is related to the present research made by Gandhi et al. (2010) [14] to examine the velocity profiles for different open-channel geometries utilizing CFD code, specifically the FLUENT. The resulting CFD model for a real open channel was first validated by comparing the velocity profile obtained from FLUENT to the actual estimation in a comparable channel using a current meter. It was discovered in the current study that computational fluid dynamics (CFD) models are fairly easy to accomplish if the equations underlying the models are properly understood. CFD is also used to solve complex fluid problems from very basic 2D equations to 3D by considering complex Eddies phenomena. In this study, it was found that overall, the numerical simulation via. the k-ɛ model was more accurate as compared to the RS model in velocities along with the mentioned points at the right/left banks of the river. Overall, the numerical simulation via. the k-ɛ model provided more accurate calculations as compared to the RS model in water-depths at different locations within the river geometry. Various aspects of river engineering, such as upstream and downstream boundary conditions, riverbank detail, an understanding of hydraulic resistance and open channel flow turbulence, description of model selection and model calibration, all helped to strengthen the theoretical background related to river hydraulics for the simulations [15–16]. Many of the early findings derived on this topic were based on the results of the Flood Channel Facility (FCF) program implemented in the United Kingdom in the 1990s The FCF geometry was described as having the potential to lead to conclusions based on a channel architecture that was not entirely representational of nature. It implies that the flow structure changes as a function of the channel width-to-depth ratio, necessitating the use of various turbulence model methodologies to appropriately compute this. The standard k– has been proved to be insufficient. It was also shown that the bank slope was influential in determining the flow structure, and the flatter the slope the more likely it was to present increasing difficulties for modeling [15–17]. A limited number of CFD simulations have been conducted by using the commercial software FLUENT. In particular, mean velocity distributions for the rectangular open channel transitions were used for model validation. A physical model was also validated and calibrated in the present research shows the same conditions of research carried out in this literature. The two-dimensional Reynolds-Averaged Navier Stokes (RANS) equations and the two equations RNG k-ɛ models have been used. The findings of experimental research on subcritical flow through progressive expansion in rectangular rigid-bed channels used by CFD for various flow values have been presented previously. Alhashimi (2018) [18] analyzed the efficiency of the transitions generated by different values of discharge by creating velocity distributions of flow via the transition models. An attempt had been made by Patel & Gill (2006) to simulate secondary flows in curved open channels using three-dimensional CFD analysis. Besides the classical center-region cell, a counter-rotating outer bank cell was often observed which could play an important role in the mechanism of sediment transport. The CFD analysis was carried out on the 120° curved open channel bend using the commercial software package FLUENT. Same CFD software with the turbulent model used in the current study to determine flow parameters as used in this literature. The volume of fluid (VOF) model was used to simulate the air-water interaction at the free surface and the turbulence closure was obtained using the Reynolds stress model. The Reynolds stress model was shown to be capable of accurately predicting both circulation cells. The results demonstrate that the core of maximum velocities was discovered near the separation between both circulation cells and below the free surface, which is consistent with experimental data [19].

The present research studied the various flow and turbulence properties of the open channel reach about 9.65 km or 6 miles downstream of the Chashma barrage. In the current study, the flow parameters were determined (Water depths at various points within river propagation and velocity measurements along left and right banks of river) experimentally by physical modeling. Experimental results were then compared with numerical simulation results through ANSYS FLUENT using different turbulent models (k-ɛ model and RS model). It was inferred that error between experimental and simulation results of velocities along the mentioned points and water-depths at different locations was found within 25% from the k-ɛ model and gave satisfactory results as compared to the RS model. The impacts of vegetation on flow through numerical models have been investigated by various researchers. Zhao and Huai (2016) [20] used a large eddy simulation (LES) model and examined the impacts of intermittent inundated vegetation patches on turbulent flow in an open channel. Two laboratory flume experiments were performed to validate the large eddy simulation (LES) model. The obtained LES data were in good agreement with the experimental data. They were also highly accurate in capturing the secondary peaks of the mean velocity near the channel bed. The coherent vortices, which were generated by the shear between the slower canopy flow and the faster overlying flow, were found associated with the velocity inflection and maximum Reynold’s stress around the interface. The gap regions’ mean velocity was lower than that of the canopy regions. A high canopy density and Reynolds number were more conducive for the fully developed flow state of discontinuous vegetation patches. The velocity distinctly increased within the first two patches with a high canopy density. The velocity profile in the wide gaps was more stable than in the small gaps below the vegetation height, but the influence of patch distribution in the overlying flow layer was not noticeable. The turbulence of flow across discontinuous vegetation patches is influenced by two vortex sizes, namely stem-scale and shear-scale vortices, according to a spectral study. Jalonen et al. (2015) [21] observed the physically-based characterization of mixed floodplain vegetation employing terrestrial laser scanning (TLS). The work aimed at developing an approach for deriving the characteristic reference areas of herbaceous and foliated woody vegetation, and estimating the vertical distribution of woody vegetation. The field investigations were conducted in a 200 m long two-stage channel having 20 m long test reaches of different floodplain vegetation in Sipoo in southern Finland. The two-stage channel had a bankfull width of 11 m, where the width of the floodplain was 4–6 m. Zhu et al. (2014) [22] investigated experimentally the effects of rigid vegetation on the characteristics of flow, the vegetations were modeled by the rigid cylindrical rod. The flow field was measured under the conditions of submerged rigid rod in a flume with a single layer and double-layered vegetation. Experiments were performed for various spacings of the rigid rods. The vegetation models were aligned with the approaching flow in a rectangular channel. Vertical distributions of time-averaged velocity at various streamwise distances were evaluated using an acoustic Doppler Velocimeter. The results indicated that, in submerged conditions, it was difficult to describe velocity distribution along the entire depth using a unified function. The characteristic of the vertical distribution of longitudinal velocity was the presence of the inflection. Stone and Shen (2002) [23] conducted various laboratory experiments on the hydraulics of flow in an open channel with circular cylindrical roughness. The laboratory study consists of an extensive set of flume experiments for flows with emergent and submerged cylindrical stems of various sizes and concentrations. The results show that the flow resistance varies with flow depth, stem concentration, stem length, and stem diameter. The stem resistance experienced by the flow through the vegetation was best expressed in terms of the maximum depth-averaged velocity between the stems. Physically-based formulas for flow resistance, the apparent channel velocity, and flow velocities in the roughness and surface layers were also developed. Steffler and Yee-Chung (1993) [24] worked on the velocity profile in the curved open channels by considering the hydrostatic pressure distribution by developing a 2D numerical model. Duan (2004) [25] analyzed the various flow parameters like velocity and pressure distribution profiles in curved open channels, which involves the momentum equations by 2D averaged models. Two laboratory experimental cases, flow in mildly and sharply curved channels, were selected to test the hydrodynamic model. The comparison of the simulated velocity and water surface elevation with the measurements indicated that the inclusion of the dispersion terms has improved the simulation results. Nagaosa (1999) [26] worked on Direct Numerical Simulation (DNS) for open channel flows by considering the free surface of the water had a rigid slip condition whose vertical moment was ignored. First, the effect of the free surface on fully developed turbulence statistics was described. Anisotropy of velocity and vorticity under the free surface were given. Next, the dynamics of the intermittent vortex tubes beneath the free surface were stated. The genesis and development of these coherent structures and their interactions with the free surface were demonstrated. The role of the vortex/surface interactions on the dynamics of turbulence under the free surface, particularly intercomponent energy transfer due to the pressure–strain effect was discussed. Borue et al. (1995) [27] also worked on DNS for open channel flows, but they considered the linearized free surface boundary conditions. Lien et al. (1999) [28] presented a 2D depth-averaged model for simulating and examining flow patterns in the channel bends. In particular, their study proposes a 2D depth-averaged model that takes into account the influence of the secondary flow phenomenon through the calculation of the dispersion stresses arising from the integration of the products of the discrepancy between the mean and the true velocity distributions. The proposed model used an orthogonal curvilinear coordinate system to simulate the flow field efficiently and accurately with irregular boundaries. As for the numerical solution procedure, the two-step split-operator approach consisting of the dispersion step and the propagation step with the staggered grid was used to numerically solve the flow governing equations. Two sets of experimental data from de Vriend & Koch (1977) [29] and Rozovskii (1961) [30] were used to demonstrate the model’s capabilities. The former data set was from a mildly curved channel, whereas the latter was from a sharply curved channel. The simulations considering the secondary flow effect well agreed with the measured data. Furthermore, an examination of the dispersion stress terms showed that the dispersion stresses play a major role in the transverse convection of the momentum shifting from the inner bank to the outer bank for flows in both mild and sharp bends. Onitsuka and Nezu (2001) [31] observed that by using the LES model, one can use the rigid slip surface condition instead of the free surface condition by considering the internal flow methods with minor changes. Meftah et al. (2008) [32] analyzed flow patterns in partly vegetated open channels. The presence of emergent vegetation strongly affected the flow hydrodynamic structures, forming a transversal abrupt velocity-transition region at the interface between the obstructed and the unobstructed domains. Because the transversal mean flow velocity distribution at the interface closely resembles a boundary layer characteristic, we used the universal law of the wall to predict the fully developed zone’s transversal profile. Vegetation was simulated using an array of emergent steel cylinders mounted on a large rectangular channel in the Department of Civil, Environmental, Building Engineering and Chemistry of the Technical University of Bari, Italy. The three components of the flow velocity were measured using a 3D Acoustic Doppler Velocimeter. Therefore, the current study conducted simulations on the complex river reach of the Chashma barrage by using the common turbulence models at different flow rates and velocities. Although, modern computer systems can use more complex 3D modeling of open channels to deal with irregular channel shape, wave movement of the free surface, and even the presence of vegetation and bed roughness. But, most of the work has also been done in 1D or 2D with a very limited application of 3D models, on studying various properties of the open channel [33]. Meftah et al. (2016) [34] focused on the study of flow structures in a channel partially obstructed by arrays of vertical, rigid, emergent, and vegetation/cylinders. Special attention was given to understanding the effect of the contraction ratio, on the flow hydrodynamic structures and to analyzing the transversal flow velocity profile at the obstructed-unobstructed interface. A large data set of transversal mean flow velocity profiles and turbulence characteristics were reported from experiments carried out in a laboratory flume. The flow velocities and turbulence intensities have been measured with a 3D Acoustic Doppler Velocimeter. It was observed that the arrays of emergent vegetation/cylinders strongly affect the flow structures, forming a shear layer immediately next to the obstructed-unobstructed interface, followed by an adjacent free-stream region of full velocity flow. The experimental results showed that the contraction ratio significantly affects the flow hydrodynamic structure. Adaptation of the Prandtl’s log-law modified by Nikuradse, has led to the determination of a characteristic hydrodynamic roughness height to define the array resistance to the flow. The flow and bed morphodynamics through rigid, emergent cylinders which were regarded as the vegetation was computed using a three-dimensional numerical model by employing a large-eddy simulation approach with a ghost-cell immersed-boundary method. The scour and transport processes were solved using sophisticated sediment transport and morphodynamic models in a physics-based manner. In an infinitely long patch, the vegetation density significantly influenced the flow and morphodynamic behavior. Under a low vegetation density, the scour and deposition were similar to those of an isolated cylinder, while there were significant variations at a higher vegetation density. The cylinder-interval variation had a negligible impact on the maximum scour depth, which was similar to that in an isolated cylinder case [35]. The ability to simulate flow characteristics is one of the most important issues in the design and application of open-channel bends. Three-dimensional computational fluid dynamics (CFD) and multi-layer feed-forward artificial neural networks (MLFF-ANNs) have been used in modeling the flow depth and velocity field in sharp bends. CFD was modeled in two phases, i.e., in water and air, by using the volume of fluid method. The backpropagation algorithm was applied in the training process of the ANN model. An experimental study of a 90° curved channel was undertaken to verify and compare the efficiency of the CFD and ANN models. The results showed that both CFD and ANN methods can be successfully applied to the modeling of open channel bend characteristics [36] The comprehensive 3D numerical investigation highlighted the driving mechanisms for junction-induced energy losses. Furthermore, the 1D and 3D investigations compared the departure of 1D approximations and underlying assumptions from the ‘actual’ resulting flow field. The previous study also shed light on improving the accuracy of the 1D large network modeling through the parameterization of the complex 3D feature of the flow field and correction of interior boundary conditions at junctions of larger angles and/or with substantial lateral inflows. Moreover, the enclosed numerical investigations may enhance the understanding of the primary mechanisms contributing to hydraulic structure-induced turbulent flow behavior and increased hydraulic resistance [37]. ANSYS CFX 18.2 was used to analyze the vertical velocity distribution and other flow characteristics as resistance to varying densities, length, and positioning of solid cylindrical rods representing vegetation. The CFD approach has been used to identify, determine, and measure the parameters that contribute to additional resistance due to vegetation. The aim was to better understand hydraulics in stream-flow with vegetation systems and to suggest a design tool for evaluating the potential effect of vegetation on stream water management and ecology in Albania. It was found that the model for the three considered cases gave different results for each of the evaluated parameters, therefore, a correlation exists between the development of the flow hydraulic properties and the vegetation configurations. Also, the obtained results showed that vegetation has a great influence on the characteristics of the flow [38]. The k-turbulent model, which has been proven to be successful for numerical simulations, may be used in a more advanced study to further minimize inaccuracies. Numerical simulations based on CFD may be used to better understand turbulence and flow characteristics, as well as to assess and develop barrage engineering.

5. Conclusions and Recommendations

In the study, the flow parameters were determined experimentally and using the most important turbulent models like the k-ɛ model and RS model in ANSYS FLUENT. The turbulence properties were also analyzed to understand the complex turbulence phenomenon which was impossible to visualize experimentally. The error between experimental and simulation results of velocities along the mentioned points and water-depths at different locations was found within 25% from the k-ɛ model. Future research can be conducted to perform the 3D modeling of the complex river reach by using the ANSYS FLUENT software, to determine the velocity and shear stress profiles at the critical points. The analysis can be conducted for the evaluation of the erosion and deposition of the bed material depending upon the velocity and flow at various points at the start and endpoints of bellas. The movement of bed material by using SSIIM (Sediment Simulation in Intakes with Multiblock) software can also be analyzed. The dynamic wave propagation on the free surface of the water by the 3D simulation can also be evaluated.

6. Limitations

The physical measurements were not available for turbulent intensity as well as the total pressure for the Chashma barrage. Therefore, the comparisons of turbulent intensity and total pressure, etc. between the physical and numerical modelings were not conducted.

Supplementary Information

eer-2021-369-suppl.pdf

Acknowledgments

We are much thankful to the Irrigation Research Institute (IRI) department, Nandipur Gujranwala for their continuous support in data acquisition and for giving us a proper understanding regarding physical modeling. We are also thankful to National Engineering Services Pakistan (NESPAK), Lahore for the provision of the Chashma barrage layout plan.

Notes

Conflict-of-Interest

The authors report no conflict of interests. No funding was available for this study.

Author Contributions

M.U. (MS student) conducted all simulations and results. S.S. (Associate Professor) edited results and wrote the manuscript. S.A. (Professor) designed and supervised the study. M.K.U. (Professor) conducted the literature review.

References

1. Lane S, Bradbrook K, Richards K, Biron P, Roy A. The application of computational fluid dynamics to natural river channels: three-dimensional versus two-dimensional approaches. Geomorphol. 1999;29(1–2)1–20.

2. Phanindra K. Study of Hydraulic Characteristics in an Open Channel Flow with vegetation [dissertation]. Rourkela: Department of civil engineering national institute of technology; 2015.

3. Kim SJ. 3D numerical simulation of turbulent open-channel flow through vegetation [dissertation]. Atlanta: Georgia Institute of Technology; 2011.

4. Kamel B, Ilhem K, Ali F, Abdelbaki D. 3D simulation of velocity profile of turbulent flow in open channel with complex geometry. Phys Procedia. 2014;55:119–28.

5. Wang W, Huai W-x, Gao M. Numerical investigation of flow through vegetated multi-stage compound channel. J Hydrodynamics. 2014;26(3)467–73.

6. Zeng C, Li C-W. Measurements and modeling of open-channel flows with finite semi-rigid vegetation patches. Environ Fluid Mech. 2014;14(1)113–34.

7. Anjum N, Ghani U, Ahmed Pasha G, Latif A, Sultan T, Ali S. To investigate the flow structure of discontinuous vegetation patches of two vertically different layers in an open channel. Water. 2018;10(1)75.

8. Koutrouveli TI, Fourniotis NT, Demetracopoulos A, Dimas A. Numerical Simulation of Turbulent Flow in Open Channel with Groynes. Department of Civil Engineering, University of Patras; Patras, Greece: 2014. c2020. [cited: 30 November 2020]10.1201/b17133-91Available from: https://www.researchgate.net/profile/A-Demetracopoulos/publication/288816435_Numerical_simulation_of_turbulent_flow_in_open_channel_with_groynes/links/568b8ef808ae1e63f1fd6d2a/Numerical-simulation-of-turbulent-flow-in-open-channel-with-groynes.pdf

9. Ghisalberti M, Nepf H. The limited growth of vegetated shear layers. Water Resour Res. 2004;40(7)1–12.

10. Yokojima S, Kawahara Y, Yamamoto T. Impacts of vegetation configuration on flow structure and resistance in a rectangular open channel. J Hydro-environ Res. 2015;9(2)295–303.

11. Järvelä J. Effect of submerged flexible vegetation on flow structure and resistance. J Hydrol. 2005;307(1–4)233–41.

12. Shoiti N, Yoshizawa A. Turbulent channel and Couette flows using an anisotropic k-epsilon model. AIAA J. 1987;25(3)414–420.

13. Singh P, Kumar A, Khatua KK. Concept of Turbulence Modelling and Its Application in Open Channel Flow. 2016. c2020 [cited: 30 December 2020]. Available from: http://dspace.nitrkl.ac.in/dspace/bitstream/2080/2599/1/2016_Hydro_PSingh_Concept.pdf

14. Gandhi B, Verma H, Abraham B. Investigation of flow profile in open channels using CFD. In : 8th Intl Conference on Hydraulic Efficiency Measurement. IGHM; 21–23 Oct. 2010; IIT Roorkee, India. 243–251. c2021 [cited 20 January 2021]. Available from https://citeseerx.ist.psu.edu/viewdoc/download?doi=10.1.1.1083.2412&rep=rep1&type=pdf

15. Knight DW. River hydraulics–a view from midstream. J Hydraul Res. 2013;51(1)2–18. https://doi.org/10.1080/00221686.2012.749431

16. Cunge JA. River hydraulics–a view from midstream. J Hydraul Res. 2014;52(1)137–138. https://doi.org/10.1080/00221686.2013.855269

17. Morvan HP. Channel shape and turbulence issues in flood flow hydraulics. J Hydraul Eng. 2005;131(10)862–865.

18. Alhashimi SAM. Numerical Modelling of Turbulent Flow in Open Channel Expansion. J Eng Sust Develop. 2018;22(3)152–161.

19. Patel T, Gill L. Volume of fluid model applied to curved open channel flows. WIT Trans Eng Sci. 2006;52:1–9.

20. Zhao F, Huai W. Hydrodynamics of discontinuous rigid submerged vegetation patches in open-channel flow. J Hydro-environ Res. 2016;12:148–160.

21. Jalonen J, Järvelä J, Virtanen J-P, Vaaja M, Kurkela M, Hyyppä H. Determining characteristic vegetation areas by terrestrial laser scanning for floodplain flow modeling. Water. 2015;7(2)420–37.

22. Zhu C, Hao W, Chang X. Vertical velocity distribution in open-channel flow with rigid vegetation. Sci World J. 2014;2014(3)146829.

23. Stone BM, Shen HT. Hydraulic resistance of flow in channels with cylindrical roughness. J Hydraul Eng. 2002;128(5)500–506.

24. Steffler PM, Jin Y-C. Depth averaged and moment equations for moderately shallow free surface flow. J Hydraul Res. 1993;31(1)5–17.

25. Duan JG. Simulation of flow and mass dispersion in meandering channels. J Hydraul Eng. 2004;130(10)964–76.

26. Nagaosa R. Direct numerical simulation of vortex structures and turbulent scalar transfer across a free surface in a fully developed turbulence. Phys Fluids. 1999;11(6)1581–1595.

27. Borue V, Orszag SA, Staroselsky I. Interaction of surface waves with turbulence: direct numerical simulations of turbulent open-channel flow. J Fluid Mech. 1995;286:1–23.

28. Lien H, Hsieh T, Yang J, Yeh K-C. Bend-flow simulation using 2D depth-averaged model. J Hydraul Eng. 1999;125(10)1097–1108.

29. De Vriend HJ, Koch FG. Flow of water in a curved open channel with a fixed plan bed. Rep on Experimental and Theoretical Investigations, Delft Uni Technol R675-VM1415, Part I. 1977;10.13140/RG.2.1.4134.7044

30. Rozovskii IL. Flow of water in bends of open channels Kiev, Academy of Sciences of the Ukrainian SSR, Israel Program for Scientific Translations. Washington, D.C.: available from the Office of Technical Services, U.S. Dept. of Commerce; 1961. p. 233.

31. Onitsuka K, Nezu I. Numerical prediction of rectangular open-channel flow by using large eddy simulation. In : Proceedings of the Congress-International Association for Hydraulic Research. International Association for Hydro-Environment Engineering and Research; 16–21 September 2001; Beijing. p. 196–203.

32. Meftah MB, De Serio F, Malcangio D, Mossa M. Resistance and boundary shear in a partly obstructed channel flow. River Flow 2016 – Constantinescu. Garcia , Hanes , editorsLondon: Taylor & Francis Group; 2016. p. 795–801.

33. Morvan H, Knight D, Wright N, Tang X, Crossley A. The concept of roughness in fluvial hydraulics and its formulation in 1D, 2D and 3D numerical simulation models. J Hydraul Res. 2008;46(2)191–208.

34. Meftah MB, Mossa M. Partially obstructed channel: Contraction ratio effect on the flow hydrodynamic structure and prediction of the transversal mean velocity profile. J Hydrol. 2016;542:87–100.

35. Kim HS, Nabi M, Kimura I, Shimizu Y. Computational modeling of flow and morphodynamics through rigid-emergent vegetation. Ad Water Resour. 2015;84:64–86.

36. Gholami A, Bonakdari H, Zaji AH, Akhtari AA. Simulation of open channel bend characteristics using computational fluid dynamics and artificial neural networks. Eng Appl Comput Fluid Mech. 2015;9(1)355–369.

37. Luo H, Fytanidis DK, Schmidt AR, García MH. Comparative 1D and 3D numerical investigation of open-channel junction flows and energy losses. Adv Water Resour. 2018;117:120–139.

38. Mehmetaj I, Ndini M. Computational Fluid Dynamics Modeling of Submerged Vegetation in OpenChannels. In : 4th International Balkans Conference on Challenges of Civil Engineering, BCCCE; 18–19 Dec., 2020; EPOKA University, Tirana, Albania. 64–70. c2021. [cited: 16 December 2021] Available from http://dspace.epoka.edu.al/bitstream/handle/1/1931/BCCCE%202020%20Book%20of%20Proceedings-64-73.pdf?sequence=1

Table 1

Conversion Factors or Scale Ratios of Different Parameters for Physical Modelling

Features	Symbols	Conversion Factors	Scale
Length	L_r	L_r	1/300
Flow Depth	Y_r	Y_r	0.02
Flow Area	A_r	L_r Y_r	1/15000
Time	T_r	L_r /Y_r^1/2	1/42.43
Flow Velocity	V_r	Y_r^½	1/7.07
Discharge	Q_r	L_r Y_r^3/2	1/106066.02
Roughness Coefficient	n_r	Y_r ^2/3 / L_r ^1/2	1/0.78

Table 2

Different Values of Discharges for Model Operation

Discharge Type	Discharge Values
Low Discharges	50,000 Cs; 100,000 Cs; 200,000 Cs
Medium Discharges	300,000 Cs; 400,000 Cs; 500,000 Cs; 588,123 Cs
High Discharges	700,000 Cs; 800,000 Cs; 900,000 Cs; 957,289 Cs; 1,038,873 Cs

Table 3

Measurements of Water Levels (m) at Various Gauges

Discharge Q (Cs)	Discharge in Cubic M/S	Chashma Barrage *d/s			J-H Spur at Kahloon				Alluwali Guide Wall

		G-4	G-4A	G-5	G-5A	G-6	G-6A	G-7	G-7A	G-8
50,000	1,415.84	185.06	185.21	184.30	-	183.54	-	183.11	183.14	182.93
100,000	2,831.68	185.37	185.37	184.91	-	184.60	-	184.09	184.12	183.84
200,000	5,663.37	187.20	187.35	186.59	-	185.98	-	185.21	185.24	185.06
300,000	8,495.05	187.50	187.80	187.26	-	186.74	-	186.10	186.13	185.98
400,000	11,326.74	188.02	188.11	187.80	-	187.35	187.20	186.89	186.92	186.80
500,000	14,158.42	189.18	189.24	188.87	188.87	187.96	187.96	187.44	187.47	187.32
585,123	16,568.84	189.33	189.48	189.05	188.72	188.41	188.26	187.80	187.87	187.74
700,000	19,821.79	189.63	189.70	189.33	189.33	188.87	188.87	188.26	188.29	188.11
800,000	22,653.47	190.18	190.24	189.79	189.63	189.02	188.87	188.57	188.60	188.26
900,000	25,485.16	190.55	190.61	190.09	190.15	189.33	189.39	188.81	188.87	188.57
957,289	27,107.40	190.55	190.67	190.40	189.94	189.79	189.54	188.99	189.02	188.69
1,038,873	29,417.61	190.85	190.91	190.70	190.24	189.94	189.94	189.18	189.07	188.87

Key: Cs= Cusecs; M/S = Meter/Second; d/s = Downstream

Table 4

Velocities along Left & right River Banks

Discharge Q (Cs)	Velocity (m/sec)

	Velocities Along Right River Bank						Velocities Along Left River Bank

	V-1	V-2	V-3	V-4	V-5	V-6	V-7	V-8	V-9	V-10	V-11	V-12
500,000	2.32	2.29	2.23	1.83	2.30	2.22	0.71	0.83	1.34	1.68	1.88	1.95
585,123	2.38	2.32	2.35	1.89	2.35	2.26	0.71	0.94	1.68	1.77	1.88	2.07
700,000	2.41	2.42	2.44	2.04	2.41	2.30	1.17	1.17	1.89	1.95	1.98	2.13
800,000	2.44	2.43	2.65	2.16	2.42	2.36	1.65	1.52	2.23	2.12	2.23	2.29
900,000	2.53	2.44	2.74	2.50	2.52	2.53	1.65	1.34	1.77	2.26	2.30	2.35
957,289	2.59	2.56	2.90	2.65	2.68	2.71	1.70	1.47	1.88	2.47	2.50	2.53
10,388,873	2.76	2.80	3.41	2.68	3.01	2.88	1.83	1.52	2.12	2.65	2.68	2.68

Table 5

2D Simulation Considering Different Discharges and Velocities at the Inlet Point

For different discharges, the velocities for simulation at inlet point w.r.t G4 are: (used in 2D simulation)

Sr. #	Q (cusecs)	Water level (m)	Avg. bed level (m)	Water Depth (m)	Width of Barrage (m)	Area (m²)	Velocity (m/s)
1	50,000	185.06	183.15	1.9	1,084.14	2065.52	0.683
2	500,000	189.17	183.15	6.02	1,084.14	6527.04	2.167
3	800,000	190.18	183.15	7.03	1,084.14	7617.64	2.975
4	957,289	190.54	183.15	7.39	1,084.14	8014.22	3.283

Table 6

Velocity Comparisons between Physical Modelling and Numerical simulation along Left and Right Banks at Q = 500,000 cusecs and at Q = 800,000 cusecs

Velocity comparison at various points along the river banks on d/s of Chashma Barrage

	Sr. No.	Velocity		Physical Simulation	Using turbulent models in Ansys Fluent

				Experimentally	Using k-ɛ model	Using RS model
For Q = 500,000 cusecs	1	Along right bank (m/s)	V1	2.32	2.78	2.86
	2		V2	2.29	1.94	1.55
	3		V3	2.23	2.75	2.63
	4		V4	1.83	2.13	2.25
	5		V5	2.3	2.68	2.94
	6		V6	2.22	2.64	2.81

	1	Along left bank (m/s)	V7	0.71	0.85	0.90
	2		V8	0.83	0.95	1.15
	3		V9	1.34	1.68	1.80
	4		V10	1.65	1.97	2.18
	5		V11	1.88	2.39	2.18
	6		V12	1.95	1.55	1.38

For Q = 800,000 cusecs	1	Along right bank (m/s)	V1	2.43	2.83	3.10
	2		V2	2.42	1.58	1.93
	3		V3	2.65	3.27	3.52
	4		V4	2.16	2.63	2.95
	5		V5	2.42	3.2	2.87
	6		V6	2.36	2.94	3.11

	1	Along left bank (m/s)	V7	1.65	2.05	2.28
	2		V8	1.52	1.9	2.10
	3		V9	2.26	3.15	2.83
	4		V10	2.12	2.56	2.97
	5		V11	2.23	3.1	2.76
	6		V12	2.29	2.81	3.07

d/s = Downstream

Table 7

Water Depths Comparison between the Physical Modelling and Numerical Simulation at Various Gauges

Water depth comparison within the river geometry on d/s of Chashma Barrage

Considering Average bed level of the river = 600.75 ft or 183.15 m

	Sr. No.	Water depth at various gauges (m)	Physical Simulation	Using turbulent models in Ansys Fluent

			Experimentally	Using k-ɛ model	Using RS model
For Q = 500,000 cusecs	1	G-4	6.02	5.27	5.6
	2	G-5	5.71	4.68	4.91
	3	G-6	4.8	4.68	3.55
	4	G-6A	4.8	2.55	2.51
	5	G-7	4.28	3.55	3.22
	6	G-7A	4.31	3.55	3.51
	7	G-8	4.16	3.55	3.51

For Q = 800,000 cusecs	1	G-4	7.03	8.38	9.25
	2	G-5	6.63	8.3	7.87
	3	G-6	5.87	7.15	5.94
	4	G-6A	5.72	4.51	3.4
	5	G-7	5.41	4.51	2.86
	6	G-7A	5.44	4.51	3.4
	7	G-8	5.11	4.51	3.86

d/s = Downstream

Table 8

Comparison of Velocity Percentage Errors

	Sr. No.	Velocity along right bank (m/s)	b/w experimental results and k-ɛ model (%)	b/w experimental results and RS model (%)	Velocity along left bank (m/s)	b/w experimental results and k-ɛ model (%)	b/w experimental results and RS model (%)
For Q = 500,000 cusecs	1	V1	19.83	23.28	V7	19.72	26.76
	2	V2	15.28	32.31	V8	14.46	38.55
	3	V3	23.32	17.94	V9	25.37	34.33
	4	V4	16.39	22.95	V10	19.39	32.12
	5	V5	16.52	27.83	V11	27.13	15.96
	6	V6	18.92	26.69	V12	20.51	29.23
	Average		18.37	25.16	-	21.09	29.49
For Q = 800,000 cusecs	1	V1	16.46	27.57	V7	24.24	38.18
	2	V2	34.71	20.25	V8	25.00	38.16
	3	V3	23.40	32.83	V9	39.38	25.22
	4	V4	21.76	36.57	V10	20.75	40.09
	5	V5	32.23	18.60	V11	39.01	23.77
	6	V6	24.58	31.78	V12	22.71	34.20
	Average		25.52	27.93	-	28.51	33.27