Development of a Three-Dimensional CFD Model and OpenCV Code by Comparing with Experimental Data for Spillway Model Studies

Abstract

This article presents a three-dimensional CFD model and OpenCV code by comparing the flow over the spillway with the experimental data for use in spillway studies. A 1/200-scale experimental model of a real dam spillway was created according to Froude similarity. In the experimental studies, velocity and water depth were measured in four different sections determined in the spillway model. A three-dimensional ANSYS Fluent model of the spillway was created and the simulations of the flows occurring during the flood were obtained. In the numerical model, the two-phase VOF model and k-epsilon turbulence model are used. As a result of the numerical analysis, velocity, depth, pressure, and cavitation index values were examined. The velocity and depth values obtained with models were compared and a good agreement was found between the results. In addition, in this study, a different technique based on image processing is developed to calculate water velocity and depth. A floating object was placed in the spillway channel during the experiment and the movement of the object on the water was recorded with cameras placed at different angles. By using the object tracking method, which is an image processing technique, the position of the floating object was determined in each video frame in the video recordings. Based on this position, the velocity of the floating object and its perpendicular distance to the bottom of the channel was determined. Thus, an OpenCV-Python code has been developed that determines the velocity and water depth of the floating object depending on its position. The floating object velocity values obtained by the algorithm were compared with the velocity values measured during the experimental model, and new velocity correction coefficients were obtained for the chute spillways.

1. Introduction

The spillway structures are the most important structures for ensuring the safety of the dam. Their task is to pass the flood discharge downstream of the dams efficiently and safely. These safety structures are designed to operate at a very low risk. Theoretical equations and physical modeling are the two main techniques commonly used to analyze the performance of dam spillways. For a long time, physical scale modeling has been used to design and study hydraulic water structures. Experimental studies for flow over a spillway structure require sensitive measurements and must be appropriately designed to provide reliable information [1]. However, such studies are time-consuming and may adversely affect the cost of the project. Therefore, researchers have sought different methods.

Due to developments in computer technology, numerical simulations for hydrodynamic processes, including flow over spillways, have become widespread. Computational fluid dynamics (CFD) is a branch of computational modeling developed to solve problems involving fluid motion. The methods developed within the scope of CFD aim to analyze the movements of fluids under different conditions. However, the realism and applicability of the data obtained from CFD models is a topic of debate in current discussion and research. In this respect, there is a need to increase and diversify studies for the verification of numerical findings with experiments.

In the literature, numerous studies make experimental and CFD comparisons for spillway modeling. Olsen and Kjellesvig [2] numerically modeled the water flow over a two- and three-dimensional spillway by choosing different geometries to estimate the spillway capacity. The k-ε turbulence model was chosen, and the equations of motion were solved accordingly. Numerical results and experimental studies were compared, and close values were obtained. Dargahi [3] investigated the flow field on a spillway to simulate the flow through a three-dimensional numerical model. The fluid volume (VOF) model was used to calculate the free surface flow over the spillway. The k-epsilon turbulence model was used in the study. The water surface profiles and discharge coefficients were estimated in the range of 1.5–2.9%, depending on the operating height of the spillway. Based on these studies in the literature, the VOF model and the k-epsilon turbulence model were used in the CFD part of this study. Kumcu [4] hydraulic characteristics of Kavsak Dam and Hydroelectric Power Plant (HEPP), which are under construction and built for producing energy in Turkey, were investigated experimentally by physical model studies. In order to evaluate the capability of computational fluid dynamics for modeling spillway flow, a comparative study was carried out by using results obtained from physical modeling and computational fluid dynamics (CFD) simulation. It was shown that there is reasonably good agreement between the physical and numerical models, in terms of flow characteristics. Demeke [5] studied the structure of the Tendaho Dam spillway in Ethiopia. In the spillway structure, under the designed capacity, overflows were observed during a flood and, therefore, a 3D CFD study was carried out. As a result of the studies, it was concluded that the spillway structure was not safe. Green [6] examined three main techniques commonly used to analyze the performance of existing dam spillways. These are theoretical equations, physical modeling, and computational fluid dynamics (CFD). The specified modeling methods were applied for a spillway and comparisons were made. The advantages and disadvantages of each method were discussed. Gadhe [7], in a study, compared the results obtained by the spillway model of the New Umtru Dam with the CFD model. It was observed from the studies that the original design of the spillway and energy dissipater required revision. Several spillway studies have examined the cavitation problem. Cavitation often creates harmful effects on dam spillways. For this reason, researchers have used various velocity measurement techniques, such as Particle Image Velocimeter (PIV) and Acoustic Doppler Velocimeter (ADV) [8,9,10]. ADV was used in this study. Aydın [11] analyzed the spillway aerator of a 100 m high roller-compacted concrete dam using a two-phase computational fluid dynamics model to overcome cavitation damage at the spillway surface. Numerical analysis was performed with prototype dimensions for various flow conditions (5223, 3500, 1750, and 1000 m³/s flow rate) and the obtained results were compared with experimental observations in the literature. Numerical and experimental results have shown that cavitation occurs after a particular downstream point on the surface, based on cavitation indices.

Researchers working on open-channel flow attempt to explain the velocity, one of the most important parameters in open-channel flows. Velocity can be measured with a measuring device and direct methods, or it can be determined by indirect methods such as the float method, or with mathematical models and empirical equations [12,13,14]. The velocity measurement is a task requiring great effort and expense [15].

In open-channel flows, the velocity varies with depth. It is very important to calculate the mean and maximum velocity values in the velocity distribution depending on the depth. Determining the velocity of the free water surface is much easier than determining the mean and maximum velocities in open channels [16]. Free water surface velocity can be easily determined with an object that is movable on the water’s surface and not too heavy, such as leaves, twigs, etc. Other methods, such as acoustics, optics, or floats, are used to estimate surface velocity. However, the cheapest and easiest way to determine water surface velocity is to simply float something down the stream and see how fast it travels [17]. Once the velocity of the floating object is determined, it should be multiplied by the correction coefficients for the mean flow velocity. The correction coefficients vary according to the depth [18]. Researchers have carried out studies in the past to determine these coefficient values [19,20].

Image processing consists of processing images using digital computers. In recent years, its use has increased exponentially in many areas. One of these is in hydraulic science, where observable flow parameters can be studied with this method. Research has been carried out in the past using image processing techniques to determine velocity and water level in open-channel flows. Since the water level can be observed using these two parameters, it can be measured more easily than the velocity [21,22,23]. Because the water velocity changes depending on the depth and cannot be observed, it is more difficult to measure with this method [24,25,26]. The velocity of a floating object on the water, seen in video images, can be determined by image processing methods. The movement of the floating object on the water can be measured by the object detection and tracking method, one of the image processing methods. This is a method of detecting and locating an object which is in motion with the help of a camera. The detection and tracking method is used in different engineering fields such as vehicle tracking in traffic, object detection, and security [27,28]. There are many programming languages and program libraries in which image processing methods can be applied. Recently, Python programming language and OpenCV (Open Source Computer Vision) library are preferred because they are easier to use than others.

The aim of this research is to develop a three-dimensional CFD model and OpenCV code by comparing the flow over the spillway with the experimental data for use in spillway studies. With the CFD model developed and OpenCV code, the flow parameters, flow characteristics, and changes required for the design of the spillway can be obtained in less time and at a lower cost. The CFD model established and OpenCv code can examine the flow parameters of the existing and future spillway structures. The spillway structure chosen for this purpose is the spillway structure of the Çatalan Dam and Hydroelectric Power Plant in Adana, currently in operation. The spillway discharge channel has 2 slopes, of 3% and 17%. The spillway model was created by reducing the dimensions of the prototype spillway structure to Froude similarity at a 1/200 scale. The flood flow rate and inlet velocities that would occur in the prototype spillway structure were also calculated according to Froude similarity in detail and used in the experimental and numerical model setup. Average flow velocities were measured with an acoustic Doppler velocimeter (ADV) device for four different cross-sections (at five points in each cross-section) along the spillway discharge channel. In addition, water depth was measured in four cross-sections (at nine points in each cross-section). After the experimental studies, a three-dimensional CFD model of the spillway model was created. In CFD studies, the ANSYS Fluent program, which can use the VOF method and k-epsilon turbulence model together, was used. The average flow velocities and water depts obtained along the cross-sections by the experiment are compared with the results of the CFD model and shown in tables, graphs, and figures. In addition, the pressure distributions in four different cross-sections were examined with the CFD model. These pressure values were increased to the model scale according to Froude similarity, and the cavitation index was calculated for four sections of the prototype spillway. In the second part of the experimental studies, a colored floating object was placed in the spillway channel and the movement of the object on the water was recorded with cameras placed at different angles. By using the object tracking method, which is an image processing technique, the position of the floating object was determined in each video frame in the video recordings. Based on this position, the velocity of the floating object and its perpendicular distance from the bottom of the channel was determined. Thus, an OpenCV-Python code has been developed that determines the velocity and water depth of the floating object depending on its position. The floating object velocity values obtained by the algorithm were compared with the velocity values measured during the experiment, and new velocity correction coefficients were obtained for the chute spillways.

2. Case Study

In this study, a physical model of a spillway structure was created. The spillway structure chosen for this purpose is the spillway structure of the Çatalan Dam and Hydroelectric Power Plant in Adana, currently in operation. Construction on Çatalan Dam began in 1982. The dam is used for electricity generation by the State Hydraulic Works (DSI) and was put into operation in 1997. Çatalan Dam is on the Seyhan River in the Sarıçam district of Adana, one of the important cities of Turkey. The height of the dam body from the foundation is 82 m (70 m from the stream floor), and its crest length is 894 m. The fill volume of the earth- and rockfill-type dam is 17 million m³, the lake area is 81.86 km², and the reservoir volume is 2126 billion m³. The minimum operating level elevation of the Dam is 115 m, and the maximum operating level elevation is 125 m [29].

The spillway structure belonging to the dam is a spillway with a radial gate. The spillway, designed with a capacity of 10,055 m³ s⁻¹, has 6 chambers, each of which is 11 m wide, 15.60 m high, and equipped with a radial gate. The discharge channel, which extends downstream of the Ogee crested sill, is 81 m wide, 567 m long, and ends with an energy-dissipating pool. The discharge channel slopes are 0.03 and 0.17 and are connected to a vertical curve (Figure 1) [29].

Theoretical Equations of Spillway

In the theoretical study of the spillway project, the spillway discharge capacity was calculated considering that all radial gates would be fully open. Discharge rating curve (Q/H curve) varies with the water level over the crest. The theoretical flow discharge through a spillway can be expressed by [30]:

$$Q=C_0{L}_0{H_0}^{\frac{3}{2}}$$

(1)

$$L_0=L_n-2\left[N{K}_p+K_a\right]H_0$$

(2)

where Q denotes the flow discharge, C₀ denotes discharge coefficient, L₀ denotes effective length of spillway crest or width, and H₀ denotes upstream head measured from the crest to the unaffected upstream water stage. Equation (2) is used to determine the effective length L₀. L_n is the net length of the crest, N is the number of piers, K_p and K_a are constants depending on the shape of piers and abutments. In this study, K_p of 0.01 K_a 0.1 was used. The discharge coefficient, C₀, uses different values. It is influenced by a variety of factors including the depth of approach, relation of the actual crest shape to the ideal nappe shape, upstream face slope, downstream apron interference, and downstream submergence. The C₀ coefficient was calculated as 1.97 for the discharge of Q₁₀₀₀ = 10,055 m³ s⁻¹.

The flow over the spillway is open-channel flow. In an open-channel section, the flow rate varies from one point to another. This is due to the shear stress at the bottom and sides of the channel and the presence of the free surface. Flow velocity can have components in all three Cartesian coordinate directions. However, the components of the velocity in the vertical and transverse directions are usually small and can be neglected. Therefore, only the flow velocity downstream needs to be considered. This velocity component varies from surface to depth [31].

In the past, various semi-empirical models have been used to represent the velocity profiles of turbulent open-channel flow. The velocity distribution in the viscous sublayer is generally understood to be linear. In the fully turbulent layer of the inner region, the logarithmic velocity distribution of von Karman and Prandtl, known as the law of the wall, is the universally accepted formula:

$$\frac{U}{U_{*}}=A\mathit{ln}\frac{U_{*}y}{\nu }+B$$

(3)

where $A=1/\chi$, $\chi$ = von Karman constant; $B$ = a constant, $U_{*}$ = $\left(\sqrt{\left({\tau }_0/\rho \right)}\right)=$ shear velocity, ${\tau }_0$ = shear strees, $\rho$ = density, $\nu$ = kinematic viscosity, and $y$ = distance from the wall. The value of $B$ depends on the roughness of the wall surface. Many experimental studies have been performed to determine the $A$ and $B$ values. As a result of the experiments, it was determined that $A$ = 2.5 and $B$ = 5.5 can be used for both smooth pipe flows and smooth open-channel flows [32].

The universal formula used to determine the average velocity and discharge of the current passing through the channel in open channels is the Manning formula:

$$U_{ave}=\frac{1}{n}{R}^{\raisebox{1ex}{$2$}\!\left/ \!\raisebox{-1ex}{$3$}\right.}{S_0}^{\raisebox{1ex}{$1$}\!\left/ \!\raisebox{-1ex}{$2$}\right.}$$

(4)

where n = Manning’s constant; R = hydraulic radius, and S₀ = slope of channel. The hydraulic radius is defined by dividing the cross-sectional area of the channel by the wet circumference.

The float method is one of the methods used to estimate average velocity. The method is performed as follows: the time elapsed between the start and endpoints of the floating object is measured with a stopwatch, and the velocity of the object is calculated by dividing the distance by this time. This distance is usually 3–10 m, and the experiment is repeated 3 or more times. Then, the resulting surface velocity value is multiplied by a coefficient and the average velocity is obtained. The coefficient values varying with depth are shown in

Table 1. Coefficients to correct surface float velocities to average channel velocities [18].

Average Depth (m)	Coefficient
0.30	0.66
0.61	0.68
0.91	0.70
1.22	0.72
1.52	0.74
1.83	0.76
2.74	0.77
3.66	0.78
4.57	0.79
>6.10	0.80

. The values provided in Table 1 are obtained for open channels with low slope and low flow velocities. To calculate the channel discharge, the channel cross-section is multiplied by the average velocity [18].

3. Experimental Studies

The spillway model was created by reducing the dimensions of the prototype spillway structure with Froude similarity at a 1/200 scale. The flood discharge (supercritical flow) and inlet velocities that would occur in the prototype spillway structure were also calculated according to Froude similarity and are shown in

Table 2. Froude similarity values for prototype and model.

Parameters		Dimension	Froude Scale Ratio	Prototype Value	Similarity Account	Model Value
Spillway	Width	L	λ = (1/200)	82.5 m	Lp∗λ	41.25 cm
	Height			34 m		17 cm
	Length			402 m		201 cm
Discharge (Q)		L3T−1	λ5/2	10,055 m3 s−1	Qp∗λ5/2	17.7 lt s−1
Velocity (V)	Inlet 1	LT−1	λ1/2	6.5 m s−1	Vp∗λ1/2	0.46 m s−1
	Inlet 2			6 m s−1		0.42 m s−1
	Inlet 3			5.52 m s−1		0.39 m s−1
	Inlet 4			5.42 m s−1		0.38 m s−1
	Inlet 5			5.4 m s−1		0.36 m s−1
	Inlet 6			5.9 m s−1		0.42 m s−1

.

The model scale was determined to fit the hydraulic channel in which the experiments were carried out. A 1/200 scale model was created in accordance with the 3D geometry of the prototype spillway structure (Figure 2). The approach channel, weir, and discharge channel of the spillway model were formed. The energy breaker pool at the end of the spillway structure is not included in the model.

The spillway model was produced in parts, in accordance with the spillway geometry drawn with the AutoCAD 2014 program. The materials used in model making are very light and practical. The parts, made of 5 cm thick Extruded Polystyrene (XPS) styrofoam material, were joined with silicone adhesive. The model, approximately 2 m in length, was formed in 2 parts to be joined later, in the middle, to prevent damage. In order to provide visibility in image processing studies, the edges of the model were covered with glass material. Figure 3 shows the final version of the spillway model.

In this study, a 1/200 scale model of the Çatalan Dam spillway structure was created and experimental studies were carried out in the hydraulic water channel. Experimental studies were carried out on the open-channel setup in Bartın University, central research, hydromechanics laboratory (Figure 4).

The discharge was adjusted with the help of the valve placed at the pump outlet that provides water circulation to the channels, and the flow entering the system was measured with the help of the ultrasonic flow meter (GE Pnametrics, AT 868 AquaTrans Flowmeter model, Clare, Ireland) placed at the pump inlet. Velocity measurements were made at a total of twenty points in four different cross-sections (five points in each cross-section) in the spillway channel with the ADV device (FlowTracker Handheld model, Hemmant, Australia) (Figure 5). Due to the low water depths at the measurement points and the turbulence at the tip of the device, the measurements took a long time and erroneous measurements were repeated.

4. CFD Model Studies

The flow over the spillway is an open-channel flow. In an open-channel flow, the flowing fluid has a free surface at atmospheric pressure and the driving force is gravity. When the literature is examined, it is seen that such free surface flow is simulated by the fluid volume (VOF) method as water–air two-phase flow problems. Flows over the spillway are high velocity and turbulent. According to the literature, the standard k-ε turbulence model can be used in the three-dimensional numerical simulation of the flow.

4.1. Basic Equations

The investigated open-channel flow is a 3D, turbulent, steady free surface flow.

Continuity equation:

$$\frac{\partial \rho }{\partial t}+\frac{\partial \rho u_i}{\partial x_i}=0$$

(5)

Momentum equation:

$$\frac{\partial \rho u_i}{\partial t}+\frac{\partial }{\partial x_j}\left(\rho u_i{u}_j\right)=-\frac{\partial P}{\partial x_i}+\frac{\partial }{\partial x_j}\left[\left(\mu +{\mu }_t\right)\left(\frac{\partial u_i}{\partial x_j}+\frac{\partial u_j}{\partial x_i}\right)\right]$$

(6)

Turbulence kinetic energy (k) equation:

$$\frac{\partial \rho k}{\partial t}+\frac{\partial \rho u_{i}k}{\partial x_i}=\frac{\partial }{\partial x_i}\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_k}\right)\frac{\partial k}{\partial x_i}\right]+G-\rho \epsilon$$

(7)

Turbulence dissipation rate energy (ε) equation:

$$\frac{\partial \left(\rho \epsilon \right)}{\partial t}+\frac{\partial \left(\rho u_i\epsilon \right)}{\partial x_i}=\frac{\partial }{\partial x_i}\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_{\epsilon }}\right)\frac{\partial \epsilon }{\partial x_i}\right]+C_{1\epsilon }\frac{\epsilon }{k}G-C_{2\epsilon }\rho \frac{{\epsilon }^2}{k}$$

(8)

where t is the time; u_i is the velocity components; x_i is the coordinate components; ρ is the density; µ is the molecular viscosity coefficient; P is the correct pressure; µ_t is the turbulent viscosity coefficient, which can be derived from the turbulent kinetic energy k and turbulent dissipation rates:

$${\mu }_t={\rho C}_{\mu }\frac{k^2}{\epsilon }$$

(9)

$$G={\mu }_t\left(\frac{\partial {\mu }_i}{\partial x_j}+\frac{\partial u_j}{\partial x_i}\right)\frac{\partial u_i}{\partial x_j}$$

(10)

where σ_k and σ_ε are turbulence Prandtl numbers for the k and ε equation, respectively, σ_k = 1.0, σ_ε = 1.3, C_1ε and C_2ε are ε equation constants, C_1ε = 1.44, and C_2ε = 1.92. C_μ = 0.09 is a constant determined experimentally, as described in [33].

4.2. Volume of Fluid (VOF) Model

In this study, the VOF method was used to calculate the water–air interface. This method was used for two-phase air–water flow simulation to compute the free surface of the flow. The VOF method essentially determines whether the element volumes in the computational mesh are empty, partially filled, or completely filled with water. Representing the volumetric filling ratio of the mesh elements, the mesh element is fully filled for F = 1, empty (filled with air) for F = 0, and partially filled with water for 0 < F < 1 [34]. In this approach, the tracking interface between air and water is accomplished by the solution of a continuity equation for the volume fraction of water:

$$\frac{\partial {\alpha }_w}{\partial t}+\frac{\partial {\alpha }_w{u}_i}{\partial x_i}=0$$

(11)

where α_w is the volume fraction of water. In each cell, the sum of the volume fractions of air and water is unity. Volume fractions of air, denote by α_a, can be provided as shown in [33]:

$${\alpha }_w+{\alpha }_a=1;0\le {\alpha }_w\le 1$$

(12)

4.3. Boundary Conditions for Spillway

A 1/200 scale geometry of the spillway model was made with the GAMBIT 2.2.30 drawing program. Approximately 800,000 mesh triangles were created within this geometry (Figure 6). The mesh qualities were controlled with equiangular skewness, equalized skewness, and aspect ratio in the GAMBIT program. The skewness error increased in the model due to the shape of the spillway. These errors were defined and corrected by increasing the amount of mesh with GAMBIT. However, when the mesh becomes smaller, the amount of mesh is increased. This requires additional computing capacity and time. The mesh independence test of the numerical model, the number of mesh triangles, and the spillway outlet velocity were compared; the results are shown in the Figure 7. When the figure is examined, the change in velocity values decreases after a certain amount of mesh. This showed that the flow velocity results were independent of the amount of mesh.

The three-dimensional geometry was created, and the boundary conditions of the flow formed in the spillway were defined. Accordingly, the boundary conditions of the three-dimensional numerical model were defined as follows: the approach channel was defined as six different surface velocity inputs at the entrance. The spillway outlet and its upper surfaces were defined as the pressure outlet. All other surfaces of the model were defined as the wall condition (Figure 6). In case of a flood flow of 10,055 m³ s⁻¹, the covers were fully opened and the floodwater height was calculated as 25 m in the approach channel. In CFD analysis, this value was adjusted according to the model scale, and the water inlet height was defined as 12.5 cm. In addition, in accordance with the prototype spillway project, the approach channel length was 15 m, and the length between the approach channel and the spillway outlet was 402 m. At the beginning of the approach channel, numerical analysis was initiated with the velocity values provided in Table 2.

Velocities on spillway wall faces were obtained using the standard wall function based on the recommendation of Launder and Spalding [35]. This wall function accepts a log law velocity profile close to the wall, and is determined as follows [36]:

$$\frac{u_p}{u_{*}}=\frac{1}{K}\mathit{ln}\left(E\frac{u_{*}{y}_p}{v}\right)$$

(13)

where “u_p” is the average stream flow velocity at the “p” point; “K” is the von Karman constant (0.418); “y_p” is the distance from point p to the wall; empirical constant “E” has the value of 9.79; and “u_*” is the friction velocity. The “u” uniform velocity distribution is provided to the horizontal velocity component in the x-direction at the inflow boundary. The vertical velocity component “v” in the y-direction is set to zero. The inlet velocity field to the channel consists of a forward “u” horizontal velocity and zero “v” vertical velocities at all points except points close to the channel.

The wall y⁺ is a dimensionless distance similar to the local Reynolds number that is often used in CFD to describe how coarse or fine a mesh is for a given flow. It determines whether the effects in cells adjacent to the wall are laminar or turbulent.

$$y^{+}=\frac{u_{\tau }y}{\nu }$$

(14)

$$u_{\tau }=\sqrt{\frac{{\tau }_w}{\rho }}$$

(15)

where u_τ is the friction velocity, y is the height from the wall to the midpoint of the wall-adjacent cells, v is the kinematic viscosity, τ_w is the wall shear stress, and ρ is the fluid density at the wall. Values of y⁺ close to the lower bound (y⁺ ≈ 30) are most desirable for wall functions, whereas values of y⁺ ≈ 1 are better for near-wall modelling [37,38].

The flow on the spillway passes around five sluice pillars on the sill structure, resulting in six different entry velocities. Then, it flows from three separate branches with two separating walls on the discharge channel. In spillway projects, when the gates are fully open at the time of flooding, the initial velocities in the approach channel were adjusted according to Froude similarity for the 1/200 scale model and these values were used in CFD analyses. Initial velocity values are provided in Table 2.

In the time-dependent solution process, the initial condition is F = 1 at the entrance boundary of the solution region, and F = 0 at the exit boundary of the other regions and the solution region. The time step for the turbulence model used in the numerical modeling is Δt = 0. It was chosen as 0.1 s and a solution was made for 120 s, during which the numerical solution became stable. The numerical solution of the fundamental equations according to the boundary conditions was carried out using the ANSYS Fluent package program, based on the finite volume method.

4.4. Numerical Solver

When the velocity fields into the spillway channel have complex currents such as circulation flow, problems regarding turbulent flow and secondary flow arise because the spillway channel flows are nonlinear and the velocity and pressure field are interdependent. These problems are solved using the “Coupled” procedure approach. This procedure is the iteration method and is based on the prediction-corrector approach. ANSYS Fluent (Release 19 version, USA) provides the option to choose “Coupled” pressure–velocity coupling algorithms. Since the spillway channel flow is unsteady, the fully implicit scheme was used for converting the discrete equations in the present model to provide a stable and realistic solution for the large time steps. The full implicit scheme is used in the model, since the flow is unstable and the analysis time is very long [39,40,41,42,43]. Numerical model flows were simulated in an approximately 2 m long spillway channel, similar to the experimental flow. As an initial state, the inlet channel was first filled with air and water. Then, the water in the approach channel was released into the free flow from the spillway discharge channel at determined velocities. The calculation continued for about 120 s, at which point the front had already crossed the downstream boundary and any change in flow area would be negligible. Numerical analyses were carried out with ANSYS Fluent Release 19. A workstation with a 4-core Xeon 4.0 GHz processor and 32 GB Random Access Memory (RAM) was used in the numerical analysis. The analysis took approximately 12 h. Discretization methods and solver settings are presented in

Table 3. Numerical model details.

Solver Set	Solver	Pressure-Based
	Space–Time	3D, Unsteady
Model	Multiphase Model	VOF
	Viscous Model	k-ε
Phase	Primary Phase	Air
	Secondary Phase	Water
Discretization	Pressure	Presto
	Momentum	Second Order Upwind
Pressure–Velocity Coupling	Method	Coupled
Convergence Criterion	Residuals	0.001 (Continuity)
		0.001 (Momentum)

. Convergence criteria, discretization methods, etc., are shown in Table 3.

5. Image Processing Studies

5.1. Image Processing: Python-OpenCV

Image processing can be defined as a method of performing operations on an image to obtain an enhanced image or extract some useful information from it. Nowadays, image processing is a rapidly developing technology and constitutes the main research area in the engineering and computer science disciplines. Python is one of the widely used programming languages for this purpose. Its libraries and tools help in achieving the task of image processing efficiently. One of these libraries is OpenCV, which stands for Open Source Computer Vision Library. This library consists of many optimized algorithms used for image processing. These algorithms can be used to detect and recognize faces, identify objects, classify human actions in videos, track camera movements, track moving objects, etc. [44]. Moving object detection and tracking algorithms are used in this study.

5.2. Motion Detection and Tracking Algorithm

Motion detection and tracking are important in image processing. Motion detection and tracking can be performed in three ways: background subtraction, frame subtraction, and optical flow technique. The background subtraction technique was used in this study. Background subtraction is a widely used approach for detecting moving objects in videos from static cameras. The rationale in the approach is that of detecting the moving objects from the difference between the current frame and a reference frame, often referred to as the “background image” or “background model”. Background subtraction is usually performed if the image is a part of a video stream [45]. In the next step, the moving object is tracked by framing it for each video frame. In the final step, the average velocity is calculated by dividing the distance traveled of the object, from its starting point, by the elapsed time. In this study, the object detection and tracking algorithm, using motion, is shown in the flowchart (Figure 8).

5.3. Experimental Design and Equipment

During the experiment, a floating object was placed at the entrance of the spillway model and its movement on the model was recorded with cameras placed at different angles. The cameras are standard cell phone cameras, providing 1080p (1920 × 1080) images at 30 frames per second, recorded in AVI (audio video interleave) format. An orange-colored, standard table tennis ball with a diameter of 40 mm and a weight of 2.7 g was chosen as the floating object. While making this selection, attention was paid to ensure that it was light enough to be ignored and in a color that could be noticed in the video recording. In addition, papers of black and white colors pasted into the test channel were used as reference points of known length. In total, 2 papers pasted side by side were placed so that the distance between the centers of the circles on them was 20 cm. For the centers of the circles to be better determined during image processing, the circles were divided into four equal quadrants, with black and white colors diagonally opposed so that the center of the circle could be better selected, due to the contrast created (Figure 9).

5.4. Video and Data Processing

During the experiment, video cameras were fixed in order to observe the spillway model from a wide angle. A tennis ball was placed on the water flow so that it would pass through the right, middle, and left chute channels separated by the separation walls of the spillway discharge channel. The movement of the floating object on the water was recorded with a video camera. The images obtained were preprocessed before being used in the created algorithm. In this part, the images were been cropped to prevent other movements outside the experimental setup. The prepared images were processed in the developed OpenCV-Python code. The code consists of four main parts. In the first stage, video images were read and image frames were created. In the second stage, the images were passed through filtering techniques for the detection and tracking of the floating object. In the third stage, the velocity of the object being tracked was calculated. In the final stage, the distance difference, time difference, velocity value, and lines representing the measured sections were displayed on the screen (Figure 10, Figure 11 and Figure 12).

6. CFD Model Results

At the end of the studies, it was observed that both the physical model and the numerical model (10,055 m³ s⁻¹) transferred the flood discharge downstream safely. Figure 13 shows the general view of the flow resulting from the CFD analysis on the spillway model. When Figure 13 is examined, it is observed that the side walls of the spillway chute channel are sufficient for the flood flow. However, overflows were observed at some points near Cross-section 1 of the separating walls of the chute channel. The velocity and water depth of the physical model and numerical model results are compared in tables, figures, and graphs below. Comparisons, mean absolute error (MAE), root-mean-square error (RMSE), and average percent error (APE) values are calculated and shown in the tables. MAE, RMSE, APE equations provided as:

$$MAE=\frac{1}{N}\sum _{i=1}^N\left|Y_{iobserved}-Y_{iestimate}\right|$$

(16)

$$RMSE=\sqrt{\frac{1}{N}\sum _{i=1}^N{\left(Y_{iobserved}-Y_{iestimate}\right)}^2}$$

(17)

$$APE=\frac{100}{N}\sum _{i=1}^N\left|\left(\frac{Y_{iobserved}-Y_{iestimate}}{Y_{iobserved}}\right)\right|$$

(18)

where “N” is the number of points measured, “Y_{i observed}” is the experiment measured, and “Y_{i estimate}” is the CFD measured.

6.1. Comparison of Velocity

Experimental and numerical model velocity values are shown in

Table 4. Comparison of experiment and CFD velocity values.

Cross-Section No.	Column No.	Location at y Direction (m)	Experimental Results (m s−1)	CFD Results (m s−1)	MAE	RMSE	APE%
Cross-Section 1	N1	0.0250	1.205	1.377	0.161	0.167	13.4
	N2	0.1150	1.094	1.332
	N3	0.2025	1.378	1.266
	N4	0.2900	1.403	1.276
	N5	0.3775	1.144	1.299
Cross-Section 2	N1	0.0250	1.101	1.321	0.084	0.115	7.2
	N2	0.1150	1.208	1.31
	N3	0.2025	1.288	1.28
	N4	0.2900	1.294	1.288
	N5	0.3775	1.223	1.305
Cross-Section 3	N1	0.0250	1.068	1.381	0.158	0.180	13.8
	N2	0.1150	1.298	1.231
	N3	0.2025	1.143	1.327
	N4	0.2900	1.175	1.281
	N5	0.3775	1.224	1.342
Cross-Section 4	N1	0.0250	1.491	1.821	0.160	0.196	10.0
	N2	0.1150	1.785	1.725
	N3	0.2025	1.602	1.861
	N4	0.2900	1.806	1.700
	N5	0.3775	1.793	1.748

and, comparatively, in the graphs in Figure 14. Table 4 shows the error rates by comparing the experimental and CFD analysis results.

When the table and graph are examined, the percentages of APE error in the sections were found to be 13.4, 7.2, 13.8, and 10.0. It can be seen that the error percentage of the velocities is less at the midpoints than at the edges. The percentage of error (N1 point) in Column 1 was higher than the others in all four cross-sections. Since the N1 point is close to the right side-wall of the chute channel, we believe that the turbulence occurring at this point may have caused errors in the measurements.

The velocity value contours and depth–velocity profiles obtained as a result of the CFD analysis on the spillway model are provided in Figure 15, Figure 16, Figure 17 and Figure 18 for four cross-sections. In all figures, it is seen that the velocity values increase from the wall edges to the center. If the velocity values in the cross-sections are examined, it can be observed that the velocity values of the air phase are lower after the water–air separation line. It can be observed that the velocity values were close to each other and the amount of increase was low in Cross-sections 1–3, which had a low slope (3%). However, with the increase of the slope (17%), the velocity value in Cross-section 4, located at the exit of the spillway, is higher than the others, as expected.

6.2. Comparison of Water Depth

The water depths measured as a result of CFD analysis are shown in Figure 19 in the general view for four cross-sections. Experimental and numerical model water depths are compared in the graphs in Figure 20 and in

Table 5. Comparison of experiment and CFD water depth values.

Cross-Section No.	Column No.	Location at y Direction (cm)	Experimental Results (cm)	CFD Results (cm)	MAE	RMSE	APE%
Cross-Section 1	H1	1.0000	2.900	2.865	0.074	0.080	2.2
	H2	6.4375	3.000	3.085
	H3	11.8750	3.500	3.435
	H4	14.6250	3.200	3.135
	H5	20.2500	3.000	2.955
	H6	25.8750	3.000	2.945
	H7	28.6250	3.800	3.655
	H8	34.0625	3.600	3.525
	H9	39.5000	3.500	3.405
Cross-Section 2	H1	1.0000	3.500	3.615	0.137	0.143	3.8
	H2	6.4375	3.600	3.515
	H3	11.8750	3.600	3.405
	H4	14.6250	3.600	3.405
	H5	20.2500	3.700	3.525
	H6	25.8750	3.500	3.405
	H7	28.6250	3.500	3.395
	H8	34.0625	3.900	3.765
	H9	39.5000	4.000	3.865
Cross-Section 3	H1	1.0000	3.400	3.515	0.081	0.084	2.3
	H2	6.4375	3.600	3.615
	H3	11.8750	3.700	3.615
	H4	14.6250	3.500	3.415
	H5	20.2500	3.500	3.415
	H6	25.8750	3.500	3.415
	H7	28.6250	3.600	3.515
	H8	34.0625	3.500	3.415
	H9	39.5000	3.500	3.415
Cross-Section 4	H1	1.0000	3.000	2.95	0.050	0.050	1.7
	H2	6.4375	2.900	2.85
	H3	11.8750	2.800	2.75
	H4	14.6250	3.000	2.95
	H5	20.2500	3.000	2.95
	H6	25.8750	3.000	2.95
	H7	28.6250	3.000	2.95
	H8	34.0625	3.000	2.95
	H9	39.5000	3.000	2.95

. Table 5 shows the error percentages by comparing the experimental and CFD analysis results.

According to the graphs in Table 5 and Figure 20, the experiment and CFD analysis’ water depth measurements appear to be quite compatible with each other. When Table 5 is examined, the highest APE, 3.8%, is in Cross-section 2. In points other than this, the error percentages vary around 1–2%. The cause of the error is turbulent fluctuations created by the incoming flood flow.

The water depths obtained as a result of the CFD analysis are provided for the four cross-sections in Figure 21, Figure 22, Figure 23 and Figure 24. It is seen that the water depths in Cross-sections 1–3, which have a 3% slope, were around 3.5 cm; this fell below 3 in Cross-section 4, which had a 17% slope. As expected, the depth decreases as the flow rate increases. When the figures of Cross-sections 1 and 2 are examined, it is observed that the water depths in the right and left chute channels are higher than that in the middle chute channel. On the other hand, in Cross-sections 3 and 4, the water depths in the right, left, and middle chute channels are similar. When the figures are examined, at no point did the water height exceed the side-wall height. However, at some points, it rose above the separation walls in the middle of the chute channels. Depths H3 and H7 in Cross-section 1 can be provided as examples of this; as long as the flood stays in the chute, the situation is not problematic.

6.3. Investigation of Pressure in CFD Model

The flow of water in the spillway discharge channels in the flood regime causes low pressures. In some regions, cavitation is observed due to negative pressure. Cavitation causes structural deterioration [6]. For this purpose, pressure controls should be made in the spillway discharge channels. It was observed that the pressure values decreased for each of the four sections (Figure 25, Figure 26, Figure 27 and Figure 28).

As expected, the pressure decreased with an increase in velocity. Graphs expressing vertical pressure distributions show the dynamic effect and deviation due to channel slope and flow velocity.

6.4. Investigation of Cavitation on Prototype Spillway

In cases where the flow velocity is more than 25–30 m/s, the risk of cavitation can be observed on the spillways [11,46]. The reason for this is the formation of steam bubbles in the stream that can damage the concrete as a result of the pressure in the stream decreasing to the value of the vapor pressure. The bubbles which are consequently formed impact the concrete surface at high velocity, condense, and cause wear. This wear damage, which is small in the beginning, increases over time and reaches large sizes. This causes serious risks in the structure. The type of damage that occurs in the structure in this way is called cavitation damage. The damage on the spillway thus caused is calculated with the dimensionless “cavitation index”. In this calculation method, pressure (P) and average velocity (U) values taken from certain points along the channel are used. Falvey [47] stated that in cases where this calculated dimensionless cavitation index value is lower than 0.20, cavitation damage is highly likely to occur. At a point in the current, the cavitation index is calculated by the following expression:

$$\mathsf{\sigma }=\frac{{\mathrm{P}}_{\mathrm{T}}-{\mathrm{P}}_{\mathrm{v}}}{\frac{1}{2}\mathsf{\rho }{\mathrm{U}}^2}$$

(19)

where $\mathsf{\sigma }$ is the cavitation index; P_T is the absolute pressure (P_a), including atmospheric pressure; P_v is the vapor pressure of the water (P_a); $\mathsf{\rho }$ is the density; and U is the velocity of the water. The calculated cavitation indices are presented in

Table 6. Cavitation indices for prototype spillway.

Cross-Section No.	Column No.	Location at y Direction (m)	Model Pressure Pm (Pa)	Prototype Pressure Pp (Pa)	Total Pressure Pt (Pa)	Model Velocity Um (m s−1)	Prototype Velocity Up (m s−1)	$\mathbf{Cavitation}\mathbf{Index}\mathit{\sigma }$
Cross-Section 1	N1	0.0250	324.360	64,872.000	157,673.000	1.377	19.474	0.82
	N2	0.1150	381.476	76,295.200	169,096.200	1.332	18.837	0.94
	N3	0.2025	320.449	64,089.800	156,890.800	1.266	17.904	0.97
	N4	0.2900	357.581	71,516.200	164,317.200	1.276	18.045	1.00
	N5	0.3775	310.582	62,116.400	154,917.400	1.299	18.371	0.91
Cross-Section 2	N1	0.0250	350.546	70,109.200	162,910.200	1.321	18.682	0.92
	N2	0.1150	313.742	62,748.400	155,549.400	1.310	18.526	0.89
	N3	0.2025	319.891	63,978.200	156,779.200	1.280	18.102	0.94
	N4	0.2900	297.647	59,529.400	152,330.400	1.288	18.215	0.91
	N5	0.3775	345.269	69,053.800	161,854.800	1.305	18.455	0.94
Cross-Section 3	N1	0.0250	231.060	46,212.000	139,013.000	1.381	19.530	0.72
	N2	0.1150	224.240	44,848.000	137,649.000	1.231	17.409	0.89
	N3	0.2025	197.060	39,412.000	132,213.000	1.327	18.767	0.74
	N4	0.2900	214.194	42,838.800	135,639.800	1.281	18.116	0.81
	N5	0.3775	222.327	44,465.400	137,266.400	1.342	18.979	0.75
Cross-Section 4	N1	0.0250	134.874	26,974.800	119,775.800	1.821	25.753	0.35
	N2	0.1150	149.620	29,924.000	122,725.000	1.725	24.395	0.41
	N3	0.2025	153.900	30,780.000	123,581.000	1.861	26.319	0.35
	N4	0.2900	151.555	30,311.000	123,112.000	1.700	24.042	0.42
	N5	0.3775	130.170	26,034.000	118,835.000	1.748	24.720	0.38

. While making the calculations, we considered the average temperature as 20 °C, the vapor pressure (P_v) value as 2338 Pa, and the atmospheric pressure (Patm) as 92,801 Pa. The pressure and velocity values obtained with the model were increased in scale ratio according to Froude similarity and the pressure and velocity values were determined for the prototype spillway.

When the table is examined, it can be observed that the cavitation index values gradually decrease along the discharge channel. In the prototype spillway, there is no risk of cavitation, as the index values are above 0.2 at all points in the sections.

7. Image Processing Results

The velocity algorithm, shown in Figure 9, was created using the images captured by Camera 2, and the water depth algorithm was created with the images captured by Camera 1.

7.1. Velocity Algorithm Results

The relationship between the average flow velocity measured by the ADV device during the experiment and the floating object velocity calculated with the OpenCV code was examined. These two velocity values were scaled, and new correction coefficients were obtained. These results are shown and discussed in

Table 7. Velocity correction coefficients for the current spillway model experiment.

Cross-Section No.	Location at x Direction (m)	Section Slope%	Average Water Velocity (m s−1)	Average Floating Object Velocity (m s−1)	Coefficient
Crossssection 1	0.366	3	1.094	1.061	1.03
Cross-section 2	0.766	3	1.288	1.394	0.92
Cross-section 3	1.266	3	1.143	2.788	0.41
Cross-section 4	2.01	17	1.602	4.424	0.36

. When Table 7 is examined, it is seen that the velocity of the floating body in x direction increases gradually in parallel with the water velocity and the slope of the spillway. The correction coefficients provided in Table 1 of the Case Study section, ranging from 0.66 to 0.88, were obtained for open channels with low slopes and low flow velocity. Thus, the coefficients were calculated as ranging from 0.37-1.03 in chute spillway flows with high slope and high velocity. In addition, OpenCV code screens are provided for four sections in Figure 29.

7.2. Water Depth Algorithm Results

The images obtained with Camera 1 during the experiment were transferred to OpenCV code and the water depths were calculated depending on the position of the floating object. The water depth values obtained were compared with the water depths measured during the experiment and are shown in

Table 8. Comparison of experiment and CFD water depth values.

Cross-Section	Observation No.	Location at x Direction (m)	Experimental Water Depth Results (cm)	OpenCV Code Water Depth Results (cm)	MAE	RMSE	APE%
	1	0.166	3.500	4.300	0.592	0.628	18.8
Section 1	2	0.366	3.500	4.200
	3	0.566	3.300	3.900
Section 2	4	0.766	3.500	4.000
	5	0.966	3.400	4.000
	6	1.166	3.100	4.100
Section 3	7	1.266	3.400	4.200
	8	1.316	3.400	3.900
	9	1.366	2.800	3.300
	10	1.566	2.500	3.100
	11	1.766	2.500	2.300
Section 4	12	1.966	2.500	2.300

. When Table 8 is examined, it is observed that, depending on the position of the floating body in x direction, the water depths and the spillway gradually decrease parallel to the slope. The MAE, RMSE, and APE values for the 12 measured points were 0.592, 0.628, and 18.8%, respectively.

In Figure 30, OpenCV code screens that measure depth for four sections are provided.

The water depths observed along the X direction in the experiment, calculated with the OpenCV code, are shown in the graph in Figure 31. When the graph is examined, it is seen that the water depths are compatible with each other.

8. Conclusions

In this research, a three-dimensional CFD model and OpenCV code were developed by comparing the flow over the spillway with experimental data to be used in spillway studies. The results obtained were as follows:

-

It was observed that both the physical model and the numerical model (10,055 m³ s⁻¹) transfer the flood discharge downstream safely.

-

The average velocity values measured with the ADV device generally increased along the discharge channel. We observed that the increase in velocity values was low in the cross-sections where the slope was 3%, and the velocity increase was higher in the cross-section where the slope was 17%. The velocity values increased from the wall edges to the center.

-

The error rates between the experimental and numerical analysis rates were obtained in Section 3, with the highest APE error percentage value of 13.8, as a result of the examination.

-

As a result of the studies, it was determined that the APE error rate between the experimental and numerical analysis’ water depth results was around 1.7–3.8% at most measurement points.

-

Cavitation index values were calculated as above 0.2 in all sections of the prototype spillway. Thus, there is no risk of cavitation in the spillway discharge channel.

-

It has been observed that the error rate of the water depths obtained with the newly developed float method based on image processing is higher than the simulation results when compared with the experiments.

-

With the developed float method, velocity correction coefficients were obtained for the chute spillway depending on the velocity of the floating object.