Numerical Modeling of Flow Pattern with Different Spillway Locations

The spillways are one of the most important structures for efficient operation and dam safety [1]. They represent a safety valve of dams during dams' operation to discharge water that exceeds a storage volume. The extra water flows from the reservoir and returns back to the main channel of the river over a crest of the spillway. The suitable spillway design must prevent the potential failure risk of the dam overflowing. During the high flow condition, the design must be accomplished to face the problems of high-flow kinetic energy as well as cavitation. The location of the spillway can be designed within the body, alongside, and quite away from the dam depending on many considerations, but usually, it is best built separately from the dam. The spillway's efficiency can measure with discharge coefficient (C) that represents the losses in flow [2-4]. The transition, entrance, and curvature losses form the main losses that must be added to determine the total head and evaluate the reservoir elevations [5, 6].

The change in the flow conditions upstream of the spillway can modify or change the flow properties and lead to deviation from the standard design requirements [7]. These changes require engineers to estimate whether or not the change or deviation will be detrimental to the hydraulic performance of the spillway for example when changing the location of the spillway from the middle of the dam to the side of the dam.

In a large dam when the height of the dam is high in relative to the head of water on the crest of the spillway, approach velocity can be neglected. It is different from a low spillway that has considerable approach velocity and can affect the discharge coefficient in addition to the profile of the spillway crest [8]. In contrast to large dams, when the dam height is low compare to the water head on the crest of spillway the high probability of cavitation is considered [9]. The limited hydrologic data means the evaluation of design head on the crest will be risked and expected head may be less or greater than a real head. The real head on the crest greater than the design head will cause negative pressure pockets and increase velocity for a given discharge which leads to cavitation occurred [10]. Based on the U.S. Bureau of Reclamation, the real head to design head should not exceed 1.33. To investigate all the mentioned flow patterns, the researchers have been employed different methods of modelling. These methods include Physical and numerical modelling.

Physical models were the primary tool that are used for estimating hydraulic characteristics of flow patterns over spillways. But these models have many limitations such as high construction cost which can reach about 10% of dam cost [1], time-consuming operation, and testing as well as there is uncertainty in results because of the scaling effects, especially on small scales. On small scales, there may be an effect of some physical forces on the operation of the physical model, for example surface tension, although these forces are neglected or have no effect on the flow in the structure at the real size.

Therefore, in recent years studies have increased using numerical models for studying and simulating the hydrodynamics behavior of spillways numerically with reasonable lowering for cost and time [11, 12]. The numerical model becomes indispensable for designing a huge hydraulic structure such as dams. Numerical methods can solve the complex flow pattern problems in saved time consumption and saved cost when compared with measured or experimental work [13, 14]. Almawla et al. [15] studied the strains behavior on Haditha Dam's spillway by developing a model depending on ANN techniques and they showed that it can be used for accurate evaluating of the strain on the spillway. The limitation of this study is the lack of measured data, due to the low levels of the river and the fact that the water does not reach the crest of the spillway except twice during the dam's age. Moreover, this study did not consider the effect of the spillway location on the flow patterns or the effect of hydraulic performance on the stress and strain that were resulted from the flow. In current days, the affirmation is to develop a simple technique, which implies low cost, efficient, as well as quick construction, to satisfy the requirements of water in this region [16].

Mohammed et al. [17] examined the numerical model (Flow-3D) to simulate flow on ogee-crested spillway in comparison with physical models. They concluded that the numerical model had provided an agreement with physical models for simulation of water surface profiles despite some discrepancies in cavitation or pressure results. Kim et al. [18] constructed a hydraulic stability improvement for the Karian dam's spillway in Indonesia. They used CFD numerical model and compared the results with a physical model. The numerical model showed that the flow over the spillway is stable with an agreement with the physical model results based on the rating curve and discharge coefficient. However, this study did not investigate the effects of the spillway location on the flow patterns.

Computational fluid dynamics (CFD) is a type of numerical modeling that is used for solving problems that involve fluid flow. Since CFD can provide faster and more economical solution than physical modeling, hydraulic engineers are interested in verifying the capability of CFD software. Aydin et al. [19] studied the cavitation on the spillway surface of a dam with 100m height using a numerical model in compression with experimental observation. The results showed that cavitation occurs after a certain point downstream, depending on cavitation indices.

The location of the spillway can be determined and selected according to the site topography, hydrologic conditions, requirements of water release to the downstream, geology, as well as the safety and economics of the project. The main safety requirements of a dam, spillway must be hydraulically efficient, to avoid the overtopping or overflow discharge particularly in earth-fill dams that are widely used in Iraq. In the current study, the researchers have investigated the effects of spillway different locations within the dam body on the hydraulic performance of the spillway whether it is in the middle of the dam or on one side of the dam. The statistics of the International Dams Council indicates that the major cause of the dam's failure are hydraulic reasons. These are represented by the insufficiency of the design discharge capacity of the spillway, which leads to the failure and collapse of dams. This can help engineers and designers to address any negative impacts on the operation of the watercourse resulting from site selection and avoid their impact on the designed discharge capacity of the spillway.

Numerical models are supported and calibrated by physical models which provide an effective method for designing the spillway and understanding the behavior of the structure in terms of hydraulics and performance efficiency for different operating conditions.

Despite the vast knowledge and understanding of the general ogee shape and its flow patterns, any change in spillway location can change the flow conditions, and modify the shape of the crest. This can lead to deviation from the requirement of standard design. Any changes required to evaluate the flow pattern over the crest and determine if these changes will affect the hydraulic properties of the spillway. The present study investigated the effect of the location of the spillway within the dam body on hydraulic performance, which was not taken into consideration in most previous studies, especially in Iraq.

In this study, Mandali Dam in eastern Iraq was selected as a study area. The flow in the spillway was simulated with two locations (in the middle of the dam, on side of the dam). Then the effect of spillway location on flow properties was studied to assess the hydraulic performance depending on the simulated results of hydraulic model tests. A physical model operation results have been used for calibrating the numerical model and investigating the hydraulic performance of spillways, with selected locations.

Nowadays, numerical models are widely used for their accurate result and time saver. Thus, utilizing of such simulation techniques is recommended. In this study, a numerical model is introduced. This model was built by employing Ansys fluent software 2020 R1. This software is a powerful software that is capable of simulating complex fluid flow scenarios accurately. It adopts the finite volume method and uses the unstructured triangular mesh for discretization purpose. For turbulence consideration, the software utilizes different closure models to deal with turbulence. In the present study, the k-ε model is used. The k-ε model is a powerful turbulence closure model that is commonly used for simulating flow patterns over spillways [21-23]. The multiphase flow, that includes water flow and air flow was represented by utilizing volume of fluid model (VOF). More details about the model construction are introduced in the following subsections. To analyze fluid flow problems with CFD, four stages must be achieved as following [24]:

1) Describe the flow with mathematical equations that usually are set of partial differential equation;

2) To construct the numerical analogue, fluid flow equations must be discretization;

3) Domain of fluid should be divided into cells or elements;

4) Apply the initial and boundary conditions to solve the equations.

3.1 Governing equation

The governing equation of a CFD model should be capable to capture all the hydrodynamic behavior of fluid during its flow in a domain. The general dimensional Navier Stocks Equations are utilized for this purpose. These equations are built based on the physical principle of mass conservation, momentum conservation, and energy conservation.

The first equation of the set is the continuity equation that represents the summation of the mass rate which inters a specific element of volume of a fluid, the mass rate that leaves this element, and the mass accumulation in this element. The continuity equation is introduced as below [25]:

$\frac{\partial \rho}{\partial t}=\nabla \cdot(\rho \vec{U})=0$                 (1)

where, ρ is the density (kg/m³); t is the time (s); and $\vec{U}$ is the velocity vector (m/s).

The second equation of the governing equations set is the momentum equation. This equation is representing the influence of the applied forces on a fluid moving element which equivalents the rate change of momentum according to the principle of newton's second low. The momentum equation is represented as below [26]:

$\frac{\partial}{\partial t}(\rho \vec{U})+\nabla \cdot(\rho \vec{U} \vec{U})=-\nabla p+\nabla \cdot(\tau)+\rho \vec{g}+\vec{F}$        (2)

where, p represents the pressure, τ represents the stresses tensors, $\rho \vec{g}$ is the gravitational body force, and $\vec{F}$ represents the external body forces.

$\tau=\mu\left[\left(\nabla \vec{U}+\nabla \vec{U}^T\right)-\frac{2}{3} \nabla \cdot \vec{U} I\right]$                       (3)

where,$(\mu)$ represents the viscosity coefficient and (I) represents the unit tensor.

3.2 Construction of geometry

The three dimensions geometry that represents Mandali Dam spillway and the flow domain was constructed by using Solidwork 2018 software. The geometry was exported to the Ansys fluent software after saving it as Parasold (x,t) format as shown in Figure 4.

3.3 Mesh generation and boundary conditions

Mesh generation is a significant step for numerical simulation process. It can influence the result accuracy dramatically [27]. In addition to above, the number of cells have a great impact on the model accuracy where finer mesh has the most accurate result. Furthermore, it can be time consuming in case of choosing inconvenient mesh type or cell size [28]. In the present study, tetrahedral meshing is used. To reduce the number of cells and the simulation time, symmetry and refinement with suppress the dam body technique were applied to the mesh. The cell size of 1 m is chosen with face sizing 0.4 m. The total number of elements were 1312771 cells.

After setting up the suitable mesh, the assessment of the mesh quality and mesh sensitivity is required for better numerical result where the model stability and result accuracy are governed by the mesh quality. Table 2 shows the state of the chosen mesh quality according to the required criterion that are used for assessing the mesh quality according to the ANSYS Fluent User's Gide [29].

In the numerical model, the domain faces were given different boundary conditions. At the upstream edge, the face divided into two parts, the lower part which represents the water inlet is assumed to be velocity inlet while the upper part was assumed to be air inlet. The edge face at the downstream area which represent the water outlet was assumed to be pressure outlet boundary. The surface of the domain was assumed to be air pressure outlet. For simulation time saving purpose, the boundary symmetry method was adopted. The other edge faces were assumed to be wall as no slip boundary condition. Figure 4 shows the presented three-dimensional model meshing with the boundary conditions.

4.png

Table 2. Mesh metric table