Hydrodynamic Characteristics of the Baihetan Plunge Pool

(1)

Hydrodynamic Characteristics of the Baihetan Plunge Pool

The Secondary Dam’s Top Elevation Impact on Flow Patterns

Henrik Smeds Axel Monthan

Mechanical Engineering, master's level 2018

Luleå University of Technology

Department of Engineering Sciences and Mathematics

(2)

The hydrodynamic characteristics of the Baihetan Plunge pool and the impact of changing the secondary dam’s top elevation was investigated. Quantities such as the velocity distribution, turbulence dissipation rate, water surface profile and the probability of a submerged jump forming in the plunge pool was studied.

The numerical model showed in general good agreement with data gathered from an experimental study conducted in 2012. The only exception was the maximum pressure in the plunge pool, which was 16.91 % higher for the simulation using a top elevation of 604 MASL for the secondary dam. The use of a grid convergence index (GCI) showed that the result was closer to being mesh independent in the plunge pool (GCI_plunge= 4.5 %), but not in the jet body (GCI_jet= 16.9 %).

The results indicated that no significant improvement was given for changing the top elevation of the secondary dam to 604 or 606 MASL (original height is 602 MASL) since all cases display flow pattern indicating that a submerged jump will occur. Moreover most of the turbulence was concentrated near the jet for all the cases, indicating that the plunge pool is properly designed for the purpose it is intended to do, i.e. dissipating the energy of the jets in the plunge pool and not downstream to the unprotected riverbanks.

The main conclusion is that the original design is to prefer since no advantages is given by heightening the secondary dam, and will only increase the cost of construction.

(3)

摘要

研究了白鹤潭跳水池的水动力特性以及改变二级坝顶高程的影响。数量，如速度分布，湍流耗散率，

水面剖面以及急剧下降形成淹没的可能性池被研究。

数值模型总体上与从实验中收集的数据一致研究于 2012 年进行。唯一的例外是水池中的最大压力对于使用 604 MASL 的顶部高程进行模拟的二级坝的模拟值高出 16.91％。该使用网格收敛指数

（GCI）表明结果更接近于网格独立（GCIplunge= 4.5 %），但不在喷射体内（GCIjet= 16.9 %）。

结果表明，改变顶部高程没有显着改善由于所有情况都显示，因此二级水坝到 604 或 606 MASL

（原始高度为 602 MASL）流量模式指示将发生淹没跳跃。而且大部分的动荡是所有情况下都集中在喷气式飞机附近，这表明小型游泳池设计合理它打算做的目的，即消耗跳水池中的射流的能量而不是在无保护的河岸下游。

主要结论是，由于没有优点，最初的设计更喜欢加大二级坝，只会增加建设成本。

(4)

First and foremost we would like to extend our deepest gratitudes to Dr. James Yang at Vattenfall for giving us the opportunity to do our master’s thesis at the Hydraulic Department of Tsinghua University, Beijing. We would also like to thank Energiforsk for funding this project.

Many thanks to Prof. Zhang Yongliang and Prof. Li Ling of the Hydraulics Department for guiding us throughout the project and aiding us when help was needed.

Thanks to Huifeng Yu and Gui Pong for helping us during our first days in China and showing us around, and the colleagues at the office who always brought much joy and good moods. Also many thanks to all the exchange students we’ve met throughout our stay in Beijing for giving us memories for life.

Finally we would like to thank Assoc. Prof. Gunnar Hellström at Luleå UT for being our examiner for this thesis.

Axel Monthan Henrik Smeds

Beijing, May 2018

(5)

List of Figures

1.1 Erosion of the bedrock downstreams of the Kariba dam. Source: Noret et al. (2013). 1 1.2 Secondary dam 1; plunge pool 2; main dam 3; Reservoir 4; Surface spillways 5. Source:

China International Water & Electric Corp. (2018). . . 3

1.3 Profile view and transverse flow characteristics of the plunge pool. Source: Liu (2012). 3 1.4 General layout of the Baihetan project and trajectories of the spillways. . . 4

1.5 General layout of all the six surface spillways. Source: Liu (2012). . . 5

1.6 Schematic overview of a rectangular nappe overflow (Castillo et al., 2015). . . 6

1.7 General flow characteristics of a plunge pool. Reproduced from Xu et al. (2002). . . 7

1.8 Free impinged jet. Source : Yangtza et al. (2003). . . 7

1.9 Submerged impinged jet. Source : Yangtza et al. (2003) . . . 8

1.10 Surface flow pattern in a plunge pool. Source : Yangtza et al. (2003). . . 8

4.1 A flowchart describing the methodology of the work process. . . 17

4.2 Top- and side views of the surface spillways. All units are in MASL unless otherwise stated. . . 18

4.3 Reservoir, spillway and jet trajectory body shown in one assembly. The final shape of the jet trajectory body was modelled through trial and error. . . 19

4.4 Cross sectional view of the plunge pool in its original design. . . 19

4.5 Longitudinal view of the plunge pool divided in 4 sections. Notice that the height of the secondary dam is 46 meters, which is the original height. . . 20

4.6 Isometric view of the whole model geometry. . . 20

4.7 Hexahedral mesh of the reservoir, spillway and jet combined. . . 21

4.8 Sideview of the plunge pool’s mesh. . . 21

4.9 Boundary condition locations as specified in Gambit. . . 22

4.10 The locations of the pressure inlet boundary condition as specified in Gambit. . . 23

5.1 Length of jet trajectory for different mesh sizes. . . 25

5.2 Comparisons of the air volume fraction for different mesh sizes. Violent fluctuations in air volume fraction indicates that the jet has started to break apart. . . 26

5.3 The jets velocity during its vertical ascent down from the crest. . . 26

5.4 Velocity profile in the plunge pool. . . 27

5.5 Max pressure on the plunge pool floor for three different top elevations. . . 29

5.6 The water depth adjacent to the secondary dam with a top elevation of 602 MASL. . 31

5.7 Cross section of the velocity field for both spillways, top elevation 602 MASL. . . 32

5.8 Cross-section of the flow field around the secondary dam, top elevation 602 MASL. . 33

5.9 Horizontal cross section of the turbulent dissipation rate, top elevation 602 MASL. . 33

5.12 Cross-section of the flow field around the secondary dam, top elevation 604 MASL. . 35

5.13 Horizontal cross section of the turbulent dissipation rate, . . . 36

(8)

5.16 Cross-section of the flow field around the secondary dam, top elevation 606 MASL. . 37 5.17 Horizontal cross section of the turbulent dissipation rate, top elevation 606 MASL. . 38 A1 Blueprints of spillway 1. . . 43 A2 Blueprints of spillway 6. . . 44

(9)

List of Tables

1.1 Operating conditions for the Baihetan dam. . . 4

1.2 Characteristic parameters of the six surface spillways Liu (2012). . . 5

1.3 Discharge during normal condition. . . 5

5.1 Comparison of important jet tongue parameters. . . 28

5.2 Empirical and simulated jet breakup length. . . 29

5.3 Experimental data vs numerical data of key parameters in the plunge pool. . . 30

B1 Experimental data for jet tongue. . . 45

B2 Experimental data for max pressure. . . 45

(10)

Dh Hydraulic diameter [m]

F Froude number [-]

k Turbulent kinetic energy [m²/s²] h0 Jet thickness [m]

h1 Water height before jump [m]

h2 Water height after jump [m]

Lb Jet breakup length [m]

p pressure [Pa]

¯

u Velocity [m/s]

V˙ Volumetric flow [m³/s]

x Longitudinal distance [m]

y Height [m]

z Width [m]

β Impact angle [°]

ε_T Turbulence dissipation rate [m²/s³] µ_t Eddy viscosity [m²/s]

ρ Density [kg/m³]

σ_j Dispersion coefficient [-]

(11)

Chapter 1 Introduction

China’s surge in the demand for electricity, paired with the country’s national long-term goal to replace coal with renewable energy sources, has placed China in the forefront of hydropower devel- opment. In 2016, the country had an installed hydropower capacity of 330 GW, and a hydropower generation of 1,126 TWh (IHA, 2017). Although China is the worlds largest producer of hydro- electricty, the 13th five-year plan, adopted by the National Energy Administration in 2016, aims to increase the capacity to 380 GW.

To reach these goals, a series of cascade mega hydropower projects are currently under construction in the upper reaches of the Jinsha river, between the Sichuan and Yunnan provinces.

The Baihetan hydropower station, which this study is concerned with, is one of these dams that is currently under construction and the project is expected to be completed in 2021.

The hydropower stations in this region are often characterised by large flows, high discharge heads and narrow alleys. One prominent problem with these types of high arch dams is the high- energy flood discharge from the spillways. Therefore, one major design criteria is how to ensure the safe energy dissipation downstream of the dam during flood discharge.

One necessary solution is to construct an auxiliary dam downstream of the main dam. The purpose of this secondary dam is to create a plunge pool downstream that will act as a water cushion that will safely dissipate the kinetic energy of the impinged jets. Proper design of the plunge pool and the secondary dam is therefore of high importance. Failure to safely ensure the energy-dissipation of the high head jets can lead to scouring of the plunge pool floor and downstream of the dam. This can lead to costly maintenance of the dam due to undermining of the foundation.

The Kariba dam (Fig. 1.1) is such an example of faulty design.

Figure 1.1. Erosion of the bedrock downstreams of the Kariba dam. Source: Noret et al.(2013).

It is therefore important to study the hydrodynamic characteristics of the plunge pool in order

(12)

to understand the dissipation mechanism and what causes scour and erosion. Many authors have conducted both numerical and experimental studies on this topic, and it still remains an active research area to date. Experimental studies are however costly and more time-consuming. Numerical studies, on the topic of energy-dissipation in stilling basins, by previous authors such as Castillo et al.(2013) andXu et al.(2002) have shown promising results and generally good agreement with experimental data. Numerical studies are however not without concern. The flow in plunge pools are highly complex flow characterised by large Reynolds numbers. The method chosen for this study is to use numerical simulations, and compare against data gathered byLiu(2012) on a scale model of Baihetan.

The rest of this paper will be organized as follows. The remainder of this chapter will give the reader a clear understanding of the main research aim and limitations. Furthermore, the Baihetan hydropower project will be presented and the current research on energy-dissipation and flow patterns in plunge pools will be reviewed. Chapter 2 is an extensive literature review of earlier work conducted in the same field as this thesis, where topics such as turbulence closure, meshing, experimental studies etc. is studied. Chapter 3 explains the mathematical model used by the solver in this study (FLUENT) and other mathematical theories such as mesh quality, discretization etc.

Chapter 4 will explain the general methodology and approach used when modelling and meshing.

Finally, chapter 5 and 6 will summarize the result, discuss them and present the conclusions.

1.1 Research Aim & Limitations

The main aim of this study is to conduct numerical simulations to study the effect different top elevations of the secondary dam has on the flow characteristics of the Baihetan plunge pool during flood discharge, and in doing so contribute to the research area.

In more detail this study will entail: (1) Simulate the velocity field, water waves and water surface profile; (2) Calculate the probability of a submerged water jump and by doing so, assess the safety and existing risk of the original design scheme; (3) Simulate different top elevations of the second dam and to present an optimized design scheme; (4) Confirm numerical solution with previous experimental studies conducted on a scale model of Baihetan dam.

Necessary limitations of this study, due to computational powers, is to consider the flow from only 2 of the 6 surface spillways. Furthermore, the only geometry that will be altered from the original blueprints is the top elevation of the secondary dam, which in its original condition is 602 meters above sea level (MASL). Since experimental data exists for a top elevation of 604 and 606 MASL of the second dam they are the only heights that will be examined. Lastly, the computational domain will not extend further than the secondary dam, hence the flow downstream of the secondary dam will not be studied.

1.2 Baihetan Hydropower Project

The Baihetan Hydropower project is situated in the Jinsha river, between the Sichuan and Yunnan provinces, in the southwest of China. It is a 277 m tall double-curved arch-dam and, when completed, will have a total of 16 GW of installed capacity, making it the worlds second largest producer of hydroelectricity. The dam will have a reservoir of 17.924 billion m³. The main features of the dam are marked in Fig. 1.2.

(13)

CHAPTER 1. INTRODUCTION

1

2

3 5 4

Figure 1.2. Secondary dam 1; plunge pool 2; main dam 3; Reservoir 4; Surface spillways 5. Source: China International Water & Electric Corp.(2018).

The plunge pool, see Fig. 1.3, is an asymmetric inverted arch with concrete lining. The asymmetric design decreases the need for excavation and pouring of concrete which also decreases the cost of construction. The total length of the pool is 400 m and the pool floor is located at 556 MASL.

Figure 1.3. Profile view and transverse flow characteristics of the plunge pool. Source: Liu(2012).

The general layout of the dam and the plunge pool is shown in Fig. 1.4.

(14)

Figure 1.4. General layout of the Baihetan project and trajectories of the spillways.

During the dams lifetime it is expected to have different reservoir levels that might occur from extreme weather events. These different operating conditions are listed in Tab. 1.1. The normal condition is the flow condition that the dam will see most of its lifetime. Design level is an event that will happen with a frequency of every 100 year, and check level is an extreme event that will most likely occur every 1000-10000 year.

Table 1.1. Operating conditions for the Baihetan dam.

Operating Condition Reservoir Level (MASL)

Normal 825

Design 827

Check 832

The flow condition used in this study will be the normal condition with a reservoir level of 825 MASL.

1.2.1 Surface Spillways

The dam features six surface spillways (14x15 m orifice) for regulating the flood, and seven mid- level outlets (5.5x8 m orifice) for discharging sediments, that builds up in the reservoir. The total discharge capacity for all the 13 outlets combined is 30000 m³/s. This is 70 % of the total discharge capacity of 42350 m³/s, meaning that 12350 m³/s, or 30 % is passed trough the turbines. All the surface spillways have a crest height of 810 MASL, other characteristic parameters of each surface spillway is listed in Tab. 1.2.

(15)

Table 1.2. Characteristic parameters of the six surface spillwaysLiu(2012).

Spillway No. Exit height [MASL] Exit width [m] Slope [°]

1# 800.61 17.26 15

2# 799.63 18.34 30

3# 788.38 17.26 35

4# 788.38 17.26 35

5# 799.63 18.34 30

6# 799.01 17.57 15

The design of each surface spillway differs slightly from one another. Spillway one and six are designed with a ski-jump bucket, with the aim of impinging the jets farther downstream. Spillway two and five uses a trajectory bucket design such as to allow for the jets trajectory to be closer to the dam and collide mid-air with the jet’s from the mid-level outlets. With this design the whole plunge pool is used to a higher extent. Furthermore the jets from the mid-level outlets acts as a moving water cushion, dissipating energy during the collision. Spillway three and four have nappe-splitters at the end. The aim with nappe-splitters is to spread the jet’s over a larger area and cause aeration of the jet’s, therefore lowering the impact energy in the plunge pool. The layout of the spillways is shown in Fig. 1.5.

2 1 3

5 4 6

Figure 1.5. General layout of all the six surface spillways. Source: Liu(2012).

The discharge flow of Spillway one and six during normal condition is listed in Tab. 1.3. This flow will be used as a boundary condition for the numerical simulation.

Table 1.3. Discharge during normal condition.

Reservoir (MASL) Downstream (MASL) Discharge Flow m³/s Operating Condition

825 591.64 3149 Spillway 1 & 6

(16)

1.2.2 Energy Dissipation & Flow Patterns of Plunge Pools

The main energy dissipators of the high head jets, before impacting the pool, is aeration and disintegration of the jets. Whenever the jets core breakups the jet is considered to be fully developed and the jet will thereafter only consist of large blobs of water (Castillo et al.,2015). It is therefore important to study the hydrodynamic actions of the jet before impacting since it will affect the flow field and pressure distributions of the plunge pool upon impact. Important parameter is the breakup length L_b and the impingement jet thickness B_j, see Fig. 1.6.

Figure 1.6. Schematic overview of a rectangular nappe overflow (Castillo et al.,2015).

Castillo et al.(2015) proposed the following empirical formula for estimating the jet breakup length Lb

Lb

BiF_i² = K

(KϕTuF_i²)^0.82. (1.1)

In Equation (1.1) Bi and Fi are the jet thickness and Froude number at the issuance condition that is a location at which the jet exits the spillway. Tu is the Turbulence intensity at the issuance location and can be approximated to 1.2 % for an inclined crest. K is an experimental factor which for an arch dam is defined as 0.85 (Castillo et al., 2015). This empirical relation can be used for estimating the jet breakup and to validate the numerical results gathered from simulations.

During energy dissipation of the impinged water jets, different regions in the plunge pool exhibits different types of dissipation mechanisms. According toXu et al. (2002) these regions, see Fig. 1.7, can be divided into mixing, shearing- and impact regions. Xu et al. states that the main mean of energy dissipation is through shearing of the flow. This implies that a properly engineered plunge pool maximizes the shearing region. Moreover, the impact intensity in the impact region should be minimized. Sharp pressure gradients should be avoided as this implies that shear dissipation is insufficient.

(17)

mixing region mixing region

shear region

impact region Impinged jet

Outflow

Figure 1.7. General flow characteristics of a plunge pool. Reproduced fromXu et al.(2002).

The engineering guidelines, used in China today, is a maximum allowable impact pressure difference of ∆pmax= 15 m. However, it is uncertain if this design guideline is adequate for designing plunge pools. Peiqing and Futian (2001) discusses the possibility of using the submergence coefficient σj, which is dependent on the downstream water height and the height after the jump, as a control parameter. Peiqing and Futianestablished an experimental relationship between ∆pmaxand σjand draws the conclusion that the pressure on the plunge pool floor is more a result of the flow rather than a parameter that can be directly controlled, and therefore proposed that σj is a better design parameter than the currently used ∆p.

This result shows a need for understanding the different flow mechanisms in a plunge pool. As stated in the introduction, flows in plunge pools are highly complex. They are however permissible to study on a macroscopic level. Yangtza et al.(2003) states that the flow in a plunge pool can be divided into three types of flow patterns: free impinging jets, submerged impinging jets and surface flow. The flow regime can be described by the angle of the jet β, jet thickness h0, downstream water cushion height H1 and velocity of the impacting jet u0. Free impinging jets, see Fig. 1.8, occurs when Eq. (1.2) is satisfied:

h2= h1

2 (√

1 + 8F r²₁− 1 )

, (1.2)

where F r1 is the dimensionless Froude number, F r1 = ^V¹/^√gh₁, h1 and h2 are the heights of the water before and after the jump, respectively. These types of flows generally occur in plunge pools where the water cushion depth is shallow and the discharge height is small. For high head discharge jets, as in the case of Baihetan dam, these types of flows should be avoided due to the high impact pressure and velocity distribution on the pool floor which will cause damage to the structure.

β u₀

h⁰

h1 V1

h2

V2

Figure 1.8. Free impinged jet. Source : Yangtza et al.(2003).

Submerged jets\jump, see Fig. 1.9, occurs whenever the jump height h2 is smaller than the water cushion downstream H1. The flow is characterized by good jet diffusion, a flow velocity that decreases rapidly and a water surface profile that behaves calm (Yangtza et al.,2003).

(18)

I

II III

H₁ β

u₀ h⁰

h2

Figure 1.9. Submerged impinged jet. Source : Yangtza et al.(2003)

Yangtza et al. (2003) concludes from experimental data that the criteria for submerged impinged jets is:

σ_j≥ 2 , (1.3)

where σj is the dispersion coefficient of the jet and is defined as the ratio between H1/h2. Due to the positive hydrodynamic characteristics of a submerged jet, plunge pools in high arch dams should be designed such that this type of flow is more likely to occur.

The last type of flow pattern, surface flow, occurs if the water cushion depth H1 is to large or the inlet angle β is small. The impacting jet rises to the surface and produces a surface flow pattern that creates waves and violent fluctuating of the water surface profile (see Fig. 1.10). This type of flow utilizes a smaller amount of water in the plunge pool to dissipate energy and instead dissipates the energy in the unprotected riverbed and banks downstream of the secondary dam. Therefore, a surface flow pattern in the plunge pool is highly unwanted, and should be avoided.

Vd

hd

Vu≈ 0 hu

β h0

u0

Figure 1.10. Surface flow pattern in a plunge pool. Source : Yangtza et al.(2003).

(19)

Chapter 2 Literature Review

Research regarding numerical analysis in the same field as this thesis was studied, as well as previous work done by other thesis students regarding the Baihetan hydropower project. The most useful knowledge acquired is summarized at the end of this chapter.

2.1 Numerical Studies

The numerical tool for calculating the movements of fluids is called Computational fluid dynamics, or CFD for short. It is often a more cost-effective method, and offers several advantages over the more traditional option of experimental setups. A CFD simulation can produce a more detailed result regarding e.g. the pressure or velocity distribution. It is also more flexible in the sense that one can vary the models geometry, boundary conditions etc. in a rapid manner. However, setting up a numerical model requires a priori knowledge about the underlying physics of the problem, acceptable meshing and validation of the results. Also, the limitations of the model needs to be known in order to make tolerable assumptions, both when simplifying the geometric model from a physical one and setting up boundary conditions (Casey et al., 2000).

2.1.1 Previous Studies on Baihetan Dam

Several M.Sc. theses has been conducted on the topic of dam safety regarding the Baihetan hydropower project. The work of Lönn and Dahl(2016) validates previous experimental studies on a physical scale model of the Baihetan dam at Tsinghua University, Beijing, through CFD modelling.

The study consisted of modelling a surface spillway and measuring the impinged water jets location in the downstream stilling basin. The results were validated using experimental data in order to confirm the numerical model, which was then further used in a design optimization of the spillways with the goal of improving the longitudinal trajectory of the jet. While the results of the longitudinal direction and spreading of the jet indicated good agreements with the experimental results, the transverse flow lacked accuracy. Although the authors were unable to refine the mesh and assess different turbulence models (the used model was Realizable k− ε) due to a limit in computational power, it was found that the mesh grid had converged for the transverse flow and nearly converged for the discharge length of the jet.

In a second study, by Ramqvist and Länsman (2017), the pressure distribution in the plunge pool floor was numerically simulated, and validated with experimental data, in order to find where the pressure peaks most frequently occurs. The authors obtained good agreement with the experi- mental data available, with the maximum pressure and its location only deviating 2.2 % and 9.6 %, respectively, from the experimental data. The result that deviated the most from the experimental data was the fluctuating pressure which differed 26.6%. The authors mentions a few possible sources of error as: (1) Only one surface spillway was considered in the model; (2) The experimental setup was unable to sample with a high enough frequency to capture the pressure fluctuation correctly.

(20)

As suggestions for further work and improvement, both authors list the option of employing a higher order discretization scheme, e.g. second-order upwind. This would increase the accuracy, but also have the possibility of negatively impact the stability of the solution as well as increasing the runtime. Lönn and Dahl also discusses the possibilities of using experimental data as the boundary conditions for the surface spillway’s inlet. Moreover, both studies implemented the RANS approach of modelling turbulence. Although it is computationally less expensive than e.g., large eddy simulation or Reynolds stress models, it is also likely that the accuracy could be improved using a more advanced turbulence model.

2.1.2 Turbulence Models

The choice of a turbulence model that adequately describes the turbulent properties in a fluid flow can be difficult since different models excel in different cases, and the use of an advanced model will require more computational power than a simpler one. Before the current study began a review of previous work by various authors choices, and validation, of different turbulence models was conducted. A very common turbulence model which is widely used by engineers due to its robustness and feasible efficiency is the standard k− ε model which is a Reynolds Averaged Navier- Stokes (RANS) two-equation model, meaning that has two extra transport equations (Launder and Spalding,1972).

Castillo et al. (2013) did a numerical study concerning falling jets from an overflow crest weir.

Different turbulence models were assessed and compared to laboratory measurements where they found that there was a small variation among the turbulence models. The authors concluded that the SST turbulence model matched the experimental data best, while the standard k− ε seemed to overestimate the pressure distribution, both upstream and downstream while the RNG k− ε tended to only overestimate upstream.

Rahimzadeh et al. (2012) used CFD to study the flow over a circular spillway. The authors concluded that standard two-equation models (k− ε and k − ω) did not perform well when resolving hydraulic characteristics. More complex models such as the RSM, RNG- and Realizable k− ε and SST k− ω were found to agree well with experimental data.

Jun et al.(2004) performed a numerical simulation of the plunge pool for Xiangjiaba dam. The model used for turbulence closure was the RNG k− ε, which the authors found to provide accurate results. The simulated pressure, and water depth, at the bottom slab of the plunge pool was in good agreement with test data.

Xu et al.(2002) Simulated and measured the 3-D flow fields in the plunge pools of the Xiaowan high arch dam and Laxiwa high arch dam. The simulations were run with a standard k−ε turbulence model, which showed an error between the calculated and the measured maximum pressures to be between 4.9− 7.8% for both plunge pools.

2.1.3 Mesh

In ”ERCOFTAC’s Best Practice Guidelines” by Casey et al. (2000), the most fundamental and important aspects is outlined when it comes to meshing a model in a correct way in order to ensure accurate results. These include acceptable aspect and expansion ratios, skewness and orthogonality of cells, together with refinement of the grid size in areas of the model where the geometry might be complex. These areas should however, if possible, be left out in the model or at least be simplified to the furthest extent that is possible. A multitude of options also exist when it comes to choosing a suitable mesh type e.g. polyhedral, tetrahedral, hexahedral etc. The final choice is dependent on many factors, including, but not limited to, the computational resources available, the type of geometry that is to be meshed and even the user’s opinions and previous experiences. Peric and Ferguson (2012) suggest that a polyhedral mesh may offer a substantial improvement in accuracy over tetrahedral mesh.

By definition a polyhedral element have, in contrary to a tetrahedral, many nodes in each cell and a large number of neighbouring elements, even those next to boundaries and corners, and the increased number of neighbouring elements enables a better approximation of gradients. It is shown

(21)

CHAPTER 2. LITERATURE REVIEW

that use of a coarser polyhedral mesh is more accurate (and faster) than using a finer tetrahedral one (Peric and Ferguson,2012). In the study by Peric and Ferguson, a polyhedral mesh of four times fewer elements than a tetrahedral one uses less memory and the computational time is multiple times lower, while still yielding the same result. The fewer amount of elements is due to that when the polyhedral mesh is generated, several tetrahedral elements are combined into bigger elements. The many faces of a polyhedral makes flow in their normal directions optimal. This makes a polyhedral mesh better suited for cases with recirculation flows in comparison to a standard tetrahedral mesh.

Although a polyhedral mesh seems to be a new approach for engineers and offers great advantages, it may be that a structured hexahedral mesh still outmatches it when the elements align in the flow direction. In the study about falling jets mentioned in Sec. 2.1.2 the authors conclude that the mesh size has an effect on the air volume fraction but little effect on the velocity of the jet when compared to experimental results that utilized optical fibres to measure the flow (Castillo et al., 2013). It was found that the numerically calculated velocity is smaller than the real, which was explained by air-water friction not being accounted for by the numerical solver. The mesh structure used was hexahedral cells that was aligned with the direction of flow. Furthermore, in a study carried out by Nasif et al.(2014) it was concluded that a structured mesh is better in regions where it aligns with the jet flow and a polyhedral mesh is instead better where the flow pattern is more difficult to predict.

2.2 Experimental Studies

Pettersson and Pettersson (2011) conducted pressure and velocity experiments on a scale model of the Baihetan dam at Tsinghua University, Beijing. At the time, the construction of Baihetan dam had recently begun. The aim was to measure the hydrodynamic pressure in the plunge pool and to evaluate if it was within the specified limits. When elaborating with different setups of nappe splitters, which causes the jet to aerate and spread in a wider area and thus reducing shock pressure, the authors concluded that the setup of using two nappe splitters next to each other is the most favourable and that the maximum allowable impact pressure difference was well below the recommended value of 15 m. This is due to that the jets collide mid-air and scatters easier, and the discharge does not affect the dam in a threatening way. Though, the velocity of the downstream flow is high enough to risk the occurrence of erosion and the authors recommend further studies in this particular area.

Liu(2012) studied the hydrodynamic characteristics of a scale model of Baihetan dam, the same asPettersson and Petterssonused. Different top elevations of the secondary dam was tested (602, 604 and 606 MASL) and the flow characteristics were studied. The main result was that the submerged water jump increased as the height of the secondary dam increased. Another result was that the impact pressure decreased as the water cushion increased due to the increased top elevation.

2.3 Summary & Conclusions of Literature Review

A polyhedral mesh is considered to be superior over a tetrahedral one in almost all cases. In regions where the flow is dominant in only one direction a structured mesh is a better choice than a polyhedral. The best option would then be to use a combination of a structured hexahedral and polyhedral mesh, a hybrid mesh, to really capture the different flow regimes in an optimal way.

Furthermore, a polyhedral mesh is more numerically stable than a tetrahedral mesh due to its larger number of faces and neighbouring elements.

A large number of choices are available when it comes to the topic of choosing a suitable turbu- lence model. The literature review suggest that a Realizable k− ε provides adequate results while still providing smaller computational demands. The advantages it provides are: (1) It is a better predictor of the spreading rate of planar and round jets; (2) Superior performance over the standard k− ε regarding flows involving rotations, boundary layers under strong adverse pressure gradients, separation, and recirculation. Lönn and Dahl(2016) used a Realizable k−ε for modelling turbulence

(22)

and obtained good results for certain parameters. The failure to predict the lateral spread of the jet can most probably be attributed to the mesh not being refined enough.

Both Lönn and Dahl(2016) andRamqvist and Länsman (2017) presented a mesh convergence study, but failed to quantify the convergence in a recommended manner (relative error is generally not a good method). This suggests that the use of a grid convergence index (GCI), as proposed by Roache (1994), would provide a better means of reporting the grid convergence.

The experimental results shows that the plunge pool is within the specified limit of a maximum allowable impact pressure difference of 15 m. Furthermore, an increase of the top elevation of the secondary dam increases the surface re-flux, indicating that a submerged jump increases in strength.

(23)

Chapter 3 Mathematical Model

In this chapter the underlying theory that the methods are based upon will be presented. In more detail, ANSYS Fluent’s governing equations, the Volume of Flow (VOF) method, turbulence models, mesh structure and mesh quality will be presented here.

3.1 Governing Equations

Solving the Navier-Stokes equations directly is an impractical approach due to the heavy computational effort required. One more common approach, favoured by engineers, is to instead decompose an instantaneous quantity into a time-averaged component. The pressure- and velocity field is then decomposed as

p = ¯p + p^′, u_i= ¯u_i+ u^′_i. (3.1) Using the averaged components in Eq. (3.1), the Navier-Stokes equations can be written as:

∂

∂t+∂(ρ¯ui)

∂x_i = 0 , (3.2)

∂(ρ¯ui)

∂t +∂(ρ¯uiu¯j)

∂x_j =−∂ ¯p

¯ x_i + ∂

∂x_j [

µ (∂ ¯ui

x_j +∂ ¯uj

∂x_i −2 3δij

∂ ¯um

∂x_m )]

+ ∂

∂x_j(−ρu^′iu^′_j)) , (3.3) where δij is the Kronecker delta, and −ρu^′iu^′_j are the Reynold Stresses. Equation (3.2) and (3.3) are called Reynolds-averaged Navier-Stokes equations or shortly RANS equations. In order to reach closure of Eq. (3.3), the Reynolds stresses needs to be modelled. One common method is to use the Boussinesq hypothesis (Hinze, 1975), that relates the Reynolds stresses with the mean velocity gradients, as:

− ρu^′iu^′_j = µt

(∂ui

∂xj

+∂uj

∂xi

)

−2 3

( ρk + µt

∂ui

∂xi

)

δij. (3.4)

The realizable k−ε model that was chosen for this study is an extension of the standard k −ε model formulated by Shih et al. (1995). It still uses the eddy viscosity approach to model turbulence, but it is more accurate in almost all cases of turbulent flow. The new transport equation for the dissipation rate ε is expected to enhance the numerical stability in turbulent flow calculations. Just like the standard k− ε model, it is a two-transport equation, one for the turbulent kinetic energy k, and one for the turbulent dissipation ε. The equations for the transported variables are:

∂

∂t(ρk) + ∂

∂x_j(ρkuj) = ∂

∂x_j [(

µ + µt

σ_k ) ∂k

∂x_j ]

+ Gk+ Gb− ρε − YM + Sk, (3.5)

(24)

and

∂

∂t(ρε) + ∂

∂xj

(ρεuj) = ∂

∂xj

[(

µ + µt

σε

) ∂ε

∂xj

]

+ C1Sε− ρC2

ε² k +√

νε+ C1ε

ε

kC3εGb+ Sε, (3.6) G_k and Gb represents the generation of turbulence kinetic energy from mean velocity gradients and buoyancy, respectively. The constants C1, η and S are defined as:

C₁= max [

0.43, η η + 5

]

, η = Sk

ε, S =√

2S_ijS_ij, (3.7)

σk and σε are the turbulent Prandtl numbers for k and ε, and by default have the values σk = 1.0 and σε= 1.2. The constants C_1ε and C2 are empirical constants set to 1.44 and 1.9, respectively.

Similar to the standard k− ε model, the eddy viscosity µtis computed from

µt= ρCµ

k²

ε . (3.8)

Unlike the standard k− ε model, Cµ is not a constant. Instead it is a function of mean strain, rotation rates, angular velocity of the systems rotation and the transported variables k and ε.

3.2 Discretization

ANSYS Fluent employs a discretization technique called the Finitive Volume Method (FVM). The cells that makes up the mesh can be of any computational arbitrary polyhedral shape. Furthermore, Fluent stores discrete values of the scalar ϕ at the center of each cell in the computational domain.

The discretized general transport equation of a given cell is expressed as:

∂ρϕ

∂t V

| {z }

transient term

+

N∑_{f aces}

f

ρf⃗vfϕf· ⃗Af

| {z }

convection term

=

N∑_{f aces}

f

Γϕ∇ϕf· ⃗Af

| {z }

Diffusion term

+ SϕV

|{z}

Source term

, (3.9)

where

ρ = density ,

⃗v = velocity vector , A = Surface area vector ,⃗ Γ_ϕ= diffusion coefficient for ϕ ,

∇ϕ= gradient of ϕ , Sϕ= Source of ϕ per unit volume .

In order to compute the convection term in Eq. (3.9) that accounts for the transport of ϕ due to a velocity field, the face values ϕf are needed. The face values are thus interpolated values from the cell center. This is accomplished using a second-order upwind scheme, where upwind means that ϕf is calculated ”upstreams” and normal to the velocity field. A second-order upwind scheme generally yields better accuracy than a first-order scheme, but its disadvantages is that problem with convergence can occur (Casey et al.,2000). First-order schemes are however useful for conducting a mesh independence study.

Computing the gradients is required in order to solve for the diffusive term, and velocity gradients, in Eq. (3.9). FLUENT provides three approaches; Green-Gauss Cell-Based, Green-Gauss Node- Based and Least-Squares Cell-Based. The latter mentioned is the default option of the three, and is considered to produce the best results if a polyhedral mesh is used according toANSYS^® Fluents 6.3 user guide.

(25)

CHAPTER 3. MATHEMATICAL MODEL

3.3 Volume of Fluid (VOF) Method

The VOF method (Hirt et al.,1981), available in ANSYS Fluent, is a surface tracking technique that is common to use whenever the fluids of interest are considered to be immiscible, i.e they do not form a homogeneous mix. Common applications of the VOF methods include modelling of free-surface flows, prediction of jet breakup etc. The VOF methods works by assigning each phase a volume fraction that sums to unity in a cell. Mathematically this is expressed as

∑n q=1

α_q = 1 . (3.10)

Each cell in the computational domain is assigned averaged material properties given what ratio of phases the cell consists of, e.g ρ =∑

αqρq. The VOF method accomplishes surface tracking by solving a momentum equation

∂αq

∂t + ⃗v· ∇αq = 0 (3.11)

for each phase q. Moreover, a single momentum- and transport equation is solved, and the resulting velocity field and turbulent quantities is shared by all the phases.

3.4 Grid Convergence Index (GCI)

Numerical simulations are inherently sensitive to errors due to discretization. As such, there exists a need to quantify the convergence of a particular solution. Roache(1994) proposed the use of a Grid Convergence Index (GCI) as a useful method for reporting grid refinement studies. The GCI can be thought of as an estimate of the discretization error relative the converged numerical results. The theory is based on Richardson Extrapolation, and requires the user to analyze the solution using three grid resolutions: Fine, medium and coarse. The GCI on the fine grid is computed from:

GCIf ine= Fs|ε|

r^p− 1, (3.12)

where r is the grid refinement ratio, ε is the relative error defined as ε =^(f²^{− f}¹⁾/f₁and Fsis a safety factor that, according to Roache, should range from 1.25 ≤ FS ≤ 3. The term p is the order of convergence, and for three solutions obtained with a constant grid refinement ratio, and is computed using

p = ln((f₃− f2)/(f₂− f1))

ln(r) , (3.13)

where f is a quantity of interest, e.g. pressure recovery, and is computed over the three grids, fine, medium and coarse.

It is also important that each of the solutions for a given grid is in the asymptotic range of convergence. This is simple to check by using the observed GCI that was obtained using three different grids and using Eq. (3.14) below

GCI₂₃= r^p· GCI12. (3.14)

Under the constraint that all solutions are in the range of asymptotic convergence, i.e ^r^p_GCI^·GCI¹²

23 ≈ 1, one can estimate the solution at an infinitely fine grid using Richardson Extrapolation. Assuming that the solution is of second order, one can calculate it using:

f (x, y, z, t)exact∼= f1+f1− f2

r^p− 1 , (3.15)

where f (x, y, z, t)exactis the estimation and f1 represents the value obtained using a finer mesh.

(26)

3.5 Mesh Quality Control

The accuracy of the solution is not only dependent on the grid spacing of the mesh, but also the on the quality of each cell. Furthermore, the stability of the solution can be compromised if the mesh is of low quality, and reaching convergence can become problematic. A multitude of options exist regarding the criteria for a quality mesh. The most important ones, and the ones used in this study are Face Squish Index, skewness and Orthogonal Quality. This study will focus on the use of a combination of polyhedral and quadrilateral elements and, depending on the type of mesh, different criteria applies to different mesh types and, according to ANSYS^® User’s guide, face squish only applies to polyhedral elements and is defined as

1− A⃗i· ⃗rc0/c1

| ⃗Ai||⃗rc0/c1|. (3.16)

A Face Squish Index (FQI) of 0 is considered the best, and an index of 1 is considered the worst.

Another type of criterion is skewness, of which there exist two types: Cell Equivolume Skew and Cell Equiangle Skew. The latter mentioned is applicable to all cell shapes and faces and is defined as:

skewness = max

[θmax− θe

180− θe

,θe− θmin

θ_e ]

, (3.17)

where θe = 90° for quadrilateral elements, and θe = 60° for tetrahedals. Just as for the FQI, 0 is considered to be perfect, and 1 is the worst. One important criteria, that applies to all types of elements, is the Orthogonal quality of a cell. Mathematically, the orthogonal quality is computed from:

Orthogonal Quality = min

[A⃗_i· ⃗fi

| ⃗A_i|| ⃗fi|, A⃗_i· ⃗ci

| ⃗A_i||⃗ci| ]

, (3.18)

where ⃗A_i is the area vector of a face, ⃗f_i and ⃗ci are vectors from the centroid of the cell, where ⃗f_i goes to the centroid of the same face that the particular area vector was computed from and ⃗ci goes to the centroid of the adjacent cell that shares the same face as the area vector. As expressed in Eq. (3.18) the minimum quantity is the orthogonal quality, where a value of 1 is considered the best, and value of 0 is considered the worst. When deeming the final quality of a given mesh it is important to consider all of the three options when trying to asses the quality of a mesh.

(27)

Chapter 4 Method

The approach of the work process is described thoroughly in this chapter as well as a detailed look at the modelled geometry and meshing technique.

4.1 Structure of the Work Process

In order to prevent as much errors in the simulations as possible, and therefore saving time, the approach of this work is divided into sections of process steps. This implicates e.g. construction of the model and running simulations piecewise in order to correct small errors that may occur instead of modelling the geometry as a whole at once. Figure 4.1 shows an example of how the working process was set up.

Figure 4.1. A flowchart describing the methodology of the work process.

4.2 Modelling the Geometry

The blueprints of the Baihetan dam were carefully studied in order to model the geometry of the reservoir, spillways, jet trajectory and the plunge pool. The software used to construct the models was Siemens NX 12, a powerful CAD software capable of creating assemblies. The spillways modelled in this study are number 1 and 6, which are the outer surface spillways on either ends of the array of surface spillways, see Fig. 1.5. They were the first components of the assembly to be constructed since it would simplify the design of the reservoir and the jet trajectory bodies, both of which are directly connected to the spillways. The crests of the spillways have the same elliptic shape in the form of:

x²

5.37²+(3.08− y)²

3.08² = 1 , (4.1)

which then proceeds into a slope with a 15° decline. The spillways were divided into four sections so that meshing would be easier, see Fig. 4.2. The difference between the two spillways is that the slope of spillway 6 is 3.02 m further in the longitudinal direction and causing its orifice to be wider

(28)

810.00

800.61 834.00

15°

60m

(a) Spillway 1 side view.

799.01 15°

(b) Spillway 6 side view.

17.26m

46.37 m

(c) Spillway 1 top view.

17.57m

49.39 m

(d) Spillway 6 top view.

Figure 4.2. Top- and side views of the surface spillways. All units are in MASL unless otherwise stated.

To simulate the inflow of water to the spillway more accurately, it was chosen to include the upstream reservoir in the model. To save computational time by reducing the amounts of elements, the reservoir was split into two independent bodies connected to a spillway. In Fig. 4.3 a spillway is seen together with a reservoir and the jet. The final shape of the jet trajectory body is shown in Fig. 4.3. Its shape enables the meshing software to create a good structured hexahedral mesh grid with high quality elements that aligns with the trajectory of the falling jet, as well as reducing the total amount of elements by removed dead space. The width and the angle of the jet body was found through a trial and error type of manner since no a priori information but the approximate longitudinal distance the jet would travel, was available regarding the falling water’s behaviour. This means that the final body captures the whole jet and its lateral spread until it impacts the plunge pool.

(29)

CHAPTER 4. METHOD

158m

60 m 56 m

60m

110°

Figure 4.3. Reservoir, spillway and jet trajectory body shown in one assembly. The final shape of the jet trajectory body was modelled through trial and error.

The cross-section of the plunge pool was created using Fig. 1.3 as blueprint. In Fig. 4.4 the finished spline is shown together with important measurements

164 m 140 m

106 m 68

49m

Figure 4.4. Cross sectional view of the plunge pool in its original design.

The plunge pool was divided into four sections along the longitudinal direction, see Fig. 4.5. The main reason for this approach is due to certain regions in the plunge pool exhibits low turbulence and velocities. The only region that requires a finer mesh is the impact region (2) so that the necessary characteristics and pressure patterns on the floor of the plunge pool is accurately captured. There was also the need for a different type of mesh than hexahedral elements at the end of the plunge pool where the secondary dam crest begins, since the meshing software was not capable of generating such a grid because of the slope.

(30)

400 m

46m

60m

121°

1 2 3 4

Figure 4.5. Longitudinal view of the plunge pool divided in 4 sections. Notice that the height of the secondary dam is 46 meters, which is the original height.

Figure 4.6 shows the complete assembled model. The layout of the spillways relative to each other and the plunge pool was modelled using Fig. 1.4 as reference. Once again, it is worth mentioning that the jet trajectory body is not from a blueprint, but instead was modelled trough trial and error to find the correct volume that would create a computational domain that included the whole jet.

Figure 4.6. Isometric view of the whole model geometry.

4.3 Mesh

The software used for meshing the domain was Gambit v. 2.4.6. Hexahedral elements were used in the reservoirs, spillways and jets (Fig. 4.7). The slope of the mesh was modelled such that the elements would align with the flow direction.

(31)

CHAPTER 4. METHOD

Figure 4.7. Hexahedral mesh of the reservoir, spillway and jet combined.

The plunge pool, see Fig. 4.8, was divided into four sections with the intent of decreasing computational time. Preliminary testing indicated that fewer elements were needed upstream and downstream of the impinged jets due to low velocities and turbulence. The impact region and the region adjacent to the secondary dam was assigned with tetrahedral elements that later were converted into polyhedral elements in Fluent.

Figure 4.8. Sideview of the plunge pool’s mesh.

The quality of the mesh, as reported by Fluent, was

• Minimum Orthogonal Quality = 0.31

• Maximum Skewness = 0.68

• Face squish = 0.68

(32)

which is an acceptable level of quality. The most problematic area of the mesh is concentrated to where the spillway crest is connected to the reservoir.

4.4 Boundary Conditions

The boundary conditions was set up in Gambit prior to exporting the mesh to Fluent. A velocity inlet was used to specify the inlet flow. In Fig. 4.9 the velocity inlet, interior faces and pressure outlet is shown in light grey, green and red respectively.

Figure 4.9. Boundary condition locations as specified in Gambit.

To calculate the proper inlet velocity of the water it was derived by using the total volumetric flow V given in Tab.˙ 1.3, number of inlets n and a single inlet area A (given that the area of the inlets are equal) according to:

V = A˙ inlet· u · n ⇒ u = V˙

A_inlet· n (4.2)

where the total mass flow ˙V = 3149 m³/s, Ainlet = 3486.5 m² and n = 2. Following the guidelines in Fluent, the velocity inlet was specified as ”intensity and hydraulic diameter” since the flow upstream can be considered fully developed. The turbulence intensity was set to 1% and the hydraulic diameter was calculated according to:

D_h= 4ab

2a + b (4.3)

where a is the width of the reservoir and b is the height. All the top faces, including the jet stream, was specified as pressure inlets. In Fig. 4.10 the pressure inlets are shown in light grey.

(33)

CHAPTER 4. METHOD

Figure 4.10. The locations of the pressure inlet boundary condition as specified in Gambit.

Gambit, by default, marks unassigned faces as wall, which means that the rest of the geometry have wall boundary conditions. No custom settings were used at the wall boundaries, all settings were left as default in Fluent.

4.5 Solver Settings

In Fluent the VOF module was used to model the multiphase flow. Since large body forces is present, due to gravity, the Implicit body forces was used in the VOF module. For turbulence closure the realizable k− ε model was used and the Near-wall treatments was set to standard.

In solution methods the SIMPLE scheme was used for Pressure-velocity coupling. As for the spatial discretization, Least Squares Cell Based was used for the gradient at the faces, the momentum equations was discretized with a second order upwind scheme and the turbulent kinetic energy and turbulent dissipation rate was discretized using a first order scheme. The pressure discretization used was PRESTO! since it is default whenever using the VOF module.

Under-relaxation factors was left to default. The maximum turbulent viscosity ratio was set to 1e6 since preliminary testing showed that the default value of 1e5 was insufficient since it occurred in many cells. The timestep used in all calculations was 1e-2 s. For the convergence criteria all residuals was set to 10⁻³.

The hardware used for the simulations was a desktop computer with 128 Gb ram, Intel Xeon 3100 3.6 GHz with a total of 24 cores.

(34)

Numerical Results & Discussion

In this chapter the mesh independence study is presented together with validation against experimental data. Moreover the velocity field, turbulent dissipation rate and water level fluctuations in the plunge pool is examined and discussed.

5.1 Convergence Analysis

The convergence analysis of the mesh is divided into two separate sections, one for the jet and one for the plunge pool. For simplicity spillway number six was assumed to behave similarly to changes in the mesh as spillway number one since the geometries of the jet bodies are identical. Therefore the mesh independence was only carried out for spillway one. Moreover, the different element sizes that were tested was 1.5, 1.25 and 1 m. The quantities that were studied was the longitudinal distance of the jet, the velocity and the air volume fraction

In the mesh convergence analysis of the plunge pool one parameter was studied, the vertical velocity profile downstream of the jet. The impact zone, labeled 2 in Fig. 4.5, was the only zone that was decreased in mesh size from 2.25 m, 2.0 m and 1.75 m. The remainder of the zones had a mesh size of 4 m, since inital testing showed that the velocity, and turbulence, was low in these domains.

5.1.1 Mesh Independence of Jet

Three key characteristics of the jet was studied during the mesh sensitivity analysis: (a) the trajectory and impact location of the center streamline of the jet, (b) aeration and disintegration of the jet, (c) the velocity of the jet during its ascent. The jets final impacting position and trajectory from the spillway exit is shown in Fig. 5.1, where it is seen that the finest mesh of 1 m impinges the jet farthest, 94.4 m from the spillway exit. The total number of elements used with the finest mesh size of 1 m was 537k elements in the jet trajectory. All trajectories in 5.1 begins at the spillway’s exit, which was set at a height of 0, and the jet was considered to have completed its vertical ascent when the jet impacted the water surface.

(35)

CHAPTER 5. NUMERICAL RESULTS & DISCUSSION

0 10 20 30 40 50 60 70 80 90 100

−150

−100

−50 0

Longitudal Distance x [m]

FallingDistancez[m]

Trajectory

1.5 m 1.25 m 1 m

Figure 5.1. Length of jet trajectory for different mesh sizes.

The mesh was not refined after 1 m, since it would generate a considerable amount of elements hence increasing the computational time even more.

During mesh sensitivity analysis of the jet it was noticed that the finest mesh produced the longest jet core and disintegrated later than with coarser mesh. In Fig. 5.2 the air volume fraction in the falling jet for different mesh sizes is shown. For simplicity, it was considered that the jet had started to disintegrate whenever the air volume fraction started to oscillate violently indicating that the jet consists of blobs of water. It is clear from 5.1 that with a mesh size of 1.5 m the jet is fully developed after a vertical fall of almost 90 m since the air volume fraction begins to fluctuate while the finest is fully developed after roughly 120 m vertical fall. This result shows that the air volume fraction is very sensitive for changes in the mesh size. A mesh size of 1 m was still considered to be a minimum limit due to the increasing computational time that will extend longer than the projects deadline.

(36)

0 0.1 0.2 0.3 0.4 0.5 0.6 0.7 0.8 0.9

−120

−100

−80

−60

−40

−20 0

Air volume fraction [-]

FallingDistancez[m]

Volume fraction

1.5 m 1.25 m 1 m

Figure 5.2. Comparisons of the air volume fraction for different mesh sizes. Violent fluctuations in air volume fraction indicates that the jet has started to break apart.

The mesh independence study showed that the velocity was nonsensitive for changes in the mesh size (Fig. 5.3), which is in correlation with the mesh independent results of Castillo et al. (2013).

The only difference is for the 1.5 m mesh since it has a drop in velocity the moment when the jet exits the spillway and starts its descent. A probable cause of this could be that the rougher mesh of 1.5 m is not sufficient to capture the interface between the spillway and the jet body.

0 10 20 30 40 50 60 70

−150

−100

−50 0 50

Velocity [m/s]

FallingDistancez[m]

Velocity

1.5 m 1.25 m 1 m

Figure 5.3. The jets velocity during its vertical ascent down from the crest.

Hydrodynamic Characteristics of the Baihetan Plunge Pool