CFD modelling of ski-jump spillway in Stornnforsen

CFD modelling of ski-jump spillway in Storfinnforsen

CFD-modellering av utskov med str˚ alupplyftare vid Storfinnforsen

Thesis project for the degree Master of Science Simon Eklund

Royal Institue of Technology

Sweden

December 23, 2016

Abstract

Traditionally when designing dams and spillways, experiments in physical scale models are conducted in order to determine whether or not the design fulfils it purpose, and to identify and avoid undesired problems, such as unfavourable flow patterns and unwanted water splatter. Physical models can often be expensive and time consuming to build, and often suffer from scale effects that influence the results.

Uniper and Vattenfall have recently done experiments in a physical 1:50 scale model of the dam Storfinn- forsen, in order to test new solutions for the energy dissipation from the spillways. One of the tested solutions is a flip bucket at the bottom of the right surface spillway.

In this project the same solution is numerically modelled, using the CFD software ANSYS ^® Fluent ^® , and the results are compared to those from the experiments. The CFD simulations are done both in full scale and model scale, in order to identify potential scale effects. The aspects that are compared are the height and length of the jet from the flip bucket.

In addition to the CFD simulations, the height and length are also calculated semi-empirically, using two different methods.

Altogether the results correspond quite well to the experimental values. Some possible scale effects are observed, where the jet from the full scale simulation is more dispersed than the jet from the model scale simulation. The jet trajectory from the full scale simulation is also a bit lower than the jet from the experiments and model scale simulations.

The grid independence for the simulations is not quite satisfactory, and the grid should be refined to get

more reliable results. Due to lack of time and computational power any further grid refinement is not

done in this project.

Acknowledgements

Firstly I would like to thank Vattenfall and Uniper for making this master thesis project possible.

I would also like to thank James Yang at Vattenfall R&D for arranging this project, and Carl-Oscar Nilsson at Uniper for arranging the study visits to Storfinnforsen and Uniper’s office in Sundsvall.

I also thank Penghua Teng at Vattendragsteknik at KTH for his guidance throughout the project, and

my examiner Anders Ros´ en at the Centre for Naval Architecture at KTH for support and guidance

throughout the project.

Nomenclature

Symbol Description Unit

ρ Density [kg/m ³ ]

t Time [s]

~

u Velocity vector [m/s]

p Pressure [P a]

µ Dynamic viscosity h

kg s·m

i

I Unit tensor [-]

~ g Gravitational acceleration [m/s ² ]

F ~ External body forces [N ]

ν Kinematic viscosity [m ² /s]

Re Reynold’s number [-]

κ Turbulent kinetic energy [m ² /s ² ]

 Turbulent dissipation rate [m ² /s ³ ]

λ Scale factor [-]

V Inlet velocity for full scale model [m/s]

V m Inlet velocity for scale model [m/s]

x Horizontal coordinate [m]

y Vertical coordinate [m]

x 1 Length of the jet (Method 1) [m]

y 1 Height of the jet (Method 1) [m]

x ₂ Length of the jet (Method 2) [m]

y ₂ Height of the jet (Method 2) [m]

θ Angle of the flip bucket lip [rad]

k Constant related to air resistance [-]

V ₀ Velocity at the flip bucket lip [m/s]

d Depth of the flow at the flip bucket lip [m]

h v Velocity head at the flip bucket lip [m]

˙

m Mass flow rate [kg/s]

w Width of the spillway [m]

h Distance between the spillway crest and the retention water level [m]

h 0 Height at the flip bucket lip [m]

h 1 Height at the spillway crest [m]

CFD Computational Fluid Dynamics

DNS Direct Numerical Simulation

RANS Reynolds-Averaged Navier-Stokes equations

VOF Volume of Fluid

Contents

1 Introduction 1

2 Experiment 3

2.1 Scaling . . . . 4

2.2 Measurements from the physical model . . . . 5

3 Theory 7 3.1 Governing equations . . . . 7

3.2 Turbulence model . . . . 7

3.3 Volume of Fluid (VOF) model . . . . 8

4 Numerical setup 9 4.1 Computational domain . . . . 9

4.2 Boundary conditions . . . . 9

4.3 Setup in Fluent . . . . 10

4.4 Convergence and grid generation . . . . 11

4.5 Generation of results . . . . 12

5 Semi-empirical calculations of height and length of the jet 14 6 Results 17 6.1 Mass flow rate . . . . 17

6.2 Height of the jet . . . . 18

6.3 Length of the jet . . . . 23

7 Discussion and conclusions 29

Chapter 1

Introduction

When designing dams, a large part of the process is to build models and do model tests. This is done in order to test if the design will fulfil its purpose, and to identify and avoid hidden undesired problems, such as unfavourable flow patterns and unwanted water splatter.

Traditionally physical models have been used to perform model tests, and have for a long time been the most efficient way. Nowadays when the computers are faster than ever the alternative to perform similar model tests using Computational Fluid Dynamics (CFD) is becoming more and more relevant.

An advantage of a CFD model compared to a physical model is that it does not suffer from any scale effects, as a physical model often does. CFD modelling can possibly also be cheaper than physical model test.

There is currently an ongoing project at the dam Storfinnforsen, with the aim to increase the safety and stability of the dam. Storfinnforsen is located in Fax¨ alven in Sweden. The construction of the dam was completed in 1954. It has an annual production of 536 GWh, which would be sufficient to provide about 20000 households with electricity for one year. An overview of Storfinnforsen is shown in Figure 1.1.

Figure 1.1: Storfinnforsen.

A physical hydraulic model of Storfinnforsen has been built in ¨ Alvkarleby by Vattenfall, so that different

design solutions for improving the energy dissipation can be examined. In this project a potential solution

for the right surface spillway is investigated, using CFD. When the simulations are done, the results are

compared to already existing experimental data from the physical hydraulic model, and pros and cons

of each method are discussed.

The potential solution that is investigated in this project is a flip bucket at the bottom of the spillway.

The improvement this flip bucket could result in is that it lifts the water to form jet that reaches the ground at some distance downstream of the dam, in order to avoid erosion on the base of the dam.

Another effect this flip bucket could have is a decrease in downstream velocity, and thus reduce the erosion in the downstream river bed. The hydraulic model with the flip bucket is shown in Figure 1.2.

Figure 1.2: Hydraulic model of the spillway, with the flip bucket.

The parameters that are investigated in this study are the water mass flow over the spillway crest, and the height and length of the jet.

The software used for the CFD simulations is ANSYS ^® Fluent ^® . The geometries are created in ANSYS ^® DesignModeler ^TM , and the meshing is done with ANSYS ^® Meshing ^TM

The content in this thesis includes:

• A short summary of the theory behind the CFD model, and its sub models.

• Setup and boundary conditions in the CFD model.

• Convergence study.

• Summery of the results, and comparassion between the physical scale model and the CFD model.

• Discussion of resluts, possible limitations and errors, and suggestions for improvement.

Chapter 2

Experiment

The physical hydraulic model in ¨ Alvkarleby was built in scale 1:50. The model include approximately 100 m of the upstream reservoir, and 400 m of the downstream riverbed, where also the topography is modelled. An overview of the model is shown in Figure 2.1.

Figure 2.1: An overview of the physical model, seen from the downstream end of the riverbed.

As mentioned in the introduction, it is the right surface spillway with a flip bucket that is investigated

in this project. The cross section of this spillway with the flip bucket is shown below in Figure 2.2 and

2.3. The width of the spillway is 20 m.

Figure 2.2: Cross section of the spillway, [mm].

Figure 2.3: Detail A.

2.1 Scaling

The model is built according to the Froude Number Law [1], also called the Froude law of similarity

[2]. The Froude Number Law states that for flow situations, such as this case, where the inertial forces

and gravity forces are the only dominant forces, the Froude number of the scale model and the full

scale prototype should be kept equal. When the same fluid is used in both the scale model and the prototype, and when both are subjected to the same gravitational field, scale ratios for many important physical quantities can be derived from the Froude Number Law. The scale ratios for the most important quantities in this case are presented in Table 2.1.

Table 2.1: Scale ratios for the Froude Number Law Physical quantity Scale factor

Length λ

Area λ ²

Volume λ ³

Time λ ^1/2

Velocity λ ^1/2

Discharge λ ^5/2

When using this type of scaling some inevitable non-similarities between the model and the prototype occur. These non-similarities are called scale effects and are further explained by Novak et al. [2]. In this case possible scale effects can occur from e.g. the fact that the Reynold’s number is smaller in the model compared to the prototype if the same fluid is used in both the model and the prototype. This can lead to less turbulence in the model compared to the prototype. A phenomenon which has been observed in other free-surface flow situations and is presented in several articles by Hubert Chanson and others, see for example [3], [4]. The latter also states an underestimation of air-entrainment in scale models.

2.2 Measurements from the physical model

In the experiments in the physical model, the flow is three-dimensional, which is not the case for the simulations. This might cause some differences in the results. For example, in the physical model, the length in the middle of the jet is different from the length on the sides. On the sides, the flow is affected by the walls, and water flowing over the sides of the flip bucket, see Figure 2.4. The flow case in the simulations represent the middle part of the jet. Therefore the results from the simulations are compared the measurements from the middle of the jet.

Figure 2.4: Water jet in the physical model.

The length of the jet is measured from the downstream vertical edge of the flip bucket, to where the

upper side of the jet hits the river bed. The height is measured as the vertical distance from the upper

edge of the flip bucket to the upper side of the jet, at 25 m downstream of the vertical edge of the flip bucket. See Figure 2.5 for a schematic description of how the height and length are measured.

Figure 2.5: Schematic description of how the height and length are measured in the physical model.

Chapter 3

Theory

This chapter introduces the basic equations for fluid motion, and gives a short introduction to the models used in this case when modelling a turbulent two-phase flow.

3.1 Governing equations

The governing equations of viscous fluid motion are the Navier-Stokes equations. They consist of the equations describing conservation of mass, conservation of momentum and conservation of energy. Since heat transfer and compressibility are assumed to be negligible in this flow case the equation for conser- vation of energy is not solved. The equations for conservation of mass (3.1) and momentum (3.2) can be written as

∂ρ

∂t + ∇ · (ρ~ u) = 0 (3.1)

∂

∂t (ρ~ u) + ~ u · ∇~ u = −∇p + ∇ · (µ((∇~ u + ∇~ u ^T ) − 2

3 ∇ · ~ uI)) + ρ~ g + ~ F , (3.2) where I is the unit tensor and ~ F is external body forces. Since the flow is assumed to be incompressible, and there are no other external forces than gravity, these equations can be simplified to

∇ · ~ u = 0 (3.3)

∂

∂t (~ u) + ~ u · ∇~ u = − 1

ρ ∇p + ∇ · (ν(∇~ u + ∇~ u ^T )) + ~ g. (3.4)

3.2 Turbulence model

Turbulent flows are characterized by fluctuations in the flow field quantities, and are highly non-linear.

There is no exact definition of turbulence. A simple definition of turbulence according to [5] is ”a dissipative flow state characterized by nonlinear fluctating three-dimensional vorticity”.

The governing equations can quite easily be solved with Direct Numerical Simulation (DNS) for simple

laminar flows where the Reynolds number, Re, is relatively low. As the Reynolds number increases, and

the flow starts to become turbulent, the CPU-time scales as Re ³ [6]. This means that it is not very

practical, in an engineering point of view, to simulate turbulent flows with high Reynolds number using

DNS. In most engineering applications however a time-averaging proceedure of the equations is applied,

resulting in the Reynolds-Averaged Navier-Stokes (RANS) equations. The averaging process introduces

additional terms to the governing equations, these terms need to be provided by suitable turbulence

models in order to close the RANS equations.

In this project the realizable k− model is used. The k− model is the most common turbulence model in engineering applications. The realizable k − model is the recommended variant of the k − family [7],[8].

The realizable κ −  model is like the standard κ −  model a two-equation model, which by solving two separate transport equations, one for the turbulent kinetikc energy κ and one for its dissipation rate , provides a turbulent length and time scale. The main differences between the standard and the realizable κ −  model are that the realizable κ −  model uses an alternative formulation for the turbulent viscosity, and a modified transport equation for the dissipation rate .

3.3 Volume of Fluid (VOF) model

To model flows with two or more fluid phases some sort of multiphase model is needed to track the

surface between the different phases. There are different types of multiphase models, and for this type

of simulations the Volume of Fluid (VOF) model is most suitable [9],[8]. The VOF model is tracking the

interfaces between different phases by solving a continuity equation for the volume fraction of one (or

more) of the phases. In this case there are only two phases, water and air. Water is set as the primary

phase, and therefore only one volume fraction continuity equation for air is solved. Each cell can be

either filled with air (volume fraction is 1), filled with water (volume fraction is 0) or contain a mixture

of both phases ( volume fraction between 0 and 1). The volume fraction for water can be obtained from

the constraint that the sum of all volume fractions in one cell equals 1.

Chapter 4

Numerical setup

This chapter describes the procedure to create the CFD model, and running the simulations. The way of measuring in the simulation model is explained.

4.1 Computational domain

The CFD simulations are made both in full scale, and in 1:50 scale. The reason for this is to be able to observe possible scale effects, and to see which model that corresponds better to the physical model tests. All simulations are made in 2D, and not in 3D, in order to reduce the computational time. The domain is 230 m long in total, 100 m upstream and 130 m downstream of the crest. The maximum height of the domain is 36 m. Since the river bed downstream of the spillway is quite rough it is difficult to model it in 2D, therefore a constant slope at 5.7% is assumed. An overview of the domain is shown in Figure 4.1.

Figure 4.1: Overview of the computational domain.

4.2 Boundary conditions

At the inlet boundary a constant velocity, V , of 0.68 m/s is assigned for the water phase. This velocity was calculated from the mass flow rate through the spillway given by Vattenfall [10]. At the part of the inlet where there is air, the velocity is set to 0. The bottom boundary is a wall with a no-slip condition. The top and outlet boundaries are defined as pressure inlet and pressure outlet respectively, with constant atmospheric pressure at both boundaries.

For the model scale simulations, the dimensions and the inlet velocity are calculated according to the Froude Number Law [1], which was briefly explained in chapter 2. For example the inlet velocity in the model scale simulations, V m , is calculated as

V _m = V

λ ^1/2 → V m = 0.68

50 ^1/2 ≈ 0.0954 (4.1)

The different boundaries are shown in Figure 4.2.

Figure 4.2: Computational domain with boundaries.

For all boundaries, except for the bottom, the turbulence parameters need to be defined. The choice of method for doing this is by defining the turbulent intensity and turbulent viscosity ratio. At the inlet the turbulent intensity is set to 1%, and the turbulent viscosity ratio is set to 1, since there is almost no turbulence in the reservoir where the inlet is located. Also at the top boundary the turbulence is very low, so the same values are applied here. At the outlet the turbulence a little higher, so the turbulent intensity is set to 2%, and the turbulent viscosity ratio is set to 2. These values are not scientifically calculated, they are based on recommendations from the tutor.

4.3 Setup in Fluent

The setup in Fluent is based on recommendations in the Fluent Documentation [8].

In these simulations the pressure-based solver is used. This is the only option when using the VOF multiphase model, which is the most suitable multiphase model for this type of flow, and is briefly explained in chapter 3. When modelling this type of flow, a transient simulation is needed, since the flow is time dependent. The flow is driven by gravity, and therefore a gravitational acceleration of 9.81 m/s ² is applied.

The VOF multiphase model is set up with implicit body force formulation. This can give a more robust solution and better convergence, especially for flows involving gravity, as in this case. The explicit volume fraction scheme is used, since this is recommended when simulating jets. An implicit scheme could be better when looking for a steady-state solution, and the intermediate transient behaviour is not of interest, but that is not the case. Water is set as the primary phase. The surface tension is modelled with the Continuum Surface Force model, and is set as a constant value of 0.072 N/m.

The operating pressure is set to 101325 Pa, and the reference pressure point is set above the water surface, where there is only water all the time. The operating density is set as 1.225 kg/m ³ (density of air).

The discretization schemes used are shown in Table 4.1.

Table 4.1: Computational setup Discretization schemes

Pressure-Velocity Coupling PISO

Gradient Least Squares Cell Based

Pressure PRESTO!

Momentum Second Order Upwind

Volume Fraction Geo-Reconstruct Turbulent Kinetic Energy Second Order Upwind Turbulent Dissipation Rate Second Order Upwind Transient Formulation First Order Implicit

For the pressure-velocity coupling, the PISO scheme is used. This is recommended for all types of

transient flows. The PISO scheme allows for larger under-relaxation factors, without any loss of stability,

which speeds up the simulations.

The gradients are computed using the least squares cell-based gradient evaluation method, which gives similar or better accuracy than the other available methods, while it is less computationally expensive.

This is the default method in Fluent.

The PRESTO! scheme is set as the pressure interpolation scheme. When using the VOF multiphase model, either the PRESTO! scheme or the body-force-weighted scheme should be used. PRESTO! is the default scheme for the VOF model.

For momentum, turbulent kinetic energy and turbulent dissipation rate the second-order upwind scheme is used. This scheme gives less numerical discretization error (numerical diffusion) than the first-order upwind scheme, especially in a case like this, when the flow is not always aligned with the grid. There are other schemes that may provide better accuracy for special cases as swirling or rotating flows, but in this case the second-order upwind scheme is sufficient.

For the spatial discretization of the volume fraction the Geometric reconstruction scheme is used, which is the most accurate scheme. It is important to get a correct shape of the interface between water and air in order to get good measurements of the jet.

For the transient formulation, the first order implicit scheme is used. Even though the second order implicit scheme, or the bounded second order implicit scheme would provide better accuracy, the first order scheme is considered to be sufficiently accurate in this case.

The under-relaxation factors are kept at default for all simulations, since this seems to give the fastest convergence.

For the full scale simulations the initial values for the solution are computed from all zones, and in the model scale simulations the initial values are computed from the water inlet. Both these initialization methods give the same result when the mass flow rate over the spillway crest becomes stable. Both methods are tested in order to find out if one or the other method gives a ”steady” jet faster. For both cases the volume fraction of air is initialized as 1, and after the initialization a region of water is patched in the reservoir, see Figure 4.3.

Figure 4.3: Initial state with patched water (blue) in the reservoir.

A variable time stepping method is used, where the first 100 time steps are fixed at 0.00001 s, in order to avoid convergence problem in the impulsive beginning of the simulation. After the first 100 time steps the step size is allowed to gradually increase to 0.0002 s for the full scale simulations, and 0.0001 for the simulations in model scale. This gives a good convergence for all the three grid sizes for each case (the residuals for all equations are below 0.001 at every time step).

4.4 Convergence and grid generation

To get a good solution when doing CFD-simulations, it is important to check that the solution converges.

The first step is to check residuals for the equations for continuity, velocity, κ and . A standard convergence criterion is that these residuals is kept below 10 ⁻³ for each time step. This criterion will be used for all simulations in this study.

The next step to reach good results from the simulations is to create a grid/mesh that is good enough.

To find out if the grid is good enough, a grid independence study needs to be done. This means that the

simulations are done with different grid sizes, in this case one coarse grid with 53271 cells, one medium

grid with 75155 cells, and one fine grid with 115211 cells. It is convenient to start with a coarse grid,

then refine the grid, and compare the results with the previous grid size, then refine the grid further,

and compare with the previous grid size. As the grids gets finer, the difference in the results between

the latest and the previous grid should get smaller, or finally diminish. When the difference is within acceptable limits, a grid independent solution has been obtained, and the grid can be considered good enough. To refine the grid further would possibly lead to a more exact solution, but would also result in longer CPU time to run the simulation. The flow properties that are compared, when doing the grid independence study are the mass flow rate over the spillway, and the height and length of the jet.

All parts of the grids both for full scale and model scale consists of mapped quadrilateral cells, except for a small area due to a problematic geometry, see Figure 4.4.

Figure 4.4: Unstructured part of grid marked with green.

The grid is finer at the spillway and downstream of the spillway, because the velocities and gradients are larger in these areas. Turbulence is expected to occur in the downstream area, which is another reason to make the grid finer in this area. In the reservoir the velocity is relatively low, therefore the grid can be coarser in this area. The cell size at the spillway, and downstream is 0.21, 0.175 and 0.14 m for the coarse, medium and fine grids.

4.5 Generation of results

The simulations are set up to automatically store data after a certain number of time steps. The required data can later be collected at the desired time step.

The mass flow rate over the spillway is measured by creating a surface at the top of the spillway. The total mass flow rate through the surface is then computed at the desired time step. The fact that it is the total mass flow rate that is computed means that also the air flowing through the surface is included.

This is not optimal, as it is the mass flow rate of water that is interesting, but since the density of air is much lower than the density of water the contribution from air is assumed to be negligible.

The height of the jet is obtained by computing the maximum vertical coordinate of the interface between water and air 25 m downstream of the flip bucket, see Figure 4.5. The height is not always largest 25 m from the flip bucket, but this is where it is measured in the hydraulic model, and therefore also in the simulations.

In the hydraulic model the length of the jet is measured from the flip bucket to where the upper side of

the jet hits the river bed. This is problematic to do in a consistent way for the simulations. Therefore the

length is measured from the flip bucket to the point at the downstream river bed where the maximum

static pressure occurs. This corresponds quite accurately to the point where the middle of the jet hits

the river bed. This is also shown in Figure 4.5. This difference in measuring point may affect how well the modelling methods correspond.

Figure 4.5: Schematic description of how the height and length are measured from the simulations.

Chapter 5

Semi-empirical calculations of height and length of the jet

For the semi-empirical calculations of height and length of the jet, two different methods are used.

According to ”Hydraulic Design Handbook”, [11], (Method 1) the trajectory of the jet can be estimated as

y ₁ = xtanθ − x ²

3.6Hcos ² θ . (5.1)

From (5.1) the variable x can be extracted to get

x ₁ = 3.6Hcos ² θtanθ

2 +

s

 3.6Hcos ² θtanθ 2

 ²

− 3.6Hcos ² θy. (5.2)

According to Kentaro Kawakami, [12], [13], (Method 2) the trajectory can be estimated as

y 2 = 1

gk ² ln(cosν + tanα · sinν), (5.3)

x 2 = 1

gk ² ln(1 + 2kαV 0 cosθ). (5.4)

In these equations y 1 , x 1 , y 2 and x 2 are the vertical and horizontal distance from the bucket edge. θ is the angle of the bucket lip, k is a constant related to air resistance, which in this case is determined to 0.014.

α = tan ⁻¹ (kV 0 sinθ), (5.5)

and

ν = e ^gk

^x − 1

kV 0 cosθ . (5.6)

H is calculated as

H = d + h v , (5.7)

where d is the depth of the flow, and h v is the velocity head, at the bucket lip. The velocity head is

defined as

h _v = V ₀ ²

2g . (5.8)

V ₀ is the flow velocity at the bucket lip. Both h _v and V ₀ can be calculated from Bernoulli’s equation, [5]. The flow depth d can be calculated after V ₀ is calculated, using the continuity equation, where the mass flow rate over the spillway crest is known. From Bernoulli’s equation the relation between the flow at the spillway crest and the flow at the flip bucket lip can be written as

1

2 ρV ₁ ² + ρgh ₁ + p = 1

2 ρV ₀ ² + ρgh ₀ + p, (5.9)

where p is the atmospheric pressure, V ₁ and h ₁ is the velocity and height at the crest, and V ₀ and h ₀ is the velocity and height at the flip bucket lip, see Figure 5.1.

Figure 5.1: Illustartion of the velocities and heights used in the semi-empirical calculations.

Since the density and atmospheric pressure can be considered as constant, Equation (5.8) and (5.9) gives

h v = V ₀ ²

2g = ∆h + V ₁ ²

2g , (5.10)

Equation (5.9) can also be rearranged as

V ₀ = q

V ₁ ² + 2g(h ₁ − h ₀ ). (5.11)

From the mass flow rate, ˙ m, received from Vattenfall, [10], it is possible to calculate the velocity V 1 as follows,

V ₁ = m ˙

w · h , (5.12)

where w is the width of the spillway, and h is the distance between the spillway crest and the retention water level. From the fact that the mass flow rate at the flip bucket lip is the same as the mass flow rate at the crest, and the velocity, V ₀ , is known, it is possible to calculate the flow depth, d, as

d = m ˙

V 0 · w . (5.13)

In Method 2 the horizontal distance is calculated at the point where the jet crosses the height from where

it left the flip bucket, as shown in Figure 5.2. In Method 1 it is possible to adjust at which height the

horizontal distance should be calculated, by changing the coordinate y in Equation (5.2). In this case

y = −5.2771 m, which means 5.2771 m below the flip bucket lip, also shown in Figure 5.2.

Figure 5.2: Length calculated by the different semi-empirical methods.

Chapter 6

Results

In this chapter the results from the different simulations are compared to each other, but also to the results from earlier experiments in the physical hydraulic model, and the semi-empirical calculations.

6.1 Mass flow rate

The mass flow rate over the spillway crest is logged for all simulations and all different grids, in order to check the convergence. In the beginning of each simulation some waves occur in the reservoir. By logging the mass flow rate over the spillway crest it is possible to see when the waves have settled, and the outflow from the reservoir is constant, which leads to a more stable jet. The results are shown Figure 6.1 and Figure 6.2.

Figure 6.1: Mass flow rate over the spillway crest, compared to the mass flow rate at the inlet (full scale

simulations).

Figure 6.2: Mass flow rate over the spillway crest, compared to the mass flow rate at the inlet (model scale simulations).

As can be seen in Figure 6.1 and Figure 6.2, the mass flow rate is relatively constant after 40 s, and therefore all of the following measurements are done from 40 to 50 s. The fluctuations in mass flow rate are smaller for the model scale simulations, but the full scale simulations seems to stabilize just as quick, or even quicker.

The mass flow rate can be considered grid independent in the time-interval of interest (40-50 s), with a maximum relative difference of 1.63% between the fine and medium grid, and 3.16% between the fine and the coarse grid, for the full scale simulations. For the model scale simulations the relative difference is even lower, at 0.99% between the fine and medium grid, and 0.73% between the fine and the coarse grid.

6.2 Height of the jet

The height of the jet is measured from the top of the flip bucket lip to the top of the jet 25 m downstream

of the flip bucket. The results from the simulations and the semi-empirical calculations are presented

below in Figure 6.3 - 6.10 and Table 6.1 - 6.2.

Figure 6.3: Height of the jet for all grid sizes, from the full scale simulations. The shaded area represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.4: Height of the jet from the full scale simulation with the coarse grid. The shaded area

represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.5: Height of the jet from the full scale simulation with the medium grid. The shaded area represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.6: Height of the jet from the full scale simulation with the fine grid. The shaded area

represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.7: Height of the jet for all grid sizes from the full scale simulations. The shaded area represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.8: Height of the jet from the model scale simulation with the coarse grid. The shaded area

represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.9: Height of the jet from the model scale simulation with the medium grid. The shaded area represents the height measured in the physical model tests (10.5-11.5m).

Figure 6.10: Height of the jet from the model scale simulations with the fine grid. The shaded area represents the height measured in the physical model tests (10.5-11.5m).

The figures above give an indication that the dispersion of the height measurements increase when the grid is refined, this is also supported by the increase of the standard deviation presented in Table 6.1. A possible explanation for this is that the finer grids better captures the turbulent behaviour of the jet.

Even though the dispersion of the height measurements from the fine grid differs quite a lot from the

medium and coarse grid for the full scale simulations, the time-averaged height are still quite similar

for all grid sizes, see ”Mean height” in Table 6.1, with a relative difference between the coarse and

medium grid of 1.57%, and between the medium and fine grid of 4.33%. For the model scale simulations

the corresponding relative differences are 2.05% and 6.97%. This does not indicate that the solution is

grid independent since the relative difference increases when the grid is refined. However the relative

differences between the grids are rather small, and thus this still gives an good indication of the jet

height. It would be preferable to run more simulations with finer grids to get better grid independence,

but due to lack of time, and limited computational power no further grid refinement is done.

Table 6.1: Mean height and standard deviation for all simulations.

Cells Mean height [m] Standard deviation [m]

53271 10.2859 0.3700

Full scale 75155 10.4503 0.3775

115211 10.0168 0.7313

53271 11.5210 0.1027

Model scale 75154 11.2892 0.1657

115211 12.1345 0.1660

A small difference in height can be observed between the methods, where the full scale simulations give a lower jet than the model scale simulations and the physical model tests (10.5-11.5m). The full scale simulations also give a larger spread in height measurements than the model scale simulations. The results from the two semi-empirical methods are presented below in Table 6.2, and both lies within the interval for the physical model tests.

Table 6.2: Height of the jet from the semi-empirical calculations.

Method 1 10.7827 m Method 2 11.2886 m

The difference between the full scale and model scale simulations indicate that the scale effects discussed earlier have an impact on the results, where more turbulence in the full scale simulations lead to a lower and more dispersed jet. However the impact is rather small at these flow velocities. The underestimation of air entrainment in scale models can also have an effect on the jet trajectory [14].

6.3 Length of the jet

As stated earlier, for the simulations, the length of the jet is measured from the flip bucket to the point at the downstream river bed where the maximum static pressure occurs. For the semi-empirical calculations the length is measured as shown earlier in Figure 5.2. The results are presented below in Figure 6.11 - 6.18 and Table 6.3 - 6.4.

Figure 6.11: Length of the jet for all grid sizes, from the full scale simulations. The shaded area

represents the length measured in the physical model tests (47-53m).

Figure 6.12: Length of the jet from the full scale simulation with the coarse grid. The shaded area represents the length measured in the physical model tests (47-53m).

Figure 6.13: Length of the jet from the full scale simulation with the medium grid. The shaded area

represents the length measured in the physical model tests (47-53m).

Figure 6.14: Length of the jet from the full scale simulation with the fine grid. The shaded area represents the length measured in the physical model tests (47-53m). The peak at around 49 s does not represent the actual jet length at that time, but occurred due to deficiencies in the method for retrieving

the jet length from the simulations.

Figure 6.15: Length of the jet from the model scale simulation with the coarse grid. The shaded area

represents the length measured in the physical model tests (47-53m).

Figure 6.16: Length of the jet from the model scale simulation with the coarse grid. The shaded area represents the length measured in the physical model tests (47-53m).

Figure 6.17: Length of the jet from the model scale simulation with the medium grid. The shaded area

represents the length measured in the physical model tests (47-53m).

Figure 6.18: Length of the jet from the model scale simulation with the fine grid. The shaded area represents the length measured in the physical model tests (47-53m).

As for the height the dispersion of the length measurements increase when the grid is refined, which can be seen both in the figures above and from the standard deviation in Table 6.3. Just as for the the height, a possible explanation for this could be that the finer grid better captures the turbulent behaviour of the jet.

The time-averaged length seems to be relatively grid independent for the full scale simulations, with a relative difference between the coarse and medium grid of 2.62%, and 0.12% between the medium and fine grid. For the model scale simulations the relative differences for the time-averaged length are 0.16%

between the coarse and medium grid, and 5.16% between the medium and fine grid. This can not be considered as grid independent, but as for the height the simulations still can give a relatively good indication of the jet length. Further grid refinement is needed to get better grid independence, but as stated earlier due to lack of time and computational power no further grid refinement is done.

Table 6.3: Mean length and standard deviation for all simulations.

Cells Mean length [m] Standard deviation [m]

53271 47.6510 0.9389

Full scale 75155 48.9330 1.1938

115211 48.8731 3.5389

53271 51.5845 0.2503

Model scale 75154 51.4999 0.5494

115211 54.3019 0.7735

In line with the height, the length differs a bit between the full scale and the model scale simulations.

The full scale simulations give a shorter and more dispersed jet than the model scale simulations, but the time-averaged values lies within the interval for the experimental values. The semi-empirical methods presented in Table 6.4 differ about 4.5m from each other, and whereas Method 1 is within the interval from the experiments, Method 2 is not. This is mainly due to the fact that Method 2 does not calculate the length as close to the riverbed as Method 1.

Table 6.4: Length of the jet from the semi-empirical calculations.

Method 1 48.7220 m

Method 2 44.1350 m

The difference between the full scale and model scale simulations indicate an impact of scale effects, just as for the height. It is likely that the difference in the downstream topography between the simulations and the experiments affect how well the methods correspond in matter of length.

According to Chanson and Pfister [4], the Reynolds number in the scale model should fulfil the criterion Re ≥ 1.0 × 10 ⁵ in order to avoid to large scale effects on the air entrainment. In this case the Reynolds number is defined as

Re = V h

ν , (6.1)

where V in this case is the characteristic flow velocity, h is the characteristic flow depth and ν is the kinematic viscosity. When the input for Equation 6.1 is taken from the bottom of the flip bucket in the model scale simulations at 40 s, the Reynolds number turn out as

Re = V h

ν = 3.41 · 0.02

1.0048 × 10 ⁻ 6 ≈ 67874. (6.2)

This is below the criterion stated by Chanson and Pfister, and can thus be a further indication that scale effects are influential. Juon and Hager [15] identified scale effects on jet trajectories due to viscosity and surface tension for h < 0.05 m. Below this value the height and length of the jet trajectory visibly increases. Heller et al. [16] identified similar scale effects for h < 0.04 m. For the model scale simulations in this project h ∼ 0.02, which is likely to affect the jet trajectory. It is not known what the corresponding flow depth were in the experiments, from which data were collected in this project.

Therefore no conclusion about similar scale effects regarding these can be made.

Chapter 7

Discussion and conclusions

Altogether the results from the simulations turned out quite as expected, even though the grid indepen- dence was not completely satisfactory. The jet turned out a bit lower and shorter and more dispersed in the full scale simulations compared to the model experiments and model scale simulations, which could be expected due to the scale effects.

To get better grid independence the grid would have to be refined, at least in the area downstream of the flip bucket. An idea would be to use adaptive meshing to only refine the grid around the jet, and keep a coarser grid in other areas of the domain. Thereby the total amount of grid cells could be kept relatively low.

To run a simulation took approximately 26 days for the fine grid, 21 days for the medium grid and 13 days for the coarse grid. It would probably have been possible to decrease the computational time for the medium and coarse grids a bit by increasing the time step. In this project the same time step was used for all grids, but usually it is possible to use larger time steps for coarser grids and still get good time step convergence.

The semi-empirical methods shows quite good correspondence with the other methods, and are rather simple to use, but they are depending on that the mass flow rate is known, which it mostly is not in the beginning of a design process. It might be possible to calculate the mass flow rate with good accuracy as well, but that was not investigated in this project.

It is not possible to determine whether or not any of the methods give a better representation of the actual full scale spillway, or how much the experiments are affected by scale effects since there are no experimental data from the full scale spillway. In spite of this the results from this project still shows that CFD can be a good alternative to physical models. Especially when modelling larger dams, which in order to avoid scale effects require the physical models to be larger and thereby also often more expensive.

To further develop the CFD model it would be possible to expand it to 3D, and use topographical data

to model the downstream river bed. It would also be possible to apply a boundary with hydrostatic

pressure at the inlet instead of velocity. By doing this it would be possible to independently model the

mass flow rate through the spillway, which now depends on the inlet velocity.

Bibliography

[1] R. J. Houghtalen, N. H. C. Hwang, and A. O. Akan, Fundamentals of Hydraulic Engineering Systems.

Prentice Hall, 2010.

[2] P. Novak, A. I. B. Moffat, C. Nalluri, and R. Narayanan, Hydraulic Structures. Spon Press, 2001.

[3] H. Chanson, “Physical modelling, scale effects and self-similarity of stepped spillway flows,” in World Environmental and Water Resources Congress 2008 Ahupua’a (R. B. Jr and R. Walton, eds.), (Honolulu, Hawaii, United States), pp. 1–10, Reston, VA: American Society of Civil Engineers, May 2008.

[4] M. Pfister and H. Chanson, “Two-phase air-water flows: Scale effects in physical modeling,” Journal of Hydrodynamics, vol. 26(2), pp. 291–298, April 2014.

[5] P. K. Kundu, I. M. Cohen, and D. R. Dowling, Fluid Mechanics. Elsevier, 2012.

[6] J. Blazek, COMPUTATIONAL FLUID DYNAMICS: PRINCIPLES AND APPLICATIONS. Else- vier, 2005.

[7] T.-H. Shih, W. W. Liou, A. Shabbir, Z. Yang, and J. Zhu, “A new κ −  eddy viscosity model for high Reylnold number turbulent flows,” Computers Fluids, vol. 24, pp. 227–238, 1981.

[8] ANSYS, Inc, ANSYS ^® Help Viewer, Release 15.0.

[9] C. W. Hirt and B. D. Nichols, “Volume of fluid (VOF) method for the dynamics of free boundaries,”

Journal of Computational Physics, vol. 39, pp. 201–225, 1981.

[10] J. Yang, A. Helgesson, and M. Billstein, “Storfinnforsen samms¨ akerhet, hydrauliska modellf¨ ors¨ ok 2014-15,” Tech. Rep. U 14:55, Vattenfall AB, R&D Laboratories, 2015.

[11] L. W. Mays, Hydraulic Design Handbook. McGraw-Hill, 1999.

[12] R. M. Khatsuria, Hydraulics of Spillways and Energy Dissipators. Marcel Dekker, 2005.

[13] K. Kawakami, “A study on the computation of horizontal distance of jet issued from ski-jump spillway,” Proceedings of the Japan Society of Civil Engineers, vol. 219, pp. 37–44, 1973.

[14] J. hua Wu, X. yan Zhang, F. Ma, and W. wei Wu, “Ski jump trajectory with consideration of air resistance,” Journal of Hydrodynamics, vol. 27(3), pp. 465–468, June 2015.

[15] R. Yuon and W. H. Hager, “Flip bucket without and with deflectors,” Journal of Hydraulic Engi- neering, vol. 126(11), pp. 837–845, 2000.

[16] V. Heller, W. H. Hager, and H.-E. Minor, “Ski jump hydraulics,” Journal of Hydraulic Engineering,

vol. 131, pp. 347–355, 2005.