Numerical and experimental study of appendages in racing yachts and their influence on the free surface

Transcription

1 UNIVERSIDAD POLITÉCNICA DE MADRID Escuela Técnica Superior de Ingenieros Navales Departamento de Arquitectura y Construcción Navales PHD THESIS: Numerical and experimental study of appendages in racing yachts and their influence on the free surface A Thesis submitted by Jorge Izquierdo Yerón for the degree of Doctor of Philosophy Supervised by: Dr. Ricardo Zamora Rodriguez 2015

2 Resumen Las prestaciones de un velero de regatas se estiman por medio de los Programas de Predicción de Velocidad (VPP) que incluyen las características de estabilidad y modelos aero e hidrodinámico del barco. Por esta razón, es importante tener una evaluación adecuada de las fuerzas en apéndices y de su variación en diferentes condiciones de navegación, escora y deriva. Además, para el cálculo de las fuerzas en los apéndices es importante conocer sus características hidrodinámicas cuando trabajan conjuntamente en un campo fluido fuertemente modificado por la carena. Por esta razón, se han utilizado una serie de ensayos realizados en el Canal de Ensayos de la ETSIN con el objetivo de validar códigos numéricos que permiten una evaluación más rápida y focalizada en los distintos fenómenos que se producen. Dichos ensayos se han realizado de forma que pudiera medirse independientemente las fuerzas hidrodinámicas en cada apéndice, lo que permitirá evaluar el reparto de fuerzas en diferentes condiciones de navegación para poder profundizar en las interacciones entre carena, quilla y timón. Las técnicas numéricas permiten capturar detalles que difícilmente se pueden visualizar en ensayos experimentales. En este sentido, se han probado las últimas técnicas utilizadas en los últimos workshops y se ha enfocado el estudio a un nuevo método con el objetivo de mostrar una metodologia más rápida que pueda servir a la industria para este tipo de aproximación al problema. i

3 Abstract The performances of a racing sailboat are estimated by means of the speed prediction programs (VPP), which include the ship stability characteristics and the aero and hydrodynamic models. For this reason, it is important to have an adequate evaluation of the forces in appendices and its variation in different sailing conditions, heel and leeway Moreover, for the analysis of the forces in the appendices, it is important to know their hydrodynamic characteristics when they work together in a fluid field strongly modified by the canoe body. For this reason, several tests have been done in the ETSIN towing tank with the aim to validate numeric codes that allowing faster analysis and they permit to focus on the different phenomena that occur there. Such tests have been done in a way that the hydrodynamic forces in each appendage could be measured independently allowing assessing the distribution of forces in different sailing conditions to be able to deepen the interactions between the canoe body, the keel and the rudder. Numerical techniques allow capturing details that can hardly be displayed in experimental tests. In this sense, the latest techniques used in the recent workshops have been reviewed and the study has been focused to propose a new model with the aim to show a new faster methodology which serves the industry for this type of approach to the problem. ii

4 Acknowledgments It is difficult to resume all this years in several pages, and there are a lot of people who have helped in different ways. I m very grateful to these people and institutions for their assistance during this research: Professor Ricardo Zamora, my supervisor. I will never be able to thank him enough for his support, encouragement, guidance and for giving me the opportunity to delve into the subject covered by this thesis. Taking advance of this, I would like to thank the members of the CEHINAV group Paco, Riansares, Ricardo Abad, Leo, Pepe, Elkin,... and specially to Juan who spent a lot of days on the car helping me doing the experimental tests and to professor Luis Perez Rojas who gives me the opportunity to join to his team. In addition, I would like to give special thanks to Ignacio Diez de Ulzurrun because in his department I started my career as researcher. Professor J.A Keunning, Pepijn de Jong, Peter Naaijen and their department on the TU Delft University. They gave me a warm welcome to their research group. They helped me grow as a person and as a researcher Dr. Milovan Peric, Carlo Pettinelli, Alberto Pinzello, Sven H. Enger, Francisco Ezquerra, Stephan Herrmann and all the people in the CD-Adapco office in Nurnberg. I have to thank them for accepting me and opening the doors of their office for my investigation. They helped, support and guided me when I started with CFD simulations and they taught me how a support engineer should work. I would like to thanks to my colleagues from ANSYS Pedro Afonso and Benjamin Lehugeur. It is a pleasure working with you. Thank you for teaching me new CFD topic everyday. Lubeena Rahumathulla and Vinay Kumar Gupta, thank you for your support and your suggestions. Andy Wade, thank you very much for helping me with this work. Furthermore I would like to thank ANSYS Iberia for allowing me the use of their computing resources when they were not being used. It is important to note that this research has been funded by the Spanish Administration included in the project TRA C Finally, I would like to thank my family, my parents Jose Ramón and Rosalia and my sister Maria, for their unconditional support in the good and bad moments. They are the reason that this journey has been successfully completed. (Vosotros sois la razón de que esta singladura haya llegado a buen fin!!). iii

5 Contents 1 Introduction Motivation Scope Contribution Geometry TP52 introduction The model Scale Model for experimental tests Background Theory Dimensionless Relations Resistance Viscous Resistance Wave Resistance Heel Resistance Induced Resistance Appendages hydrodynamic Experimental Setup CEHINAV Towing Tank Aim of the experiment Measurement Scheme Data Acquisition Equipment Appendages measurement arrangement Keel Measurements Rudder Measurements Turbulence stimulator Wave cut tests Uncertainty Analysis Forces uncertainty Wave cut uncertainty Experimental Results Upright Tests Appendages Keel and Rudder iteration iv

6 5.1.3 Effects on the Sink and Trim Canoe Body Lift Analyses Heel Effects Computational Fluid Dynamic Introduction The Structure of a CFD code Overview of Equations and Numeric Methods used in Marine CFD Turbulence models Near Wall Treatments Free Surface Model General Errors and uncertainties in CFD Simulations Domain discretization Unstructured Mesh Multiblock Structured Mesh Trimmed Mesh Hexcore Unstructured Mesh Boundary Conditions Numerical Setup Canoe Body Result Comparison Keel Results Study of the Bulbed-keel without free surface Numeric study of the free surface influence over the bulbed-keel Turbulence Stimulator Influence Rudder Results Study of the rudder without free surface Numeric study of the free surface influence over the rudder Complete Model Results Complete Upright Numerical Tests Leeway and Heel Numerical Study Conclusions Conclusions Future Works v

7 List of Figures 2.1 The real model sailing Lines plan of the model hull used for the experiments Rudder, Keel and Bulb used for the experiments D Model Definition Geometry used for Numerical Analyses Hull Construction Process Keel Construction Process Reduced and Increased Chord Keels Rudder Construction Process Kelvin Wave System Bow wave in phase with the stern wave Bow wave out of phase with the stern wave Effects of the heeling force F H Vortex generation around a keel [1] Vortex generation around a keel [2] Analogy between a planform and an aeroplane wing Rectangular Wave Profile Flow around a wing profile Boundary Layer Separation Hydrodinamic actions Hydrodinamic actions CEHINAV towing tank facilities Test cases Data Adquisition User Interface Block Strain-Gage Measurement Setup Heel and Leeway Mechanism (left) and Block Strain-gage (right) Device Used for Data Adquisition Signal Calibration and Transformation Data Adquisition User Interface Appendages Dynamometer Axes Measurement setup keel set keel dynamometer Rudder set Rudder canoe body intersection vi

8 4.16 Dynamometer and rudder mechanism Diagram control and data acquisition appendices sailboat Rudder complete assembly Turbulence stimulator Wave Pattern experimental setup and sketch of the data acquisition device Canoe Body forces descomposition Ship Total Resistance with different configuration Canoe Body Resistance without appendages Wave Cut for Fn=0.336 (left) and for Fn =0.420 (right) Wave Cut difference for Fn= Keel Resistance Keel Lift Wind Tunnel C L and C D Results F n = 0, Lift and Drag Rudder Curves without Keel Rudder Lift Comparisson Rudder Lift Comparisson Lift and Drag Rudder Curves Keel Lift effect over the Rudder Keel Drag effect over the Rudder C D CL 2 Rudder relations Percentage distribution of Resistance Rudder Lift Comparisson Downwash and Lift Vanishing Angle definition Sink and Trim Results HKR and HR Sink data HKR and HR Trim data Lift Canoe Body Results Decomposition of the lift forces Deterioration of the keel bulb set lift with heel HKR Leeway 0 Heel curves HKR Leeway 2 Heel curves HKR Leeway 4 Heel curves CLR positions Subdivisions of the Near-Wall Regions [3] Near-Wall Treatments [3] Wall Function separation [3] Cell Representation for Modified HRIC Scheme [3] Bulb end simplification Code errors CFD Domains Numerical diffusion along a structured mesh Numerical diffusion along an unstructured mesh Overall Unstructured Mesh Domain Free Surface inflation detail Rudder Unstructured Mesh vii

9 6.13 Sailing ship division for blocks Splitting and O-grid Schemes Block Mesh Free Surface Multiblock modelled Multiblock details Trimmed Mesh Trimmed Mesh Process Difference with and without features curves Free Surface and keel wake refinement Hexcore symmetry Hexcore Complete Model Fluent Free Surface and Keel Wake Refinement Bulb Boundary Layer Mesh Keel (left) and Rudder (right) BoundaryLayer Mesh Canoe body Appendage Boundary Layer Transition Rudder Singularity Point CFX Boundary Conditions Wave Cut Distance CFX Fn B Wave Cut CFX Fn B Wave Cut Star-CCM+ Boundary Conditions Star-CCM+ Fn B Wave Cut Star-CCM+ Fn B Wave Cut Fluent symmetry Model Boundary Conditions Fluent Boundary Conditions k ω Reconstruction Schemes Volume Fraction difference Pressure difference (Compressive-HRIC) Fluent Fn B Wave Cut Fluent Fn B Wave Cut Ventilation effects produced in Case C TP52 with bottom out of the water Ventilation effects produced with y + = Ventilation effects produced with y + = Resistance Analyses in all cases for two velocities Total Canoe Body Resistance Fn B Wave Cut Comparison Fn B Wave Cut Comparison Fn HRIC B Wave Cut Comparison Fn HRIC B Wave Cut Comparison Keel and Bulb blocks Submerged Canoe Body and Bulbed-keel mesh Submerged Canoe Body and Bulbed-keel mesh Keel Resistance Comparison Bulbed-Keel Wake Mesh Total Bulbed Keel Model Resistance Fluent HK Fn B Wave Cut Fluent HK Fn B Wave Cut viii

10 6.60 Wave Contour Comparisson CaseC09 (left) and CaseK03 fine(right) Wave Contour Comparisson Pin Model and Mesh Rudder Structured Mesh Froude C L and C D comparison Froude C L and C D comparison Froude C L and C D comparison Froude C L and C D comparison Fn HR Wave Contour Comparisson Fn HR Wave Contour Comparisson Lift and Drag Rudder Curves Case R03 β = 2 ϕ = y + values 0 (left) and 6 (right) at Fn detachament 6 (left) and 6 (right) at Fn Free Surface modelling Total Upright Results HKR Wave Cut Analyses Keel Resistance HKR Rudder Results HKR C D - CL 2 Curves HKR02 Rudder Results HKR02 C D - CL 2 Curves Free Surface modelling Velocity Field at Perpendicular Planes to the Free Surface Velocity Field at Perpendicular Planes and Free Surface modelling Velocity Field at Parallel Plane to the free Surface Velocity Field at Parallel Plane in the bulb and HKR Rudder Results β = 2 ϕ = C D - CL 2 HKR Rudder Results β = 2 ϕ = Free Surface Modelling HKR β = 2 ϕ = Velocity Field at Perpendicular Planes to the Free Surface HKR β = 2 ϕ = Velocity Field at Parallel Plane to the free Surface HKR Rudder Results β = 4 ϕ = HKR Rudder Results β = 4 ϕ = C D - CL 2 HKR Rudder Results β = 4 ϕ = y + appendages HKR Ventilation effects produced in Case HKR Free Surface Modelling HKR β = 4 ϕ = Velocity Field at Perpendicular Planes to the Free Surface HKR β = 4 ϕ = Velocity Field at Parallel Plane to the free Surface HKR Velocity vectors in plane HKR02 x=2.75 m Velocity vectors in plane HKR04 x=2.75 m Detail of Velocity vectors in plane HKR04 x=2.75 m Detail of Velocity vectors in plane x=2.75 m for β 0 ϕ 0 δ Detail of velocity field x=2.75m (left) and Total pressures on the canoe body (right) ix

11 List of Tables 2.1 Hull dimensions Appendages dimensions Uncertainty elements Maximum and minimum errors produced in the measurements Downwash and Lift Vanishing Angle. Heel Sink and Trim measures Numerical Boundary Conditions Variables Transpac CFX Bare Hull Cases Summary CFX Resistance Results Star-CCM+ Bare Hull Cases Summary Star-CCM+ Resistance Results Fluent Bare Hull Cases Summary Fluent Resistance Results Comparative Canoe Body Resistance Results Bulbed Keel Total Resistance Keel Total Resistance Fluent Canoe Body and Bulbed Keel Cases Summary Total Resistance Canoe Body and Keel Total Resistance Canoe Body and Keel Pins Resistance C L and C D rudder results in wind tunnel tests C L and C D rudder results in wind tunnel tests Fluent Rudder Cases Summary C L and C D rudder results under free surface presence C L and C D rudder results under free surface presence C L and C D Rudder Results β = 2 ϕ = C L and C D Rudder Results β = 2 ϕ = Fluent Complete Cases Summary Upright Total Resistance Results Upright Keel Resistance Results C D Rudder Results C L Rudder Results HKR03 Drag and Lift Keel Results C L and C D HKR Rudder Results β = 2 ϕ = C L and C D HKR Rudder Results β = 2 ϕ = x

12 6.31 β = 2 ϕ = 10 Total Resistance Results HKR04 Drag and Lift Keel Results C L and C D HKR Rudder Results β = 4 ϕ = C L and C D HKR Rudder Results β = 4 ϕ = β = 4 ϕ = 20 Total Resistance Results xi

13 xii

14 Nomenclature L Length B Beam D Draft H Canoe body, Hull K Bulbed-Keel R Rudder HK Hull and Bulbed-Keel HR Hull and Rudder HKR Hull, Bulbed-Keel and Rudder Fn Froude Number CLR Centre of Lateral Resistance Re Reynolds Number c Chord AR Aspect Ratio b Span S Wetted Area C T Total Resistance Coefficient Λ Sweepback angle t/c Thickness/chord ratio A lat Lateral area β Leeway Angle ϕ Heel Angle Φ Downwash Angle θ Trim angle δ Rudder Angle λ Scale factor y Distance from the wall to the first discretization point α Volume Fraction α Magnitude of gradient of volume fraction ρ Density A i Interfacial area density for phase i n Cell height normal to interface β 1 k ω model closure coefficient of destruction term, which is equal to B Damping factor µ Viscosity ϕ 0 Zero Sink and Trim condition ϕ θ Dynamic Sink and Trim condition RSM Reynolds Stress Model w downwash xiii

15 Chapter 1 Introduction The Drag and lift of the appendages of a sailing yacht have since long been an area of extensive research. The development in the design of sailing yachts has a considerable extend in this area. In particular, in the recent years, events as America s Cup, Volvo Ocean Race or the Med Cup take importance. Appendages, keel and rudder basically, have an important role in this kind of ships working along with the hull as airfoils generating the force necessary to compensate the lateral component of the forces of the sails. The vessel sails with a leeway angle due to this force, and the rudder has in addition the mission to correct that angle to maintain the control of the boat. The keel contributes volume for the ballast necessary to fulfil the stability requirements and connects structurally the bulb with the hull. When ships sail upwind, there is an increase in drag and lift due to heel and leeway. Another important aspect in the appendage drag is the interference drag between hull and appendages due to the proximity of these to the free surface. Apart from viscous effects arising from the connection of the bodies, there is also a possible interference in the wavemaking drag, in particular under leeway and heel as was already demonstrated by Beukelman and Keuning [4]. Some articles appeared later trying to explain the interaction between the appendages using diverse forms to analyze the problem, from studying the variation of the resistance to seeing as it affected through the wave cuts (ref [5], [6], [7], [8] and [9]). The conclusion in them are that there is a reduction in free stream velocity of the incoming fluid on the rudder (since it operates in the wake of the keel) and a reduction of the effective angle of attack on the rudder through the vorticity shed off by the keel caused by the lift generated on the keel, i.e. the downwash. In later publications, Keuning et al. ([10], [11]) realized a study of the keel influence on the rudder. They are continuing the works started before where an assessment method has been presented for determining the force distribution in yaw and sway over the hull, keel and rudder ([12], [13]). To investigate these interference effects it was decided to carry out a series of experiments in the ETSIN towing tank. The aim of this experiments are to measure the lift and drag of the three different components of a yacht hull, i.e, the hull, the bulbed-keel and the rudder, 1

16 separately under different combinations and conditions in order to determine their mutual interaction. Although, to facilitate the analysis of the results and check, modern Computational Fluid Dynamiques techniques based on RANSE flow simulation were used in order to determine and to visualize some of this interaction effects. RANSE simulation are flow analysis method based on the solution of the Reynolds Averaged Navier Stokes equation. Applied to hull, rudder, keel and bulb, these methods provide results comparable to towing tank obtained and allow the analysis of local flow phenomena easier than in the experimental test. Finally, towing tank tests are done according Froude scale laws, and it has an important influence in appendages measurements, which needs tests at the same Reynolds number to determinate a real force value. 1.1 Motivation The main motivation of this study was the interest of researching about the behaviour of a racing yachts. Numerical codes are widely used in the naval industry, but there is a lack of information to validate new codes and the methodology that designers use. The main approaches to study resistance in sailing yachts were done many years ago and there is few publications where new designers could use to validate their models. In the case of the shipbuilding industry, every five years a CFD workshop is held, where the most modern techniques of numerical simulation are discussed on determined ships which have tested experimentally. However, none of these ships are racing yachts, they are military ships or carrier which are the ones more used in the industry. The main advantage from conventional ships is that they do not sail under leeway and heel conditions. In this way it is easier to simulate because a symmetry model could be used. It is not the case with yacht models where the complete model is needed and there are other forces which act in the model. During this work, the main scenario was the study of the influence of the keel and rudder on the canoe body and on the free surface. To this end, experimental tests have been combined with numerical analyses to better understand the phenomena involved under the water. 1.2 Scope One of the ideas when this work was started was to develop a methodology that can help in the industry. For this study a methodology created for cargo ships was adapted to racing yachts. In an industry where the time is very important a complete automated workflow is going to be developed where engineers could analyse complete cases in reduced time. These numerical analyses serve to visualize several flow features that help to understand what is happening under the water and explain some phenomena like how the pressure fields 2

17 created by the appendages affect to the free surface. It is very complicated to observe these without numerical analyses help. In addition, in the experimental field, the test methodology has been explained in detail. Finally the study of the forces that affect the appendages and their influence on the free surface will be analysed. 1.3 Contribution The aim of this paper is to provide a test with the ship characteristic described in the next chapter, which can be a starting point for both industrial and academic future work. In recent years, in several conferences a high percentage of works has been done with the same discrete models. Tetrahedral, hexahedral and trimmed mesh are very usual in this kind of works. A new kind of mesh called hexcore where a cartesian mesh is used in combination with tetrahedral elements is presented in this report and will be displayed on the following pages. Besides a comprehensive experimental study it has shown, showing the different problems that may arise in this type of testing. In addition a comprehensive and detailed study of a racing yacht appendages has been done. This last detail is interesting because due to the secrecy involved in the analysis of these kind of models, there is not much reliable bibliography where the researchers could find information. Therefore, one of the most ambitious objectives of this paper is the first case where future researchers of these models have a starting point to work with this kind of models. To do that different alternatives have been tested. The main methods used in the industry have been used and compared. In the way to do that, different tests have been done with different kind of ships trying to understand the different methodologies. Several works has been published with the results obtained although any of them have been used in this document. Cargo vessels, fishing vessels, catamarans and military ships have been analysed and the methodology used in that works has been adapted to racing yachts with different results [14]. The most outstanding work has been done with the Combatant DTMB Several works have been done [15], [16] adapting this successful methodologies to racing yachts. 3

18 Chapter 2 Geometry 2.1 TP52 introduction The model which has been used for the measurements is a Transpac 52 class, with a higher beam/draft ratio than the old America s Cup monohull class model. The TP52 Class can be summarized as fast, fun, simple which indicate the original thoughts behind the TP52 Rule and Class. People have to read these words in contrast with designing and building one-off racing yachts for handicap rules such as IMS and IRC and in contrast with racing on handicap under whatever rule. It was felt at the time, and the organizer firmly believe this is still the case, that especially in the larger sizes quite a few owners like to race one-off yachts but are willing to constrain themselves to fixed limits on the key dimensions and design options for the benefits of boat for boat racing. A boat designed and build to a boxrule as the happy medium between racing different concepts under a handicap rule and racing a one-design boat. The TP52 Class has grown faster but it was hit hard for the effects to the global economic crisis. Actually, new teams have been appeared and there are some international circuits where this ships sails. The main focus of TP52 racing has moved from the USA to the Med with the MedCup as the magnet for this move. The MedCup is undoubtedly the hottest ticket in town when considering yacht racing other than Americas Cup or long distance offshore racing. Ideally a similar circuit should exist in other quality sailing areas, like in the USA and possibly in the UK and Australia. In these areas a large number of TP52 s race under IRC, it seems a logic step to combine this with boat for boat racing again. That boat is as much as a dual purpose racer for racing on real time as well as be fully competitive in handicap racing. The TP52 has all the features that you know of the IRC converted TP52 s and IRC custom racers. Bowsprit, square head main, all ballast in the keel, even lighter displacement and more sailarea. It is seen as the ultimate Grand Prix Racer. Moreover, it is consider one of the faster class monohull yachts only behind Open 65 class. It is a class build within a boxrule. Because of its size, the number of crew and allowing the best of materials and building techniques this was never going to be a class for small budget campaigns. The TP52 is a simple racing machine. No moving parts under water other than a single centreline rudder, no complicated issues on deck or in the rig. Just high quality components 4

19 allowing proper control of the boat and of a sails wardrobe build for optimum performance at every windangle and windspeed. The interior is the minimum required by the Safety Regulations and TP52 Rule, it is not truly aimed at offshore racing anymore, but is easy to update to the requirements of a TransPac for instance. The rules about the measures that govern this Class are available in the TP52 Webpage. 1 However, the rules that involves measures with the hull and appendages sizes are described below: - Boats under this rule shall be of the monohull type. - Maximum hull length (HL): m. - Hull Length shall be measured including any part of the boat s standing rigging. Fittings extending aft of the aftermost point of the hull shall be added to the Hull Length for the purpose of this rule, except exterior chainplates if they do not extend more than 0.012m (12mm) outside the hull. Navigation lights, antennas and tracking devices are not to be seen as fittings for the purpose of measuring Hull Length. - Maximum Hull Beam (HB): 4.420m. Minimum at widest point 4.300m. - Hull Beam shall be measured including any part of the boat?s standing rigging. Exterior chainplates may be excluded if they do not extend more than 0.012m (12mm)outside the hull. - Draft To Sheer (DTS) and Freeboard Draft Measured (FDM) shall be measured. DTS is the vertical distance from the lowest point of the boat to the sheerline at the same section, and FDM is the freeboard measured at the same section. The distance from the bow to the maximum draft section shall be recorded as SDM. The Draft of the yacht shall be calculated as follows: Draft = DTS - FDM. - A TP52 shall be fitted with one fixed centreline keel, solid in profile, which shall have a bulb, one centreline rigid-surface rudder, one bona fide propeller installation and the usual instrument transducers. - Keel Width (KWM): Maximum 0.65m. The keel shall be measured in the transverse axis and the largest measurement shall be recorded. - Bulb Height (BHM): Minimum 0.38m. The bulb shall be measured in the vertical axis and the largest measurement shall be recorded. The radius into the fin shall be ignored for this measurement. - Bulb Shape: In any direction no hollows larger than 5% (5cm over 1m) other than in the radius where the bulb meets the fin. - The rudder may not be multi surface (shall have a single blade without endplates or similar) and its axis of rotation shall be in the centreplane of the boat. - There is not any limitation about the rudder size. The rules about the rudder are collected in the ISO 12215, Part

20 2.2 The model The model used was the real ship Aifos (figure 2.1) which was launched in This ship belonged to the Spanish Navy. Figure 2.1: The real model sailing The lines plan of this hull, used for build the numerical and the experimental model, is presented in figure 2.2. From this lines and using the software Maxsurf, a first 3D model was built and then this model was improved with Rhinoceros. A clean geometry was needed not only for the physical model but also was for the CFD (figure??) Figure 2.2: Lines plan of the model hull used for the experiments The main dimensions of the hull are presented in the following table: DIMENSIONS Length [mm] LWL [mm] Beam [mm] Draft [mm] Displaz. [kg] TP , ,364 Table 2.1: Hull dimensions 6

21 The same procedure was done for the appendages. From the linesplan and knowing their dimensions, which are presented in table 2.2, the appendages were built as they are shown in figure 2.3. Figure 2.3: Rudder, Keel and Bulb used for the experiments Keel Rudder Bulb c root [m] 0,165 0,091 - c tip [m] 0,106 0,024 - A lat [m 2 ] 0,060 0,033 - S [m 2 ] ,066 0,101 AR [-] ,217 - b [m] 0,449 0,467 - c mean [m] 0,136 0,060 - Λ [ o ] 5,36 12,16 - t/c [-] 0,147 0,217 (D/L) 0,185 L [m] - - 0,486 D [m] - - 0,078 Table 2.2: Appendages dimensions Furthermore, the keel has been modified changing its chord to analyse its influence to the rudder. The chord will be incresase and decrease a 20% of its length. 2.3 Scale Model for experimental tests For towing tank tests a scaled model was made (λ = 5.5). The model was built in the facilities of the E.T.S.I.Navales. The initial assembly is defined by a 3D file shown in figure 2.4. This figure will be cleaned to be used in the numerical analyses (figure 2.5). With this we will ensure that we have the same geometry for both analyses. Each part of the final set has been drawn and 7

22 Figure 2.4: 3D Model Definition Figure 2.5: Geometry used for Numerical Analyses assembled carefully observing the minimum dimensional tolerances of the manufacturing process, including parts from third as dynamometers and rudder engines. The following sections show the manufacturing steps for each of the components seen in figure 2.4, divided into three main groups: - The hull, which is composed of all exterior and interior structure and the various anchorages needed for dynamometers. - The rudder set with the positioning mechanism and dynamometer. - The keels set with the dynamometer. 8

23 The Hull The 2.85 m length and 0.8 m wide model was made from a polyurethane foam solid block with a fiberglass coating to achieve the necessary stiffness and waterproofing. In the process, the plywood deck was previously attached to the foam block. The main stages in the carving process are presented in the figure 2.6. There are intermediate stages as carving deck and anchorages dynamometers with the same procedure carving. Figure 2.6: Hull Construction Process The Keels According to the requirements of structural rigidity, the keel model manufactured consists on a piece of wood with a core of carbon fibre laminate. Previously to the surfaces carved a coating of fibreglass was applied, the bulb is completely built by samba wood, and once assembled a layer of polyester spray was applied to waterproof the model. After that a polyurethane paint was applied for the surface to obtain a good final surface texture. In the following figure the process described is shown. Figure 2.7: Keel Construction Process The same procedure is repeated for the other keel models (figure 2.8). The assembly with the measuring system is made through a slot formed in the hull. 9

24 Figure 2.8: Reduced and Increased Chord Keels The Rudder The rudder was manufactured in wood with a steel core diameter 8 mm, then a coating of fiberglass was made, followed by the painting process used in all models described before. The manufacturing process of the rudder is summarized in the following figure. Figure 2.9: Rudder Construction Process 10

25 Chapter 3 Background Theory There are a lot of hydrodynamic concepts which should be explained in a study like this. However the aim of this work is to study the behaviour under certain circumstances of a Transpac52. The resistance has been analysed and how is modified in different sailing situations, how the centre of efforts change and the methods used for obtaining this information. The aim of this chapter is to describe the different theoretic concepts involves in this work. Concepts like ship resistance, appendages resistance will be reviewed here. However, It is important to note some of the dimensionless parameters that play an important role in this kind of simulation. 3.1 Dimensionless Relations There are several factor that we have to take account in our simulations before started. Some fluid behaviours can be predicted by means of dimensionless quantities which link different forces. In this way, one of the most important relations in Fluid Mechanics is the ratio of momentum forces to viscous forces, which is called the Reynolds Number (Re) and quantifies the relative importance of these two types of forces for given flow conditions. It is a dimensionless quantity that is used to help predict similar flow patterns in different fluid flow situations. Reynolds numbers frequently arise when performing scaling of fluid dynamics problems, and as such can be used to determine dynamic similitude between two different cases of fluid flow. They are also used to characterize different flow regimes within a similar fluid, such as laminar or turbulent flow: - Laminar flow occurs at low Reynolds numbers, where viscous forces are dominant, and is characterized by smooth, constant fluid motion. - Turbulent flow occurs at high Reynolds numbers and is dominated by inertial forces, which tend to produce chaotic eddies, vortices and other flow instabilities. The Reynolds number is defined as the product of the velocity and the length divided by 11

26 the kinematic viscosity as shown in the following expression, Re = ul ν (3.1) Other important dimensionless quantity is the Froude number (Fn). It is a dimensionless number defined as the ratio of the flow inertia to the external field (in this case the gravity field). Named after William Froude, the Froude number is based on the speed length ratio as defined by him, and is defined for hydrodynamic studies as: F n = u gl (3.2) where u is a characteristic flow velocity, g is the gravity, and l is a characteristic length. In naval architecture the Froude number is a very significant figure used to determine the resistance of a partially submerged object moving through water, and permits the comparison of similar objects of different sizes, because the wave pattern generated is similar at the same Froude number only. In these cases l is refereed to the ship length. 3.2 Resistance The total hydrodynamic resistance of a sailing yacht is divided in several components: - The resistance the boat develops when sailing upright - The additional resistance developed when the boat is heeled - The induced resistance due to leeway - The resistance developed due to the action of the wind on the water creates waves In particular, the resistance developed by a boat sailing upright in calm water can be split into two main elements: viscous resistance and wave or residuary resistance which will be detailed before. Both describe what happens when a boat moves upright through the water, as in downwind sailing. When sailing between a beam reach and close-hauled, the boat heels under the effect of the thrust of the wind on the sails and it must develop hydrodynamic lift to balance the lateral aerodynamic force. As a result the boat makes leeway (4.17). In these conditions resistance generally increases, and this increase is due to two new factors that do not appear in conventional ships: Heeled resistance and leeway resistance (also called induced resistance). Historically, it was Davidson [17] who in 1936 first illustrated a complete theory of the propulsion of a sailing boat, giving a full interpretation of heel and leeway resistance. The different forms of resistance will be discussed below. 12

27 3.2.1 Viscous Resistance Because of the viscosity, particles close to the hull are adhered to it acquiring zero relative velocity. So the velocity of the particles, as is determined by the potential flow theory, is only achieved at a given distance from the hull. This provides an area, next to the body, which increases in thickness downstream of the vessel from bow to stern, leaving a retarded flow area, where the particle velocity varies from zero at the hull to the values that determines the potential theory. This area is known as boundary layer which will be explained later. The shear forces that exist in the boundary layer, and in particular forces on the body surface are produced by the viscosity and the velocity gradient within the boundary layer, and originate frictional resistance. Besides the friction effect, there is a lack of pressure aft which makes a force on the body in the direction of advance that is what is known as drag resistance of a body in a fluid undisturbed. Hence a submerged body moving at a constant speed experiences two types of resistance, both being from viscous nature. Frictional resistance and resistance so-called form. It is assumed that the frictional resistance depends on the interface between water and hull, the wet surface S m ; the forward speed of the vessel v 2 and the dimensionless coefficient of friction resistance C f as it is shown in equation 3.3. R friccion = 1 2 ρv 2 C f S m (3.3) The value of the friction coefficient, Cf, is based on tests results done in towing tanks and wind tunnels where a plate placed in the flow direction is analysed. So it is assumed that there is no form drag or wave resistance, so anything that frictional resistance is measured. With the aim of unifying the magnitude of C f which should be used in all towing tanks, the International Towing Tank Conference (ITTC) decided in 1957, at its meeting in Madrid, adopt a single formulation in order to extrapolate the results of resistance from the model to the real scale of the vessel. It is known as the line of friction ITTC-57 and has the following expression: C f = 0, 075 (log Re 2) 2 (3.4) Although the expression is used today, new expressions are proposing like the one presented by T.Katsui in his article The proposal of a new friction line [18] proposed for validation of CFD. C f = 0, (log Re 4, 3762) 0, log Re+0,56725 (3.5) where Re is the Reynolds number based on the length of waterline in calm water. The other component of the viscous resistance is the form resistance. The origin of this component is the use of the flat plate wet surface approach which involves a two-dimensional flow instead of the three-dimensional reality. The difference between these two considerations, the two-dimensional and threedimensional, this is what comes to represent the so-called form factor. This factor must 13

28 depend only on the forms of the vessel and not on the Reynolds number, which in other words means that the model and the ship form factor are the same. This factor is usually obtained in resistance towing tank tests. There are several methods for the determination of this factor. One of the most widespread within the hydrodynamic community was originally presented by Prohaska. The hypothesis underlying this method is that at low speeds, the component of the wave resistance is proportional to the fourth power of the Froude number, F n and is null when is extrapolated for a zero forward velocity Wave Resistance The creation of waves by a boat moving through the water is basically due to the fact that the boat moves through two distinct fluids (air and water)with very different densities. The dynamic pressure produced close to the hull, as described by Bernoulli s theorem, produces variations in the level of the water (waves). These variations are not compensated because the pressure of the column of air above the waves are negligible. In this case an increment of pressure appears in the bow and stern producing two main wave systems while there is a pressure reduction in the amidships. A first approach to the study of waves systems generated by a moving ship at the free surface, was introduced by Kelvin in the last century earlies. He considered the vessel as a pressure point which moves in the presence of a free surface. This pressure point generates waves in all directions. Due to this waves velocity and the point pressure forward velocity, there is an interference between waves resulting wave systems so that at some points they cancel each other and other times the effect is increased. The waves systems thus generated are known as the Kelvin wave system and an scheme is shown in the following figure Figure 3.1: Kelvin Wave System This system of waves consisting of a series of transverse waves travelling behind the pressure point and a number of diverging waves radiated from the point of pressure. In deep waters, the entire system is contained between two straight lines forming an angle of 19ž and 28 minutes with forward pressure point direction. The height of successive transverse waves decreases as we go away from the pressure point. They have a curvature away from 14

29 the middle of the ship is transversal direction and meet divergent waves at their peaks, thus constituting the highest points of the resulting waves system. These highs decrease less rapidly than when they are compared to the decay of the amplitudes of the cross-system and therefore remain the most prominent or at least the most visible of the wave train leaves the ship. From of the point of view of wave resistance, the interaction between the transverse wave systems generated at bow and stern is of extreme importance: these are located at the two extremes where the hull touches the water, and the distance between them is known as the effective waterline length (EWL). It is clear that the two systems of divergent waves cannot interact each other, since the bow system is always wider than the stern system (3.1) and as they are at the same angle to the direction of motion. However, the transverse wave systems that move along with the boat and are parallel with each other can interact in various ways depending on the speed of the boat. Linear wave theory ([19], [2], [20])shows that the transverse waves have a propagation speed, V W and a wave length L W related to each other by the following expression: where g is the acceleration of the gravity. L W = 2π g V 2 W (3.6) Now, since the transverse waves generated by the movement of the boat travelling at a speed V B move along with the boat, their speeds must be equal: V W = V B and thus boat speed can be expressed as a function of the wave length and vice versa. L W = 2π g V 2 B (3.7) For example, a boat travelling at a 6 knots produces a system of transverse waves with a wave length of 5.65 m. It is thus clear that depending on board speed, the wave produced at the bow may arrive at the stern exactly in phase with the wave produced there, and as a result the effects are added together and the boat leaves behind a hugh stern wave [21]. Figure 3.2: Bow wave in phase with the stern wave 15

30 On the other hand, the boat speed might be such that the wave produced at the bow reaches the stern exactly out of phase with the wave produced there. As a result the waves tend to cancel each other out and the boat leaves behind a stern wave of negligible size [21]. Figure 3.3: Bow wave out of phase with the stern wave This leads to a dramatic reduction of wave resistance. The most important conclusion is that wave resistance is not, like frictional resistance, proportional to the square of boat speed, but increases or decreases according to the interaction between the two wave systems produced at bow and stern. In general, wave resistance increases with boat speed because the pressure in the system increases with boat speed. Moreover there are other effects like the inclusion of appendages which may affect this as it will be discuss later. The direct determination of the wave resistance, from measurements of the spectrum of waves during rehearsals model, was introduced in the sixties of the last century, and since then has become a very useful tool, to optimize the shapes of the vessel. The analysis of the waves generated by the model is a widely used technique, recommending ITTC analysis method proposed by Eggers, Sharma and Ward in [22] the wave function amplitude. If a boat sails at certain velocity such that the wave length, L W, of the transverse wave system produced at the bow is equal to its effective waterline length (EW L), it has been seen that, thanks to the simultaneous creation of the bow and stern wave systems, a first crest is produced at the bow, there is a trough amidships and a second crest at the stern. Furthermore, it is known that in that conditions considerable resistance to motion is developed, but there is another effect: the central part of the hull, which accounts for the majority of submerged volume and thus for the buoyancy, is in the through of the wave. In this way the boat floats lower than in normal static floating conditions: it s as if the boat were imprisoned between the bow and stern waves, and its resistance increases dramatically. The boat speed corresponding to this condition is called critical speed, V c : g V c = 2π EW L = 1.25 EW L (3.8) This speed is also called limit speed, as in practice it is the fastest a boat can go in normal conditions unless planing occurs. In this case a boat can go faster than the critical speed because the hull is capable of developing hydrodynamic lift. moreover a boat can go faster than the critical speed when surfing occurs owing to the presence of large surface waves. 16

31 From the point of view of calculating wave resistance, since this depends on the wave system produced by the hull in motion, which in turn depends on the effect of every single point of the hull it is not easy to do this kind of analyses and considering the parameters that affect this. Furthermore it is also important to note the appendages influence, which modifies the wave profile as shown below. In the case of this study the parameters involved are the prismatic coefficient, C p, the volumetric coefficient C v, the beam/draft ratio and the appendages Heel Resistance As it has been mentioned, a boat sailing without heel is subject to viscous and wave resistance, and from this point of view behaves exactly like a conventional ship. This is the case in sailing from a beam reach to directly before the wind, when the driving force is far greater than the healing force. One of the reasons that the big cruisers do not sails heeled although the big surface that is above the water. On the other hand, in sails vessels the situation changes, the aerodynamic force developed by the sails produces a significant lateral component which have the double effect (figure 4.17) of heeling the boat to leeward and producing leeway (it pushes the boat sideways so that an angle is created between the boat speed and the boat s longitudinal axis, the leeway angle β. Figure 3.4: Effects of the heeling force F H In addition, thanks to the presence of a leeway angle, the hydrodynamic appendages, specially the keel, are able to develop a lift force which balances the lateral aerodynamic force. Furthermore the canoe body acts as a lifting surface as well. 17

32 However, this lift force is also accompanied by a resistance. This added resistance formed when sailing upwind is called induced resistance. Independence of the effects linked to the presence of appendages, there is also a variation in the resistance developed by the bare hull when it is heeled. This is partly due to a change in the wetted surface and partly to the variation in the geometry of the submerged hull volumes: the effect in this case is called heel resistance Induced Resistance The induced resistance is a component which appears because of lift generation in an asymmetric flow. it is of importance for wing-like bodies such as keels and rudders, but also for hulls under certain circumstances. Typical examples from hydrodynamics are sailing yachts at non-zero leeway, rudders at non-zero angle of attack, etc. It should be noted that the induced resistance is an inviscid phenomenon, governed by Euler equations. However this additional resistance can be determined subtracting the upright resistance from the total resistance measured. R i = R Rup (3.9) The first effect of this resistance is that is closely linked to lift generation, which will be explained in the next section. The second effect are the vortices. Figure 3.5: Vortex generation around a keel [1] Figure 3.5 shows a sailing yacht keel moving at an angle of attack equal to the leeway angle of the hull. Because there is nothing preventing the flow on the pressure side of the keel to escape below the tip to the low pressure on the other side, a cross flow around the tip is generated. This means that the flow on the entire pressure side will have a downward velocity component superimposed on the main flow backward. On the suction side, the opposite is true, and the effect increases toward the tip on both sides. Thus, the flows from both sides will move in different directions when they meet at the trailing edge. As a result, they will start rotating around an horizontal axis. The v0rtex sheet leaving the trailing edge is unstable, and it ultimately rolls up into one concentrated vortex behind the keel in this case. Because the trailing vortex system contains rotational energy, it corresponds to an increase in resistance. Note that a prerequisite for the trailing vortex system to appear is a free end of the wing. If there is no free end, no trailing vortices will develop, and there will be no induced 18

33 resistance. The trailing vortex system has a very important effect on the flow. As can be seen in figure 3.6 all vortices on one side tend to generate a downward flow on the other side. They also tend to generate an upward flow outside the sheet on their own side. The result of all this is a downflow in the entire sheet, but an upflow outside the sheet. These flows are called downwash and upwash respectively. Figure 3.6: Vortex generation around a keel [2] Of particular interest is the downwash generated at the wing. The downwash velocity, denoted w, is superimposed on the undisturbed velocity U yields the total velocity U and the induced angle of attack α i. tan α i = w U α i = w (3.10) U According to the Kutta-Joukowski theorem, the lift force on a bound vortex of strengh Γ is at right angles to the approaching flows and its magnitude is ρuγ. However, the lift and drag shall be computed at right angles to, and parallel with, the undisturbed flow obtaining the following relationships. L = ρuγ cos α i (3.11) Di = ρuγ sin α i (3.12) 19

34 and it is possible to do the following approach tan α i = w V α i = C Di C L (3.13) Finally, it is important to talk about the elliptical load distribution. According to equation 3.12, the induced drag is proportional to the induced angle of attack, which in turn is caused by the trailing vortices. This is another way of relating trailing vorticity and drag, as compared to the energy explanation. But, this way to analyse these effects could be not very useful for practical calculation because the circulation and induced angle of attack are not easily obtained. However the integrated effect of the trailing vortices may be obtained analytically with the following definitions: L C L = 1 2 ρs pu 2 (3.14) C Di = 1 (3.15) 2 ρs pu 2 where L and D i are the total lift and induced drag forces and S p the projected wing area, the following simple expression are obtained ([23], [24] and [25]) C L = D i 2π α (3.16) AR C Di = (3.17) πar The numerator 2π in the previous equation is for symmetric wins in inviscid flow and with α radians. AR is the aspect ratio of the wing, defined for an arbitrary planform as: C2 L AR = b2 S p (3.18) where b is the span. For a trapezoidal wing, the aspect ratio is the span divided by the mean chord. The projection of the area shall be taken in a direction at right angles to the plane of the wing. In addition, this demonstrates a linear relation between C 2 L and C Di, which can be used to check the measurements. Finite wing theory also shows that the elliptical circulation distribution gives minimum induced drag and that it may be obtained with a wing of elliptical platform. Furthermore, the computation of the lift and induced drag for arbitrary lift distributions is complicated and no simple expressions like the previous showed exist. Instead, the concept of an effective aspect ratio, AR e, is introduced. This is always smaller than the geometrical one defined previously. ARe = C2 L πc Di (3.19) where C L and C D are here the lift and induced drag coefficients for the non-elliptical distribution. 20

35 If two wings are mounted in tandem (which is the case with keel and rudder), to calculate the lift of the last wing it is important to know how much the direction of the flow has been altered by the first wing, or, in other terms, what the magnitude of the angle of downwash is. A simple approach which has been used for some time is as follows: the angle of downwash is half the leeway angle, or: Φ = 0.5β (3.20) When it is approached theoretically, as explained by Hoerner [26] this angle can be calculated from: Φ = 2C L πare k (3.21) Hoerner also states that for aircraft wings (ie. wings with high aspect ratios) and an endplate at one end perpendicular to the wing (for instance an aircraft fuselage or, in this case, the hull) this angle can be calculated from: Φ = 1.6C L πare k (3.22) All formulas in the last section assume an elliptical lift distribution over the wing. Because of the shape of the keel and rudder and of the presence of the hull which induces interaction effects this assumption is anything but valid. To be able to calculate proper values for these formulas, use will be made of the effective aspect ratio. This effective aspect ratio is dependent on planform of the wing and the dimensions of the hull, but a good approximation can be made by applying: ARe = 2AR (3.23) 3.3 Appendages hydrodynamic To introduce appendages, it is interesting to talk first about the wing section theory which explains the mechanisms of interaction between the various parts of the planform (especially the keel and the rudder) and the surrounding water, ad in particular the reasons why an object (which below we will refer to as a profile) is able to generate lift. This theory comes from the aeronautical industry, and it has made a determining contribution to the development of sailing boats although the aeronautical industry is younger than the naval industry. This is in fact owing to to the substantial morphological analogy between a planform and an aeroplane wing. In aerodynamics - and in hydrodynamic as well - a wing profile means a solid body immersed in a fluid in motion, with a shape that tends to be elongated in the direction of the incident flow. The main dimensions that define a profile are the chord c and the wingspan t If the flow of the fluid moving from left to right is represented and consider the profile placed at right angles to the incident flow, the fluid path lines around the profile is shown in figure 3.12 with the dynamic pressure distribution around it. The entire lower part is 21

36 Figure 3.7: Analogy between a planform and an aeroplane wing Figure 3.8: Rectangular Wave Profile invested by a positive pressure field which is thus directed towards the wing surface and tends to push it upwards, while the upper surface has a field of depressions, and hence forces that tend to suck the wing upwards. And, contrary to what one may intuitively think, the effect of the depression is far greater than that of the pressure in the lower part. Figure 3.9: Flow around a wing profile The consequence is that the result of this pressure distribution is a force called the aerodynamic force which has one component directed upwards, called lift, and one directed backwards, called resistance or drag. If the angle of incidence of the flow on the profile is increased, there is also an increase in the aerodynamic force (hydrodynamic in the case of a liquid) but a new phenomenon intervenes. A depression is generated in the after part of the upper surface of the wing can reach values that cause partial detachment of the boundary layer and hence vortex shedding. 22

37 This causes an increase in the resistance component due to the energy lost by the turbulence. In addition, if the angle of incidence is increased, the turbulence will invest the entire upper of the wing can reach values that cause partial detachment of the boundary layer and hence vortex shedding. This causes an increase in the resistance component due to the energy lost by the turbulence and a drastic reduction of lift. Figure 3.10: Boundary Layer Separation For the analysis of the pressure distribution on the profile faces, the pressure coefficient is used. It is a dimensionless coefficient obtained simply applying Bernoulli s theorem between a point on the surface profile and a free flow point at infinity. C p = p q 0 = p p 0 q 0 = 1 ( ) 2 v (3.24) where: p and p 0 is the static pressure at a point in the profile and in the free flow respectively, v and v 0 the velocities and q 0 the dynamic pressure in the flow undisturbed. v 0 q 0 = 1 2 ρv 0 2 (3.25) An example of C p distribution through a profile in both sides is shown in the following figure. Figure 3.11: Hydrodinamic actions 23

38 It is possible to see that there is an area with high pressures (negatives and positives) in the profile leading edge, with C p = 1 in the stagnation point. C p distribution through the profile gives an idea about the lift distribution in it, where the lift center will be close to the leading edge. Furthermore, figure 3.12 shows a general idea about lift. However it is important to note that ships work in both sides and because of this the profiles are symmetric unlike in aeronautics that they are asymmetrical. From a mechanical point of view, the interaction between the fluid and the profile can be summed up as the coming into being of dynamic actions whose resultant is applied to a point on the profile (this is called the aerodynamic force) and a moment M (called the aerodynamic moment) whose value depends on the point where the resultant is applied. The resultant of the aerodynamic forces can then be broken down into two components in the direction of the relative speed and perpendicular to it. These are, respectively, drag D and lift L. Figure 3.12: Hydrodinamic actions If the profile is fixed and the fluid in movement with speed V, the expressions for the aerodynamics (hydrodynamic) actions are: D = 1 2 C DρAv 2 (3.26) L = 1 2 C LρAv 2 (3.27) where A is the wing surface, ρ the density of the fluid and v the velocity of the fluid. The aerodynamic coefficients C D C L are known respectively as the drag and lift coefficients of the profile, and for wide ranges of the Reynolds number depend solely on the angle of attack. It is known [21], [27], [28], [29] that as the angle of attack increases, the coefficient of lift C L increases more or less in proportion until it reaches its maximum value (which for wing profiles is usually around 20 ); once this value is exceeded there is a sharp drop in lift corresponding to the situation of stall described before. Note also that for null angles 24

39 of incidence C L is null( no lift is produced) and the drag coefficient C D is minimal. On the other hand, as the angle of attack increases, so too does the drag coefficient C D, but more than in proportion and to be precise as function of the square of the angle of attack. This relation is extremely important because it shows that the production of lift is always accompanied by a rapid increase in resistance. In fact the efficiency of a wing η is defined by the relation: η = C L C D (3.28) From this it is clear that the efficiency of a wing is maximum for values of the angle of attack well away from stall. In the case of the current hull appendage, it is needed to mention other factors of difference compared to the theoretical case: - The wing is connected with the hull and the flow in this area will be different from the theoretical expected. - The appendage is close to the free surface and this too makes for a difference from the theoretical situation. - The free surface produces a reduction of the lift curve slope and added resistance due to surface waves originating from the pressure field around the keel. - Wingspan is finite and thus there will be tip vortices. - When the boat heels the hull appendages come close to the free surface, modifying the flow around them. 25

40 Chapter 4 Experimental Setup 4.1 CEHINAV Towing Tank Experimental tests have been carried out in the towing tank of the ETSI Navales (U.P.M). Inaugurated in 1967 with dimensions of 56 meters in length, 3.8m. wide, and 2.2m. of depth, its length was later increased to 100m. It was projected by Luis de Mazarredo in order that students of naval architecture would be put in contact with the methods of experimentation in hydrodynamics. In addition to academic labour it is also used for the optimization of ship hull design and forward resistance assessment. Figure 4.1: CEHINAV towing tank facilities There is a car made of a steel structure that pulls the models. the car rolls on two lines of tracks anchored in the lateral parapets of the channel. The alignment and levelling of these tracks have taken place with great precision to avoid alterations of the speed of the car during the tests. The car can reach a maximum speed of up to 4,5 m/s which allows to carry out tests for high speed vessels. On the other hand the maximum models length is 3 meters, according the scale laws, to avoid that the waves generated by the model could affect the measures. 26

41 4.2 Aim of the experiment The scope of this work is obtaining more information about the hydrodinamic aspect of the hull and the appendages, their behaviour and their influence on the hull. In the analyses procedure used for yaw moment, the actual side force distribution between the keel and the rudder is of significant importance in assessing the yaw moment (Kartgert [30]). This distribution however is strongly and influenced by the underlying assumptions made in the Extended Keel Method (J. Gerritsma [31]) on the influence of the keel on the rudder. This influence makes itself felt through: - A reduction in free stream velocity of the incoming fluid on the rudder (since it operates in the wake of the keel) - A reduction of the effective angle of attack on the rudder through the vorticity shed off by the keel caused by the lift generated on the keel, i.e. the downwash. Furthermore the appendages could have also a beneficial effect on the hull. In order to account all these effects, several experimental and numerical tests have been done Measurement Scheme The measurements have been carried out systematically according to a present scheme. An identical series of tests have been carried out with the model with and without appendages as it is shown in figure 4.2 in upright condition and under leeway and heeled condition. Figure 4.2: Test cases With the conditions described, the following tests have been done - To be able to determine the total resistance of the hull and appendages, tests with the ship in upright condition in the speed range from Fn = 0,16 up to Fn = 0,60 (4 kn up to 14 kn ) according to Froude law scaling. These runs have also been used to measure the total and the residual resistance of the appendages. 27

42 - Tests modifying leeway angles β = 0, +2, +4, +6 and heel angle ϕ = 0, 10, 20 - For the intermediaries velocities 8 and 10 knots (Fn. = and 0.420), the tests previously mentioned has been done moving the rudder angle. The rudder angles were also chosen to provide a wide range of test data for δ = 12 to δ = 12 varying rudder angle each 2, except tests were high angle rudder measurement were out of range. In these cases the following data have been taken: Drag and Lift measurements on the hull and on the appendages in all tests, and Wave cut profiles, in some tests, at different distances as has been described in the experimental chapter. To obtain these data, different elements needed to be mounted. In the following sections, how this devices are mounted on the different elements are explained. 4.3 Data Acquisition Equipment The car is equipped with a complete data acquisition systems (abbreviated with the acronym DAS or DAQ) which allows convert analogic waveforms from the dynamometers installed in the models into digital values for processing. The components of DAQ includes the following elements: - Sensors that convert physical parameters to electrical signals. In this case the dynamometres and other devices. - Signal conditioning circuitry to convert sensor signals into a form that can be converted to digital values. - Analog-to-digital converters, which convert conditioned sensor signals to digital values. When the car starts, the model is joined to the car by means of a pliers and the dynamometers. After achieving the sail speed the model is freed and the resistance is measured by the drag resistance dynamometer. However this kind of experiment is different from the conventional ships because they usually sail with leeway and heel. For this reason additional dynamometers are set on the ship (2 and 4 in figure 4.3), which are available to measure the lateral forces on the model. In this case, two blocks strain-gage dynamomenters (figure 4.4) have been used. Figure 4.3: Data Adquisition User Interface 28

43 Figure 4.4: Block Strain-Gage The way that resistance is measure in this kind of yacht is little different from conventional ships. However, the method used in this study is the most commonly used in yacht tests (Van Oossanen [32], and Zamora et al.[33]) where the model is restrained in the amidships position at a pre-determined leeway angle by means of arms fixed to the model fore and aft (figure 4.5).These arms are built in such a way no vertical or longitudinal forces are exerted on the model. This permits to set up the model in the dynamic sail position, and it is possible to do measures with a certain heel and leeway like the real model and allows that the model freely sink and trim with speed. Figure 4.5: Measurement Setup 29

44 These sink and trim mentioned before are measured by means of two vertical lasers installed in the car, one forward and other aft, which measure vertical displacement fore and aft, and another one situated longitudinally which is used to measure longitudinal displacement. These measures are needed to calculate the model sink and trim. In the following pictures, it is showed how the arms are assembled on the hull (figure 4.6 left) and how the block strain-gage is connected (figure 4.6 right). Figure 4.6: Heel and Leeway Mechanism (left) and Block Strain-gage (right) Forces on the car dynamomenter (drag) and forces on blocks strain-gage dynamometers (lift) are measured according tank axes. The required angle of heel at speed is usually realized by moving a weight transversely along the deck before the run starts, which position is the often fine-tuned to compensate for the change in transverse stability of the model with speed and to avoid dynamometers overloads. The resistance of the model, equal to the towing force, is measured in the towing connection between carriage and model, which connecting is also able to accommodate any vertical movement of the model. Although for this kind of models ballast weights need to be moved longitudinally between each run to compensate for the fact that the model is not towed from the center of the resultant aerodynamic force. But in this case the tests have been realized without moving these ballast weights in order to calculate forces in the same initial waterlines with and without appendages approximately, (fig. 4.6). Once the measures have been taken by the devices and following the previous scheme, the data acquisition is done by a SPIDER8 (device made by HBM, see figure 4.7). Forces and Moments are recorded independently and showed in real time by CATMAN software prepared for this kind of tests (figure 4.8). This is the software used in CEHINAV and was adapted to obtain data not only from the hull with the appendages, but also from the appendages separately [34]. An acquisition card is connected to the computer via LTP port, and CATMAN program HBM is responsible for processing the digital signals from the card. The software used allows to assign one measure for each channel and allows to calibrate the signals before starting the runs and avoid that any noise could affect to the measure. Figure 4.8 shows a screen of the software used and how the channels could be assigned and figure 4.9 shows the user interface created for this work 30

45 Figure 4.7: Device Used for Data Adquisition Figure 4.8: Signal Calibration and Transformation Figure 4.9: Data Adquisition User Interface 31

46 4.4 Appendages measurement arrangement Forces and moments on keel and rudder are measured separately with their own dynamometers. They are attached to these dynamometers in such a way that the forces acting on them are only absorbed by them, and not partly by the hull. In this way when the model or the element is moved, the axis of the dynamometer changes. Figure 4.10: Appendages Dynamometer Axes Moreover there is a small gap between the appendages and the hull to avoid the hull interference in the measurement. In the following figure the final setup with all of the dynamometers assembled is shown. Figure 4.11: Measurement setup Keel Measurements A five-component dynamometer, incapable of measuring z- direction forces is used on the bulbed-keel. This required a special configuration which is shown in figure 4.6. The keel is set in a fixed position (figure 4.12). To seal the junction between the keel and the hull, a moldable paste has been used that allows light keel movements and prevents water can get into the boat. 32

47 Figure 4.12: keel set Attached to the keel, a block made of high density polyurethane is set. It works as a clamp as well to allow easy exchange with other keel models. Data recorded is done by an other HBM Spider 8-channel acquisition card, which have used for the keel and the rudder. Finally, a dynamometer and conditioning signal power supply are incorporated in the acquisition card. Figure 4.13: keel dynamometer Rudder Measurements On the other hand, the rudder is attached in such a way that it is possible to quickly set a rudder angle, unlike the keel the rudder is not fixed to the hull. In this case it was not possible to use the same paste because the aim was to move the rudder without taking out the model from the water. A simple mechanism was improvised to permit that the rudder could turn and the water does not inundate the ship. A six-component dynamometer, capable of measuring forces and moments in the x-, y- and z- directions, are used to measure the forces on the rudder. The measurement and 33

48 positioning system consists of 4 components as seen in the figure, along it enables angular positioning of the rudder with a resolution of degrees, and excellent repeatability thanks to the closed-loop control. (figures 4.16) Figure 4.14: Rudder set Figure 4.15: Rudder canoe body intersection Figure 4.16: Dynamometer and rudder mechanism 34

49 The first component is the capsule made with polyurethane that connects the engine to the dynamometer, the second component refers to the engine and gearbox, technically, it is refereed to a GP32A engine Maxon Motors with a gear box EC32 made by the same manufacturer, the control system includes a motor driver of EPOS7010 type, overall it has a 80 Watts brushless motor, on a reduction of 43: 1 and 500 encoder pulses per revolution integrated with the shaft. This set is coupled with the control card and the control card is controlled by means of LabVIEW, which controls the rudder movement by means of a graphical interface prepared for it (figure 4.9). The third element is the piezo-resistive six components dynamometer Fx, Fy, Fz, Mx, My, Mz (Manufacturer and reference MC3A AMTI). Finally, the last element is the rudder made of polyurethane with a steel core coated with fiberglass. In the next figures, schemes about the measures have been taken in the appendages is presented (fig 4.17) and how the rudder equipment is assembled are presented (fig 4.18) Figure 4.17: Diagram control and data acquisition appendices sailboat 35

50 Figure 4.18: Rudder complete assembly 4.5 Turbulence stimulator Since the speeds at which the tests are done are relatively low (which is caused by the fact that the speed of the model has been scaled according to Froude s scaling laws), there is a chance that the flow around the hull will remain laminar when the flow close to the real model will be turbulent. In order to achieve dynamic similitude between a ship and a model, the flow within a model s boundary layer must mimic the flow in a ship s boundary layer and around the appendages as well. Figure 4.19: Turbulence stimulator Consequently, to make a model s boundary layer more representative of a ship, the boundary layer flow must be made turbulent. The primary method to make the flow with in a 36

51 model s boundary more turbulent is turbulence stimulation. Turbulence stimulation consists of tripping, or causing the laminar flow to transition into turbulent flow. In order to trip the flow, foreign objects are generally placed on the forward portion of the model s hull. These objects include sand grains, small pins, Hama strips, and trip wires. In this case, as it is shown in figure 4.19 the chosen option has been small pins. Turbulence stimulators introduce instability to the flow around a model. This instability disrupts the flow and causes it to be turbulent. So, while the flow that would normally be associated with the model should be laminar, the turbulent stimulator causes the flow to become turbulent. This turbulent flow more closely represents the flow experienced within the boundary layer of a ship and her appendages and increases the frictional drag experienced by the model, more closely aligning the model s frictional drag with that of the full-size ship. All these items are featured on models in the Hydromechanics Lab and are designed to disrupt the smooth, constant shape of the hull design and thus prevent the water flowing around the model from remaining laminar. An effective turbulence stimulation method will allow reliable frictional and residuary resistance data to be obtained. It would appear that, through the use of turbulence stimulation, the problem of similitude between model and ship has essentially been resolved. However, a new problem has emerged with turbulence stimulation. There is no set methodology for determining the location, type, or amount of turbulence stimulation. There are limited guidelines, primarily of empirical nature, to answer questions about what type of stimulators should be used and/or where a given type of stimulator should be placed on a model. Currently, the answers to the above questions are different for each ship-model testing facility and ship-model tester. There is no consistent method, based on flow physics, that can be used for a given ship type or model size between the various towing tanks around the world. It is left for each person to discover his or her own method based on trial and error and the constant tweaking of results to achieve the desirable outcome. In this work a numerical analysis has been done to study their influence in the final results, [35]. 4.6 Wave cut tests It is assumed that the model moves in a deepwater region not limited horizontally or in a tank sufficient to consider infinite dimensions. However, these assumptions are not indispensable to the evaluation methods of waves, and can adapt the method of analysis to address the case of a long rectangular channel beam and finite depth, so it is easy to model numerically the case. The aim of the wave cutting tests is to determine the wave resistance, and in this work they are used to obtain a qualitative analyses about how this resistance is modified with the different elements added. For this method the longitudinal section described by Bravo Ramos [36]. The system for height measurement is based on a probe of the resistive type and comprises two main parts wave height sensor: the support and the electrodes which are assembled on a movable cross slide that was able to move transversally to the direction of the model motion (Fig. 4.20). The electrodes are two stainless steel tubes 30 cm in length are dipped partially into the 37

52 channel. The conductivity between the two electrodes is a linear function of the length of the submerged electrodes. Changes in water level in the channel (due to the passage a wave for example) are instantly transformed into proportional changes conductivity by the signal conditioner, they are transformed into voltage. Figure 4.20: Wave Pattern experimental setup and sketch of the data acquisition device Each probe recorded a time history of the wave elevation related to a value of the y coordinate. Water level variations in the towing tank are transformed instantaneously into proportional variations of conductivity, which by means of a signal conditioner, are transformed into electrical signals and change to the real value in millimetres again. Due to the high repeatability of the wave pattern generated by the model, the wave field has been reconstructed by means of a series of time-dependent readings. Moving the probe array each run, it has been possible to cover a large portion of the generated wave pattern. These tests were done with to obtain new experimental data to compare with the numerical analysis and to observe the appendages influence in the residual resistance. Probes are situated in three different positions 0,5665B, 1,058B and 1,5508B where B is the beam of the sailing ship. These distances were chosen because the estimators needed to analyse the wave making resistance are known, and they are necessary for analyse wave making resistance. 4.7 Uncertainty Analysis Forces uncertainty One of the aims of this work is compare numerical results with experimental. The experimental tests have an uncertainty due to the instruments (acquisition, calibration and set up) and the environment where the test is done. These are called systematic errors. In table 4.1 the main errors are presented. 38

53 Item Type of error Size Velocity Carriage set up 0,004 m/s Temperature environment 0, 1 Heel Error Misalignment set up 0, 25 Model Misalignment set up 0, 1 Keel Misalignment set up 0, 1 Rudder Misalignment set up 0, 025 Carriage Dynamometer acquisition 0,00012 mv/ V 2 Components Dynamometer (H) acquisition 0,00012 mv/ V 5 Components Dynamometer (K, Kb) acquisition 0,00012 mv/ V 6 Components Dynamometer (R) acquisition 0,00012 mv/ V Table 4.1: Uncertainty elements Furthermore, there are other kinds of errors due to the impossibility to repeat the same measure twice. They are the precision errors and are estimated as two times the standard deviation of the sample series. In this case four measures for the same point were taken to determinate it. Finally, the total uncertainty of a single measurement is calculated as: [ n ] U 2 2 = b i + P 2 (4.1) i=1 where b 1..N are the bias errors of the N elementary error sources and P the precision of the samples series. [37] For each case, errors have been analyzed independently. The following table presents a resume with the maximum and minimum values obtained. H + K + R K R Drag Lift Drag Lift Drag Lift Max [%] 3,25 5,67 4,75 2,31 6,62 5,10 Min [%] 1,43 4,22 3,01 1,90 3,56 1,75 Table 4.2: Maximum and minimum errors produced in the measurements In addition, as it is possible to observe in figure 4.9, measures were taken once the ship has achieve her dynamic equilibrium. In this way, the variation of the measures taken vary very little Wave cut uncertainty On the other hand, those errors are not the only ones. Wave elevations measurement have their own uncertainty. They are measured in parallel plane to the ship s center line at a given 39

54 distance from the hull. We make dimensionless with the following definition: ζ W = z L (4.2) where ζ W is the dimensionless wave elevation, z the measured wave height and L is the model length between perpendiculars. In earlier tests (Souto-Iglesias et al. [38]), the wave cut uncertainty analysis in the ETSIN where developed. On the basis that the bias error in the model length was negligible, two elemental bias errors for ζ W were considered. The first is associated with the error in the electric current conversion ( ) and the second is associated with the static calibration ( ). The error in vertical orientation of the probe was considered to be very small in comparison with the other errors. About 100 x-station were considered in that test at a constant distance from the ship s center line, and the bias error due to the situation was estimated as 1 mm. The precision error depends upon the x-station. Some values were taken and evaluated. The worst error was approximately 5,3% and the best one was 0,55%. 40

55 Chapter 5 Experimental Results In the previous chapter (section4.2.1) the tests done in this work were described. In the following section, these results will be analysed. The canoe body, the bulbed keel and the rudder will be analysed together and separated. 5.1 Upright Tests The first tests done are with the ship in upright condition where the resistance could be analysed with and without a certain leeway. This allows us to obtain the induced resistance. First, the canoe body has been tested to analyse the influence of the resistance components. Analysing the results, the influence of the viscous resistance over the total resistance is shown. Figure 5.1: Canoe Body forces descomposition In the previous figure, it is observe how the viscous resistance is increasing with the velocity, but its influence over the total resistance decreases. In the lower velocity, almost the total resistance is due to viscous effects and for the higher is close to the 40%. After analysing the canoe body results, the next step will be to analyse the overall resistance when the appendages are added, as it is shown in figure

56 Figure 5.2: Ship Total Resistance with different configuration As it was explained in the nomenclature H is used to refer to the Canoe body, HK refers to the canoe-body and bulbed-keel set, HR is used for the Hull and the rudder and finally HKR is used for the tests where all the components are mounted. It this figure (5.2) the overall resistance is increasing according new elements are added to it. As the bulbed-keel is bigger than the rudder is normal to expect than the total resistance will be higher. However, if we compare the resistance over the canoe body, subtracting the resistance measured on the appendages to the total resistance, we could evaluate the effect of each component on it. Figure 5.3: Canoe Body Resistance without appendages In figure 5.3 it is observed that the canoe body resistance with the rudder is lower than the case without appendages. One of the reason of this could be the effect of the wave produced by this appendage that helps to decrease the hull resistance. The keel increases the resistance on the canoe body while the presence of both appendages increase as well the 42

57 resistance. However, in the presence of both appendages the effect is very similar to the case with the keel and is not lower as it could be expected at the first moment. If the wave contours are compared, we could see the different profiles obtained in each situation: Figure 5.4: Wave Cut for Fn=0.336 (left) and for Fn =0.420 (right) In figure 5.4 all the wave cut at the distances described in section 4.6 are presented. In these figures it is possible to see the effects of the appendages on the generated wave. In these figures the dimensionless length of the ship is represented (ship is situated from 0 to 1) with the wave height. In all figures the higher amplitudes are presented in the hull with all the appendages. In the closer distance ( times the beam) it is observed the position of the appendages in the places where the changes are more significant. 43

58 Furthermore, adding the keel the values compared with the canoe body alone tests are increased in general. The amplitudes and the area under the curve are higher in both cases. The values obtained are similar to the cases where the keel and the rudder are mounted. On the other hand, lower values are obtained in the cases where the rudder is mounted. It seems that the rudder wave opposes the wave-pattern of the hull decreasing its resistance [9],[39]. Trying to obtain more information, we have studied the influence of the appendages subtracting the wave produced by the appendage to the wave produced by the canoe body. Figure 5.5: Wave Cut difference for Fn=0.336 The conclusion from these analyses was that adding the keel should increase the wavepattern resistance and it has a negative influence on the canoe body. The main reason of that is crest lines from the keel waves generally lie on crest lines from the bare hull waves; whereas adding the rudder should reduce the wave-pattern resistance, because the crest lines lie on troughs from the bare hull for the velocities tested. The rudder has more effect on the model with keel only (as compared with the bare model) because the waves are larger for this model and so interferences within the wave-pattern have more effect. This is the reason the waves do not increase so much when both appendages are mounted Appendages Once the canoe-body has been analysed, the next step will be the study of the appendages coupled with the canoe-body in upright condition and with certain yaw. Keel In the case of the keel only resistance analyses for leeway 0 and 2 are presented as it is shown in figure 5.6 and how the lift changes with the velocity with different leeway angles (5.7) The resistance behaviour looks normal. The resistance is increased with the velocity and with the leeway angle. In the lift case, it is interesting to note the keel behaviour. The values with the higher velocities are influenced by the deterioration suffered in lift. In the following figure it is 44

59 Figure 5.6: Keel Resistance possible to see how the profile begins to stall for high speeds close to 4 degrees. For the other velocities the lift behaviour is within the straight part. Figure 5.7: Keel Lift In this case, the values it looks that the stall starts with very low values. One of the possible reasons of this behaviour may be due to the reduction of the incidence angle because of the cross flow influence below the hull. It is important to note that more studies have been done with the keel changing its geometric parameter but they are not been included in this work, but they will be presented in future works. Rudder In the case of the rudder, two configurations were tested experimentally and the results are presented in this section. First the rudder without the keel presence has been studied and then with the keel presence. The goal of these experiments is to observe how the flow disturbed by the keel arrives at rudder and the effects that the flow produces in the rudder. 45

60 To analyse the rudder, this was tested firstly in a wind tunnel, where the C L and C D results for F n = 0, 252 (Re = ) where compared with the results obtained in the towing tank (figure 5.8). After wind tunnel tests, the analyses in the towing tank for the velocities studied were done, in different leeway situation obtaining the results presented in figure 5.9. Figure 5.8: Wind Tunnel C L and C D Results F n = 0, 252 Figure 5.9: Lift and Drag Rudder Curves without Keel 46

61 In figure 5.8 a good approach is obtained in the lift results but it is not the case in the resistance analyses. In these ones, negative values were obtained for negative rudder values that is very strange. There is several reasons why these values are obtained. There are several reasons why these values can be obtained. Among them could be a bad performance of the tests or the existence of possible asymmetries in the model. On the other hand, in figure 5.8 it is observed how the rudder lift curves are shifted in the y positive values direction with a variation according to the leeway angle. Furthermore, if we try to obtain the trend line we could observe that the slope is the same for all of them. Finally, it is important to remark that the rudder angle 0 is always the rudder amidships. Trying to see this phenomena better, we have compared the results of the rudder isolating it. To do that the rudder angle have been subtracted by the leeway angle, so we can compare the rudder forces values in the same position. Figure 5.10: Rudder Lift Comparisson To obtain more information about the rudder behaviour wave cut analyses were done to observe its influence when it is placed amidships and with a certain angle. Figure 5.11: Rudder Lift Comparisson 47

62 In these figures are shown that not only the viscosity resistance is modified when the rudder is turned but also the residual resistance as well. In addition, in this tests the wave cut at this distance is shown but in the numerical analyses it will be shown how the free surface is modified in both sides Keel and Rudder iteration In the previous sections, the keel and the rudder have been analysed alone. When they are mounted together there are some interesting effects that have influence in the resistance values. In this part we will focus on the rudder behaviour and how the keel presence forehead can affect its efficiency. First the results obtained for the rudder for different angles and with different leeway in upright position are presented in figure Figure 5.12: Lift and Drag Rudder Curves The results follow the same trend seen in the case of hull with rudder without keel 5.9, the higher leeway, the higher lift and resistance. However, if we compare the results, we could observe that for identical cases like leeway 0 or 2, the values differ. As it is seen in figure 5.13 the values are similar close to the angle 0. The presence of the keel forward modify the lift rudder behaviour especially in higher angles. However when the ship sails with leeway, this effect is more accentuated. In this case, not only affect the downwash produced by the keel but also the downwash produced by the canoe body. 48

63 Figure 5.13: Keel Lift effect over the Rudder The same analyses have been done for the drag, comparing the results with and without the keel as it is shown in the following figure. Figure 5.14: Keel Drag effect over the Rudder Looking the figures, both the upright and the leeway cases it is possible to observe that 49

64 when the rudder is aligned with the keel or in the forward direction there is an advantage, but when the rudder is turned this advantage is lost, because the resistance with the keel is higher. When the rudder is out of the keel wake influence different phenomena like the cross flow could influence on the rudder. In addition, the C D C 2 L relation (figure 5.15) has been also compared. It is seen that with no leeway for the same drag the rudder has more lift in the case with the keel. But when there is a certain leeway this advantage appears only for positive rudder angle values and obtaining a worse behaviour for negative angles. Figure 5.15: C D C 2 L Rudder relations After this comparison,it is interesting to know the relative importance of the different resistance components when considering the upright resistance of a sailing yacht hull. To do that, the figure 5.16 has been set up. In it, the relative contribution of the three elements: canoe body, bulbed-keel and rudder as function of the forward speed of the yacht, is presented. There is a change in the rudder behaviour when both appendages are mounted. In this way, to observe this, the rudder resistance in free flow with and without the presence of the bulbed-keel in front of it and the reduction of the velocity in the wake of it was measured. As it was expected the rudder resistance (figure 5.17 left) decreases in presence of the 50

65 Figure 5.16: Percentage distribution of Resistance keel. This phenomena is related with the reduction of the flow velocity behind the keel as it is shown in figure 5.17 (right). The only way to quantify this is to calculate the difference in the resistance of the rudder with and without keel, in both upright and leeway/heeled conditions. Dividing the resistance without keel by the resistance with keel yields a fraction of which the square root is the fraction of the flow velocity. (This is because resistance is a function of flow velocity squared) The expression is the following one: V K V wk = RK R wk (5.1) where V K and R K are the velocity and the resistance in presence of the keel and V wk and R wk are the velocity and the resistance without the keel presence. Figure 5.17: Rudder Lift Comparisson The keel acts as a barrier that slowing the fluid down. The consequence is the flow arrive to the rudder with a lower velocity and the resistance is also lower. Downwash The phenomena seen before is called downwash and basically is the change in direction of water deflected by the hydrodynamic action of a wing (airfoil, keel, rudder...) in motion, 51

66 as part of the process of producing lift [40]. Applying this definition to the case studied, theoretically, if it did not have modification of the flow, when the boat sails with a leeway and heel angle, the angle of attack of the flow in the rudder would have been βcosϕ. This is not the real situation, the flow modifies in the presence of the keel and hull so that this angle is reduced. Following Keuning [30] downwash angle, averaged throughout the rudder span can be calculated looking for the angle of zero lift in the rudder δ 0. To determine these values, first as it was done in the case with the rudder alone the resistance and lift results but in this case in the situation with the keel is forward. Figure 5.18: Downwash and Lift Vanishing Angle definition The most interesting conclusions from these tests are obtained when we compare the cases with and without keel and was analysed in the previous section (figures 5.13 and 5.14) With neither leeway or heel, the resistance for small rudder angles is lower in the case that the keel is forward the rudder. However for high angles this advantage is lost and the resistance with the keel is higher. The same effect occurs with a certain leeway. The lift changes and the resistance is increased as well. Lift Vanishing Angle Downwash Leeway Fn Fn Fn Fn Table 5.1: Downwash and Lift Vanishing Angle. Heel 0 Van Oosanen [32] recommends a reduction of effective value of the angle of attack of the rudder βcosϕ by half. In table 5.1 results for heel 0 are found. The values of side force are given in figure 5.12 (positive rudder angle in weather helm). Results suggest that a reduction of a 50% in the angle of incidence is exaggerated for the tested keel and rudder, probably due to the high aspect ratio of the keel. Another surprising result is that downwash reduces when increasing the speed, which is to say when increasing the load of the keel. 52

67 5.1.3 Effects on the Sink and Trim After analysing the different results obtained in the experimental tests, other effect evaluated was the ship dynamic behaviour and how the appendages can affect to it. In this way, the first analyses consist on compare the results in the upright tests with and without appendages. In figure 5.19 it is observed sink and trim results. If we analyse the sink, we can check as effectively as the velocity increases, the boat sink is higher. It also curious the behaviour at low speeds where one of the velocities studies shows a decrease of depth which value is lower than in the equilibrium position. This is influenced by the trim. Figure 5.19: Sink and Trim Results However, if we observe the sink results is observed that for high velocities the higher sink is produced in the case that the hull is alone and the lower in the case for with the hull and the rudder. This effect was explained before and it is related with the waves generated by the appendages. On the other hand, analysing the trim, we can observe that for low velocities the bow is sunk. Once the hull speed is reached the trim changes and the bow is raised. It is related as well with the ship sink but the differences are not accentuated as in the case of sink. After analysing the results for all velocities in the upright tests, we are going to compare what happens when the rudder is turned and if there is any effect on it. In the sink case, is below the hull speed and is above it. Both velocities have similar behaviour and the sink is higher in the cases with more leeway. However for positive angle this trend changes for leeway 2 and 4. It is interesting to observe that the sink is not symmetric in the case with leeway 0 and the sink is increasing once the amidships is exceeded. Furthermore, in cases with leeway 2 and 4 the results are practically equal, but in the case of leeway 0 it looks like the keel influences over the sink. Althought the results for HKR do not look so good, the effect is that with keel the sink is lower and for the other velocity is reversed. As we see previously this effect will be related with the trim which is studied below. 53

68 Figure 5.20: HKR and HR Sink data However, if we observe the sink results is observed that for high velocities the higher sink is produced in the case that the hull is alone and the lower in the case for with the hull and the rudder. This effect was explained before and it is related with the waves generated by the appendages. On the other hand, analysing the trim, we can observe that for low velocities the bow is sunk. Once the hull speed is reached the trim changes and the bow is raised. It is related as well with the ship sink but the differences are not accentuated as in the case of sink. After analysing the results for all velocities in the upright tests, we are going to compare what happens when the rudder is turned and if there is any effect on it. In the sink case, is below the hull speed and is above it. Both velocities have similar behaviour and the sink is higher in the cases with more leeway. However for positive angle this trend changes for leeway 2 and 4. It is interesting to observe that the sink is not symmetric in the case with leeway 0 and the sink is increasing once the amidships is exceeded. Furthermore, in cases with leeway 2 and 4 the results are practically equal, but in the case of leeway 0 it looks like the keel influences over the sink. Althought the results for HKR do not look so good, the effect is that with keel the sink is lower and for the other velocity is reversed. As we see previously this effect will be related with the trim which is studied below. 54

69 Figure 5.21: HKR and HR Trim data In the case of the higher velocity the trim is higher in the case with HR. This is consecuence of two factors, the ship is looking for the glide condition once the hull speed is exceeded. The bow tends to rise and the sink is accentuated, more in the case that the rudder is alone. In the case of the lower velocity the bow tends to be lower and is helped by the keel. Furthermore, these effects are lost when the ship sails with leeway because the results are practically the same Canoe Body Lift Analyses Once the appendages have been analysed, and their lift results are known, we are going to study how the canoe body change with the leeway effect. It was no possible to measure directly the lift on the canoe body without the appendages. However, it is possible to subtract the appendages values from the total measures as it was done with the drag. It was not possible to do with heel conditions because the dynamometer used for the keel has only five components and the z component is important when the heel is involved. In figure 5.22 lift forces on the canoe body are presented under different leeways for the two velocities studied. In these figures is possible to see how for the same leeway different lift values are obtained. These changes are produced mainly by the rudder as it is shown in figure In these figures two different leeways for the higher velocity have been chosen. In the left figure (leeway the rudder creates several flow changes that affect to the pressure field under the hull and modifies these lift values. In the right figure it is seen how the lift 55

70 Figure 5.22: Lift Canoe Body Results Figure 5.23: Decomposition of the lift forces is increased with the leeway. In this case, we have not only the canoe body lift but the appendages influence in this case is higher as well. 56

71 5.2 Heel Effects Once the tests in several conditions without heel have been studied, the effect of the heel is going to be evaluated in order to analyse the induced resistance in the appendages. The induced resistance presented is the additional resistance due to side force production only. To determine this additional resistance, the resistance of the combination under consideration at a given leeway and heel has been compared with the lift of the same combination under the same heeling angle without side force production. First the effects on the keel are evaluated as it is shown in the following figure. As the keel is fixed with the canoe body, the only parameters that can change are the velocity and the heel angle. In the case of the rudder, as it is not fixed we can analyse the effects with the rudder angle. Figure 5.24: Deterioration of the keel bulb set lift with heel In figure 5.24 is seen that with more leeway without heel the maximum lift is obtained. On the other hand when the heel is increased, it is detrimental for the lift. After checking the results with the keel, the rudder is going to be studied. In the following figures the rudder results for the two velocities and for the same conditions studied previously are presented (Fn and 0.420, leeway 0, 2 and 4, heel 0, 10 and 20). In these figures it is possible to observe how the resistance is lower when the heel is increase in all the cases and there is a lift lost. However, there are cases when increasing the heel and the leeway the relation C D C L is higher and improves the performance of our sailboat. 57

72 Figure 5.25: HKR Leeway 0 Heel curves 58

73 Figure 5.26: HKR Leeway 2 Heel curves In the previous figures it is interesting to note that the side force decreases with the heel. It is the same phenomena described with the keel. Moreover the behaviour is repeated in situations with the rudder alone and with the keel presence. On the other hand, when the rudder is turned with negative angles values, if we evaluate the absolute results, the side force is increased with the heel. it is the same phenomena described for the keel, but in this case the values are displaced toward y negative values. 59

74 Figure 5.27: HKR Leeway 4 Heel curves Another important data that can be obtained from these analyses is the position of the Centre of Lateral Resistance (CLR). The CLR is the center of pressure of the hydrodynamic forces on the hull of a boat. The center of pressure is the point on a body where the total sum of a pressure field acts, causing a force and no moment about that point. The total force vector acting at the center of pressure is the value of the integrated vectorial pressure field. The resultant force and center of pressure location produce equivalent force and moment on the body as the original pressure field. Pressure fields occur in both static and dynamic fluid 60

75 mechanics. Specification of the center of pressure, the reference point from which the center of pressure is referenced, and the associated force vector allows the moment generated about any point to be computed by a translation from the reference point to the desired new point. [41] The relationship of the aerodynamic center of pressure on the sails of a sailboat to the hydrodynamic center of lateral resistance on the hull determines the behaviour of the sailboat in the wind. This behaviour is known as the helm and is either a Weather helm or lee helm. A slight amount of weather helm is thought by some sailors to be a desirable situation, both from the standpoint of the feel of the helm, and the tendency of the boat to head slightly to windward in stronger gusts, to some extent self-feathering the sails and pointing into oncoming waves. Other sailors disagree and prefer a neutral helm. The fundamental cause of helm, be it weather or lee, is the relationship of the center of pressure of the sail plan to the center of lateral resistance of the hull. If the center of pressure is astern of the center of lateral resistance, a weather helm, the tendency of the vessel to want to turn into the wind. If the situation is reversed, with the center of pressure forward of the center of lateral resistance of the hull, a lee helm will result, which is generally considered undesirable, if not dangerous. Too much of either helm is not good, since it forces the helmsman to hold the rudder deflected to counter it, thus inducing extra drag beyond what a vessel with neutral or minimal helm would experience. The center of lateral resistance is used in comparison with the center of effort(ce), which is the geometric center of the sailplan. In comparing these two area centers, the fore/aft distance between the two is called the lead In order to have proper balance and just the right amount of weather helm, the CE should lead the CLR by a certain amount, which is dependent on the shapes of the hull, the appendages, and the sailplan. The vertical distance between the CE and CLP is the heeling arm, and is indicative of how much the boat will heel when underway (longer arm = more heel at any given wind speed). Naval architects and yacht designers use the CE and CLR for general design purposes because they are convenient and easy to calculate. In reality, the aerodynamic forces do not really go through the CE, and the hydrodynamic forces do not really go through the CLR, at least not constantly, although they may do momentarily. It is actually quite impossible to calculate the precise centres of the actions of the aero/hydrodynamic forces with any degree of accuracy because they are constantly changing as the boat moves through the waves. Therefore, using the geometric centres is a useful tool that gets the job accomplished and can be used for comparison between differing boat designs. The results for the CLR obtained in the towing tank tests are presented in figure In these figures it is possible to note that the CLR comes forward with the heel. All these measures are taken from the transom. In the case CLR Leeway 2 with lee helm, the last value for heel 20 is higher than expected. If we compare with other situations this value is too high. Some of these situations could be unreal because of the model is fixed in the towing tank experiment and in the real sitaution the model is free. 61

76 Figure 5.28: CLR positions Finally the general behaviour is the expected. In weather helm, when the rudder angle is increased the CLR comes aft and on the other hand, in lee helm the CLR comes forward when the rudder angle is increased. 62

77 Chapter 6 Computational Fluid Dynamic 6.1 Introduction In marine industry, CFD are chiefly concerned with problems in hydrodynamics. In the majority of problems solved, global pressures and fluid velocity components are calculated. In this way, it is possible to further calculate the forces and moments acting on the vessel, whether steady or unsteady. It is customary to treat the working fluid, in this case water, as incompressible and isothermal. However, it is also possible to make further assumptions regarding the behaviour of the flow, depending upon the nature of the problem in hand and the leading order effects of interest. In general, Commercial CFD software tools have been written to solve the more general cases of compressible, viscous, turbulent flows with heat transfer, but may be applied to problems in hydrodynamics, so long as the correct choices are made regarding equations of state, fluid properties, and boundary conditions. The definitions given below should provide those attempting problems in hydrodynamics with a guide to how the equations of most interest are derived Furthermore, CFD techniques based on RANS (Reynolds Average Navier Stokes Equations) flow simulation are used to visualize and determinate some of the effects that are difficult to observe in the experimental tests. A number of valuable advantages are achieved following a CFD approach to a fluid dynamic problem: CFD is faster and cheaper. A considerable reduction of time and costs for solving the problems is offered compared to the traditional approaches. A conscious assessment of different solutions is available in the early phase of the design process, in order to fit with the requested tasks. Thus, experimental tests would be done just on few models, re- sulted from the CFD analysis. Full-size analysis is hard to perform and expensive for large systems or non-scaled analysis, in these cases CFD study is a favourable choice. A key-important quality of CFD are the detailed solutions allowed by the recent techniques (and computer technologies), even for time-dependent flows and complex systems. 63

78 The numerical models of the physical problems have good accuracy and reliability, due again to the newest mathematical improvements of solution schemes and of turbulence models. Due to the last two advances, in most of the cases the prediction of a fluid dynamic problem does not require a dedicated powerful workstation and sometimes a personal computer might be sufficient. CFD solvers are only a tool. It is the user who has to precise and understand the physical phenomena. All the relevant variables involved in the simulation must be taken into account from the beginning, including geometry, mesh, boundary conditions, to be defined in the simplest way, but without introducing extreme errors with the hypothesis. Nevertheless, a number of simplifications is always accepted, and is inevitable in order to model properly fluid dynamics problems The Structure of a CFD code A comprehensive overviews of the techniques used to solve problems in fluid mechanics on computers are described, among others, by Anderson [42], Versteeg [43] or by Ferziger and Peric in [44].Commercial codes give us a friendly interface where the user has the possibility of easy setting the analysis and obtain the results. Every CFD code could be divided in three parts, which correspond to the phases of the problem analysis. First of all there is the pre-processor, which is used to build the problem. It is in this program where the mesh is imported.it is the phase where the physical problem is implemented into the mathematical model. The computational domain is now defined and divided into a certain number of elements, which constitute the mesh or grid. Nowadays all commercial software have associate a mesh tool. In this work, as it will be shown later, ICEM was used with CFX, Star-CCM+ has it own mesh generator within the program and finally for Fluent, Fluent Meshing has been used in order to demonstrate its features. After this, the domain and the type of analysis (multiphase, VOF, turbulence,... ) are defined and the boundary conditions are set. Since the CFD solution is given locally, the global accuracy depends on the total number and quality of the mesh elements. A good strategy in order to optimize the simulation is meshing finer where higher are the variables gradients and coarser in the region characterized by smooth changes in the flow. For this, structured meshes like the used here are very useful because of it is easier to have more control in the mesh with them. The final success of a CFD simulation strongly depends on the preprocessing and therefore a special attention might be paid to the choice of the mesh and of boundary conditions. Furthermore, It is the program that checks if there are enough conditions but does not check for some over-specified cases (different speeds at inflow and outflow). These kind of programs made initialization for better convergence, in some cases a previous potential analysis is done to have a first solution approach. All of them allow the possibility to define extra variables and expressions. 64

79 The second module is the solver. The numerical solution algorithm is the core of a CFD code. All the main solvers work with the following procedure. The problem unknowns are modelled by means of simple analytical functions and after discretizing the governing equations, CFD programs solve the algebraic system of equations. This kind of programs could run without any window and builds the backup and result files from the definition file. Sometime the user prefers to see how the program goes on and the analysis could be controlled by means of the residuals or a specified variable. This is very helpful to see the good achievement of the problem, to have a rapid and easy eye on its convergence or not. It can be launched or not without affecting the solver. It allows to stop a solver running and thus get a result file sooner, and then it can be relaunched the problem from the current point or from any initial or backup point. This allows to stop a problem in case of sudden divergence, before it crashes and look at what happens. Finally there is a third module called the postprocessor. Under this definition the analysis of solution results is included. The solver output is a set of solution variables, associated to the given grid nodes or volumes. These data must be collected, elaborated in the most suitable way for the analysis, in order to produce a physical representation of the solution. Some CFD software package contains a post-processing section, like Fluent or Star-CCM+. Other solvers need an external tool for data treatment, which can be a commercial one (several complete packages exist for the scope) or a dedicated in-house code. Anyhow, one might be able to do the following post-processing operations needed to analyse locally the simulation: - Domain and grid visualization - Vectorial plots of solution variables - Linear, surface, volume integrals - Iso-level and contour plots of solution variables, within selected domain zones - Drawing two-dimensional and three-dimensional plots - Tracking path-lines, stream traces, etc. - Algebraic and analytical operations within the variables - Dynamic representations, animations etc. In general, we should refer to the solved flow field as it had been an experimental test situation. Among the given data set, we could operate as we were using real instruments, by selecting the position of virtual probes or control surfaces where our interest is focused. [45] 6.2 Overview of Equations and Numeric Methods used in Marine CFD To analyse the features described in the Theory Chapter, the general equations of fluid flow are used. They represent mathematical statements of the conservation laws of physics, such that: 65

80 Fluid mass is conserved The rate of change of momentum equals the sum of the forces on a fluid particle The rate of change of energy is equal to the sum of the rate of heat addition to and the rate of work done on a particle. For the process performed with constant temperature, will not make sense to apply the law of conservation of energy. Furthermore, the reference system used is always taking the Cartesian sense of z positive contrary to gravity. The conservation of mass law is a property of kinematic nature and it is independent from the characteristics of the fluid. This equation can be written as follows: ρ t + (ρv) = S m (6.1) Equation 6.1 is the general form of the mass conservation equation and is valid for incompressible as well as compressible flows. The source is the mass added to the continuous phase from the dispersed second phase (for example, due to vaporization of liquid droplets) and any user-defined sources. For incompressible flow such as we require for hydrodynamics, and assuming that the fluid is Newtonian and that the viscosity is constant throughout the flow, the continuity equation becomes: v = 0 (6.2) The conservation of momentum and the equation movement is used as a result of applying the second law Newton on a fluid particle. The fluid is assumed as continuous, isotropic and linearly viscous. For a fluid Newtonian equation of motion becomes the equation Navier Stokes presented below: (ρ v) + (ρ v v) = p + ( τ) + ρ g + F t (6.3) where p is the static pressure, τ is the stress tensor (described below) and ρ g and F are the gravitational body force and external body forces The stress tensor τ is given by: ) τ = µ [( v + v T 23 ] vi (6.4) where µ is the molecular viscosity, I is the unit tensor, and the second term on the right hand side is the effect of volume dilation. Whilst the above equations are sufficient for the description of incompressible, laminar flow, and being a description of a continuum, in principle apply to all scales, they are also non-linear and subject to instability. Furthermore, under the point of view of computational 66

81 fluid dynamics, most of the flows that occur in nature and technology, exhibit an instability form, called turbulence. This change of regime occurs when the flow velocity or more precisely the Reynolds number (3.2), seen in section 3.1 reaches a certain critical value. On the other hand this renders the equations impossible to solve analytically, and requires that numerical methods be formulated to solve for particular (statistically stationary) states within the flow. It is assumed that the components of the flow velocity, and the pressure, consist of a mean value with superimposed fluctuations. These fluctuations are bounded to remain within a spectrum of values in terms of frequency and amplitude. This spectrum of the turbulent kinetic energy can be analysed and operated on using statistical tools, from which a variety of formulations for the mass and momentum conservation can then be derived. There are several approaches to simplify the problem and to reduce the computational cost, which differ in the approximations or assumptions that are assumed in the treatment of the equations used in the study. All these methods introduce new variables to the equations governing the behavior of fluids that need to be modeled to achieve a correct solution. The different ways to treat these new variables and solving equations are called turbulence models. In the RANS (Reynolds averaged Navier-Stokes) approach to turbulence, all of the unsteadiness in the flow is averaged out and regarded as part of the turbulence. The flow variables, in this example one component of the velocity, are represented as the sum of two terms u i = ū i + u i (6.5) where ū i and u i are the mean and fluctuating velocity components Likewise, for pressure and other scalar quantities: Φ i = Φ i + Φ i (6.6) where Φ denotes a scalar such as pressure, energy, or species concentration. Substituting expressions of this form for the flow variables into the instantaneous continuity and momentum equations and taking a time (or ensemble) average (and dropping the overbar on the mean velocity,ū ) yields the ensemble-averaged momentum equations. They can be written in Cartesian tensor form as: ρ t + (ρu i ) = 0 (6.7) x i t (ρu i) + (ρu i u j ) = p + [ ( ui µ + u j 2 )] x j x i x j x j x i 3 δ u i ij x i + x j (ρu iu j) (6.8) Equation 6.7 and equation 6.8 are called Reynolds-averaged Navier-Stokes (RANS) equations. They have the same general form as the instantaneous Navier-Stokes equations, with 67

82 the velocities and other solution variables now representing ensemble-averaged (or timeaveraged) values. Additional terms now appear that represent the effects of turbulence. These Reynolds stresses, ρu iu j must be modeled in order to close equation 6.8. The Reynolds-averaged approach to turbulence modeling requires that the Reynolds stresses in equation 6.8 are appropriately modeled. A common method employs the Boussinesq hypothesis [46] to relate the Reynolds stresses to the mean velocity gradients: ( ρu iu ui j = µ t + u ) j 2 ( ) u k ρk + µ t δ ij (6.9) x j x i 3 x k The Boussinesq hypothesis is used in one and two equations models. The advantage of this approach is the relatively low computational cost associated with the computation of the turbulent viscosity, µ t. In the case of one equation model, the equation representing the turbulence viscosity is solved. In the case of the two equation model, the transport equation for the turbulence kinetic energy k and either the turbulence dissipation rate, ɛ, or the specific dissipation rate, ω are solved. In this cases µ t is computed in function of k and ɛ or k and ω. The disadvantage of the Boussinesq hypothesis as presented is that it assumes µ t is an isotropic scalar quantity, which is not strictly true. However the assumption of an isotropic turbulent viscosity typically works well for shear flows dominated by only one of the turbulent shear stresses. This covers many technical flows, such as wall boundary layers, mixing layers, jets, and so on. The alternative approach, embodied in the RSM, is to solve transport equations for each of the terms in the Reynolds stress tensor. An additional scale-determining equation (normally for ɛ or ω ) is also required. This means that five additional transport equations are required in 2D flows and seven additional transport equations must be solved in 3D. In many cases, models based on the Boussinesq hypothesis perform very well as it happens in resistance analyses, and the additional computational expense of the Reynolds stress model is not justified. However, the RSM is clearly superior in situations where the anisotropy of turbulence has a dominant effect on the mean flow. Such cases include highly swirling flows and stress-driven secondary flows. The discretised set of RANS equations can be solved with various solution procedures such as either pressure-based and or density-based methods (for a review, see Ferziger and Peric [44], Fletcher [47] or Hirsch [48]). The solution algorithms make use of numerous tuning parameters, such as artificial time-steps, under-relaxation, etc., to improve convergence behaviour and robustness of the code. The field of application of a code and the modelling technique included influence the choice of the numerical method and the solution procedure. In spite of there are several models included in any commercial softwares, two-equation models have been used in this research: Realizable k ɛ and k ω SST [49] Turbulence models Realizable k ɛ The most popular version of two equation models is the k ɛ model, where ɛ is the rate at which turbulent energy is dissipated by the action of viscosity on the smallest eddies 68

83 (Launder and Spalding [50]). A modelled transport equation for ɛ is solved and then L is determined as C µ k 3/2 /ɛ where C µ is a constant. The k ɛ model has been enhanced in several ways, for instance using Renormalization Group Theory (Yakhot et al.,[51]). The major differences in the k ɛ models can be summarized with the method of calculating turbulent viscosity, turbulent Prandtl numbers governing the turbulent diffusion of and the generation and destruction terms in the equation. By remodeling some of the terms in the equations, the Realizable k ɛ model was developed by NASA (Shih, Zhu and Lumley, [52]). This model differs from the standard model in two interportant ways: - The realizable k ɛ model contains an alternative formulation for the turbulent viscosity. - A modified transport equation for the dissipation rate, ɛ, has been derived from an exact equation for the transport of the mean-square vorticity fluctuation. The term realizable means that the model satisfies certain mathematical constraints on the Reynolds stresses, consistent with the physics of turbulent flows. Neither the standard k ɛ model nor the RNG k ɛ model are realizable. One of the advantages is that k ɛ model has been proven to be stable and numerically robust and has a well-established regime of predictive capability. For general purpose simulations, the model offers a good compromise in terms of accuracy and robustness. SST k ω Rather than solving for the dissipation rate ɛ directly, an equation for the specific dissipation rate ω = ɛ/k is solved. The physical significance of ω has been a matter for discussion for a long time and a good review is given by Wilcox [53]. It is not the scope of this work to repeat this discussion here. it is enough to note that the k ω model has shown superior performance when predicting ship flows, as compared to the k ɛ model. Replacing the dynamic viscosities µ and µ τ by their kinematic equivalents. ν = µ ρ ν τ = µ τ ρ the equations in the k ω model are as follows: ν τ = k ω k t + u k j = τ ij u i β kω + [ (ν + σ ν τ ) k ] x j ρ x j x j x j ω t + u ω j = α ω τ ij u i βω 2 + [ (ν + σν τ ) ω ] x j k ρ x j x j x j The empirical constants are as follows (6.10) (6.11) (6.12) (6.13) α = 5/9 β = 3/40 β = 9/100 σ = 1/2 σ = 1/2 69

84 One difficulty with the ω equation is that it is hard to define a robust boundary condition at the outer edge. On the hull surface, ω goes to infinity, but this problem can be handle in different ways. Because ɛ has a well-defined value at the boundary layer edge, Menter [54] proposed a blending of the two transport equations such that the resulting equation represents only ω at the surface and only ɛ outside of the boundary layer, taking the strengh features of both models. This modification of the original method is referred to as the Baseline (BSL) k ω model. Menter also suggested a further modification of the BSL model, by which an improved prediction of the principal shear stress is obtained in adverse pressure gradients. This is known as the Shear Stress Transport (SST) model. Turbulence Damping In free surface flows, a high velocity gradient at the interface between two fluids results in high turbulence generation, in both phases. in the present work, this increment has been detected and following the general recommendations, turbulence damping has been enabled in the interfacial area to model such flows correctly. It is important to remark that turbulence damping is available only with k ω models. The following term is added as a source (Egorov [55]) to the ω equation [ ] 2 B6µi S i = A i nβ 1 ρ i (6.14) β1ρ i n 2 where A i is the interfacial area density for phase i, which is calculated as A i = 2α i α i (6.15) The grid n size is calculated internally using grid information. β 1 is the k ω model closure coefficient of destruction term, which is equal to 0.075, B is the Damping factor, which is spezified by the user. For analyses like this, the default value of 10 is enough. Finally, µ is the viscosity of phase i and ρ is the density of phase i Near Wall Treatments Turbulent flows are significantly affected by the presence of walls. Obviously, the mean velocity field is affected through the no-slip condition that has to be satisfied at the wall. However, the turbulence is also changed by the presence of the wall in non-trivial ways. Very close to the wall, viscous damping reduces the tangential velocity fluctuations, while kinematic blocking reduces the normal fluctuations. Toward the outer part of the near-wall region, however, the turbulence is rapidly augmented by the production of turbulence kinetic energy due to the large gradients in mean velocity. The near-wall modelling significantly impacts the fidelity of numerical solutions, inasmuch as walls are the main source of mean vorticity and turbulence. After all, it is in the nearwall region that the solution variables have large gradients, and the momentum and other scalar transports occur most vigorously. Therefore, accurate representation of the flow in the near-wall region determines successful predictions of wall-bounded turbulent flows. 70

85 Figure 6.1: Subdivisions of the Near-Wall Regions [3] Numerous experiments have shown that the near-wall region can be largely subdivided into three layers. In the innermost layer, called the viscous sublayer, the flow is almost laminar, and the (molecular) viscosity plays a dominant role in momentum and heat or mass transfer. In the outer layer, called the fully-turbulent layer, turbulence plays a major role. Finally, there is an interim region between the viscous sublayer and the fully turbulent layer where the effects of molecular viscosity and turbulence are equally important. Figure 6.2: Near-Wall Treatments [3] Traditionally, there are two approaches to modeling the near-wall region. In one approach, the viscosity-affected inner region (viscous sublayer and buffer layer) is not resolved. Instead, semi-empirical formulas called wall function are used to bridge the viscosity-affected region between the wall and the fully-turbulent region. The use of wall functions obviates the need to modify the turbulence models to account for the presence of the wall. In another approach, the turbulence models are modified to enable the viscosity-affected region to be resolved with a mesh all the way to the wall, including the viscous sublayer. For the purposes of discussion, this will be termed the near-wall modeling approach. 71

86 Looking at the Wall Function approach, the viscosity-affected region is not resolved, instead is bridged by the wall functions. In this way, High-Re turbulence models can be used. On the other hand, in the Near Wall Model Approach the near-wall region is resolved all the way down to the wall and the turbulence models ought to be valid throughout the near-wall region. Wall Function This is the procedure most commonly used in industrial practice. The difficult near-wall region is not explicitly resolved with the numerical model but is bridged using so called wall functions (Rodi [56] and Wilcox [53]). In order to construct these functions the region close to the wall is characterised in terms of variables rendered dimensionless with respect to conditions at the wall. The wall friction velocity u τ is defined as (τ w /ρ) 1/2 where τ w is the wall shear stress. Let y be normal distance from the wall and let U be time-averaged velocity parallel to the wall. Then the dimensionless velocity, U + and dimensionless wall distance, y + are defined as u/u τ and y ρ u τ /µ respectively. If the flow close to the wall is determined by conditions at the wall then u + can be expected to be a universal function of y + up to some limiting value of u +. This is indeed observed in practice, with a linear relationship between u + and y + in the viscous sublayer, and a logarithmic relationship, known as the law of the wall, in the layers adjacent to this (so-called log-layer). The y + limit of validity depends on external factors such as pressure gradient and the penetration of far field influences. In some circumstances the range of validity may also be effected by local influences such as buoyancy forces if there is strong heat transfer at the wall. The turbulence velocity k 1/2 and length scales, when treated in the same way also exhibit a universal behaviour. These universal functions can be used to relate flow variables at the first computational mesh point, displaced some distance y from the wall, directly to the wall shear stress without resolving the structure in between. The only constraint on the value of y is that y + at the mesh point remains within the limit of validity of the wall functions. A similar universal, nondimensional function can be constructed which relates the temperature difference between the wall and the mesh point to heat flux at the wall (Rodi [56]). This can be used to bridge the near-wall region when solving the energy equation. The meshing should be arranged so that the values of y + at all the wall adjacent mesh points is greater than 30 (the form usually assumed for the wall functions is not valid much below this value). It is advisable that the y + values do not exceed 300 and should certainly never be less than 11. Some commercial CFD codes account for this by switching to alternative functions if y + is < 30. In addition, the values of y + at the wall adjacent cells strongly influence the prediction of friction and hence drag. Thus particular care should be given to the placement of near-wall meshing if these are important elements of the solution. However, wall functions become less reliable when the flow conditions depart too much from the ideal conditions underlying the wall functions. Examples of this are severe pressure gradients leading to boundary layer separations like occurs when the rudder is turned and strong body forces. 72

87 Figure 6.3: Wall Function separation [3] Figure 6.3 shows an example where the wall function is not a good approach. In situations where there is a boundary layer separation, logarithmic-based wall functions do not correctly predict the boundary layer profile and the viscous sublayer has to be resolved Near Wall Resolution Under such circumstances the wall-function concept breaks down and its use will lead to significant error (figure 6.3). The alternative is to fully resolve the flow structure through to the wall. Some turbulence models can be validly used for this purpose, others cannot. For example, the k ω two-equation model can be deployed through to the wall as can the one-equation k L model (e.g. Wolfshtein [57]).The standard k ɛ and RSM models cannot. Various so-called low-reynolds number versions of the k ɛ and RSM models have been proposed incorporating modifications which remove this limitation (Patel et al. [58] and Wilcox [53]). Alternatively the standard k ɛ and RSM models can be used in the interior of the flow and coupled to the k L model which is used to resolve just the wall region. This is known as a two-layer model. Whatever modelling approach is adopted, a large number of mesh points must be packed into a very narrow region adjacent to the wall in order to capture the variation in the flow variables. With y defining the distance from the wall to the first discretization point, a nondimensional distance from the surface y + may be obtained. y + = yu τ ν where u τ is a scaling parameter, known as the friction velocity and defined as (6.16) u τ = τω ρ (6.17) When the boundary layer is solved, y + should be not larger than 1 for the no-slip conditions to be applied, so the point has to be well within the viscous sublayer (see figure 6.1) Free Surface Model The primary difficulty with free surface calculations is that the position and shape of the free surface is not known, and often involves non-linear effects such as wave breaking and 73

88 fragmentation. There are essentially two approaches to free surface modelling for viscous flows using RANSE solvers: interface tracking and interface capturing. Interface tracking involves generation of a grid covering just the liquid domain. One of the domain boundaries is then, by default, the free surface where the boundary conditions are applied. The grid is adapted to the position of the free surface at each time step. Grid adaptation may be made computationally more efficient by methods such as moving points along predefined lines or by updating the free surface position only after several time steps, having solved the free surface using the pressure boundary condition at intermediate steps. The method can currently only be used in the absence of steep or breaking waves to avoid contortion of the grid. Use of unstructured meshes may improve these limitations [59]. The alternative approach, interface capturing, involves solving the RANS equations on a predetermined grid which covers the whole domain. Three main methods cover this category: - Marker-and-cell - Volume of Fluid - Level Set Technique Marker-and-cell could be the most accurate method to build the free surface. In it, massless tracer particles are introduced into the fluid near the free surface and tracked throughout the calculation. This scheme can cope with non-linearities such as breaking waves and has produced some good results. However, it is computationally expensive and this is one of the reasons that Volume of Fluid and Level Set Methods are commonly used in commercial software. Volume of Fluid The method is based on the idea of a scalar fraction function α defined locally on each cell of the mesh whose value depends on the fraction of the volume occupied by each fluid. In the simplest formulation when 2 fluids A and B are separated by a free surface, when the cell filled with the fluid A, the value of α is zero; when the cell is full of fluid B, α = 1; and when both fluids share a cell and consequently the interface cuts the cell, then 0 < α < 1. As result, cells with α values between zero and one must contain free surface. The most general equation to model the volume fraction of one (or more) phases. For the α q phase, this mass conservation equation has the following form: 1 ρ q [ t (α qρ q ) + (α q ρ q v q ) = S αq + ] n (ṁ pq ṁ qp ) p=1 (6.18) where S αq is the mass Source term for the phase q and ṁ pq is the mass transfer from phase p to the phase q. In the case studied in this work, there are two phases water and air and due to the low velocity of the tests, both phases can be considered as incompressible. The tracking of the 74

89 interfaces between the phases is accomplished by the solution of a continuity equation for the volume fraction of phases. For the q-th phase, this equation has the following form. α q t + ν α q = 0 (6.19) The volume fraction equation is not solved for the primary phase, but based on the following constraint n α q = 1 (6.20) q=1 A single momentum equation is solved throughout the domain, and the resulting velocity field is shared among the phases. The momentum equation depends of on the volume fractions of all phases through the fluid properties, which are determined by the presence of the component phases in each cell. In the case of turbulence quantities, a single set of transport equation is solved, and the turbulence variables are shared by the phases throughout the field. Level Set Method The level-set method is a popular interface-tracking method for computing two-phase flows with topologically complex interfaces. This is similar to the interface tracking method of the VOF model. In the level-set method [60],the interface is captured and tracked by the level-set function, defined as a signed distance from the interface. Because the level-set function is smooth and continuous, its spatial gradients can be accurately calculated. This in turn will produce accurate estimates of interface curvature and surface tension force caused by the curvature. However, the level-set method is found to have a deficiency in preserving volume conservation [61]. On the other hand, the VOF method is naturally volume-conserved, as it computes and tracks the volume fraction of a particular phase in each cell rather than the interface itself. The weakness of the VOF method lies in the calculation of its spatial derivatives, since the VOF function (the volume fraction of a particular phase) is discontinuous across the interface. The level-set function ϕ is defined as a signed distance to the interface. Accordingly, the interface is the zero level-set, ϕ(x, t) and can be expressed as Γ{x ϕ(x, t) = 0} in a two phase flow system as ϕ(x, t) = + d if x the primary phase, ϕ(x, t) = +0 if x Γ or ϕ(x, t) = d if x the secondary phase where d is the distance from the interface. The evolution of the level-set function can be given in a similar fashion as to the VOF model: ϕ + ( uϕ) = 0 (6.21) t where u is the underlying velocity field. On the other hand the momentum equation can be writen as: ) (ρ u) + (ρ u u) = p + µ ( u + u T + ρ g + F t (6.22) In this case F is the force arising from surface tension effects. 75

90 Coupled Level Set - VOF As it was explained, VOF methods are widely used. It is itself a proof of its efficacy, but it is a model that presents numerical diffusion, which will depend on the model chosen to reconstruct the interface after convection. On the other hand, Level set Methods are easy to implement into any finite volume code and it does not smear the interface, (it usually has not got numerical diffusion) but it has serious problems when the interface becomes a multivalued function. Furthermore it is not usual seen this method in naval problems. To overcome the deficiencies of the level-set method and the VOF method, a coupled level-set and VOF approach is provided in Fluent and used in some of the analysis done in this research. Reconstruction Models Since the volume fraction at the current time step is a function of other quantities at the current time step, a scalar transport equation is solved iteratively for each of the secondaryphase volume fractions at each time step. In addition, the volume fraction equation may be solved either through implicit or explicit time discretization. When the implicit formulation is used, the volume fraction equation is discretized in the following manner: α n+1 q ρq n+1 αq n ρq n V + t f [ ( ) ρq Uf n αq,f n n = (ṁ pq ṁ qp ) + S αq ]V (6.23) where n and n + 1 are the index for the previous time step and the index for the current time step respectively, α the face value for the fraction volume, V the volume of cell and U f the volume flux through the face, based on normal velocity. The implicit formulation is iterative and can be used with either the Steady or Transient solver. It is well-suited to steady-state applications as the solution information propagates much faster compared to the explicit formulation. For steady-state flow applications, either a steady-state or a transient simulation may be required, depending on the characteristics of the flow: - Steady-state simulation: If the final steady-state solution is not affected by the initial flow conditions and there is a distinct inflow boundary for each phase. - Transient simulation: If the final steady-state solution is dependant on the initial flow conditions and/or you do not have a distinct inflow boundary for each phase. For transient flow applications, the implicit formulation may allow you to use a much larger time step than the explicit formulation due to the implicit formulations unconditional stability. However, the implicit time-step size may be limited by truncation errors. The implicit formulation produces more numerical diffusion than the explicit formulation when using the First Order transient formulation. Therefore, the implicit formulation should be used along with higher-order transient formulations to achieve better numerical accuracy. 76 p=1

91 Since the volume fraction at the current time step is directly calculated based on known quantities at the previous time step, the explicit formulation does not require and iterative solution of the transport equation during each time step. In addition, the explicit formulation is non-iterative and is time-dependent. Thus it can only be used with the Transient solver. It exhibits better numerical accuracy compared to the implicit formulation. However the time step size is limited by a Courant-based stability criterion. α n+1 q ρq n+1 αq n ρq n V + t f [ ( ) ρq Uf n αq,f n n = (ṁ pq ṁ qp ) + S αq ]V (6.24) p=1 The face fluxes can be interpolated using interface tracking or capturing schemes such as Geo-Reconstruct, CICSAM, Compressive, and Modified HRIC The Geo-Reconstruct scheme is an interface tracking scheme based on geometrical information. It is the most accurate scheme, but is more computationally expensive than the other schemes. Geo-Reconstruct is the preferred scheme when solving on meshes of poor quality. Furthermore it is only available with explicit formulation and in transient simulations. The geometric reconstruction scheme represents the interface between fluids using a piecewise-linear approach. In Fluent this scheme is the most accurate and is applicable for general unstructured meshes. The first step in this scheme is calculating the position of the linear interface relative to the centre of each partially-filled cell, based on information about the volume fraction and its derivatives in the cell. The second step is calculating the advecting amount of fluid through each face using the computed linear interface representation and information about the normal and tangential velocity distribution on the face. The third step is calculating the volume fraction in each cell using the balance of fluxes calculated during the previous step. The Compressive scheme is a second order reconstruction scheme based on the slope limiter. The theory below is applicable to zonal discretization and the phase localized discretization, which use the framework of the compressive scheme. φ f = φ d + β φ d (6.25) where φ f is the face VOF value and φ d is the donnor cell VOF value. When the cell is near the interface between two phases, a donor-acceptor scheme is used to determine the amount of fluid advected through the face (Hirt [62]). β is the slope limiter value that for a compressive scheme has a value of 2. Moreover, the compressive scheme discretization depends on the selection of interface regime type. When sharp interface regime modeling is selected, the compressive scheme is only suited to modeling sharp interfaces. However, when sharp/dispersed interface modeling is chosen, the compressive scheme is suited for both sharp and dispersed interface modeling. For the VOF model, it is possible to specify the interface regime that it will be modeling. This will determine the availability of the various volume fraction discretization schemes (Spatial Discretization Schemes for Volume Fraction). The following options are available for Interface Modeling Type in Fluent: - Sharp: Recommended when a distinct interface is present between the phases 77

92 - Dispersed: Recommended when the phases are interpenetrating - Sharp/Dispersed: A hybrid approach for flows consisting of both sharp and dispersed interfaces. Recommended to capture mildly sharp interfaces For analysis like the scope of this work, Sharp model has been used. Moreover, an Interfacial Anti-Diffusion treatment. This treatment is applied only in interfacial cells and attempts to suppress the numerical diffusion that can arise from the volume fraction advection schemes. Among other functions, this algorithm can help to eliminate problems like numeric ventilation, a phenomena that can appear under the hull. When the sharp interface model is used, it is also possible to enable the Interfacial Anti-Diffusion treatment. This treatment is applied only in interfacial cells and attempts to suppress the numerical diffusion that can arise from the volume fraction advection schemes. The use of this treatment can have adverse effects on convergence, especially with aggressive settings and large time step size. Therefore, it should be used in cases that use a coarse mesh, that have high aspect-ratio cells, that have large cell-volume jumps in the vicinity of the fluid-fluid interface, or that suffer from excess numerical diffusion. Finally, for simulations using the VOF multiphase model, upwind schemes are generally unsuitable for interface tracking because of their overly diffusive nature. Central differencing schemes, while generally able to retain the sharpness of the interface, are unbounded and often give unphysical results. In order to overcome these deficiencies, ANSYS Fluent uses a modified version of the High Resolution Interface Capturing (HRIC) scheme. The modified HRIC scheme is a composite NVD scheme that consists of a nonlinear blend of upwind and downwind differencing (Muzaferija [63]) First, the normalized cell value of volume fraction, φc, is computed and is used to find the normalized face value, φf, as follows: φ c = φ D φ U φ A φ U (6.26) Figure 6.4: Cell Representation for Modified HRIC Scheme [3] where A is the acceptor cell, D is the donor cell, and U is the upwind cell, and, φ c φc < 0 or φ c > 1 φ f = 2 φ c 0 φ c φ c 1 (6.27) 78

93 The modified HRIC scheme provides improved accuracy for VOF calculations when compared to QUICK and second-order schemes, and is less computationally expensive than the Geo-Reconstruct scheme. 6.3 General Errors and uncertainties in CFD Simulations The deficiencies or inaccuracies of CFD simulations can be related to a wide variety of errors and uncertainties. A recent publication of the AIAA guide for the verification and validation of computational fluid dynamics simulations [64] provides useful definitions of error, as a recognisable deficiency that is not due to lack of knowledge, and uncertainty as a potential deficiency that is due to lack of knowledge in CFD. Typical known errors are the round-off errors in a digital computer and the convergence error in an iterative numerical scheme. In these cases, the CFD analyst has a reasonable chance of estimating the likely magnitude of the error. Unacknowledged errors include mistakes and blunders, either in the input data or in the implementation of the code itself, and there are no methods to estimate their magnitude. Uncertainties arise because of incomplete knowledge of a physical characteristic, such as the turbulence structure at the inlet to a flow domain or because there is uncertainty in the validity of a particular flow model being used. According to this, different sources has been detected and has been taken account in the numerical analyses: Convergence errors As it has been shown iterative algorithms are used for steady state and transient solutions methods and for procedures to obtain an accurate solution. Progressively better estimates of the solution are generated as the iteration count proceeds. There are no universally accepted criteria for judging the final convergence of a simulation, and CFD users have found no formal proof that a converged solution for the Navier-Stokes equations exists. In some situations the iterative procedure does not converge, but either diverges or remains at a fixed and unacceptable level of error, or oscillates between alternative solutions. In these simulations the most commonly levels of convergence have been used: - Changes in solution variables from one iteration to the next are neglegible. In this case residuals values have been used. The main criteria was that all the values were below 1e 3 - Overall property conservation is achieved. There is an imbalance mass flow rate global conservation. - A quantity of interest, in this case canoe-body and appendages drag and lift, has been monitored and they have reached steady values. Model error and uncertainty These are defined as errors due to the difference between the real flow and the exact solution of the model equations. This includes errors due to the fact that the exact governing 79

94 flow equations are not solved but are replaced with a physical model of the flow that may not be a good model of reality. For viscous simulations, the most well publicised error in this category is the error from turbulence model and for potential flow calculation viscous effects are neglected altogether. In addition, in this case steady simulations have been done but it is possible that transient phenomena occurs, mainly when the ship is sailing with heel and leeway. In this cases, different turbulence models have been tested to see their influence. Application uncertainties Inaccuracy that arises because the application is complex and precise data needed for the simulation is not available. Examples of this are uncertainties in the precise geometry, uncertain data that needs to be specified as boundary conditions and uncertainties as to whether the flow is likely to be steady or unsteady. steady and transient simulations have been done to eliminate this error. Figure 6.5: Bulb end simplification In this case the way that the appendices end, so sharp, could be a problem. However the difference between the complete appendage and the appendage cutted could be assumed (figure 6.5). Discretisation or numerical error These are defined as errors that arise due to the difference between the exact solution of the modelled equations and a numerical solution on a grid with a finite number of grid points. In general, the greater the number of grid cells, the closer the results will be to the exact solution of the modelled equations, but both the fineness and the distribution of the grid 80

95 points affect the result. This type of error arises in all numerical methods and is related to the approximation of a continually varying parameter in space by some polynomial function for the variation across a grid cell. In first order schemes, for example, the parameter is taken as constant across the cell. In short, discretisation errors arise because we do not find an exact solution to the equations we are trying to solve but a numerical approximation to this. It is usual to do a independence grid analyses, however in cases like this where the experimental analysis exists it is easier to avoid this issue. On the other hand, simulations started with first order discretization and after ensuring convergence was changed to second order. When the model has been honed second order has been used directly. Iteration or convergence error These are defined as errors which arise due to the difference between a fully converged solution on a finite number of grid points and a solution that is not fully converged. The equations solved by CFD methods are generally iterative, and starting from an initial approximation to the flow solution, iterate to a final result. This should ideally satisfy the imposed boundary conditions and the equations in each grid cell and globally over the whole domain, but if the iterative process is incomplete then errors arise. In short, convergence errors arise because the user is impatient or short of time or the numerical methods are inadequate and do not allow the solution algorithm to complete its progress to the final converged solution. User and Code Errors These are defined as errors that arise due to mistakes and carelessness of the user. In cases like this it is avoidable due to the existence of experimental tests and the high number of simulations that have been performed. On the other hand, code errors are due to bugs in the software. It is very difficult to have this kind of errors with commercial software. however for this work, beta release has been used and this kind of error could be possible to appear. In figure 6.6 it is possible to observe the difference between two releases. Figure 6.6: Code errors 81

96 Round-off errors These are defined as errors that arise due to the fact that the difference between two values of a parameter during some iterative scheme is below the machine accuracy of the computer. This is caused by the limited number of computer digits available for storage of a given physical value. Double precision has been used in order to minimise this possible error source. 6.4 Domain discretization When a CFD project for a resistance analyses is started, the engineer only have the hull with the elements needed to calculated, for example the propeller or like in this case the appendages. It is necessary to introduce the ship in a domain which will be discretized where the momentum and continuity equations and, as well as of turbulent and VOF equations (the models described before) have been solved. Values of the dependent variables will be computed at the grid nodes or in the center of the cells. Different domains could be used for sailing ships, but the most used are cylindrical and parallelepiped (or boxes) form. The first one has the advantage that the same geometry could be used for different leeway and heel conditions and it is better when the sails behaviour is studied. On the other hand, a rectangular form is used in hydrodynamic because it is possible to take advantage of the symmetry of the model and in cases like this where the complete hull is studied, meshes need less elements as the cylindrical domains. Figure 6.7: CFD Domains As this work is focused in hydrodynamic, parallelepipedal domains have been used. First, the model is chosen, the next steps are the size of the domain that should be large enough so that the boundary conditions imposed on its walls not substantially affect the behavior of fluids in the vicinity of the vessel. At the same time, the boxes should be small enough so that the resulting problem can be resolved with the available memory in the machine. Domain sizes will be explained below. Once the domain is chosen, the next step is how the domain is filled. If the geometry is simple (e.g. rectangular or circular), choosing the grid is simple: the grid lines usually follow 82

97 the coordinate directions. However if the geometry is more complex, as a ship hull with appendages, the choice is not at all trivial. In this way, meshes could be divided in two main types: structured meshes, where all nodes are connected on a regular basis, using simple elements of two or three dimensions. Therefore only be obtained as elements quadrilateral (2D) or hexahedral (3D), being a good example of this type the Cartesian meshes. This is not so for unstructured mesh, which is identified by irregular connectivity. It cannot easily be expressed as a two-dimensional or three-dimensional array in computer memory. This allows for any possible element that a solver might be able to use. Compared to structured meshes, this model can be highly space inefficient since it calls for explicit storage of neighborhood relationships. These grids typically employ triangles in 2D and tetrahedra in 3D. Finally, there is a case, hybrid meshes, where elements of both types are used. The difference between the models described above is mainly how the elements or nodes are arranged and the how volume is discretized. This is an important question because if the flow is not perpendicular to the faces of the cells, it will not move from cell to cell but entered into multiple cells at once, so an error is generated. This error will be reproduced in each iteration if the cells are not sorted. This is one of the main differences between structured and unstructured mesh. In the case of structured meshing, all cells must follow more or less the same direction, so that if the flow is not parallel to them, a more or less constant over different domain for each orientation error. Figure 6.8: Numerical diffusion along a structured mesh In the case of unstructured meshes cells are oriented differently. The parallel flow will only some of the cells. In this case the error will be constant and the same for each orientation. Looking back over the past ten years, it is seen in various articles published in various conferences, which are focused on the CFD the naval sector as Tokyo [65] or Gothenburg [66], or in Chesapeake and Auckland congress that are more focused on sailing vessels, how the meshing methodology in recent years has evolved. Following this trend, various models have been tested obtaining accurate results [15] [16] with multiblock structured meshes and with trimmed meshes. However in this case, apart from working with the most used meshes 83

98 Figure 6.9: Numerical diffusion along an unstructured mesh and with the ones which better results have been obtained, we have decided to go one step further and try a kind of meshing little used so far such hexcore meshes, where a combination of structured and unstructured is used. Accuracy is also improved if one set of grid lines closely follows the streamlines of the flow, especially for the convective terms. This cannot be achieved if triangles and/or tetrahedra are used, but is possible with quadrilaterals and hexahedral. In this work, different methodologies has been used trying to compare the trying to compare the benefits of each other models, but focus on the hexcore method because it is a new methodology used for this kind of simulations Unstructured Mesh The first mesh used was the easiest one to generate, the unstructured mesh. Building this kind of mesh using any program is quite simple and little laborious, but build a good mesh of this type is quite complicated. Starting from a CAD geometry that should be closed, the main parts will be named assigning each a number of properties, size elements and inflation for the boundary layer. Depending the program a different algorithm will be used to fill the domain. A parallelepiped domain is commonly used and the dimensions of this box in [X;Y;Z] are given by [1L,-3L;0,-1.5L;0.75L,-1.5L]. For this kind of mesh, and with the tools used in this work, Delaunay triangulations are used to fill the domain and to maximize the minimum angle of all the angles of the triangles in the triangulation; they tend to avoid skinny triangles [67]. Nowadays, all commercial programs include an option that permits to do this kind of mesh automatically. Initially unstructured meshes were used for the first results. This decision was agreed with other colleagues when this work started in 2006, they specially emphasized that a 84

99 Figure 6.10: Overall Unstructured Mesh Domain prism boundary layer should be used around the free surface to obtain an accurate wave profile calculation [15]. In figure 6.10 It is possible to see an example of this kind of mesh with the Transpac52 inside. The main problem of this kind of mesh is the join between the free surface inflation with the hull inflation, in this kind of ships. The main problem is that the transom is too close to the free surface and the slope of the hull is too stretched. Moreover when it is needed different sizes as it is showed in Figure 6.11: Free Surface inflation detail On the other hand, this kind of mesh could be a good choice to see in a short time the size of the elements needed or if the interest consists in the analysis of the study of the appendages, it is a good option to use this kind of meshes, where the free surface is not modelled. In figure 6.12 it is observed a mesh of this type used for the analyses of the rudder (model) at the same Reynolds number in a wind tunnel. Finally if an optimization algorithm is going to be used, this option is could be one of the choices because if it is easy to generate and modify the mesh automatically. 85

100 Figure 6.12: Rudder Unstructured Mesh Multiblock Structured Mesh The advantage of the structured grid is that they are computationally efficient. The disadvantage is that it is very difficult to represent complex boundaries. For instance, it is very difficult to incorporate appendages on a hull, such as fins, brackets, or shafts. However, Rudders and keels in sailing yachts, placed in the symmetry plane, are somewhat easier to include, but even that is difficult. If the grid, as it is shown, is divided into different blocks, the flexibility is increased. However in test like this where the ship sails with certain heel,leeway and the rudder is turned the difficulty and the time spent on generate this kind of meshes is very high compared with the other methods described in this work. Figure 6.13: Sailing ship division for blocks For this kind of meshes the software ICEM was used. The reason was that when this work started, it was the best way to generate a mesh for ANSYS CFX. In addition, this program uses a block method to build structured meshes, which involves dividing the domain into blocks which are meshed later. Each block is a hexahedron, but this form can be modified by 86

101 deleting an edge or face, in which case the mesh will be not constituted by regular hexahedral elements. In this case, the hull is enclosed in a box which dimensions in [X;Y;Z] are given by [2L,-6L;0,2.5L;1L,-1.25L]. Furthermore, each edge or face of a block can be associated to a geometric element so that the mesh will project each of the block elements on this surface. If a block is removed, the area will not be meshed and the faces of the block were projected on adjacent geometric elements as contour. So, the way to build a mesh is to find areas of interest in the domain, removing the blocks within the ship saving elements. The edges of the blocks can be modelled according to our geometry using spline tangent or other functions. There are two basic methods for wrapping a body in a mesh, by creating standard blocks (Spliting) consisting of cutting blocks or by means of O-grid. The idea is that a square with a body inside is divided into nine blocks using the first method and five blocks using O-grid as it is shown in the figure If the body is touching one or more sides of a smaller number of domain blocks are generated. Figure 6.14: Splitting and O-grid Schemes Figure 6.15: Block Mesh To mesh a sailing ship with this technique, a multiblock mesh was performed with particular interest in the areas close to the hull. This model has the added difficulty that the 87

102 free surface is very close to mirror greatly hindering its meshing. To overcome this difficulty, closely they fitted blocks by the O-grid technique to the hull.in addition, as it is shown, the shape of the waves generated by the hull are follow to obtain more accuracy. Figure 6.16: Free Surface Multiblock modelled Figure 6.17: Multiblock details Unlike for conventional ships, where the domain is cut by a plane that matches with the flotation plane, and it helps to obtain adjacent blocks (upper and lower) that allows easily to have the same number of elements in the vertical plane and spaced the same distance. This is not possible with this model, therefore, an intermediate block is created in the hull so that the waterline becomes a flotation volume so that when it evaluates numerically, the free surface can be moved within optimizing the solution volume. 88

103 With this method, the boundary layer is created manually. It is the user who can determinate the growing of the elements. This is set from the lateral edges of the block instead the surface from they grow up. Another disadvantage to this method is the difficulty to use it with shape optimization algorithm due to the possibility to create bad elements when the mesh is changed Trimmed Mesh The trimmed meshing model, included in Star-CCM+, utilizes a template mesh constructed from hexahedral cells from which it cuts or trims the core mesh based on the starting input surface. The process starts defining the domain in the program where only the body have been imported. In the case that we are working on, the strategy used to mesh has been to create a box which dimensions in [X;Y;Z] are given by [1L,-3L;0,1.5L;0.75L,-1.5L]. Figure 6.18: Trimmed Mesh After that, the process continuing covering the solution domain with a coarse Cartesian grid, and adjust the cells cut by domain boundaries to fit the boundary. The problem with this approach is that the cells near curve boundaries are irregular and may require special treatment. To obtain more accuracy in the curve boundaries feature curves are generated to retain the sharpness of edges throughout the whole meshing process. In figure 6.20 it is possible to observe the difference between selecting the edges (right) or not (left) However, if this is done on a very coarse level and the grid is then refined several times, the irregularity is limited to a few locations and will not affect the accuracy much but the degree of boundary irregularity is limited. In order to move the irregular cells further away 89

104 Figure 6.19: Trimmed Mesh Process Figure 6.20: Difference with and without features curves from walls, one can first create a layer of regular prisms or hexahedral near walls; after this, the outer regular grid is cut by the surface of the near-wall cell layer. This approach allows fast grid generation but requires a solver that can deal with the polyhedral cells created by cutting regular cells with an arbitrary surface. In the case of ship with appendages, the challenge comes from the strategy to mesh in this areas where it is interested to reproduce the phenomena that is important. For example, refined area will be set near in the free surface plane and in the appendages wake trying to capture the velocity reduction produced in that area. In the following figures the refinement areas are showed. Furthermore, a prism boundary layer is created around the hull and the appendages. From the hull, four layers are used in order to model the the fluid behaviour close to the wall, while around the appendages 12 layers looking for a y + = 1 where the boundary layer is solved. The trimmer is expected to produce best results when working with multiphase flow and free surface (due to its ability to describe the smooth free surface) [16], [66]. Two of the main advantages of this method is the possibility to align refine volumes and the use of anisotropic elements that are essential to define the free surface. On the other hand one of the disadvantages is it use for complex geometries due to their surface treatment. 90

105 Figure 6.21: Free Surface and keel wake refinement Hexcore Unstructured Mesh Hexcore grid is a hybrid meshing scheme that generates Cartesian cells inside the core of the domain and tetrahedral cells close to the boundaries. Furthermore, the transition between the tetrahedral and the Cartesian mesh zones is managed by the introduction of pyramids. Hanging-nodes (or H-) refinements on the Cartesian cells allow efficient cell size transition from boundary to interior of the domain. The Polyhedral mesh is generated by converting a firstly-created tetrahedral mesh. The polyhedral conversion allows keeping the same boundary layer refinement as the underlying tetrahedral mesh and, as the same time, to reduce the cell count by approximately a factor of two or more in the latest releases. On the other hand this method does not have the tool to mesh anisotropic in one direction directly and it is not possible to aligned cells. Two different strategies have been tested for this purpose. The first one has been to try to reproduce the anisotropic mesh. To do this a a first box has been defined where a first mesh has been done. The dimensions of this box in [X;Y;Z] is given by [1.5L,-1.5L;0,-2L;1.33L,- 1.33L]. This box will be the core from the mesh will be built as it is shown in the following image. It features a tetrahedral/hybrid mesh adjacent to walls and a Cartesian mesh in the core flow region. Wedge elements are created only when boundary layers are attached on faces pre-meshed with triangular elements. To ensure that there is no disturbance in the free surface, the mesh has been extruded 3L fore and 5L aft. For this simulation, trying to test this new methodology half of the canoe body was taken. The second strategy that has been used is using a conventional box to mesh the volume without taking advance the anisotropic advantage. This is one of the aim of this thesis, compare this methodology with the ones used commonly. This methodology was used to test the model with appendages and in leeway and heel conditions (fig In this case the dimensions of the box used in [X;Y;Z] is given by [L,-3L;1.5L,-1.5L;0.5L,-1.33L]. There are some differences between both methodologies. First the mesh used for the 91

106 Figure 6.22: Hexcore symmetry Figure 6.23: Hexcore Complete Model symmetric model needs interface due to the mesh is not conformed. Furthermore, to save cells, these interfaces are to close to the ship and they could give problems when the appendages are added. Without appendages bad elements where found close to the interface and the cell growth is not uniform completely, the cells decrease until the interface and then they have a uniform size bigger until they are close to the ship. In addition, in conditions with leeway and heel the complete model has to be mesh and the first model uses more cell to discretize the domain. As it was said before, one of the aims of this work is to compare and validate this mesh with others more used. In the case the appendages are added, the mesh is refined, as it was done with the Star-CCM+ mesh, with small elements in the keel downwash trying to capture the velocity reduction produced there. 92

107 In the case of the canoe body, boundary layer could be solved or modelled. In these cases the meshing strategy will be different. As it was discussed in section 6.2.2, when the boundary layer is modelled it is not needed more than four layers to model it, like it was done with the other mesh methodologies. However, when the boundary layer is solved more layers are needed. Figure 6.24: Fluent Free Surface and Keel Wake Refinement As it was explained previously, the wall treatment is effective in situations where there is not detachment, like the canoe body case. On the other hand, in the case of lifting surfaces like the appendages, the boundary layer has to be solved to avoid phenomena like the one seen in fig 6.3, which are common in situations with leeway and heel. To solve this, a very fine first layer is needed and more than ten layers looking for obtaining a y + lower than one. Following this, for the ship appendages 12 layers where placed to capture the fluid behaviour close them. Figure 6.25: Bulb Boundary Layer Mesh In the figure 6.25 the bulb is meshed following this methodology. In the picture it is possible to see the layers growth and how the aft part of the bulb was modelled and also meshed. With the keel and the rudder, the same methodology was used as it is shown below: However, in this case some issues have been found. The first one is the transition from the four layers from the canoe body to the twelve layers existed in the appendages. When this work with this mesh started, the problem has not solved directly in the release used for this (ANSYS 15.0). It was needed to workaround it and it was not worked in all the cases. But, in the release 16.0 this changed and it was easier to do that. 93

108 Figure 6.26: Keel (left) and Rudder (right) BoundaryLayer Mesh Figure 6.27: Canoe body Appendage Boundary Layer Transition The second issue find in all the codes was the lower part of the rudder. It is a singularity point and the boundary layer is difficult to mesh. The boundary layer is crushed near the this point. Figure 6.28: Rudder Singularity Point 94

109 6.5 Boundary Conditions The numerical solution of the equations of fluid motion provided above, for any given hydrodynamic problem, require boundary conditions to be defined. These represent a unique description of the state of the flow at the geometrical boundaries of the three dimensional space within which the equations are to be modelled. There are in general, two types of boundary condition that can be applied, namely: - Where a fixed or prescribed value is defined for the variable of interest at known points on the boundary (Dirichlet boundary condition) - Where the gradient (usually normal to the boundary) of the variable is known (Neumann condition) Typical examples of the first kind can be found in the calculation of the flow field around a ship moving at constant forward speed, in an axis system moving with the vessel, and with the computational domain formed by a large control volume around the vessel within which the numerical solution is to be carried out. In this case, the fluid is assumed to enter the domain at an upstream boundary or inlet such that the ship appears stationary and the water flows past it. The inlet boundary velocity in this case is set to be a fixed value equal to the speed of the ship, and in the opposite direction. Similarly, on the ship surface, the values of the fluid velocity components are all set to zero (the so-called no-slip condition). Examples of the second type of boundary condition can also be found in the numerical solution of steady ship flow problems. A symmetry plane is often assumed to lie along the ship s centreline that has the practical benefit of reducing the size of the computational domain. In cases for which the free surface effects are small or simply not of interest, the water-plane can also be assumed to be a symmetry plane (the so-called double-body problem). The symmetry boundary condition for the scalar pressure, and velocity components tangential to these boundaries, is that their gradients normal to these boundaries are zero. The numerical implementation of these boundary conditions is dependent upon the type of solution method adopted. Here the conditions used for the analyses described in this work are described. Inlet In most CFD methods for the flow around the hull, the inlet plane is located well in front of the hull, where undisturbed conditions may be applied. It is common to place the hull in the direction of the x axis, and therefore the x velocity is then set equal to the ship speed and the other components are set to zero. There are two ways to set this inlet condition. By means of a velocity inlet or by a pressure inlet. In ANSYS fluent, that is the software used in the majority of test the pressure inlet condition has been used. In this, the total pressure is given and the free surface position is determined. It is assumed to be horizontal and normal to the direction of gravity (in this case z negatives). 95

110 Outlet At the outlet plane the flow is not known, even if it is placed far downstream, because the wake from the hull has to pass the plane. Therefore, velocities or turbulence quantities cannot be specified. The usual choice is to specify a Neumann condition for these quantities. Zero variation of the quantities normal to the plane is thus assumed. Alternatively, zero diffusion may be assumed, which means zero second derivative normal to the plane of these variables. As to the pressure, the Neumann condition could be specified as well, but if this condition has also been applied upstream, the pressure must be given at one point at least. Otherwise, the magnitude of the pressure in the computational domain would be undetermined; only the gradients could be computed. If the plane is far away, depending on the authors from at least to half a ship length to three ship length, the pressure may be assumed undisturbed. In this case, a pressure outlet condition has been used. This condition requires the specification of a static (gauge) pressure. A set of backflows conditions is also specified in case there is a flow reverse direction during the solution process. As the outlet is far enough, this issue has not appeared in the simulations. Symmetry Symmetry conditions are normally applied at the centerplane outside the hull (in the double model approach). At the centerplane, this is a true condition only if the (symmetric) hull is moving straight ahead and there is not propeller action. Furthermore, this model is not valid for sailing yacht because this kind of ships sails with certain leeway and heel and in the tests some for this work is interesting to see the influence of the turned rudder over the hull. The only test where this condition is possible to be used with a symmetryc model is in upright simulations. This assumption reduces, when is possible to be used, the computational effort considerably because the grid has to cover only one side of the hull. Symmetry conditions for tangential velocities, pressure and turbulent quantities are zero gradient normal to the surface (i.e. A Neumann Condition). For the velocity component normal to the surface, a Dirichlet condition applies, the velocity component is zero. In spite of there is not symmetry condition in the middle of the hull, this condition has been used in the boundary walls of the domain (top, bottom and both sides). Commercial CFD s like Fluent assumes a assumes a zero flux of all quantities across a symmetry boundary. There is no convective flux across a symmetry plane: the normal velocity component at the symmetry plane is therefore zero. There is no diffusion flux across a symmetry plane: the normal gradients of all flow variables are therefore zero at the symmetry plane. The symmetry boundary condition can therefore be summarized as follows: - zero normal velocity at a symmetry plane - zero normal gradients of all variables at a symmetry plane Since the shear stress is zero at a symmetry boundary, it can also be interpreted as a slip wall when used in viscous flow calculations, taking advance of this component and avoiding to use walls that could give reflection issues. 96

111 Opening An opening boundary condition allows the fluid to cross the boundary surface in either direction. For example, all of the fluid might flow into the domain at the opening, or all of the fluid might flow out of the domain, or a mixture of the two might occur. An opening boundary condition might be used where it is known that the fluid flows in both directions across the boundary. Wall For the hull and the appendages the wall no-slip boundary condition is used., where all velocity components are zero. With zero tangential velocity, the pressure gradient normal to the wall is also zero according to the relation between streamline curvature and pressure gradients. A Neumman condition can thus be applied on the surface. The no-slip condition implies that the fluctuating part of the velocity is also zero, which means that k is zero on the surface. As shown by Wilcox [53], ω tends to infinity as y approaches zero. A finite value can be determined, however, if the surface is assumed to have roughness. This value is given by defect by the program. On the other hand, talking about turbulence models, the surface boundary condition for ɛ is more difficult to express in a simple way because the ɛ equation cannot be directly integrated thorough the viscous sublayer. A large number of so-called low Reynolds number correction to the equation have been proposed. In the Near Wall Treatment section has been explained how the boundary layer is solved close to the wall. 6.6 Numerical Setup Historically, in naval industry the turbulence models described in section 6.2,k ɛ and SST k ω, are the most often used. In ship hydrodynamics, the k ɛ model and its variants have always been a popular choice which good results have been obtained. At all workshops, there has been a number of works employing this method (e.g. Izquierdo and Gonzalez [16] in Gotheborg 2010). However, it has become increasingly clear that the detailed features of the ship wake cannot be obtained in this way. The wake contours, which are often quite irregular, are smoothed out. It is well known from other fluid mechanics applications that the model is not suitable for flows with strong streamwise vorticity, and it is known the ship wake is dominated by such vorticity, generated at the aft bilges. Therefore, a somewhat different approach, the k ω, has gained in popularity and maybe today is the most used. For the case without appendages, both turbulence models have been used trying to compare their effects. Depending on the turbulence model, different strategies to treat the boundary layer can be chosen. When the viscous sublayer is not solved it could use different wall-function approach to improve robustness and accuracy when the near-wall mesh is very fine. In the case of k ɛ the scalable wall function enables solutions on arbitrarily fine near-wall grids, which is a significant improvement over standard wall functions. However standard two-equation 97

112 turbulence models often fail to predict the onset and the amount of flow separation under adverse pressure gradient conditions. This is an important phenomenon in many technical applications and the scientific community has developed a number of advanced turbulence models. The models developed to solve this problem have shown a significantly more accurate prediction of separation in a number of cases. Separation predictions are important in many applications like appendages behavior. The based Shear-Stress-Transport (SST) model [68] was designed to give a highly accurate predictions of the onset and the amount of flow separation under adverse pressure gradients by the inclusion of transport effects into the formulation of the eddy-viscosity. This results in a major improvement in terms of flow separation predictions. For free shear flows, the k ω SST model is identical to the k ɛ model but one of the advantages of the formulation is the near wall treatment for low- Reynolds number computations where it is more accurate and more robust. As it has been told, different programs have been used during this project. In a first step, results of all of them are presented in the canoe body resistance. But the aim to this is to compare from a numeric point of view the strength of the hexcore mesh in steady simulations. Once the mesh is chosen, other factor that is taken account in this simulation is if the simulation is transient or we can test it in a steady state. This could affect how Navier Stokes equation are discretized and the form of the equations shows linear dependence of velocity on pressure and vice-versa. This inter-equation coupling is called velocity pressure coupling. A special treatment is required in order to velocity-pressure coupling. Two iteration methods have been used, the SIMPLE-algorithm (StarCCM +) that uses a relationship between velocity and pressure corrections to enforce mass conservation and to obtain the pressure field, and a Couple approach trying to take advantage of the steady state solution provided by FLUENT and CFX. When the SIMPLE algorithm is used an approximation of the velocity field is obtained by solving the momentum equation. The pressure gradient term is calculated using the pressure distribution from the previous iteration or an initial guess. The pressure equation is formulated and solved in order to obtain the new pressure distribution and the velocities are corrected and a new set of conservative fluxes is calculated. The discretized momentum equation and pressure correction equation are solved implicitly, where the velocity correction is solved explicitly. This is the reason why it is called Semi-Implicit Method. The algorithm may be summarized, taking account the basic steps updates, as follows: - Set the boundary conditions. - Compute the gradients of velocity and pressure. - Solve the discretized momentum equation to compute the intermediate velocity field. - Compute the uncorrected mass fluxes at faces. - Solve the pressure correction equation to produce cell values of the pressure correction. 98

113 - Update the pressure field: p k+1 = p k + urf p where urf is the under-relaxation factor for pressure. - Update the boundary pressure corrections p b - Correct the face mass fluxes: ṁ k+1 f = ṁ f +ṁ f. - Correct the cell velocities: v k+1 = v V ol p ; where p is the gradient of the a v P pressure corrections, a v P is the vector of central coefficients for the discretized linear system representing the velocity equation and Vol is the cell volume. - Update density due to pressure changes. The coupled algorithm solves the momentum and pressure-based continuity equations together. The full implicit coupling is achieved through an implicit discretization of pressure gradient terms in the momentum equations, and an implicit discretization of the face mass flux, including the Rhie-Chow pressure dissipation terms. In the momentum equations, the pressure gradient for component k is of the form p f A k = f j a u kp p j (6.28) Where a u kp is the coefficient derived from the Gauss divergence theorem and coefficients of the pressure interpolation schemes. Finally, for any ith cell, the discretized form of the momentum equation for component u k is defined as u a k u k ij u kj + j j a ij u k p p j = b i u k (6.29) In the continuity equation, Equation, the balance of fluxes is replaced using the flux expression, resulting in the discretized form: pu a k ij u kj + k j j a ij pp p j = b i p (6.30) As a result, the overall system of equations (6.29 and 6.30), after being transformed to the δ-form, is presented as [A] ijxj = B i (6.31) j More Details of discretization and solution methods can be found in the literature and will not be given here. [3],[69],[70], [71]. After speaking about the different options available, every analysis with different codes are going to be detailed. 99

114 6.7 Canoe Body Result Comparison The first tests done in this work were the analyses of the bare hull resistance where all the features described before have been tested. These analyses have been done with three different codes where their features are compared. Each code has its own philosophy and their uses could be more or less extended in this field. However in the cases described below some features in common have been taken account, analyses in upright position with zero sink and trim ϕ 0 or in dynamic equilibrium ϕ θ have been done for different Fn number. According to the experiments the final dynamic position does not look too significant in the magnitude orders that we are working but it is important to analyse its influence. Furthermore, the minimum change in the position could change the results as it is will be demonstrated. To do this analyses, in table 6.1 the dynamic position measured in the experimental tests is summarized. Different mesh types and tests where the boundary layer has been solved or treated by a wall function, have done. In addition, the two most commonly turbulence models used k ɛ and SST k ω have been compared with the main reconstruction schemes. Fn Trim [ ] Sink [mm] 0,336 0,1-4,63 0,420-0,42-23,07 0,504-1,42-47,61 0,588-1,9-58,48 Table 6.1: Sink and Trim measures As it has been told before, three codes have been used in this first step. First simulation were done with CFX, then some tests with Star-CCM+ and finally with Fluent, where a new kind of mesh no frequently used in this kind of works is researching. In all cases, it will be interesting not only measure and compare global results like the resistance but also local result like wave elevations. Each program has its own best practices to solve this kind of problem. The best way to solve this will be compared and this work will analyse the strong and weak points of the different cases. The setup used for each is described below. CFX is a program that it has been used in the America s Cup by the Emirates Team New Zealand until this edition. When this work started, it was the first CFD used. For this tests, as CFX does not have its own mesh generator, a third party program was used, ICEM CFD Hexa. One of the advantages of this, is the possibility to use hexa elements generating the mesh manually, but on the other hand the user need a lot of time to create a good mesh. After testing different types of meshes including tetra, one mesh like the one shown in figure 6.15 was used following the results obtaining with other ships [15]. In this case and taking account that the experimental tests have been done, independence mesh analyses have not done. The maximum number of elements according the licenses requirement were used. 100

115 With CFX, the influence of Sink and Trim has been analyzed and the metholodogy used with conventional ship as well. Two cases were done following the setup seen previously in other works [15]. In the first one, the model has been fixed at zero sinkage and trim and fixed at dynamic sinkage and trim. The attitude of the model with respect to the coordinate axes was set according to the experimentally measured sinkage and trim values before starting the mesh process. The boundary conditions chosen in this test have been a velocity condition in the inlet and for the outlet. Furthermore, a pressure outlet condition has been tested as well without any significant difference. Frictionless wall has been used at the top and the bottom while friction wall was used on the hull. However, the side walls will vary, since the model has not been cut by the centreline plane, the complete model is simulated and two option were for them. Frictionaless wall condition like it was used for the bottom and the top and symmetry conditions, resulting in both cases virtually the same solution. Figure 6.29: CFX Boundary Conditions In addition, with CFX is possible to customize the boundary conditions. As we are solving an initial value problem, we can help to the program to obtain an easy convergence and accuracy adding some parameters to the setup as it is shown in the following table. Moreover, taking advance of CFX characteristic, some expressions were created in order to use them as parameters. It is a way to automatized the process changing only this field and avoid to review all the setup everytime a characteristic is changed. In both cases, a transient SST k ω turbulence model with wall functions was used and the HRIC VOF capturing technique implemented in CFX [62]. All the numerical equations were solved using algebraic multi-grid acceleration with implicit smoothing. In this case a segregated algorithm was used in a transient simulation where the timestep used is reflected in table

116 Expresions Airini 1.0-Watini BoatSpeed Froude * sqrt(g * Len) DeltaTime 0.15*(Len/BoatSpeed) DenA [kg m 3 ] DenW [kg m 3 ] Froude [] Len 2.78 [m] UnitLength 1.0 [m] UnitTime 1.0 [s] Watini max(0.0,min(1.0,0.5-(z-wavh)*(0.5/zwid))) Wavh 0 [m] hypres DenW*g*(Wavh-z)*Watini-DenA*g*(z-Wavh)*Airini zwid [m] Table 6.2: Numerical Boundary Conditions Variables Transpac 52 In table 6.3 the cases done with this code are summarized and in table 6.4 the resistance results obtained in both cases are presented. Case Solver Description Case C01 CFX ϕ 0, transient SST k ω, y + = 30, HRIC, Segregated Case C02 CFX ϕ θ, transient SST k ω, y + = 30, HRIC, Segregated Table 6.3: CFX Bare Hull Cases Summary Fn Exp. Results [N] Case C01 [N] Case C02 [N] Table 6.4: CFX Resistance Results Both cases have been done in the same conditions. A better approach is obtained in Case C02. Values lower than the expected are obtained in Case C01 obtaining error higher than the 10%, showing in this case the importance to put the model in her right position. In addition the wave cut analyses described in section 4.6 for the closed distance, times the beam as it is shown in figure 6.30, have been compared for two velocities: Fn and Fn In figures 6.31 and 6.32 it is seen that a good approach is obtained with the CFX configuration. A dimensionless ship length has been taken to compare the results in x axis. In this the ship is situated from 0 to 1. In the other axis the wave height in meters has been used. 102

117 Figure 6.30: Wave Cut Distance Figure 6.31: CFX Fn B Wave Cut Analysing these figures with the low velocity the shape of the graphic is follow in spite the first peaks are not coincident. On the other hand, with the high velocity a better approach is obtained. However the the behaviour in the aft part with the variation produced in 0.75 is not reproduced. Finally, it is important to mention that parallel computation on a 2 processors PC was adopted to reduce the required computational time and increase the number of elements used. After working with CFX, and taking account that CEHINAV had been acquired Star- CCM+, some tests were done with this code to compare with CFX. It was interesting to compare the automatic trimmer mesh included in this code with the manual way seen in 103

118 Figure 6.32: CFX Fn B Wave Cut CFX and how it could build the free surface. In time terms, a good quality mesh could be done in hours while with ICEM hexa days were needed, for the first case. Once the first mesh is done, blocks could be used for other cases. After discussing with Star-CCM+ Technical Support and taking advance of their experience, we decided to change the boundary conditions adapting them to the methodology of this code. The boundary conditions chosen in these tests have been a velocity condition in the inlet and a pressure outlet for the outlet. In this case, symmetry conditions have been used for the rest of conditions. Friction wall was used on the hull, and in the appendages in the case tested with them. Figure 6.33: Star-CCM+ Boundary Conditions 104

119 With Star-CCM+, implicit unsteady simulations were done trying to compare the code solutions with the experimental tests. Two turbulence models are compared in a first instance (bare hull case) the k ɛ and SST k ω model. A segregated method, SIMPLE, is implemented in the code, and it is used to couple the pressure and the velocity. Second order methods were used with the discretization parameters to obtain a better accuracy. Furthermore, taking advance of the SST k ω, a test with a boundary layer where the y + = 1 have been done. Finally a case where the damping function for turbulence existing in this code has been used to improve the results. To reconstruct the free surface, the HRIC VOF capturing reconstruction scheme was used, taking advance with the possibility to align the mesh. Moreover, although the simulation is transient, we can manage the solver trying to obtain a fast convergence. In this sense, for obtaining a more accurate method, Courant number must be less than 1 on the free surface at any time. The solution is physical through the simulation. On the other hand if the Courant number is in magnitude order 10 or more, it is possible to increment the time step and only the steady-converged free-surface has physical meaning loosing accuracy in other features. For example, Phenomena like breaking waves or water film separations are captured only using the time-accurate approach. In this case, the fast transient method is used with a time step close to 0.05 sec. The cases done in this case are summarized in the following table: Case Solver Description Case C03 Star-CCM+ ϕ 0, transient SST k ω, y + = 30, HRIC, Segregated Case C04 Star-CCM+ ϕ θ, transient SST k ω, y + = 30, HRIC, Segregated Case C05 Star-CCM+ ϕ θ, transient k ɛ, y + = 30, HRIC, Segregated Case C06 Star-CCM+ ϕ θ, transient SST k ω damping, y + = 30, HRIC, Segregated Case C07 Star-CCM+ ϕ θ, transient SST k ω, y + = 1, HRIC, Segregated Table 6.5: Star-CCM+ Bare Hull Cases Summary With this code the study have been focused in two velocities, obtaining the following results: Fn Exp. Res. Case C03 Case C04 Case C05 Case C06 Case C07 [N] [N] [N] [N] [N] [N] Table 6.6: Star-CCM+ Resistance Results The same trend is observed like the previous code when we compare the simulations between ϕ 0 and ϕ θ. There is a huge difference between the values although the sink difference is small. As it was expected the simulation using k ɛ gives a value lower due to its theoretically worst behaviour in the wall zones. On the other hand k ω gives better approach, and if the damping option is used, the accuracy is higher. However, although Star-CCM+ is well known for its good approach in Naval Applications, the Resistance values are not 105

120 accuracy in the case that the boundary layer is solved. With this kind of ships where the bow is rounded, ventilation numeric issues appear when a y + = 1 layer is used. Talking in resistance terms the best results are obtained with the Case06. It is interesting if the wave cut is compared the differences between using the damping option or not. The mesh used in both case has been the same. As it was said in the previous case, the x-axis represents the dimensionless of the canoe body (length from 0 to 1) and the y-axis is the wave height in this position. Although the global result are better for the case with damping, the local ones are slightly better without damping as it is possible to see in figures 6.34 and Figure 6.34: Star-CCM+ Fn B Wave Cut In these figures it is possible to observe that only the case with damping (Case C06) is capable to achive the first peak. However the elevation in the second maximum does not exceed the zero level as it happens in the real case. On the other hand although the other case does not reproduce the first maximun and minimum, it reproduces better the behaviour in the middle part of the ship. Furthermore none of them is able to reproduce the oscillation occurs close to the third quarters part of the ship. Both described an approach to this part. To finish this analyses with this code, the number of elements was reduced to 2000K elements based in the experience with other ships. Increasing the number it was not possible to reproduce with more accuracy the wave generated behaviour. Parallel computation on a cluster were done with 8 cores. Approximately one day was needed for these simulations. Finally after work in this problem with these two codes, we try to reproduce the same results with Fluent using the hexcore methodology for meshing. Some reasons have encouraged us to try to solve this problem with Fluent, first that it is a program that is not used as often as others for this kind of problems and there is not much researches using hexcore for this kind of problems. 106

121 Figure 6.35: Star-CCM+ Fn B Wave Cut First tests were done using a symmetric model for the canoe body, trying to imitate the methodology used in the trimmed mesh where an anisotropic mesh was used,it was done as it was discussed in section The boundary conditions chosen in these tests are the same used in the Star-CCM+ cases. A velocity condition in the inlet and a pressure outlet for the outlet. In this case, symmetry conditions have been used for the rest of conditions. Friction wall was used on the hull, and in the appendages in the case tested with them. Figure 6.36: Fluent symmetry Model Boundary Conditions However, the use of this method generates a pair of interfaces that have to be linked and 107

122 treated numerically as it was shown in As interfaces have been created, the program has to calculate the results of the physics variables in both sides interpolating on it. It takes more time for prepare and calculate the case. Avoiding the interface a mesh for the complete model was created which will be use in the cases with appendages. The boundary conditions are a velocity inlet for the forward plane, a pressure outlet for the aft plane and symmetry conditions in the lateral, top and bottom Figure 6.37: Fluent Boundary Conditions In the case of this program, the Coupled algorithm was used for pressure-velocity coupling and the Second Order Upwind scheme was used for discretizing either the convection and diffusion terms. For this case two turbulence models were used: k ɛ Realizable and SST k ω both with wall functions and with a pseudotransient mode. In the second case, a turbulence damping was used for the accurate modeling of the interfacial area (free surface area). The reason to use this is that there is a high velocity gradient at the interface between two fluids results in high turbulence generation in both phases. In addition, with fluent is possible to couple the VOF method with the Level set method as it was explaining previously in section Although different reconstruction schemes exists in the code, some of them like the Geo-Reconstruct that is an explicit scheme and good approach gives, two implicit schemes have been used in this simulation. The HRIC [72] that solves the free surface typically with one cell when the interface is expected to be sharp and the Compressive scheme, which is a second order reconstruction scheme based on the slope limiter [73]. The reason to use implicit schemes is to demonstrate that with steady simulations in few time good results could be obtained. Following this, several cases have been prepared to see the accuracy of the model. Like the previous cases models with ϕ 0 and with ϕ θ have been tested. All cases are summarized in the following table. 108

123 Case Solver Description Case C08 Fluent ϕ 0, Steady SST k ω, y + = 30, Compressive, Coupled Case C09 Fluent ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled Case C10 Fluent ϕ θ, Steady k ɛ, y + = 30, Compressive, Coupled Case C11 Fluent ϕ θ, Steady SST k ω, y + = 30, HRIC, Coupled Case C12 Fluent ϕ θ, Steady k ɛ, y + = 30, HRIC, Coupled Case C13 Fluent ϕ θ, Steady SST k ω, y + = 1, Compressive, Coupled Table 6.7: Fluent Bare Hull Cases Summary For these cases the number of elements was reduced to 7000K elements after doing a sensibility mesh study. Parallel computation on 8 processors with a 3.1 Ghz 8 physical cores processor and 256 GB of ram. Each simulation took approximately 5 hours. The results obtained for the same velocities that were studied previously are presented in the following table: Fn Exp. Res. Case C08 Case C09 Case C10 Case C11 Case C12 [N] [N] [N] [N] [N] [N] Table 6.8: Fluent Resistance Results Figure 6.38: k ω Reconstruction Schemes Volume Fraction difference Like the previous cases, with the model at fixed zero sinkage and trim the results were underestimated as well, but a good approach has been obtained in the other situation). In addition, better results are obtained with the k ω model for the same velocities studied. 109

124 It is possible to observe that the results depends of the reconstruction model. This is logical because there are differences in the free surface on the the hull and as it was mentioned, small lengths produces significant differences. Moreover, if the Water Volume of fraction on the hull is compared for the smaller velocity for example, figure 6.38, it is observed the difference of the reconstruction over the hull. Both presents similar graphics but the HRIC model presents more diffuse values between the air and the water (green part on HRIC figure). Moreover if subtract the values from the Compressive schemes it is shown that the wave height over the hull is not the same. Figure 6.39: Pressure difference (Compressive-HRIC) In addition if difference pressure is analysed, there are differences as it is shown in figure There, the main differences are found at the bow and in midship. These values could be expected if the results obtained before are taken account. If we represent the wave cut values obtained in each simulation, it is remarkable that the reconstructions schemes present coincident values independent of the turbulence model as it is shown in figures 6.40 and 6.41 It is important to mark that in both cases, resistance and wave cuts, the best results are obtained with the configuration done for Case C09. Although the case C13 has been noted, its results have been not presented because, like happens in the case with Star-CCM+, ventilation numeric issues have been found, as it is shown in figure 6.42 In this figure, it is seen that the Volume Fraction on the hull is not continue. The blue color represents the areas where the Volume Fraction of water is 1 and the red ones areas where the Volume of Fraction of air is 1. There are areas below the floating line where are air and in the experimental tests this does not occur. 110

125 Figure 6.40: Fluent Fn B Wave Cut Figure 6.41: Fluent Fn B Wave Cut In sailing ships there are sail situations where the bottom is not completely submerged as it is presented in fig 6.43 or the floating line is close to the lower part of the bow. In this case the numerical codes could have problems to solve the interface where a y + = 1. As it is shown in 6.42 there is a layer of air between the hull and the water. There are two ways to workaround this problem, the easiest one is using a wall treatment, a minimum of four layers with y + = 30, because in these cases there is not any detachment of the boundary layer, and it possible to model it saving cells. However, this problem could 111

126 persist if the mesh is not done correctly (figure 6.44). Figure 6.42: Ventilation effects produced in Case C13 Figure 6.43: TP52 with bottom out of the water Figure 6.44: Ventilation effects produced with y + =

127 Then, it will be necessary use functions that help us to avoid these issues. It is possible to program a function that helps to solve it or in the case of Fluent is recommended to use a sharp interface regime (figure 6.45). Figure 6.45: Ventilation effects produced with y + = 30 Finally to finish this section the best results obtained with each code have been compared together. Summarizing the results for the two reference velocities the following table is obtained. Fn Exp. Res. CFX Case C02 Star-CCM+ Case C06 Fluent Case C09 [N] [N] [N] [N] Table 6.9: Comparative Canoe Body Resistance Results Seeing the results, the best case looks the one done with Fluent. For both velocities, it has the better approach. Moreover if we compare the results as it is shown in figure 6.46 all the results are within the experimental error limits. In the CFX and Fluent cases, the analyses for more velocities have been done and presenting the results in the figure In this, the Fluent results are always within the error bars. On the other hand it is not the CFX case. In it, as the velocity is increased, the value is farther from the experimental analyses. After analysing the global values, the wave cut, a local quantity, is also compared (figure 6.48). In this case, it is interesting to remark that for CFX and Star-CCM+, the reconstruction scheme used is the HRIC model, and in Fluent the Compressive Scheme is used in the best case. For the low velocity, Case C06 and Case C09 obtain a good approach of the first peak, but none of the three is capable to capture the first minimum. Moreover we were not able to cross the x axis to reach the second maximum with the Case C06. In the same way the inflection produced between the points 0.75 and 1 neither is it obtained. The final shape after the transom is well reproduced for all the codes. 113

128 Figure 6.46: Resistance Analyses in all cases for two velocities Figure 6.47: Total Canoe Body Resistance In the case of the higher velocity (Fn = 0.420), it seems that the better results are obtained with CFX. With this code we were able to capture the first maximun and the first minimum, but it was not possible to approach the inflection and the two peaks after the transom. However with the other codes the results are not as good as in the Case C02 because the peaks are not reached, but the shape of the profile is obtained. More over there is an inflection in both analyses and the shape beyond the ship is more similar to the experimental. 114

129 Figure 6.48: Fn B Wave Cut Comparison Figure 6.49: Fn B Wave Cut Comparison Following this study, it is interesting to compare how the three codes deal with the HRIC scheme as it is shown in the following figures: In these cases, where the same scheme is compared, better Fluent results were expected, but we are not able not only to obtain similar values to the Compressive scheme used but also are worst than the results obtained in the other cases. 115

130 Figure 6.50: Fn HRIC B Wave Cut Comparison 6.8 Keel Results Figure 6.51: Fn HRIC B Wave Cut Comparison After testing the canoe body behaviour, an extensive numerical analyses of the bulbed keel has been done. The bulbed keel has been studied alone and coupled to the canoe body, comparing the numerical results with the ones. Moreover the effect of the turbulence stimulator has been analysed as well. 116

131 6.8.1 Study of the Bulbed-keel without free surface When this project started, one of the aims was to analyse the appendages behaviour separately from the canoe body. This was done in the early part of this study [14] Different mesh methodologies were applied to this case. As it is a very simple case, an unstructured mesh was done firstly for a quick analyses. However the prism layer is too deformed close to the bulb, and as we explained previously, this is not the most efficient mesh where the flux has a characteristic direction. Therefore a structured mesh was created. In this occasion two scenarios were created. The first one (Case K01) was to consider the bulk without the canoe body, like the analyses are done in a wind tunnel, while in the second one (Case K02) the keel is coupled to the submerged part of the canoe body. For the size of the volume control, it has been taken as characteristic length the scaled bulb length which measures is about half a meter (0.5 meters). The coordinates origin for this simulation has been taken on the upper front end of the keel. Two times bulb dimensions ahead will be left, two times at the sides and bottom and five times aft. With this, the volume control dimensions can be defined by a rectangular box which ends coordinates are (1,1,0) and (-2.5, -1, -1). After determining the size of the volume control, the top of the keel is set to the top plane. The most complicated part of this process is cutting both surfaces as it may cause problems if tolerances have not been determined properly. Moreover the geometry has been retouched and simplified to facilitate the mesh process as it was explained previously (6.5). Once the geometry was prepared, the multiblock mesh was set. Several volumes have been defined according the body geometry. Thus the keel and the bulb part has been divided into three parts as shown in the following figure. Figure 6.52: Keel and Bulb blocks Similar methodology was used in the case where the submerged part of the canoe body has been included, obtaining the mesh shown in figure 6.53 Boundary conditions change from the ones seen in the free surface simulations. In this tests, we try to reproduce the same conditions given in a wind tunnel. So that, sides wall and bottom are defined as free slip walls. however for the top part, there were two alternatives, 117

132 Figure 6.53: Submerged Canoe Body and Bulbed-keel mesh free slide wall or symmetry plane. Finally, the second option was chosen to avoid detachment problems in this area. Finally the bulbed-keel has been divided in two parts to analyse them independently. Figure 6.54: Submerged Canoe Body and Bulbed-keel mesh 118

133 About the outlet (named outflow), different conditions were tested but the better approach was obtained with a pressure outlet condition. For the inlet (named inflow) a velocity condition was provided, and in this case the Reynolds number was the reference to determine the velocity inlet. Moreover some turbulence input parameters were tested being the most approximate the lowest value. After simulating both models the results obtained are presented in the following table (6.10): Velocity Fn Experimental Case K01 Case K02 [m/s] [-] C T x 10 3 C T x 10 3 C T x Table 6.10: Bulbed Keel Total Resistance Comparing the results, we can observe that the results are better in Case K02, when the keel is attached to the canoe body. In this point it is important to remark that we cannot consider the keel infinite and the way that is attached to other element is significant. If the resistance are compared with the measures taken the following graph is obtained. In this it is possible to see that Case K02 is inside the error bars of the experimental test, except one tests but numeric errors have not taken account. Figure 6.55: Keel Resistance Comparison 119

134 Furthermore, it was separated the keel from the bulb to see the influence of each part. It is possible to observe the influence of them over the overall resistance Velocity Fn Case K01 Case K02 [m/s] [-] C T x 10 3 C T x Table 6.11: Keel Total Resistance It is possible to observe than the total coefficient is decreasing when the velocity is increased. The main cause of this effect is that the viscous forces are the most important in this case. This phenomena is seen in the case the keel is coupled to the hull but is not appreciate in the other case Numeric study of the free surface influence over the bulbedkeel Once the bulbed keel has been studied alone, the next step is its study with the model and with the free surface effects. For these case only Fluent simulations were done in order to see the model accuracy and taking advance of the tools provided by ANSYS, comparing the effects of the keel on the free surface. The methodology used is the same that was presented in section 6.7, in the Fluent case with the same boundary conditions. The only difference is in the way that the elements have been meshed. For the canoe body hull the same boundary layer has been used (four layers and y + > 30) but for the keel and for the bulb twelve layers have been used as it was described in the hexcore subsection (6.4.4). Only the following case was tested with this configuration: Case Solver Description Case K03 Fluent ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled. Bulbed Keel y + = 1 Table 6.12: Fluent Canoe Body and Bulbed Keel Cases Summary However, although one methodology has been studied, two kind of mesh have been compared. In the first one, the re-meshing only has been done for the keel and the other one, the wake mesh has been refined as well. The aim of this test if to see if there is any difference between them without the rudder. 120

135 Figure 6.56: Bulbed-Keel Wake Mesh In figure 6.56 both meshes are shown. The fine mesh has 16 millions cells and the coarser one has 4 millions. In the tests done there was a difference between them and in the coarser mesh the keel resistance was underestimated. In these test two kind of results have been studied. First the overall resistance and then appendage resistance. First, the results obtained with the finer mesh for are summarized in the following table and graph: Fn Experimental Case K03 - [N] [N] Table 6.13: Total Resistance Canoe Body and Keel If we compare the results only for the keel bulb, it is interesting to see that they are different from the obtained in the wind tunnel condition. Fn Experimental Case K03 Keel Coeffic [-] C T x 10 3 C T x 10 3 C T x Table 6.14: Total Resistance Canoe Body and Keel It is seen that the results with the free surface are lightly higher than without it. Moreover the keel resistance is in this case approximately the 60% of the resistance. In addition, to finish this part the wave cut has been obtained for the coarser and for the finer mesh 121

136 Figure 6.57: Total Bulbed Keel Model Resistance Figure 6.58: Fluent HK Fn B Wave Cut In this figure it possible to see that not only the resistance values are more accurate with the wake refinement, but also the wave cut approach. In this is possible to observe the curvature change when the keel is past and the shape is more similar. As it was done for the previous cases, the wave cut profile for the same distance was analysed as well for the other Froude number (0.420). As it is shown the maximum and the minimum are not well obtained but on the other hand the shape of the wave is approached. Finally the wave elevation when the keel is attached is compared with the bare hull 122

137 Figure 6.59: Fluent HK Fn B Wave Cut situation. In this it is observed that the bow wave is higher in bare hull case. This is normal due to the different trim in both cases. Furthermore the wave elevation after the transom is higher as well, but the wave displacement is larger in the situation with the keel. Figure 6.60: Wave Contour Comparisson CaseC09 (left) and CaseK03 fine(right) 123

138 Figure 6.61: Wave Contour Comparisson Turbulence Stimulator Influence After reviewing the results obtained, it is observe a difference between the experimental results and the numerical ones. According the several error causes described in section 6.3, it could be possible that exist a model error when the turbulence stimulator have been neglected. In numerical analyses is not common to model this because of the size is very small and we need small elements to represent them properly and the number of elements to do a case like this will be huge. Furthermore, in CFD the turbulence is introduce artificially and this behaviour is represented. However, we consider interesting to study the influence of this elements and for this reason some tests were done to specify their added resistance. To do this one element was analysed as it is shown in the image and it was meshed with an unstructured grid. Figure 6.62: Pin Model and Mesh 124

139 Tests for each velocity were done obtaining the following results: Velocity Resistance [m/s] [N] 1,316 0,005 1,755 0,01 2,193 0,015 2,632 0,022 Table 6.15: Pins Resistance Depending on the elements mounted and the velocity, the added resistance is significant. In the cases studied the drag added values are between 0,3-0,45 N and they affect to the keel results. On the other hand, in the rudder case they are not needed because the flow arrives disturbed. 6.9 Rudder Results Similar methodology as the used with the keel has been done with the rudder. Numerical studies have been done to compare and study the rudder behaviour in presence of the free surface Study of the rudder without free surface Like it was done with the rudder, first an unstructured mesh has been tested. Following the different methodologies seen in For this model the best way was to create a density with very small elements placed around the rudder like the images showed in A layer of small thickness prisms is introduced to capture the fluid behaviour close to the wall. Figure 6.63: Rudder Structured Mesh 125

140 The results were not the expected, because the irregularity of the mesh produced lateral forces much greater than expected. Therefore a structured mesh was tested like the one done for the keel was tested, creating a fine boundary layer to capture the phenomena produced close to the wall. The boundary conditions in this case are the same that were studied in the keel case. However, because of the situation of the rudder only the wind tunnel condition without the canoe body part was studied. On the other hand, like the rudder is an important part of this work, not only the tests was done using the model scale but also the real scale. Tests in this case were done as the same Reynolds number. Experimental results were obtained from wind tunnel experiments done in the E.T.S.I.Aeronauticos facilities. The results obtained for this situation, called Case R01 for Froude are presented in table 6.16 and also compared in figure Furthermore the same study has been done for the velocity corresponding to Froude and the results are shown in table 6.17 and in figure 6.65 Rudder Angle Experimental Case R01 Experimental Case R01 [ ] C L C L C D C D 0 0,002 0,000 0,021 0, ,131 0,171 0,023 0, ,276 0,334 0,024 0, ,431 0,463 0,030 0, ,527 0,553 0,046 0, ,617 0,595 0,053 0, ,697 0,555 0,068 0,114 Table 6.16: C L and C D rudder results in wind tunnel tests Figure 6.64: Froude C L and C D comparison After comparing both graphics,it is important to note that the coefficient results are practically the same in both velocities. However, although the results should be the same, it looks like there is a slight error taken in the slower velocity, because the results are a little be 126

141 Rudder Angle Experimental Case R01 Experimental Case R01 [ ] C L C L C D C D 0 0,001 0,000 0,020 0, ,162 0,175 0,022 0, ,265 0,340 0,024 0, ,398 0,473 0,032 0, ,531 0,564 0,045 0,046 Table 6.17: C L and C D rudder results in wind tunnel tests Figure 6.65: Froude C L and C D comparison different than the expected. On the other hand, there is a very good approach in the higher velocity case as it is shown in the table and in the graphs Numeric study of the free surface influence over the rudder Once the rudder has been studied alone, the next step is to compare the results obtained when it is working in the presence of the free surface and with the canoe body. In this case the results with the experimental tests are going to be compared. Furthermore situations that was not tested experimentally have been done numerically to observe the effects. For these case, like it was done with the keel, only Fluent simulations were done in order to see the model accuracy and taking advance of the tools provided by ANSYS, comparing the effects of the rudder on the free surface. The methodology used is the same that was presented in section 6.7, in the Fluent case with the same boundary conditions. The only difference is in the way that the elements have been meshed. For the canoe body hull the same boundary layer has been used (four layers and y + > 30) but for the rudder twelve layers have been used as it was described in the hexcore subsection (6.4.4). Furthermore, as we did with the keel, a refinement volume was created to have more accuracy with the results. In this case, some tests have been done changing the model position and giving them a certain heel and leeway to observe its effects. The cases studied will be resumed in the 127

142 following table. Case Solver Description Case R02 Fluent Upright position, ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled. Rudder y + = 1 Case R03 Fluent β = 2 ϕ = 10 ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled. Rudder y + = 1 Table 6.18: Fluent Rudder Cases Summary As it was done in the previous section, the rudder was turned to obtain its behaviour under different angles. In this way the results obtained for the upright position in presence of the free surface are presented in the following table: Rudder Angle Experimental Case R02 Experimental Case R02 [ ] C L C L C D C D Table 6.19: C L and C D rudder results under free surface presence Furthermore the following graphs are presented to compare the trend between the experimental and the numerical analyses. Figure 6.66: Froude C L and C D comparison In the case of the lower velocity it is possible to observe a good approach in the smaller angles, and something worst for the higher ones. on the other hand the coefficient values are slightly higher than the wind tunnel condition. There is an influence but lower than in the keel case. 128

143 The same comparison has been done for the case of the other velocity trying to repeat the same phenomena with this velocity. Rudder Angle Experimental Case R02 Experimental Case R02 [ ] C L C L C D C D Table 6.20: C L and C D rudder results under free surface presence Figure 6.67: Froude C L and C D comparison In this case the approach is better as occurs in the wind tunnel condition. It is possible to observe how the C D results matches perfectly. On the other hand there is a difference in the lift results. Error bars with a 3% has been drawn and the difference is higher than this value. Now, the results differ in both cases when the results should be similar. The presence of the free surface adds a new component that increase the values of the coefficient. If the rudder influence on the canoe body is analysed, the resistance of the canoe body is increased, as it was seen in the experimental case. Furthermore the results obtained in the numerical case are a 12% worse. However in the case of higher velocity the error obtained is lower than the 2% which is under the values expected. Once resistance values have been analysed, the free surface is going to be studied as it was done in the keel case. For this the same wake cut profile is compared for both velocities. In the case is shown that the wave is not in phase with the experimental one. This phenomena occurs in the other cases as well. However the maximum peaks are obtained. On the other hand is not the case of the minimum. The part before the rudder is not approached with all the details. 129

144 Figure 6.68: Fn HR Wave Contour Comparisson Figure 6.69: Fn HR Wave Contour Comparisson The second wave cut maintain the same shape, but it was not possible to obtain the last peak. There is a good approach between the global and the local results with this velocity. In addition, analyses with heel and leeway have been done to see the behaviour of the rudder in this conditions. In this case we have focused in one of the most common navigation situation, heel 10 and leeway 2 with the conditions described in As it was done in this section, the same two velocities have been studied obtaining the following results: 130

145 Rudder Angle Experimental Case R02 Experimental Case R02 [ ] C L C L C D C D -6-0,513-0,477 0,024 0, ,258-0,248 0,019 0, ,133-0,169 0,018 0, ,010 0,026 0,018 0, ,292 0,287 0,024 0,024 Table 6.21: C L and C D Rudder Results β = 2 ϕ = 10 Rudder Angle Experimental Case R02 Experimental Case R02 [ ] C L C L C D C D -4-0,409-0,404 0,022 0, ,267-0,272 0,020 0, ,160-0,131 0,018 0, ,009 0,015 0,017 0, ,127 0,158 0,018 0,020 Table 6.22: C L and C D Rudder Results β = 2 ϕ = 10 Figure 6.70: Lift and Drag Rudder Curves Case R03 β = 2 ϕ = 10 In this case it is observed a good correlation in the case of the lift. For the lower velocity, the results are practically coincident except in one case while for the higher velocity the 131

146 problems come in the positive values where the values are a little bit different. In the case of the drag the differences are higher and only in the lower velocity for the positive angles the values are identical. however it is observed that the trend is very similar in both cases although for the higher negative values in both cases the error is unacceptable. In this case to see if the parameters are well calculated and what is happening over the rudder, in one of the points we have analyse first if the y + is the values allowed for this kind of simulation. Figure 6.71: y + values 0 (left) and 6 (right) at Fn Looking at the previous figure, it is seen that the values are within the recommended values in the main part of the domain. There is two critical parts that are the attack edge and one part in the bottom where there is a singularity which gives problems with the mesh, but it is seen the yplus values are similar obtaining good results in the case of 0. If the detachment is evaluated, we can see that in both sides when the rudder is turned at the maximum angle the results are practically equivalent but changing the face where it is produced. Figure 6.72: detachament 6 (left) and 6 (right) at Fn Finally, the free surface profile is evaluated to understand how the rudder can modify the wave contour due to its movement. In this case, there are not experimental results, but 132

147 as the methodology was the same that we did for the upright cases and the global results are acceptable, we could use it to evaluate it. In the following figure, 6.73, the free surface is modelling from left to right and up to down with 6, 2, 0, 2 and 6. Figure 6.73: Free Surface modelling It is observed how the contour behind the transom is modified with the rudder movement. The maximum high is achieved with the rudder has 0 degrees. It is possible to see how the contour shape is deformed and change with the rotation. It is also seen that the wave in the keel area change as well. This is mainly due to the different sink and trim that the ship has for every simulation and it was showed that it change with the rudder movement. In these case, the mesh used has 12 million cells and each case has been run in a cluster using 32 cores. 10 hours were needed to converge each case. 133

148 6.10 Complete Model Results Once the different appendages has been studied separately and knowing the methodology, the problem with both appendages is solved. in addition, this later section will be divided into two subsection. In the first one, the upright condition, cases HKR01 and HKR02 will be evaluated and then the effect of the leeway and heel, the other cases, will be analysed in the second one. In the following table the cases studied are summarized: Case Solver Description Case HKR01 Star-CCM+ Upright position, ϕ θ, Steady SST k ω, y + = 30, HRIC, Segregated ;Keel y + = 30; Rudder y + = 1 Case HKR02 Fluent Upright position, ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled; Keel y + = 1; Rudder y + = 1 Case HKR03 Fluent β = 2, ϕ = 10, ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled; Keel y + = 1; Rudder y + = 1 Case HKR04 Fluent β = 4, ϕ = 20, ϕ θ, Steady SST k ω, y + = 30, Compressive, Coupled; Keel y + = 1; Rudder y + = 1 Table 6.23: Fluent Complete Cases Summary In this section, it is important to mark that in the case of Star-CCM+ the number of elements used in each simulation was about 8 million cells due to the calculation capacity and the experience obtained with other models. With symmetrical model 4 million cells were used obtained very good results [16]. In the Fluent case, the number of cells finally used, 20 millions, was decided after the sensibility analyses done in the previous cases and with more elements the results do not vary so much. In this case 20 hours were needed to convergence the case with 48 cores Complete Upright Numerical Tests To analyse the Upright condition with the canoe body and the appendages, we use the results obtained with Star-CCM+ and its trimmed mesh, Case HKR01, which were done in an early phase of this work. These results with this software and methodology validated [16], [74]. Furthermore, this results will be used to compare the methodology implemented in this work with the hexcore mesh. For these tests, first we are going to compare the results for whole ship and for the appendages for the velocities studied in this work, Fn = and Fn = In this tests the rudder is amidships. The results are presented in table 6.24 and in figure There is not a good approach in both cases. The main cause is the high dependence of the ship position. If there is any error to determine it the results will not be as accurate as we expect. After calculate this global quantity, where the results are not as good as we would like to expect, in the next step the wave cut is analysed and after that the appendages separately. 134

149 Fn Exp. Results [N] Case HKR01 [N] Case HKR02 [N] Table 6.24: Upright Total Resistance Results Figure 6.74: Total Upright Results Figure 6.75: HKR Wave Cut Analyses 135

150 These results show that both software used are capable to obtain the shape of the wave cut but not with enough accuracy. This problem happens in the precious cases where it was difficult to reach the main peaks. If every case is analysed separately, we can see that for the lower velocity there is a very good approach of the Case HKR01 obtaining the curvature changes in the first cut and doing all the maximum and minimum in the second. However a better approach in resistance term was obtained with the other case. Furthermore Case HKR02 is not capable to reproduce well the area close to the keel and the curvature changes that happens close to the rudder. Finally, it is important to note that neither cases got close to the minimum. Comparing the second case (high velocity), the same behaviour is reproduced, but in this case a better resistance approach is obtained with Case HKR01. Furthermore the same problem is obtained with the curvature changes close to the rudder position. It is not well reproduced with Case HKR02. Finally in the second cut both cases follow very well the shape of the cut but neither of them reach the maximum and the minimum. Reviewing both results it is possible to detect what could be the problem that did not allow to obtain a very good approach at it could happen in the bare hull case. It is possible that the error made taking the sink and trim measures could be higher and did not allow to put the ship in her real position. The sink for this cases should be higher. The next step is reviewing the keel results in both cases. It will be interesting to review if the position could affect to the results as well. Fn Exp. Results [N] Case HKR01 [N] Case HKR02 [N] Table 6.25: Upright Keel Resistance Results Figure 6.76: Keel Resistance 136

151 Comparing the results we see that with the trimmed mesh, the value is overestimated while with the case with the hexcore the result is underestimated. On the other hand both approach have an error below the 7% and in the case of the higher velocity below the 3%. The case HKR01 was run with four boundary layers and y + = 30 because the angle of attack is 0 and the profile is symmetric. Later and watching the results, the boundary layer was created to analyse the problem in this condition and to use the same mesh in cases with leeway and heel. Later some tests were done with trimmed mesh and results similar to the obtained in Case HKR02 were obtained. If we add the drag of the pins to the values obtained, the result is over the experimental analyses. The resistance results here, are very similar to those obtained in the case where the keel was tested alone without the rudder presence and with the free surface Case K03 with a refinement behind the keel. Finally the rudder results are evaluated. In this case the high velocity results are going to be compared. Rudder Angle Experimental Case HKR01 Case HKR02 [ ] C D C D C D 0 0,015 0,019 0, ,018 0,020 0, ,024 0,025 0, ,036 0,032 N.A 8 0,052 0,054 0,042 Table 6.26: C D Rudder Results Rudder Angle Experimental Case HKR01 Case HKR02 [ ] C L C L C L 0 0,001 0,000 0, ,137 0,155 0, ,295 0,312 0, ,473 0,459 N.A 8 0,658 0,567 0,533 Table 6.27: C L Rudder Results Looking the results obtained, there is a good approach in both case. In the Case HKR02 there is a good correlation for the drag in small angles. However for the higher one the result is worse. On the other hand, it is possible to see that the results for the rudder are overestimated in the first case, but the difference is too low not only for the lower angles but also for the higher one. In the case of the lift in the Case HKR01 the results are more approximated to the experiment. In this occasion in the second case the values obtained are too lower. It looks like neither of the codes are capable to obtain with accuracy the stall point. 137

152 Figure 6.77: HKR Rudder Results Finally, we have also obtained the C D - C 2 L curves in figure In this figure is interesting to observe the difference in both numerical tests, the cases are one on each side of the experimental curve, and with HKR02 is obtained a very good approach. Figure 6.78: HKR C D - C 2 L Curves Additionally, for the case HKR02 some tests were done for the lower velocity. In figure 6.87 the results are summarized: In these curves it is observed that in this occasion the results do not fit as well it did for the higher velocity. If we obtain the C D - C 2 L curve, the line has not the same approach as it was obtained previously. These tests are penalized by high values and the lower one whose error affect to the approach. After testing the global results, the wave elevation has been obtained in order to understand and compare the flow behaviour with the rudder turned. 138

153 Figure 6.79: HKR02 Rudder Results Figure 6.80: HKR02 C D - C 2 L Curves In the figure (6.81) the images represent the wave height when the rudder is turned (from left to right) 0, 4 and 8 degrees. In them it is seen how the wave field is moving to the starboard side. It is also observed that changes are produced before the fluid arrives to the rudder. In addition, a study of the flow under the free surface has been done first with cut at several planes perpendicular to the fluid flow. The planes have been taken has been x=0.25 m, x=1.25 m, x=2 m and x=2.75 m. The upper figures represent the flow when the rudder in amidships and 4 degrees and the lowest one 8 degrees. It is observed that in the figures with 4 and 8 degrees the field velocities in the cut behind the keel are different. These figures are not symmetric like the first case. Furthermore in the last cut, it is possible to observe how there is a velocity reduction area close to the hull in the starboard side. 139

154 Figure 6.81: Free Surface modelling Figure 6.82: Velocity Field at Perpendicular Planes to the Free Surface Moreover the marked velocity changes produced behind the keel are influenced as well by the free surface as it is observed in the next figure. The areas where the velocity is increased match with the minimum wave height areas. Finally the velocity field has been obtained in a plane parallel to the free surface (z= m)to see how this field affect to the rudder (figure 6.84). 140

155 Figure 6.83: Velocity Field at Perpendicular Planes and Free Surface modelling Figure 6.84: Velocity Field at Parallel Plane to the free Surface In figure 6.84 is represented the velocity field in the plane described. It is observed how the fluid changes close to the rudder and how the reduction is increased in the fore part of the rudder and in the aft. The velocity reduction is not straight as it could be expected. Following this study, the same study have been done in the bulb plane obtaining the following result: 141

156 Figure 6.85: Velocity Field at Parallel Plane in the bulb It is interesting to see how the velocity field is decreased at both rudder sides but stay at higher velocity amidships Leeway and Heel Numerical Study Once the upright tests have been done and compare, some numerical analyses with heel and leeway have been done trying to see the fluid behaviour under the free surface. This part is very difficult to see in the towing tank and in experimental tests and we will serve the numerical tools to research what is happening there. Heel 10 Leeway 2 For this first case, the methodology used is the same that was presented in section 6.7, in the Fluent case with the same boundary conditions. The only difference is in the way that the elements have been meshed. For the canoe body hull the same boundary layer has been used (four layers and y + > 30) while for the appendages twelve layers (y + = 1)have been used following the methodology used in the previous tests and described for the Case HKR03 in 6.23 In this case we have analysed all the components separately. First we evaluate the results obtained with the keel. Fn Exp Drag [N] Drag HKR03 [N] Exp Lift [N] Lift HKR03 [N] Table 6.28: HKR03 Drag and Lift Keel Results In this occasion the results have being averaged because although in resistance the results do not change, they change in the lift case with the rudder. In all the cases the error is under the 5%. 142

157 After analysing the keel, the next step is reviewing the rudder results. For this analyses, the rudder has been moved to obtain the values in different positions as it was done in other cases. In the following tables, the results for both velocities are presented. Rudder Angle Experimental Case HKR03 Experimental Case HKR03 [ ] C L C L C D C D Table 6.29: C L and C D HKR Rudder Results β = 2 ϕ = 10 Rudder Angle Experimental Case HKR03 Experimental Case HKR03 [ ] C L C L C D C D -4-0,209-0,194 0,020 0, ,046-0,040 0,017 0, ,088 0,105 0,020 0, ,224 0,244 0,025 0, ,348 0,378 0,037 0,033 Table 6.30: C L and C D HKR Rudder Results β = 2 ϕ = 10 In the following figures, C L and C D curves are represented to compare graphically the results obtained. Comparing the results, it is observed a good approach in the case of the higher velocity. The lift results are practically the same and it was seen in the table The drag results are also good in general except in the extreme points where the results are worse. In the lower velocity the lift approach is also good but the drag results are not as good as in the higher velocity case. This is very strange because the better values could be obtained for the lower velocity where the detachments effects are lower. Finally to obtain more information about what is happening, the C D - C 2 L curves have been obtained. The correlation obtained is the expected according the results seen previously. The numerical data are within the experimental curve envelop. Although the data could be slightly different, the numerical results obtained are coherent. Furthermore, it is possible to observe how some experimental value is a little out of the logical values. Once the appendages have been analysed, resistance in the same situation as it was done for the upright condition is evaluated, rudder at 0 degrees for the two velocities studied. It is observed that in this case the numerical results are very similar to the experimental, but the numerical values are slightly higher. 143

158 Figure 6.86: and HKR Rudder Results β = 2 ϕ = 10 Figure 6.87: C D - C 2 L HKR Rudder Results β = 2 ϕ = 10 Fn Exp. Results [N] Case HKR03 [N] 0,336 9,66 9,21 0,420 21,07 21,99 Table 6.31: β = 2 ϕ = 10 Total Resistance Results After obtaining the numerical values, and as we did in the previous cases, the wave elevation is obtained and compared with the results obtained in

159 Figure 6.88: Free Surface Modelling HKR β = 2 ϕ = 10 In figure (6.88) the images represent the wave height when the rudder is turned (from left to right, up to down) -6,-2,0, 2 and 6 degrees. If we compare these results with the obtained in figure (6.73) it is observed how the wave train is modified by the presence of the keel which dumps the waves. The first remarked effect is the wave contour in the area close to the keel. The contour is changed by it presence. If we look to the transom area it is possible to observe that although there is a peak and the behaviour is the same, the shape is slightly different in both situations. Moreover the flow behind the canoe body the same damping effect is produced deleting some wave elevations. In addition, a study of the flow under the free surface has been done using the same planes that were used in the previous subsection (figure 6.82). The upper figures represent the flow when the rudder in amidships and 4 degrees and the lowest one 8 degrees. 145

160 Figure 6.89: Velocity Field at Perpendicular Planes to the Free Surface HKR β = 2 ϕ = 10 In figure 6.89 the flow under the canoe body is studied when the rudder is turned 6 and -2 degrees. If these results are compared with those obtained with the upright situation in 6.83, it is observed that the velocity increment produced close to the canoe body is higher in this situation. Moreover is easy to observe the effects of the heel and the leeway to flow behind the keel and how they produce changes in the canoe-body lift. Figure 6.90: Velocity Field at Parallel Plane to the free Surface 146

161 Heel 20 Leeway 4 The other sail condition analysed numerically was HKR04. In this condition the heel and leeway have been increased to 20 and 4 degrees respectively. The same methodology seen in the previous cases and presented in section 6.7 has been used. The characteristic of this simulation, case HKR04, was summarized in 6.23 As it was done in the previous case, the keel is evaluated first obtaining the following results Fn Exp Drag [N] Drag HKR04 [N] Exp Lift [N] Lift HKR04 [N] Table 6.32: HKR04 Drag and Lift Keel Results As it was done in the previous subsection, the results have being averaged, because in the numerical simulations the differences between tests are not higher than in the experimental one where it looks like there is a rudder influence. Anyway after comparing the results is observed that in this case the difference are in both cases higher than it was expected. In the lift case the error is low but in the case with the drag. After analysing the keel, the next step is reviewing the rudder results. For this analyses, the rudder has been moved to obtain the values in different positions as it was done in other cases. In the following tables, the results for both velocities are presented. Rudder Angle Experimental Case HKR04 Experimental Case HKR04 [ ] C L C L C D C D -4-0,258-0,131 0,011 0, ,047 0,126 0,019 0, ,285 0,375 0,041 0,041 Table 6.33: C L and C D HKR Rudder Results β = 4 ϕ = 20 Rudder Angle Experimental Case HKR04 Experimental Case HKR04 [ ] C L C L C D C D -4-0,064-0,079 0,016 0, ,205 0,195 0,025 0, ,383 0,454 0,037 0,041 Table 6.34: C L and C D HKR Rudder Results β = 4 ϕ = 20 Unlike it happens in the previous analyses, in this study the results are not as good as expected, and as it is observed in the following graphics 147

162 Figure 6.91: HKR Rudder Results β = 4 ϕ = 20 Figure 6.92: HKR Rudder Results β = 4 ϕ = 20 The results are under the expected values in lift, and over the expected in drag terms. Except one value in the lower velocity, any of the experimental results match exactly. It is interesting to mark tat if we observe the C D - C 2 L curves the values match better. The differences in lift and drag term are compensated. Figure 6.93: C D - C 2 L HKR Rudder Results β = 4 ϕ =

163 The correlation obtained is the expected according the results seen previously. The numerical data are within the experimental curve envelop. Although the data could be slightly different, the numerical results obtained are coherent. Furthermore, it is possible to observe how some experimental value is a little out of the logical values. Figure 6.94: y + appendages HKR04 In this case where there is detachment the characteristic of the mesh is evaluated, specifically the boundary layer and the mesh method that has not been modified. In this way a Yplus analyses has been done in the appendages to see if the boundary layer has been solved properly. In the previous figure it is seen that the y + is between 1 and 3. The best approach should be obtaining values under 1. It was difficult due to the shapes of the appendages to reduce more the boundary layer without change so much the number of elements. Once the appendages have been analysed, resistance in the same situation as it was done for the upright condition is evaluated, rudder at 0 degrees for the two velocities studied. Fn Exp. Results [N] Case HKR04 [N] 0,336 10,38 11,51 0,420 22,27 28,10 Table 6.35: β = 4 ϕ = 20 Total Resistance Results In this case, the numerical results do not match as well as it was done in the other cases. Moreover with high leeway and heel values, in general the approach obtained differs from the experimental values as it was seen in all the elements. To review that the case is well done, it was reviewed that there is not any ventilation issue. It is observed like the free surface is well represented and there is not any numerical ventilation below the hull. On the other hand, it is observed like there is water volume of fraction represented on the transom and the depth of the hull seems to high. The error in the measures could be produced because of probably the sink and trim measures are not correct, and the high depth explains this difference in the values obtained. 149

164 Figure 6.95: Ventilation effects produced in Case HKR04 Although these values are not the best ones, the wave elevation is obtained and compared with the results obtained in the previous cases. It is interesting for this work to see how is the free surface behaviour with the appendages. In the following figure the images represent the wave height when the rudder is turned (from left to right) -4,0 and 4 degrees. Figure 6.96: Free Surface Modelling HKR β = 4 ϕ = 20 If we compare these results with the obtained in the previous cases, figures 6.81 and 6.88, 150

165 it is observed in the transom area how two peaks are produced in the middle case, the one where the rudder is amidships. In the other cases there is only one peak in the starboard side. With the rudder turned 4 degrees, more amplitude waves are observed. in this situation the rudder is situated in a symmetric position respect to the flow. The next step, as it was done in the previous cases is a study of the flow under the free surface. The same planes that were used in the previous subsections (figure 6.82) have been used. In figure 6.97 the velocity planes are represented for the cases studied when the rudder is turned, -4 (left) and 4 (right) degrees are represented in the upper part, and 0 degrees in the lower part. There is not any significant change, except in the case of 0 degrees where a velocity increment is produced behind the rudder. Moreover, the velocity field has been obtained in a plane parallel to the free surface (z= m) to see how this field affect to the rudder. In this figure 6.98, there are three pictures representing the velocity field in the three rudder position studied for the low velocity, 4 (left) and 4 (right) are represented in the upper part, and 0 degrees in the lower part. It is possible to observe how the flow behind the keel is not modified when the rudder is turned - 4 degrees. The velocity reduction produced by the keel is maintained without any perturbation. On the other hand, when the rudder is turned an although it is not situated in the direct keel wake, there is some changes in the flow behaviour. Figure 6.97: Velocity Field at Perpendicular Planes to the Free Surface HKR β = 4 ϕ = 20 Finally, trying to obtain more information about what is happened in this situation, vector velocity plots have been obtaining in the last plane (x=2.75m) and compare with the 151

166 Figure 6.98: Velocity Field at Parallel Plane to the free Surface HKR04 upright position. When the ship is in upright position the only significant perturbation is produced by the bulb. As it is shown in the following figure, there is a velocity reduction in the keel and rudder wake and two vorticities are produced by the bulb, one clockwise and the other in reverse direction as it is shown in the next picture. Figure 6.99: Velocity vectors in plane HKR02 x=2.75 m However the situation is different when the ship sails under leeway and heel as it was seen in the following picture: 152

167 Figure 6.100: Velocity vectors in plane HKR04 x=2.75 m In this picture is possible to see how the flow behaviour changes in this position. The two vortices generated in the upright position are replaced by one and it is interesting to observe the vortex generated by the rudder tip. Figure 6.101: Detail of Velocity vectors in plane HKR04 x=2.75 m It is interesting to note that the same vortex is created by the rudder in upright position when it is turned as it is shown in the figure It is shown how the velocity profiles changes and how the velocity field behaviour changes close to the hull changing the pressure field in the canoe body and increasing her lift as it was predicted in experimental chapter. 153

168 Figure 6.102: Detail of Velocity vectors in plane x=2.75 m for β 0 ϕ 0 δ 8 Figure 6.103: Detail of velocity field x=2.75m (left) and Total pressures on the canoe body (right) 154