Design of Rim Driven Waterjet Pump for Small Rescue Vessel Master’s Thesis in Nordic Master in Maritime Engineering Thor Peter Andersen Department of Shipping & Marine Technology Division of Marine Design Chalmers University of Technology Department of Mechanical Engineering Division of Fluid Mechanics, Coastal and Maritime Engineering The Technical University of Denmark Gothenburg, Sweden 2014 Master’s Thesis 2014:6 This page is intentionally left blank. MASTER’S THESIS IN THE NORDIC MASTER IN MARITIME ENGINEERING Design of Rim Driven Waterjet Pump for Small Rescue Vessel Thor Peter Andersen Department of Shipping and Marine Technology Division of Marine Design Chalmers University of Technology Gothenburg, Sweden 2014 . Design of Rim Driven Waterjet Pump for Small Rescue Vessel Thor Peter Andersen © Thor Peter Andersen, 2014 Master’s Thesis, X-14/302 Department of Shipping and Marine Technology Division of Marine Design Chalmers University of Technology SE-412 96 Gothenburg Sweden Telephone: +46 (0)31-772 1000 Gothenburg, Sweden 2014 Design of Rim Driven Waterjet Pump for Small Rescue Vessel Master’s Thesis in the Nordic Master in Maritime Engineering Thor Peter Andersen Department of Shipping and Marine Technology Division of Marine Design Chalmers University of Technology & Department of Mechanical Engineering Division of Fluid Mechanics, Coastal and Maritime Engineering The Technical University of Denmark Abstract The hydrodynamic design and performance analysis of a pump with an electromagnetic rim driven impeller and with an open centerline is performed. The pump is the driving force of a waterjet system for a small rescue vessel. The rim-engine driving the pump is already developed and generates dimensional constraints for the pump design. The purpose of the open centerline is to avoid entanglement, and thereby downtime, if ropes are sucked into the system. The rescue boat is used to tow multiple life rafts and a high bollard pull force of 4 kN is therefore required, a top speed of approximately 20 knots is desired. The design work have been carrier out using TurboDesign1 and the performance is analysed using computational fluid dynamics, specifically Menters SST k − ω turbulent flow model in Ansys Fluent. Three pump configurations are analysed and compared in order to study the effect of the open centerline and if a pump design without guide vanes is feasible. The performance analysis shows that a pump without guide vanes is unable to provide the required thrust and thereby not feasible. The thesis concludes that the final concept design for the rim driven hubless pump is able to deliver the force needed to reach a top speed of 25 knots. The required force for the bollard pull condition is, however, not achieved due to cavitation in the pump. A maximum efficiency of approximately 70% is reached. This is an acceptable efficiency, but it is low compared to similar standard waterjet pumps. The low efficiency reduces the cavitation properties of the pump, compared to regular pumps with similar dimensions, as the loading of the blades must be higher to achieve a force production similar to a standard pump. A goal of the future work should be to improve the cavitation properties of the system. There are several ways to improve the cavitation properties, however, the most efficient measure is a redesign of the inlet duct and an increased impeller diameter, meaning a redesign of the electromagnetic engine driving the pump. This page is intentionally left blank. Design of Rim Driven Waterjet Pump for Small Rescue Vessel Master’s Thesis in the Nordic Master in Maritime Engineering Thor Peter Andersen Department of Shipping and Marine Technology Division of Marine Design Chalmers University of Technology & Department of Mechanical Engineering Division of Fluid Mechanics, Coastal and Maritime Engineering The Technical University of Denmark Resume I denne afhandling er det hydrodynamiske design af en rem dreven pumpe med åben centerlinje fuldført. Endvidere er en analyse af ydeevnen udført. Pumpen skal drive et waterjet system p̊a et mindre hurtigg̊aende redningsfartøj. Pumpen designes til en nyudviklet elektromagnetisk remmotor. Form̊alet med den åbne centerlinje er at undg̊a at reb vikler sig ind i pumpen i tilfælde af at dette suges ind i systemet. Derved undg̊as downtime p̊a grund af reb i pumpen. Redningsfartøjet skal kunne trække op til flere sammentøjrede redningsfl̊ader, derfor er en høj trækkraft ved lav fart en nødvendighed. Pumpen designes derfor s̊aledes, at en trækkraft p̊a 4 kN pro- duceres af waterjet systemet. Tophastigheden skal mindste være 20 knob. Designet af pumpen er udført ved brug et pumpe design software kaldet TurboDesign1 og analysen af pumpens ydeevne er udført ved hjælp af numerisk fluid mekanik, specifikt ved brug af Menters SST k − ω turbulens model i Ansys Fluent. Tre forskellige konfigurationer af pumpen er testet for at undersøge effekten af at have en åben centerlinje, og om det er muligt at opn̊a en acceptabel ydeevne med et design uden statorblade. Analysen af ydeevnen viser, at en pumpekonfiguration uden statorblade ikke kan producere den nød- vendige trækkraft. Det konkluderes at redningsfartøjet kan opn̊a en hastighed omkring 25 knob ved brug af det endelige konceptuelle design. Resultaterne viser dog, at den nødvendige trækkraft ikke opn̊as, da pumpen oplever kavitation i denne tilstand. En maksimal effektivitet p̊a omkring 70% er opn̊a et med det endelige pumpe design. Dette er en acceptabel effektivitet p̊a trods af at den er lav sammenlignet med en standard waterjet pumpe af samme dimensioner. Den lave effektivitet er imidlertid grunden til, at pumpen opleves store kavitationsudfordringer n̊ar den maksimale trækkraft skal op- n̊as. Pumpebladene skal belastes h̊ardere for at producere den samme trækkraft som en standard pumpe, og der opleves derfor mere kavitation ved denne tilstand. Det fremtidige arbejde indebær en forbedring af pumpen, s̊aledes at kavitation ikke er et udslagsgivende problem for den maksimale trækkraft. Pumpedesignet kan ændres p̊a flere punkter, men en ændring af pumpens diameter er den mest effektive metode til at opn̊a den ønskede effekt. Dette vil dog medføre en konstruktionsændring af den remdrevne motor, der driver pumpen. This page is intentionally left blank. Preface This master thesis is the final project of Thor Peter Andersen on the master study program Nordic Master in Maritime Engineering at the Technical University of Denmark (DTU) and Chalmers University of Technology. The project is carried out at Chalmers: Department of Shipping and Marine Technology, in cooperation with DTU Department of Mechanical Engineering and Rolls-Royce AB, Kristinehamn. This thesis consist of a significant amount of coloured figures, it is therefore recom- mended to be read in a coloured version. Acknowledgements Supervisors Rickard Bensow, Chalmers Shipping and Marine Technology For supervising within hydrodynamics and thesis structure. Poul Andersen, DTU Mechanical Engineering For supervising within hydrodynamics and thesis structure. Reima Aartojärvi, Rolls-Royce AB Kristinehamn For supervising within waterjet pump design and hydrodynamics. Others Urban Svennberg, Rolls-Royce AB Kristinehamn For great help in setting up and understanding the required CFD analyses. Fredrik Falkman, The Swedish Sea Rescue Society For providing an interesting project and information about the operation of the rescue boat. Thor Peter Andersen, Gothenburg 2014/05/28 This page is intentionally left blank. Contents 1 Introduction 1 1.1 Background . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 1.2 Objective . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 1.2.1 Technical Specifications . . . . . . . . . . . . . . . . . . . . . . . . 3 1.3 Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 1.4 Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 1.5 Changes form a Regular to a Rim Driven Waterjet Pump. . . . . . . . . . 6 1.6 Outline of the Thesis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 2 The Rescue Boat 9 2.1 Thrust Prediction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 3 The Waterjet Propulsion System 13 3.1 Processes of The Waterjet System . . . . . . . . . . . . . . . . . . . . . . 13 3.2 Thrust . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 3.3 The Pump . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 3.3.1 The Pump Configuration Cases . . . . . . . . . . . . . . . . . . . . 16 4 The Design Process 17 5 Design Tools and Methods 21 5.1 TurboDesign1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 5.1.1 Potential Flow Theory . . . . . . . . . . . . . . . . . . . . . . . . . 21 5.1.2 Design Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 5.2 Computational Fluid Dynamics Analysis . . . . . . . . . . . . . . . . . . . 23 5.2.1 Steady State Analysis . . . . . . . . . . . . . . . . . . . . . . . . . 23 5.2.2 Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 23 5.2.3 SST k − ω Turbulent Flow Model . . . . . . . . . . . . . . . . . . 24 5.2.4 Mixture Flow Model . . . . . . . . . . . . . . . . . . . . . . . . . . 24 5.2.5 Schemes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24 i CONTENTS 5.2.6 Solver Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25 5.2.7 The Computational Mesh . . . . . . . . . . . . . . . . . . . . . . . 25 5.2.8 y-plus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25 5.2.9 Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25 5.2.10 The CFD Code - Ansys Fluent . . . . . . . . . . . . . . . . . . . . 26 5.2.11 Postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 6 Energy Model 27 6.1 Assumptions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27 6.2 The Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28 6.2.1 The Head Losses . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30 6.3 Key Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33 6.3.1 Maximum Efficiency Prediction . . . . . . . . . . . . . . . . . . . . 35 6.3.2 Engine Load . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 6.4 Discussion of Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 7 Steady Flow CFD Pump Model 37 7.1 The Computational Grid . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38 7.1.1 Simplified Grid Dependency Study . . . . . . . . . . . . . . . . . . 38 7.2 Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 7.3 Calculation Settings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 7.4 Discussion of the Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 8 Transient Flow CFD Pump Model 43 8.1 The Computational Grid . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 8.2 Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 8.3 Calculation Settings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 8.4 Multiphase Flow Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 8.4.1 Settings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 8.5 Discussion of the Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 9 Blade and Pump Design 49 9.1 Constant Design Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . 49 9.1.1 The Meridional Channel Shape . . . . . . . . . . . . . . . . . . . . 49 9.1.2 The Thickness Distribution . . . . . . . . . . . . . . . . . . . . . . 50 9.1.3 Fluid Properties and Design Specifications . . . . . . . . . . . . . . 51 9.1.4 Number of Blades . . . . . . . . . . . . . . . . . . . . . . . . . . . 53 9.2 Non-Constant Design Parameters . . . . . . . . . . . . . . . . . . . . . . . 53 9.2.1 Vorticity Distribution . . . . . . . . . . . . . . . . . . . . . . . . . 53 9.2.2 Blade Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54 9.2.3 Stacking Condition . . . . . . . . . . . . . . . . . . . . . . . . . . . 56 9.3 Leading and Trailing Edge Modification . . . . . . . . . . . . . . . . . . . 56 9.4 The Final Pump Concept . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 ii CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CONTENTS 10 Performance of the Final Pump Concept 59 10.1 Convergence Study . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 10.2 Performance Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 10.2.1 The Efficiency Definition . . . . . . . . . . . . . . . . . . . . . . . 62 10.2.2 Steady Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 10.2.3 Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 73 10.2.4 Cavitation Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 78 10.3 Discussion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81 10.4 Rope in Pump Discussion . . . . . . . . . . . . . . . . . . . . . . . . . . . 82 11 Conclusion 85 11.1 Future Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86 Bibliography 90 A Savitsky’s Thrust Prediction Method 91 B Mathematical Model Matlab Script 95 C Meshing Settings 103 D CFD Convergence Study 107 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 iii CONTENTS This page is intentionally left blank. iv CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 List of Figures 1 Illustration with key pump expressions. . . . . . . . . . . . . . . . . . . . xiii 2 Illustration with key blade expressions. . . . . . . . . . . . . . . . . . . . . xiii 1.1 The figure contains a picture of the issue with rope entanglement (figure 1.1a) and a picture of a rim driven hubless thruster (1.1b). . . . . . . . . . 2 1.2 Comparison of regular waterjet (figure 1.2a ) and the Rim-Jet (figure 1.2b). 6 2.1 The initial boat design. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 2.2 The thrust curve produced by the Savitsky prediction method and the same curve corrected with a 20% seamargin. . . . . . . . . . . . . . . . . 11 2.3 Trim curve produced by the Savitsky prediction method. . . . . . . . . . 11 3.1 Waterjet principle model: Point 0. Free stream, Point 1. Stream tube inlet, Point 2. Duct inlet, Point 3. Pump inlet, Point 4. Pump center Point 5. Pump outlet, Point 6. Nozzle outlet and Point 7. Jet minimum diameter. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13 3.2 Comparison of regular waterjet (figure 1.2a) and the Rim-Jet (figure 1.2b). 15 3.3 Sketches of the three pump cases. . . . . . . . . . . . . . . . . . . . . . . . 16 4.1 Illustration of the iterative design process. . . . . . . . . . . . . . . . . . 17 5.1 Meridional plot of the channel shape. The hub is included as it is a requirement for the input to TD1. . . . . . . . . . . . . . . . . . . . . . . 22 6.1 Waterjet principle model: Point 0. Free stream, Point 1. Stream tube inlet, Point 2. Duct inlet, Point 3. Pump inlet, Point 4. Pump center Point 5. Pump outlet, Point 6. Nozzle outlet and Point 7. Jet minimum diameter. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27 6.2 Plot of the inlet loss factor polynomial. . . . . . . . . . . . . . . . . . . . . 32 6.3 Plot specifying the head rise required to produce the necessary thrust. . 34 6.4 Plot of performance prediction for pumps of varying type. Source: [Bren- nen, 1994, p32, figure 2.8]. . . . . . . . . . . . . . . . . . . . . . . . . . . 35 v LIST OF FIGURES 7.1 Steady flow simulation set-up. Blue: Stationary walls. Green: Rotating impeller blade and shroud. Yellow: Free flow pipe. . . . . . . . . . . . . . 37 7.2 example of computational domains. . . . . . . . . . . . . . . . . . . . . . 38 7.3 Example of computational mesh. . . . . . . . . . . . . . . . . . . . . . . . 39 8.1 Unsteady flow analysis set-up. . . . . . . . . . . . . . . . . . . . . . . . . . 43 8.2 The figure visualises the mesh used for the transient analysis of the un- steady flow through the pump. . . . . . . . . . . . . . . . . . . . . . . . . 44 9.1 Meridional plot of the channel shape. The hub is included as it is a requirement for the input to TD1. . . . . . . . . . . . . . . . . . . . . . . 50 9.2 Plot of the thickness distribution in three spanwise positions. The leading and trailing edge is modified at a later stage. . . . . . . . . . . . . . . . . 51 9.3 The contour figure showing the axial velocity field entering the guide inlet. The orange blade is a guide vane and the grey is the nozzle wall. The direction of the look into the pump is upstream. . . . . . . . . . . . . . . 52 9.4 Vorticity distribution for the impeller and guide vane blade. . . . . . . . . 54 9.5 Plot of the resulting blade loading for the impeller blade. . . . . . . . . . 55 9.6 Plot of the resulting blade loading for the guide vane. . . . . . . . . . . . 55 9.7 Figure explaining the use of the edge defining ratio. source: [TD1, 2012b] 56 9.8 The impeller blade and guide vane blade with modified leading and trail- ing edges are shown free and in connection with the final pump Case 1. configuration. The rotation of the impeller follows the right hand rule around the z-axis (blue arrow in the right hand corner of figure 9.8c). . . 57 10.1 Plot of convergence study of Case 1. It is evident from the figure that the torque of the system is constant though with small fluctuations. Please note that this figure is based solely on the last 200 iterations displayed. . 60 10.2 Computational history for the bollard pull condition. . . . . . . . . . . . . 61 10.3 The three pump configurations are displayed in 3D. The rotation is follow- ing the right hand rule for the flow direction (towards the nozzle). Note that the impeller is upstream of the guide vanes. . . . . . . . . . . . . . . 62 10.4 Plot of the produced head rise and axial efficiency at given flow rates for the case 1 pump configuration. . . . . . . . . . . . . . . . . . . . . . . . . 65 10.5 Figure 10.5a displays head rise produced and required. Figure 10.5b dis- play the torque requirements and the maximum limit . . . . . . . . . . . . 67 10.6 Picture of Case 3. pump configuration with the pressure distribution as contours. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67 10.7 Figure 10.7a displays total impeller efficiency of the impeller for Case 1. and 3. Figure 10.7b displays axial impeller efficiency of the impeller for Case 1. and 3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68 10.8 Case 1. pressure at the pump inlet (point 3 figure 3.1). The pressure is given relative to atmospheric pressure, here the vapour pressure is −99 kPa. 70 vi CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 LIST OF FIGURES 10.9 Figure 10.9a and 10.9b displays the results of the CFD evaluation of the pump (Case 1.) operating at the two points of equilibrium. . . . . . . . . 70 10.10The pressure distribution of the Case 1. pump configuration at the two points of head rise equilibrium. . . . . . . . . . . . . . . . . . . . . . . . . 71 10.11Plot of the produced head rise and axial efficiency at given flow rates for the transient analysis of Case 1. . . . . . . . . . . . . . . . . . . . . . . . . 73 10.12The fluctuating pressure in the pump is apparent, especially at the guide vane. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 74 10.13Figure 10.13a displays the head rise production. Figure 10.13b displays torque requirements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 10.14Figure 10.14a displays the total impeller efficiency. Figure 10.14b displays axial efficiency. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 76 10.15The backflow observed in the operational points of low flow rate is visualized. 77 10.16The fluctuating pressure in the pump is visual, especially at the guide vane. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79 10.17The fluctuating pressure in the pump is visual, especially at the guide vane. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80 10.18Figure of the flow through the pump at the bollard pull condition with steamlines visualizing the flow through the pump. Note the swirl in the centerline. The figure is based on the transient cavitation analysis. . . . . 82 C.1 Grid settings for the general mesh sizing. . . . . . . . . . . . . . . . . . . 104 C.2 Grid settings for the inflation layer. . . . . . . . . . . . . . . . . . . . . . . 105 C.3 Grid settings for the face sizing on the blade. . . . . . . . . . . . . . . . . 105 D.1 Plot of convergence study of Case 1. It is clear from the figure that the torque of the system is constant with minor fluctuations. . . . . . . . . . . 108 D.2 Plot of convergence study of Case 2. It is clear from the figure that the torque of the system is constant with minor fluctuations. . . . . . . . . . . 108 D.3 Plot of convergence study of Case 3. It is clear from the figure that the torque of the system is constant with minor fluctuations. . . . . . . . . . . 109 D.4 Plot of convergence study of Case 1. transient analysis. The x-axis dis- plays the time steps the study is based on. The actual number of time steps is displayed in table D.2 . . . . . . . . . . . . . . . . . . . . . . . . . 109 D.5 Plot of convergence study of Case 1. transient cavitation analysis. Note that the Qe = 1.09 condition is not converged fully. . . . . . . . . . . . . . 110 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 vii LIST OF FIGURES This page is intentionally left blank. viii CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 List of Abreviations TD1 TurboDesign1 CFD Computational Fluid Dynamics SSRS Swedish Sea Rescue Society LOA Length over all BP Planning breath LCG Longitudinal center of gravity LCB Longitudinal center of buoyancy SOLAS Safety of Life at Sea ix This page is intentionally left blank. Notations Greek letters ξ Inlet loss factor ρ Density of fresh water at 20◦ µ Viscosity of fresh water at 20◦ ν Kinematic viscosity of fresh water at 20◦ τ Torque η Efficiency λ Stream tube and duct velocity ratio β Dead rise angle Roman letters P Pressure V Average velocity in axial direction H Head rise h Head loss g The gravitational constant T Thrust ṁ Mass flow rate Q̇ Volume flow rate Q̇e Normalised volume flow rate W Work Ė Energy flow rate n Revolutions per minute d Diameter L Length R Radius xi This page is intentionally left blank. Key Pump Expressions Here the key expressions related to the pump and blade design are presented with visu- alisation in figure 1 and 2. Figure 1: Illustration with key pump expressions. Figure 2: Illustration with key blade expressions. xiii This page is intentionally left blank. 1 Introduction Rescue boats and other vessels operating near ships or marine structures in distress are vulnerable to floating debris. Such debris can get stuck in the propulsion system and cause vessel downtime. Floating lines, e.g. buoyant lines connected to life rafts, are especially problematic in conjunction with waterjets. After a few revolutions, a tangled polyester line will melt around the shaft and course a breakdown of the engine (see figure 1.1a). The engine can be damaged and the removal of melted or entangled lines can take several hours. Hours which are crucial in a rescue operation. The Swedish Sea Rescue Society has initiated the development of a new type of waterjet propulsion system in cooperation with Rolls-Royce. The goal is to minimize problems with debris and floating lines. The new propulsion system has been named a Rim-Jet. The Rim-Jet improves the operational ability of the small rescue craft as its vulnerability to floating debris is reduced. A decrease of the efficiency of the rim driven pump compared to a regular pump is expected, this is, however, an acceptable cost of reducing the downtime of the vessel. The increased ability to perform rescue operations in waters with floating debris improves the sustainability of the rescue operation. 1.1 Background The Rim-Jet is inspired by the relatively newly commercialised rim driven thrusters (see figure 1.1b for an example.) which have shown great capabilities in handling debris in water. These thrusters are, however, neither capable of delivering the speed required of a rescue vessel, nor the safety of an enclosed propulsion system. No commercial rim driven waterjet systems has, to the author’s knowledge, been developed and research within the topic is very limited. Rolls-Royce has started the development with two separate master’s theses. One thesis dealing with the mechanical design aspects of the system and one dealing with the hydromechanics of the rim driven waterjet pump as a main focus. This project is focused on the hydromechanics design and performance of the rim driven axial pump which powers the waterjet propulsion system. 1 CHAPTER 1. INTRODUCTION (a) Entangled shaft. Pic- ture courtesy of Fredrik Falkman (The Swedish Sea Rescue Society). (b) Rim driven hubless thruster by Brunvoll (see [unknown, 2014]). Figure 1.1: The figure contains a picture of the issue with rope entanglement (figure 1.1a) and a picture of a rim driven hubless thruster (1.1b). 1.2 Objective The objective of the thesis is to develop and analyse the performance of a rim driven hubless axial pump with the capabilities of delivering the power required of the waterjet propulsion system to achieve the design speed and bollard pull. The design focus is mainly the hydrodynamic performance of the system and secondly on handling ropes in the pump. One impeller and guide vane blade design is developed and studied using three sep- arate pump cases. • Case 1. A hubless rim driven pump with guide vanes. • Case 2. A hubless rim driven pump with no guide vanes. • Case 3. A rim driven pump with guide vanes and a hub. Case 1. and 3. are used to study the effect of removing the hub and driving the pump at the rim. The purpose of Case 2. is to study the effect of removing the guide vane from Case 1. pump, Case 2. is expected to deliver the lowest pump efficiency, but the best handling of ropes in the pump. The impeller and guide vane blades are developed using an iterative process based on results from computational fluid dynamics (CFD from here on out) analysis of the Case 1. pump configuration. The final concept design must meet the following technical specifications of the system (see table 1.2.1). Ultimately a final concept design is to be recommended for further development. 2 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 1. INTRODUCTION 1.2.1 Technical Specifications The Swedish Sea Rescue Society (SSRS from here on out) has defined some main tech- nical requirements for the Rim-Jet. These requirements are summarised in table 1.1. Table 1.1: The technical specifications the client. Requirement Value Unit Vessel speed, Vs 20 - 25 knots 10.3 -12.9 m/s Maximum engine speed, n 4000 rpm Maximum engine torque 132 Nm Delivered power @ max rpm 55 kW Maximum impeller diameter 195 mm Bullard pull(Thrust), T 4 kN The propulsion system is designed for a vessel of four meters. The substantial bollard pull required of the vessel originates from the operational pattern of the boat. The rescue boat must have enough thrust to pull several connected liferafts. A more detailed system specification is necessary in order to perform the design work. Detailed specifications were created in cooperation with the mechanical designer. The relevant specifications are found in table 1.2. Some of these values are specified by the dimensional limitations of the engine and some are chosen based on ratios from previous waterjet designs in order to simplify the design process. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 3 CHAPTER 1. INTRODUCTION Table 1.2: The detailed technical specifications. NOTE: Values given in brackets () are required by SOLAS, the boat is, however, not going to be operated in these conditions. Pump specifications Impeller diameter 195 [mm] Impeller and guide vane axial length 100 [mm] The ”hub” diameter 60 [mm] Outlet/inlet diameter ratio 60-80 [%] Number of impeller blades 4 [-] Number of stator blades 7 [-] Elevation of nozzle outlet, 164.25 [mm] Fluid Properties [ITTC, 2011] Fluid Water Temperature 20 [◦C] Density (ρ) 998 [kg/m3] Vapour pressure 2.3 [kPa] Design Target Bollard pull 4 [kN] Impeller rotational speed 2000 - 4000 [rpm] Torque delivered 132 [Nm] Design speed 20(6) [knots] Displacement 800(1250) [kg] 1.3 Method Basic fluid dynamics is used to develop a energy model of the waterjet system. The model is used to calculated the requirements of the pump based in the inputs given by SSRS and estimations from previous waterjet designs. The pump design software, TurboDesign1 (known as TD1 form here on out), is used for the 3D modelling of the impeller and the guide vane blades. This software uses potential flow theory and an inverse 3D design procedure which simplifies the designing of impeller and guide vane blades creating the desired flow. The initial design is based on estimates of the head rise, flow rate and blade loading distribution needed to deliver the necessary thrust. The design is then improved using an iterative process with design changes based on viscus CFD evaluations of the performance of the pump. The software used for the CFD evaluation is Ansys Fluent 14.5. A steady flow analysis is conducted for the initial design and a transient flow analysis is conducted 4 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 1. INTRODUCTION on the final concept design to give a higher accuracy of the pump performance evaluation, a simple multiphase analysis is furthermore conducted in order to estimate the cavitation performance in bollard pull. The evaluation of rope in pump performance is based on a simple study of the flow through the pump. The interaction between the blades and a rope is not easy to simulate with any tools readily available, and a literature study showed that no studies have been published on the topic, to the author’s knowledge. 1.4 Limitations The impeller diameter is defined by the geometry of the electromagnetic engine, this limits the design freedom significantly. TD1 is not designed to create hubless blades, the pump is therefore designed with a cylindrical hub which is then removed in the CFD evaluation. This procedure has been used in other research projects, according to Turbo Design support, and it is therefore assumed to be a valid method for a rapid geometry definition. There are, to the author’s knowledge, no programs capable of generating hubless pump blades. This fact, combined with Rolls-Royce significant experience in using TD1, is why the blade design is carried out using TD1. This is potentially limiting the achievable efficiency of the rim driven hubless pump, as the design tool is not created for this particularly use. Due to the limited time frame of the project, only an initial CFD analysis is pos- sible and there is no time to experimentally validate the specific CFD set-up. The consequences of this is that the models used are considered valid based on experience from Rolls-Royce and previous pump studies. An experimental pump test should be conducted in order to validate the CFD method for this specific pump type. The study of rope in pump is, as mention in the previous section, not something that has been done before. There is, therefore, a limitation to conclusion of this study regarding rope in pump. The most effective way to test the rope in pump capabilities of the final design would be an experimental set-up, this is however not possible within the time frame of the thesis. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 5 CHAPTER 1. INTRODUCTION 1.5 Changes form a Regular to a Rim Driven Waterjet Pump. From a mechanical point of view the main difference between a regular and a rim driven pump is the absorption of the thrust (produced axial force). Usually, it is absorbed through the shaft. In this case it will have to be absorbed by a bearing solution in the rim. A comparison between a regular waterjet system and the Rim-Jet is seen in figure 1.2 for clarification. The driving engine is electric and mounted around the pump itself. An electric engine has a constant torque-rpm curve, this results in greater freedom when choosing the rpm at which the pump operates. (a) Axial waterjet pump by [Thad et al., 2008]. (b) Rim driven waterjet pump. Figure 1.2: Comparison of regular waterjet (figure 1.2a ) and the Rim-Jet (figure 1.2b). The largest impact of the hydrodynamic design is the removal of the shaft and hub. The removal of the shaft reduces the disturbances in the wake field entering the pump, leaving this mainly dependent on the inlet design. A less disturbed wake field will in general make it possible to have a more efficient pump and while maintaining good cavitation properties. The amount of fluctuating forces on the impeller blades are also lowered when the wake field is more homogeneous. The missing hub is expected to cause problems. In a regular waterjet pump the gab between the shroud of the blade and the pump wall courses pressure leaks. This is reduced using a number of methods, one being a cavitation layer filling the gab. Driving the blade at the shroud and removing the hub leave a gab in the center of the pump allowing for pressure leaks to occur. The blades are designed with low loading towards the center to minimize these pressure leaks. Having this large gab in the center is likely to result in an overall reduced efficiency compared to a regular pump or a rim driven pump with a hub, it is however this gab that allows the pump to avoid entangling in ropes. A significant design difference between the blade design of a regular and a hubless pump is the ability to manipulate the axial flow velocity through the pump. This is usually done by increasing the hub diameter over the length of the impeller. The rim 6 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 1. INTRODUCTION driven pump has a constant average axial flow velocity through the impeller, the flow is therefore only accelerated in the nozzle. An electrical rim driven waterjet pump has a number of desirable differences com- pared to a regular waterjet when it comes to the design of the boat. The engine and generator can be placed anywhere without having to consider the shaft. This gives a greater flexibility in the propulsion system. The boat in question is, however, a small rescue craft, the flexibility is therefore limited. The initial boat design is presented in chapter 2. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 7 CHAPTER 1. INTRODUCTION 1.6 Outline of the Thesis The thesis consists of 11 chapters and appendices. A brief description of the content of the thesis is presented below. Chapter 1 introduces the background of the project and defines the objective of the thesis. Chapter 2 presents the rescue boat in question and the results of a trust prediction. Chapter 3 describes the processes in a waterjet system and discusses pumps used for waterjet propulsion. Chapter 4 presents the design process used for the development of the rim driven hubless waterjet pump. Chapter 5 presents the tools and methods used in the design process, it includes references to the theory behind these methods. Chapter 6 describes the energy model used to calculate certain design input pa- rameters and benchmarking results for the evaluation of the performance of the concept design. Chapter 7 introduces the steady state CFD model used for initial performance estimations and the comparison of the pump configurations. Chapter 8 introduces the transient CFD model used for the final performance evaluation. Chapter 9 presents the result of design process. The final pump concept is pre- sented as wells as the major design changes throughout the design process are briefly discussed. Chapter 10 presents the results of the CFD models introduced in Chapter 7 and 8. The performance of the final concept design is presented and discussed. A brief cavitation analysis is conducted in order to estimate the cavitation properties of the pump, and a flow analysis is conducted to evaluate the rope in pump performance of the pump. Chapter 11 is the concluding chapter in which the main results of the thesis are summarised and the conclusions on the projects objectives are drawn. Future work suggestions are presented in a separate section. The appendices presents the Matlab programs created for the thrust prediction and the energy model. The result of the convergence study and the settings for meshing are also presented. The result files are available upon request. 8 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 2 The Rescue Boat The boat design is ongoing, however, SSRS has provided a sketch of the craft (see figure 2.1). The main dimensions of the boat are formulated based on these drawings, interaction with the SSRS and estimations, see table 2.1. These dimensions are used to create a thrust prediction for the boat. Figure 2.1: The initial boat design. The weight and design speed in table 2.1 reflect both the transit condition with one pax on board (800kg) and with six pax on board (1250kg).The condition with six pax onboard is a requirement from the SOLAS regulations (requirement provided by SSRS), the boat is not meant to transport six pax. The condition prescribed by the SOLAS regulations are not specifically investigated in this thesis. 9 CHAPTER 2. THE RESCUE BOAT Table 2.1: Main particulars of boat Main particulars Value Unit Length, LOA 4 m Planing breath, BP 0.97 m Draught, T 0.54 m Total weight 800(1250) kg Longitudinal center of gravity, LCG 1.675 m Longitudinal center of buoyancy, LCB 1.69 m Vertical center of gravity, VCG 0.4 m Angle of deadrise, β 15 ◦ - SOLAS pax capacity 6 - Design speed 20(6) knots 2.1 Thrust Prediction Savitsky’s method of thrust prediction is used to predict the thrust needed from the water jet propulsion system [Savitsky, 1964]. This Savitsky’s prediction method provides a good estimate for planing vessels, such as the rescue boat in question, at an early design stage. The interested reader is referred to Savitsky’s article ”Hydrodynamic design of plan- ing hulls”, see [Savitsky, 1964], and the matlab script used for the prediction in appendix A. The thrust prediction model created in connection with this thesis is in compliance with results from Orca3D provided by SSRS (Orca3D also uses the Savitsky’s prediction method.). In short Savitsky’s prediction method is a 30 step thrust prediction method based on a large number of test data. The method predicts the required thrust for a certain speed, the trim angle and if the planing vessel is stable at that specific speed. The method is widely used to get an initial thrust prediction for small planing crafts with a constant dead rise angle (which is the case for the vessel in question). There are, to the author’s knowledge, no better methods suited for a craft of this size, before the hull is designed and a resistance test is conducted. (Note that it is a thrust prediction method, not a resistance prediction method, as it takes the angle of the propulsion system into account. This angle results in the need for a larger thrust than the total resistance in certain cases.) The thrust prediction curve is shown in figure 2.2. Here the so called resistance bump is seen with its peak around 14 knots. The boat starts planing when the resistance bump is passed, and as the wetted area of the vessel is reduced so is the resistance. A 20% seamargin is added to the thrust prediction to ensure the boat’s ability to operate in smaller waves which causes added resistance on the hull. Larger waves causes a very 10 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 2. THE RESCUE BOAT unstable speed for such a small vessel and a specific max speed is difficult to reach even with extra power. 5 10 15 20 25 30 900 1000 1100 1200 1300 1400 1500 1600 1700 Vessel Speed [knots] R eq u ir ed T h ru st [N ] incl. 20% sea margin Figure 2.2: The thrust curve produced by the Savitsky prediction method and the same curve corrected with a 20% seamargin. In figure 2.3 the trim curve is shown, it is seen that once the vessel start planing it moves towards neutral trim when the speed is increased (often ending at a certain design trim). It is also observed that the aft of the vessel is experiencing a suction at lower speeds, this creates the very steep resistance rise in the hump as it is not only the increased speed, but also the increased wetted surface which result in increased friction on the hull. 5 10 15 20 25 30 3.5 4 4.5 5 5.5 6 6.5 7 7.5 8 8.5 Vessel Speed [knots] T ri m A n g le [◦ ] Figure 2.3: Trim curve produced by the Savitsky prediction method. The thrust predicted with added seamargin is used as input for the mathematical model of the waterjet system. The thrust requirement is used to estimate the velocity of the jet leaving the nozzle and thereby the flow rate through the propulsion system. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 11 CHAPTER 2. THE RESCUE BOAT This, in combination with the pressure loss, is governing the head rise needed from the pump and is therefore essential for the design of the waterjet propulsion system. 12 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 3 The Waterjet Propulsion System In this chapter the general function of a waterjet propulsion system is described briefly. A simple sketch, following the ITTC standard (see [ITTC, 2005]) of a waterjet propulsion system is shown in Figure 3.1 7. 6. 5. 0 Figure 3.1: Waterjet principle model: Point 0. Free stream, Point 1. Stream tube inlet, Point 2. Duct inlet, Point 3. Pump inlet, Point 4. Pump center Point 5. Pump outlet, Point 6. Nozzle outlet and Point 7. Jet minimum diameter. 3.1 Processes of The Waterjet System The processes throughout the system is presented in relation to the seven points shown in figure 3.1. 0. The free stream. The water flows free with a speed matching the speed of the boat through water. 1. The stream tube inlet. This is the part of the flow beneath the hull which enters the waterjet system. Here the average velocity is smaller than at point 0 due to the boundary layer built up on the keel. The cross section area is usually modelled as a rectangle with 1.35 times the width of the duct pipe diameter (Rolls-Royce standard) and a height determined by the mass flow rate through the waterjet. 13 CHAPTER 3. THE WATERJET PROPULSION SYSTEM 2. The duct inlet. Here the water enters the physical propulsion system. A grid is installed in the inlet to avoid larger debris entering the system. The inlet geometry and the grid results in a significant pressure loss. This loss is dependent on the ratio between the average axial flow velocity in the duct (point 3.) and in the stream tube (point 1.). 3. The pump inlet. The wake field entering the pump is defined at this point. The pressure can be both higher and lower than the pressure at point 1. depending on the operation of the vessel. The pressure at this point is dependent on the mass flow rate rate of the system, the vessel speed and the pressure loss experienced in the duct inlet. 4. The pump center. Here, right after the rotor, the static pressure is at its max- imum. The flow is highly rotational, but with the same average axial velocity as at point 3. 5. The pump outlet. The guide vanes are mounted in the nozzle and are running from point 4. to 6. transforming static pressure into a dynamic pressure as the water is accelerating through the nozzle. The guide vanes reduce the head rise required to produce a specific thrust by recovering some the the energy bound in the swirl. 6. The nozzle outlet. Here the accelerated jet leaves the physical propulsion system. 7. Jet maximum Vena contraction. The jet continues to contract after leaving the nozzle (at point 6.) due to the Vena contraction phenomena, see [ITTC, 2005]. This is the point at which the diameter of the waterjet is at its minimum, the point is considered the end point of the propulsion system. At this point the maximum average velocity of the jet is reached and the thrust of the system is determined. The contraction between point 6. and point 7. is, however, often insignificant. 3.2 Thrust Thrust is an expression used to define the force a waterjet system produces on a vessel. Thrust is defined as a the forward acting force produced by propelling water backwards. The system follows Newton’s third law by exceeding a force on the water in the jet which then exerts a force on the blades which is then transferred to the boat, propelling it forward. The thrust equation is defined in [Allison, 1993, Chap. 16.] and shown in equation 3.1. T = ṁ(V7 − V1) (3.1) Where V represents the average axial velocity at points defined by the subscripted numbers, see figure 3.1, ṁ is the mass flow and T is the produced thrust. As the steamtube velocity (V1) is dependent on the vessel’s velocity through water (V0) it is 14 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 3. THE WATERJET PROPULSION SYSTEM apparent that the thrust is reduced when increasing the vessel speed (V0), if the jet velocity (V7) is kept constant. Bollard pull is the definition of the thrust produced at zero speed and represents the maximum pulling force a propulsion system can produce at a specific rotational speed and torque. 3.3 The Pump The pump is the heart of the waterjet propulsion system. This is where the energy is transferred from the engine to the water via the impeller blades. Most waterjet pumps consist of two stages; the impeller and the nozzle stage in which the guide vanes are integrated parts of the nozzle, see figure 3.2 for reference (Note that the colours of the impeller and guide vane blades are reversed in figure 3.2). (a) Axial waterjet pump by [Thad et al., 2008] with labeling. Impeller: Orange. Guide vane: Green (b) Rim driven waterjet pump with label- ing. Impeller: Green. Guide vane: Orange Figure 3.2: Comparison of regular waterjet (figure 1.2a) and the Rim-Jet (figure 1.2b). The rotating impeller adds energy to the fluid, creating a pressure rise and sustaining the flow rate of the system by counter acting the pressure loss throughout the system. The static pressure is high after the impeller due to a high degree of swirl in the flow introduced by the rotating impeller. The water is accelerated through the nozzle stage transforming the high static pressure to dynamic pressure (kinetic energy). The trans- formation from static to dynamic pressure is achieved by narrowing the channel (the nozzle) and streamlining the flow in the axial direction via the guide vanes. The guide vanes introduces extra friction in the pump, but the steamlining of the flow reduces the the required head rise, by converging swirl to axial flow, to such a degree that the overall axial pump efficiency is increased. Energy bound in the swirl after the nozzle is lost energy as it does not contribute to the propulsion of the vessel. The interested reader is referred to [Brennen, 1994] for an in depth presentation of the theoretical function of a pump. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 15 CHAPTER 3. THE WATERJET PROPULSION SYSTEM The two main types of pumps, used for waterjets propulsion systems, are the mixed- flow and the axial flow pump. A mixed flow pump relies on increased average axial velocity of the flow over the impeller blades, this, however, is not possible when the hub is removed, the Rim-Jet is therefore based on an axial flow pump. An axial pump can be designed with a constant average axial flow velocity, but a velocity increase over the pump, induced by the hub shape, is used to achieve a high impeller efficiency. An example of a axial flow pump is seen in figure 3.2a. An axial flow pump is usually used for high flow rates and small head rises, making it ideal for high speed with lower thrust and less than ideal for bollard pull production. 3.3.1 The Pump Configuration Cases The cross section of the three pump configuration cases considered are sketched in figure 3.3. This displays the projected cross section area of an impeller blade and a guide vane. Note that the Case 2. configuration is shorter than Case 1. and 3. as there is no guide vanes the nozzle is shortened. 0 50 100 150 200 250 300 350 400 450 −20 0 20 40 60 80 100 120 Impeller Guide Shroud Axis of Symmetry Case 1 z-axis r- a x is (a) Case 1 2D sketch. 0 50 100 150 200 250 300 350 400 −20 0 20 40 60 80 100 120 Impeller Shroud Axis of Symmetry Case 2 z-axis r- a x is (b) Case 2 2D sketch. 0 50 100 150 200 250 300 350 400 450 −20 0 20 40 60 80 100 120 Impeller Guide Shroud Axis of Symmetry Hub Case 3 z-axis r- a x is (c) Case 3 2D sketch. Figure 3.3: Sketches of the three pump cases. 16 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 4 The Design Process The design process is an iterative process consisting of a number of sub-processes, see figure 4.1 for a visualisation of the design process. The design process is based on the Rolls-Royce standard process with inspirations from design studies such as [Bonaiuti et al., 2010]. The pump design has a large number of variables and few limiting factors as it is a completely new design. Figure 4.1: Illustration of the iterative design process. 17 CHAPTER 4. THE DESIGN PROCESS The processes shown in figure 4.1 are briefly described in the below list. - Thrust Requirement The pump design is based on an estimation of the required thrust of the vessel. This estimation would usually be based on a towing tank test. In this case the final hull is yet to be designed, and the thrust is therefore estimated based on the main particulars using the Savitsky’s prediction method, see section 2. - Pump Dimensions The pump diameter is limited by the rim engine. The length of the pump, the impeller blades and the guide vanes are chosen based on ratios from previous waterjet designs. - Pump Specifications The operational revolutionary speed and the number of impeller and guide vane blades are selected. The number of blades are kept low in order to reduce the complexity of the pump and reduce the chances of debris getting stuck. - Mathematical Model The flow rate and the required torque are estimated based on the thrust prediction and the nozzle outlet diameter. The outlet diameter of the nozzle is corrected so that the minimum torque is well within the engine specification. The average impeller blade loading is estimated using a simple empirical method from the TD1 application manual [TD1, 2012a]. - Blade Design The impeller and guide vane blades are designed using TD1, inputs from the above mentioned processes and studies of high performing designs from the literature, such as [Thad et al., 2008] and [Bonaiuti et al., 2010]. - Steady State CFD Analysis The CFD pump performance analysis consists of a number of analyses. The per- formance of the initial designs are estimated based on a steady flow analysis in order to reduce the computation cost. - Evaluation of The CFD Analysis The results of the CFD analysis are evaluated. If the pump performance is accept- able a concept design has been reached. If the pump performance is unacceptable the design process starts over. In such a case it must be considered whether an acceptable performance can be reached by mainly changing the blade loading or if other design parameters, such as the rotational speed of the impeller and the nozzle outlet diameter, need to be changed as well. At a certain point it must be considered if the performance goal is reachable within the design limitations or if these must be reconsidered. 18 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 4. THE DESIGN PROCESS - Final Concept Design Once a final concept design is reached a transient analysis is conducted to evaluate the overall performance of the pump, including the expected pump efficiency and an estimation of the cavitation properties, using a multiphase model added to the transient analysis. The next stages of the pump design are working towards the final production design. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 19 CHAPTER 4. THE DESIGN PROCESS This page is intentionally left blank. 20 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 5 Design Tools and Methods In this chapter the tools and methods, used for the pump design, are introduced. These are TurboDesign1, using potential flow theory for the design of the blades, and a viscus CFD code is used for the performance analysis of the pump design. 5.1 TurboDesign1 TurboDesign is a design tool package for designing of turbo machinery. The tool used in this case is TurboDesign1. TD1 is designed to create a 3D blade geometry based on a number of input parameters. TD1 uses an inverse 3D design method to rapidly create blade geometries, this method was developed by M. Zangeneh [Zangeneh, 1991]. This is achieved by designing the blade based on a specific in and output velocity field. The impeller and guide vane blades are designed independently, but the guide vane blade uses the output velocity field from the impeller as the base of its input velocity field. The TD1 design process starts with an initial blade shape presented by a vorticity field from which the outlet velocity field of the pump is calculated. Potential flow theory is used to calculate the flow, this enables a fast computation time as the flow is assumed inviscid, which reduces the complexity of turbulence flow simulation. The output velocity field is compared to the wanted velocity field. A new blade profile is created and the vorticity is calculated, a new output velocity field is calculated from the vorticity field, and the iterative process continues until the blade matches the specified output velocity field. The blade design is created including a hub as the software cannot design a hubless blade. The hub is then excluded in the viscus CFD performance evaluation. The ex- cluded hub is, however, considered when designing the blades by unloading the blades towards the center of the pump. 5.1.1 Potential Flow Theory In potential flow theory the flow around a body is assumed inviscid, and mass and momentum are assumed constant. Potential flow theory is used based on the assumption that viscosity primarily has an important impact on a flow in the boundary layers on walls. Potential flow theory is described in detail in many textbooks, see for example White [1974]. Potential flow theory works well for rapid flow analysis, but the system is without damping and losses caused by friction. This makes it an ideal system, a viscus analysis is needed to evaluate the actual performance of the system. 21 CHAPTER 5. DESIGN TOOLS AND METHODS 5.1.2 Design Parameters An example of a pump designed using TD1 and CFD analyses is presented in [Bonaiuti et al., 2010]. The design parameters used by TD1 are seen below. 1. Meridional channel shape. A drawing of the channel shape including the hub, shroud and the projected area of the impeller and guide vane blades. See figure 5.1 −50 0 50 100 150 200 250 300 350 400 0 20 40 60 80 100 120 Impeller Guide Hub Shroud MERIDIONAL GEOMETRY z-axis r- a x is Figure 5.1: Meridional plot of the channel shape. The hub is included as it is a requirement for the input to TD1. 2. Thickness distribution. The thickness distribution of the blades are defined along the camber line at the hub, the mid and at the shroud. The spanwise (going from hub to shroud) thickness distribution is then linearly interpolated in between these sections. A separate thickness distribution can be defined for the impeller and guide vane blades, however, in this thesis the same thickness distribution is used for both the impeller and the guide vane blades. 3. Fluid properties and design specifications. The working fluid, the rotational speed and the inlet velocity and pressure field is specified. 4. Number of blades. The number of impeller and guide vane blades are chosen. There is in general more guide vane blades than impeller blades. 5. Vorticity distribution. The blade loading is spanwise specified by a given vor- ticity at the hub and shroud at the leading and trailing edge. 6. Blade loading. The streamwise (following the camber line from leading to trailing edge) blade loading is imposed at two or more span locations. The program makes a linear interpolation of the loading between the defined spanwise positions. 22 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 5. DESIGN TOOLS AND METHODS 7. Stacking condition. The stacking condition defines a spanwise line (at a specific streamwise position) as the starting point of the blade design. It defines if the blade is leaning towards or against the rotational direction at that specific streamwise position. The blade can freely adjust according to the defined blade loading and vorticity distribution everywhere else along the chord length. These are the seven main design parameters. Some of these parameters are limited by other design limitations, such as the design specifications, others are based on ratios from excising waterjet designs and kept constant or only slightly modified throughout the entire design process to reduce the amount of variables. 5.2 Computational Fluid Dynamics Analysis Computational fluid dynamics covers a wide range of numerical ways to solve the Navier Stokes’ equations. In this section the methods used for the CFD analysis are presented. There is a large number of CFD methods each with their own advantages, the two main considerations for all CFD calculations are the quality of the results contra the cost of computation. These two parameters are often connected; if results of excellent quality is required, the computation is costly. A steady flow analysis is the foundation of the performance evaluation as it has a low cost of computation, and a great number of analyses are done to evaluate the effect of design changes. The quality of the steady flow computation is decent, but a transient analysis is conducted for the final concept design to obtain a more precise indication of the pump performance. 5.2.1 Steady State Analysis The steady state analysis is a cost efficient analysis. It is used to evaluate the pump performance and to visualise where changes are needed. The analysis excludes any time dependent effects and estimates the flow through the pump as steady. The rotation of the impeller blade is modelled by introducing a simulated rotation of the grid surrounding the impeller blade. Thereby modelling the rotation of the blade in a constant flow rate and causing the correct lift and loading on the impeller blade. The guide vane is, however, kept at a constant relative position compared to the impeller blade, this is a consequence of the steady state model. A transient analysis includes the time dependent effects. 5.2.2 Transient Analysis A transient analysis is a study of a time dependent unsteady flow, with a high compu- tational cost. It is used to study how unsteady flow evolves over time. The impeller blades are rotating, and thereby shifting their relative position compared to the guide vanes over time, this results in a time dependent unsteady flow. The transient analysis is therefore a more accurate model of the flow in the pump than the steady state analysis. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 23 CHAPTER 5. DESIGN TOOLS AND METHODS The final solution of the flow is a repeated cycle of fluctuating results. The analysis is conducted for constant flow rates but with fluctuating and dynamic effects between the impeller and guide vane blades. 5.2.3 SST k − ω Turbulent Flow Model The turbulent flow in both the steady and transient analysis is modelled using the SST (Shear-Stress Transport) k−ω turbulent flow model proposed by Menter in 1992 [Menter, 1993]. This model combines the standard k − ε model with the Wilcox k − ω model, using the best properties of both models. The k − ε model is functioning well when applied on a free stream flow, however, a wall dampening function is needed when evaluating the flow near a wall. The Wilcox k − ω model works well at predicting flows near a wall, thus removing the need for a wall function, it is however more unstable in free stream. The combination of the two models results in a stable turbulent model capable of modelling the flow both in the free stream and near the wall. See [Versteeg and Malalasekera, 2007, Chap. 3] and [Menter, 1993] for reference and a more detail description. This specific model is regarded as an efficient and flexible model, and Rolls-Royce has had positive experiences using this model. 5.2.4 Mixture Flow Model A multiphase analysis is conducted using the mixture flow model ([Ansys, 2013]). The analysis is used to evaluate the cavitation properties of the pump. It is applied in combination with the turbulence flow model in the transient analysis. The two phases of the water is defined as water-liquid and water-vapour, and a mass transfer function is defined. This function defines when cavitation occurs using a defined vapour pressure given as input. It is difficult to obtain a stable calculation using the mixture model, especially if there is a large amount of cavitation in the pump. A first order scheme is therefore used to calculate the volume fraction and the momentum equation, this increases the stability of the calculation, but decreases the model accuracy. The model is, however, regarded as a good method to establish an indication of the cavitation properties of the pump. A cavitation analysis is usually adjusted to match experimental results, this however is not an option in this thesis. The results of the cavitation analysis are therefore only regarded as an indication numerical cavitation properties of the pump. 5.2.5 Schemes The second order upwind scheme is used in the steady and transient flow analyses. As the flow is mostly in the axial direction the second order upwind scheme is a good choice resulting in second order accuracy of the results and a high stability. An implicit scheme is used when evaluating over time steps in the transient analysis. The first order upwind scheme is used for the momentum and volume fraction calculations in the 24 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 5. DESIGN TOOLS AND METHODS cavitation analysis. The first order scheme is less accurate than the second order, but the stability is better. For more details regarding the theory behind the different schemes the interested reader is referred to [Versteeg and Malalasekera, 2007]. 5.2.6 Solver Algorithm The algorithm used to solve the pressure and velocity in the steady flow model is the SIMPLE algorithm. The SIMPLE algorithm is a simple iterative solver with great calculation stability properties. The algorithm introduces under-relaxation, for increased computation stability, using the guess and correct solver approach, see [Versteeg and Malalasekera, 2007, p.186-190] for reference and a detail description. The solver runs through the cells one at a time making it possible to run on computers with a small amount of memory. A modified version of the SIMPLE solver is used to solve the equation system in the transient analysis. Here a time dependence is added to the solver making it possible to solve unsteady flow problems, see [Versteeg and Malalasekera, 2007, sec. 8.7]. 5.2.7 The Computational Mesh The computational grid or mesh is generated using a CAD/mesh tool in the Ansys Workbench. The mesh is structured at the walls to ensure a sufficient resolution of the boundary layers. The blades are also considered as walls, but are modelled with smaller cells in order to construct the complex geometries and obtain sufficiently low y- plus values. The remaining computational domain is constructed using an unstructured mesh. A short grid dependence study is conducted to ensure sufficient grid independence. 5.2.8 y-plus The size of the first cell at a wall determines the y-plus size. The incorporated wall treatment of the turbulent flow model is design for a specific y-plus value range. The resolution of the boundary layer have to be fine enough to ensure that the y-plus of the mesh has a sufficient size for the turbulent flow model. It is however costly to obtain a small enough y-plus value for research purposes (y-plus around 1) an industry standard range of 30-60 is used as it has a low cost/benefit ratio (Rolls-Royce standard). A more detailed description of y-plus can be found in [Versteeg and Malalasekera, 2007, Chap. 9.]. 5.2.9 Convergence To determine if a computation has converged one needs to define convergence. There are different definitions of convergence when looking at the steady and unsteady flow analysis. In this project steady flow convergence has been defined as a minimum reduc- tion of a factor ten for the residuals and a maximum fluctuation of 1% of the torque on the impeller blade over the last 200 iterations. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 25 CHAPTER 5. DESIGN TOOLS AND METHODS The unsteady flow convergence is defined as a cyclic fluctuating solution with a time average difference of less than 1% from cycle to cycle. 5.2.10 The CFD Code - Ansys Fluent The tool used for the viscous computational fluid dynamics analysis of the pump is Ansys Fluent. This is an efficient and widely used CFD code for enclosed flows. 5.2.11 Postprocessing The post-processing is conducted using Ansys Post. Using the post-processing tool the flow is visualised and studied. Data used for calculations of the pump performance is extracted from the CFD calculations. 26 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 6 Energy Model In this chapter a simple mathematical model is developed to create an overview of the energy flow through the system. The development of the model is necessary in order to calculate the data required for the inputs, assumptions and benchmarking of the pump design. The model is a compilation of different methods of estimating the energy flow, the head losses and the thrust required of the waterjet system. The energy model covers the waterjet propulsion system from the steam tube inlet to the jet outlet. In figure 6.1 the sketch displayed in section 3 is shown in order to create a better overview of the system, the points displayed in the figure are referred to and used as subscriptions throughout the energy model. 7. 6. 5. 0 Figure 6.1: Waterjet principle model: Point 0. Free stream, Point 1. Stream tube inlet, Point 2. Duct inlet, Point 3. Pump inlet, Point 4. Pump center Point 5. Pump outlet, Point 6. Nozzle outlet and Point 7. Jet minimum diameter. 6.1 Assumptions The assumptions used in the energy model are presented in the following list: • The flow rate is assumed constant. The mass flow rate is changed to simulate a number of operational points, but is constant at each operational point in order to simplify the model. • Temperature variations are assumed insignificant and are therefore neglected. The temperature variations are minimal for pressure changes in a fluid. 27 CHAPTER 6. ENERGY MODEL • It is assumed that the Vena Contraction is insignificant or that the actual nozzle size results in a Vena Contraction matching the jet output area considered here. This effectively sets the velocity and pressure at point 7. equal to that of point 6 (in figure 6.1). • The duct of the boat is assumed to be a standard Rolls-Royce duct. Experimental data for this duct enable a calculation of the expected pressure loss through the duct. The method is described in an internal Rolls-Royce report [Rolls-Royce, 2010]. • The steam tube is assumed to have a rectangular cross section with a width of 1.35 times the impeller diameter (point 1.). This is a Rolls-Royce standard assumption for the calculation of the flow velocity in the steam tube. • A grid loss factor of ξgrid = 0.05 is assumed and added to the inlet loss factor. This assumption is a rough estimate based on Rolls-Royce experience. 6.2 The Model The energy model models the energy flow through the propulsion system, and is used to evaluate the head rise needed to maintain the required thrust for a given operational speed (See figure 2.2). The system is modelled using the energy equation (A Bernoulli equation modified to include losses) presented in [Carlton, 2007]. The variables are rearranged slightly in order to create a simple connection between this mathematical model and the following CFD model. The energy is, according to tradition, referred to as meter water column, making the unit of the energy equation meters. P1 ρg + V 2 1 2g +H = P7 ρg + V 2 7 2g + ∆h+ hduct + hpump (6.1) H is the total head rise delivered by the pump, ∆h is the head loss related the the elevation of the outlet above the keel (see figure 2.2), hduct the head losses in the duct and hpump is the head loss in the pump. V1 is the average velocity at the stream tube inlet and V7 is average the velocity of the jet at the maximum Vena contraction. By expanding P7 to P7 = P1 − h1ρg equation 6.1 is reduce to: H = V 2 7 − V 2 1 2g + h2 + hduct + hpump (6.2) (6.3) The power delivered to the pump is proportional to the head rise produced by the pump. Ppump = ṁgH (6.4) (6.5) 28 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 6. ENERGY MODEL The thrust delivered by the jet is equal to the mass flow times the difference in speed between the average axial stream tube velocity (point 1.) and jet average axial velocity (point 7.). As the thrust is known from the Savitsky prediction in figure 2.2 the average velocity at point 7 is determined using the thrust equation. T = ṁ(V7 − V1) (6.6) The size of the stream tube is, however, dependent on the mass flow, this makes the average velocity in the stream tube (V1) dependent on the mass flow. The cross sectional area of the stream tube is divided into two areas, the boundary layer and the free flow area (going perpendicular to the flow direction) each with different average velocities. The average axial velocity and the cross sectional area of the boundary layer are estimated using theory describing the turbulent boundary layer on a flat plate, see [White, 1974, p.433-434]. The free flow area of the stream tube is calculated so that the mass flow requirement is reached (The free flow area is defined by the difference between the mass flow in the boundary layer and the needed flow rate of the stream tube). The mass flow is, as mentioned earlier, dependent on the average stream tube velocity thus making it necessary to solve the problem (ṁ,V1 & V7) using a simple iterative solver. See appendix B for the full Matlab program containing the mathematical model. The work done in propelling the vessel is based on the trust, and is expressed by the following equation [Allison, 1993]. Wjet = TV0 = ṁ(V7 − V1)V0 (6.7) The propulsion efficiency is defined as the ratio between the work done in propelling the vessel (equation 6.7) and power delivered by the pump (equation 6.5) [Allison, 1993; Carlton, 2007]. ηpropulsion = TV0 ṁgH = (V7 − V1)V0 1 2(V 2 7 − V 2 1 ) + g(h2 + hduct + hpump) (6.8) It is desirable to achieve the highest possible propulsion efficiency as this results in the minimum fuel consumption and thereby minimise the operational cost. The propulsion efficiency is often increasing with increased velocity for a waterjet propulsion system, this growth is, however, dependent on how rapid the head loss (hduct) in the duct is growing. The velocity term in the numerator of equation 6.8 is growing linearly while the denominator is experiencing quadratic growth, until a point is reached where the head loss in the duct increases rapidly. A more interesting way of evaluating the efficiency of the system is the efficiency of the pump (ηpump). The pump efficiency is of greater interest as it is also evaluated at the bollard pull condition(V0 = 0). This efficiency is based on the total energy input (equation 6.5) and the effective head rise (Heffective) produced by the pump. The effective head rise is equal to the total head rise (H) subtracted the internal head loss in the pump (hpump) and the energy in leftover swirl in the jet after the nozzle (hswirl) (point 7), see equation 6.9. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 29 CHAPTER 6. ENERGY MODEL Heffect = H − hpump − hswirl (6.9) The efficiency of the pump is of great importance as the pump is the heart of the thrust production. The pump efficiency is defined as the ratio between the effective head rise (Heffective) and the total head rise (the total energy input) (H). ηpump = Heffect H (6.10) From the CFD analysis the total energy input to the system (H) is determined using the torque on the blades and the angular velocity of these. Ptotal = τω (6.11) H = Ptotal ṁg (6.12) With τ being the torque delivered by the engine and ω being the angular velocity of the impeller rotation. The efficiency expression used for the pump in this thesis is expressed using equation 6.10 and 6.12 ηpump = ṁgHeffect τω (6.13) The head loss related to the duct (hduct) must be estimated in order to effectively predict the needed effective head rise of the pump. The duct head loss consists of a number of losses, see [Carlton, 2007]. The losses related to the duct are shown in equation 6.14. hduct = hinlet + hsf + hbend (6.14) These losses are related to the inlet loss (hinlet), the skin friction (hsf ) throughout the duct and the pressure loss caused by a bending pipe hbend. All of these losses are estimated based on an internal Rolls-Royce report, see section 6.2.1. The internal pump loss (hpump ) includes the loss related to the outlet nozzle and the guide vanes. This loss is not estimated as it is evaluated in the CFD models and defines the pump efficiency. The model for prediction of the head losses are presented in the following section. 6.2.1 The Head Losses The total head loss of the duct (htotal), including the elevation of the nozzle, is esti- mated based on experimental data available from Rolls-Royce [Rolls-Royce, 2010] and the dimensions of the boat. 30 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 6. ENERGY MODEL The Inlet and Duct Head Loss The head loss (hduct) from the duct inlet (point 1. to 2.) to the pump inlet (point 3.) is related to the inlet geometry (including the inlet grid), the mass flow rate of the system and the speed of the vessel. The head loss is estimated using an empirical method (based on model scale tests) recommended in an internal Rolls-Royce report [Rolls-Royce, 2010]. The duct velocity factor, λ, is defined as the ratio between the average flow velocity in the stream tube (V1 figure 6.1) and the average velocity in the duct (V3). λ = V1 V3 (6.15) An inlet loss factor ξ is determined using a polynomial with λ as a variable fitting the experimental data (see figure figure 6.2). This polynomial is connected to the specific method used to predict the total energy at point 3. in figure 6.1. The inlet loss factor (ξ) defines the amount of energy lost from the duct inlet to the pump inlet (point 3.), see equation 6.18. The y-axis and the specific polynomium used is excluded from the report and the mathematical model in the appendix due to intellectual property rules from Rolls-Royce. A grid loss factor(ξgrid) of 0.05 is added (see assumptions, section 6.1) to the inlet loss factor to include the pressure loss caused by the inlet grid. Thus the total inlet loss factor is ξtotal = ξ + ξgrid (6.16) In figure 6.2 the inlet loss factor with and without inlet grid correction is plotted. It is clear from the figure that the inlet loss factor is sensitive to large λ values and the smallest inlet loss occurs just before λ = 1. The energy input at point 1. is evaluated with still water at the depth of the keel as reference. Ė1 = ( 1 2 ρV 2 1 )Q̇ (6.17) where Q̇ is the volume flow rate into the system and Ė is the energy flow rate in watts (kg/m3 · (m/s)2 ·m3/s = kg ·m2/s3 = Nm/s = W ). The total energy at point 3 is determined using a simple energy equilibrium. The inlet loss factor (ξ) is used to evaluate the energy at the duct outlet (or the pump inlet (point 3.)) (Ė3). The definition of Ė3 from the Rolls-Royce report is used and rewritten, using equation 6.15, in order to make it possible to evaluate the head loss in the bollard pull operation (V1 = 0). CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 31 CHAPTER 6. ENERGY MODEL 0 0.5 1 1.5 2 2.5 Inlet velocity ratio (λ) In le t lo ss fa ct o r (ξ ) ξ ξ + ξ grid Figure 6.2: Plot of the inlet loss factor polynomial. Ė3 = Ė1 − ξE1 λ2 (6.18) Ė3 = Ė1 − ξ 12ρV 2 1 Q̇( V1 V3 )2 (6.19) Ė3 = Ė1 − ξ 1 2 ρQ̇V 2 3 (6.20) The duct head loss is the energy loss from point 1. to 3. given in meters. hduct = Ė1 − Ė3 Q̇ρg (6.21) Pump Elevation and The Pressure Before The Pump The head loss caused by the nozzle (the pump outlet, point 6.) elevation above sea level is h2 in figure 3.1. When the boat is planing h2 is approximated as dh and when the boat is in bollard pull operation the nozzle is submerged making the elevation loss zero (as it is counteracted by a positive pressure at the inlet). The pressure at point 3. (figure 3.1) is determined using the energy equation [Carlton, 2007] and the known pressure losses in the duct. 32 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 6. ENERGY MODEL P1 + 1 2 ρV 2 1 = P3 + 1 2 ρV 2 3 + (hduct + h2)ρg (6.22) P3 = P1 + 1 2 ρV 2 1 − (htotal)ρg − 1 2 ρV 2 3 (6.23) The resulting losses and pressures are presented in section 6.3 for a number of oper- ational points. 6.3 Key Results In this section the key results relevant for the blade design and pump benchmarking are presented. The two main operational points of relevance are the transit design speed of 20 knots and the bollard pull condition. The flow rate of these conditions are presented in table 6.1. The flow rate achieved at the bollard pull condition (V0 = 0 knots) is representing the minimum achievable flow rate (and highest head rise) at a given blade loading and rotation speed. Table 6.1: Design conditions. Vessel speed (V0) [knots] 0 20 Q̇ [m3/s] 0.28 0.29 Q̇e [-] 1.07 1.13 The flow rate (Q̇) is normalised (Q̇e) by equation 6.24, in which n is the speed of revolution in rounds per minute and dimp is the impeller diameter. Qe is presented as unitless to avoid confusion (the unit is [rpm/s]). Q̇e = Q̇ n 100d 3 imp (6.24) This normalisation represents a pump with a 1 m diameter running at 100 rpm. This is a Rolls-Royce standard for normalisation of the flow rate. A number of operational points are chosen to establish a benchmark for the perfor- mance of the pump design. The CFD analyses of the pump are then performed at the same operational points. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 33 CHAPTER 6. ENERGY MODEL The key results used for the pump benchmarking and design corrections are the effective head rise, i.e. the thrust and the flow rate. These key results are presented in table 6.2, the effective head rise is plotted in figure 6.3. The figure visualizes the portion of the required total head rise caused by head losses outside of the pump. The required head rise at the bollard pull condition is so much larger than that of the 20 knots condition that the vessel top speed is expected to exceed the design speed of 20 knots. The benchmarking therefore includes operational points equivalent to a top speed of 26 knots. Table 6.2: Key results from the mathematidal model V0 [knots] 0 19 20 21 22 23 24 25 26 T [kNm] 4.00 1.54 1.52 1.51 1.50 1.49 1.49 1.50 1.51 Heffect [m] 12.15 7.28 7.30 7.33 7.38 7.45 7.54 7.65 7.78 htotal loss [m] 1.97 0.23 0.25 0.27 0.30 0.33 0.36 0.39 0.43 V3 [m/s] 9.3 9.6 9.8 10.1 10.3 10.5 10.8 11.0 11.3 Q̇ [kg/s] 0.28 0.29 0.29 0.30 0.31 0.31 0.32 0.33 0.34 Q̇e [−] 1.07 1.11 1.13 1.16 1.18 1.21 1.24 1.27 1.30 1.05 1.1 1.15 1.2 1.25 1.3 1.35 0 2 4 6 8 10 12 14 Flow rate factor (Qe) [-] H ea d ri se [m ] Thrust Duct loss Elevation Figure 6.3: Plot specifying the head rise required to produce the necessary thrust. It is clear from figure 6.3 that around 20% of the head rise needed to produce the bollard pull thrust is related to the duct losses. 34 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 6. ENERGY MODEL 6.3.1 Maximum Efficiency Prediction The expected efficiency of a standard pump is estimated based on the specific speed and the pump type. The specific speed is defined in [Brennen, 1994, p28, equation 2.22], here shown in equation 6.25. Ω is the shaft rotational speed in rad/s, Q̇ is the volume flow in m3/s and H is the effective head rise (Heffect). N = ΩQ̇ 1 2 (gH) 3 4 (6.25) For the pump considered here, the design specific speed at 20 knots is ND = 2.78 based on the results from 6.2. This should according to [Brennen, 1994, p32, figure 2.8] (copied to figure 6.4 for easy reference) equal an estimated maximum efficiency of 70% for an axial flow pump. In [Brennen, 1994] axial pumps generally have a lower efficiency than mixed flow pumps operating at similar specific speeds, other sources (e.g. [Bulten, 2008]) are, on the contrary, indicating that similar efficiencies are achievable. However these similar efficiency are achieved with a axial flow pump running at a lower specific speeds than an axial pump usually does. Figure 6.4: Plot of performance prediction for pumps of varying type. Source: [Brennen, 1994, p32, figure 2.8]. 6.3.2 Engine Load From the key results the required torque is estimated for a number of operational points. In table 6.3 the ideal torque (τmin) and the required torque at 70% pump efficiency is CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 35 CHAPTER 6. ENERGY MODEL shown for the pump running at 3500 rpm and a nozzle and impeller diameter ratio of 80%. Table 6.3: The ideal engine torque and the torque required at 70 per cent pump efficiency. V0 [knots] 0 19 20 21 22 23 24 25 26 τmin [kNm] 90 56 57 59 61 63 65 68 70 τmin ηp=0.7 [kNm] 128 80 82 84 87 89.00 93 96 101 From this table it is clear that the rim engine is able to produce the head rise needed if a sufficiently high pump efficiency is reached, but only just. It is also apparent that the bollard pull condition is the most power consuming operation of the vessel. 6.4 Discussion of Model It is obvious from table 6.2 that the main challenge is to produce the 12.3 meters head rise demanded by the bollard pull condition. The high head rise is related to a high thrust requirement and a large head loss at the inlet. The model is in general useful for testing the impact of smaller design alterations on the pump requirements. The diameter ratio of the nozzle outlet is variable along with the rpm of the pump, making it possible to adjust the required torque to match the engine limitations. It is evident from table 6.3 that the engine can deliver power to achieve specified bollard pull thrust if a pump efficiency around 70% is reached. The model is based on rough estimates, both for the head losses and for the thrust prediction. It is a good basis for the conceptual design, but experimental or CFD data predictions of both the inlet losses and the hull resistance are necessary for the final production design of the pump. The efficiency predicted is low compared to other axial pumps, axial pumps are however usually designed for larger specific speeds. The expected efficiency would be around 85%-89% if the specific design speed of the pump would have been around five (see equation 6.25). The specific speed of the pump could be increased by increasing the rotational speed to 4000 rpm, but it would only increase the specific speed to around 3. The efficiency prediction method is based on old shaft driven designs (the original source data used for figure 6.4 is from 1981) and the resulting efficiency will deviate from this prediction as the pump is rim driven and hubless. The efficiency prediction is however useful for benchmarking the pump performance. 36 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 7 Steady Flow CFD Pump Model The set-up of the computational fluid dynamics model for the steady state analysis is presented in the following sections. The model is build upon the methods specified in section 5.2. The steady flow model is used to test the effect of the design changes throughout the design phase. The steady flow simulation set-up is displayed in figure 7.1, this set-up is generally used to get an indication of the pump performance at a low computational cost, see [Aartojärvi and Heder, 2008; Bulten, 2008]. Figure 7.1: Steady flow simulation set-up. Blue: Stationary walls. Green: Rotating impeller blade and shroud. Yellow: Free flow pipe. The set-up consists of two computational domains; one for the impeller (e.g. in figure 7.2b) and on the for guide vane (e.g. in figure 7.2a). The computational cost is minimised by only having to simulate one blade in each domain which is possible because of the of the pump symmetry. The volume flows in the domains are not of same value as there are four impeller blades and seven guide vanes. A mixing plane is introduced to cope with this difference. The mixing plane exchanges 37 CHAPTER 7. STEADY FLOW CFD PUMP MODEL (a) Computational domain for the guide vane, Case 1. (b) Computational domain for the impeller blade, Case 1. Figure 7.2: example of computational domains. information about the averaged pressure and velocity at a given radius between the upstream area (the impeller outlet) and the downstream area (the guide vane inlet). This insures energy and mass conservation throughout the total volume of the pump. The dynamic interaction between the impeller and guide vane blades are, however, lost as their relative positions are constant and the computation is therefore independent of time. 7.1 The Computational Grid The computational domains (figure 7.2) are divided into a number of small cells creating the computational grid. Both grids are constructed with similar grid specifications to ensure a stable computation. The amount of cells in and the quality of the mesh are controlled by a maximum and minimum cell size as well as a minimum cell skewness(the angle between the walls of the cell). An example of the resulting mesh is shown in figure 7.3. The detailed mesh specifications are found in appendix C. The rotational symmetry of the grid is ensured by controlling the cells which defines the two periodic boundaries (the walls meeting in the centreline, see figure 7.1). A sufficient y-plus value is ensured by controlling the size of the cells in the boundary layer. 7.1.1 Simplified Grid Dependency Study A minor mesh dependency study is conducted to establish the solution dependency of the computational grid, the results are shown in table 7.1. The study is conducted on the Case 1. with three different flow rates. Mesh no. 2 in table 7.1 has roughly half the volume of each cell compared to mesh 1. The grid dependency study shows a maximum result difference around 1% between the two meshes. With mesh no. 2 resulting in higher pump performance. In a full mesh dependency study a number of meshes, each with half the average cell volume, should be 38 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 7. STEADY FLOW CFD PUMP MODEL (a) The mesh used for the guide vane do- main, Case 1. (b) The mesh used for the impeller domain, Case 1. Figure 7.3: Example of computational mesh. Table 7.1: Simplified grid dependency study for case 1. Mesh no. 1 2 Impeller mesh: Number of elements [-] 812,775 1,549,961 Minimum element size [mm] 0.236 0.130 Maximum element size [mm] 45.19 25.07 Maximum face size [mm] 5 2.89 Guide vane mesh: Number of elements [-] 296,604 526,052 Minimum element size [mm] 0.059 0.0339 Maximum element size [mm] 11.7390 6.7718 Maximum face size [mm] 5 2.89 Mesh differences mesh 1 / mesh 2 Bollard pull 20 knots 25 knots Torque ratio 1.0100 1.0119 1.0127 Head rise ratio 1.0003 1.0030 1.0032 Pump efficiency ratio 0.9900 0.9908 0.9900 investigated until the difference is regarded insignificant. A 1% difference is a significant difference. The performance impact of the mesh dependency is however avoided by using meshes with similar settings, thus ruling out differences caused by differences in mesh sizing. A small grid dependency is acceptable when using this strategy to avoid its CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 39 CHAPTER 7. STEADY FLOW CFD PUMP MODEL impact on the design changes. A more refined, and thereby more correct solution or, a model scale test should be conducted for the final design. The development of the pump is in no way hindered by a small grid dependency as long as the grid properties are relative comparable, a full grid dependency study is therefore beyond the scope of this project. 7.2 Boundary Conditions The boundary conditions are stated in table 7.2. Table 7.2: Boundary conditions. 1. Walls and blades No slip condition. 2. Free-flow pipe Slip condition. 3. Impeller blade inlet Velocity inlet 4. Guide vane outlet Pressure outlet 5. Axial domain boundaries Periodic boundaries. The slip condition in the free-flow pipe (boundary 2.) is emulating a free jet. At the velocity inlet (boundary 3.) the flow rate through the system is defined as a constant average velocity. Changing this point changes the operation point of the pump, making it possible to produce a Q−H plot for the pump. The periodic boundaries (5. in table 7.2) are simulating the neighbouring blades by projecting the output from the one boundary and to the opposite boundary. This is possible as the mesh on both periodic boundaries are similar [Versteeg and Malalasekera, 2007, p. 281]. 7.3 Calculation Settings The main calculation settings used for the analysis in Ansys Fluent is summarised in table 7.3. 40 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 7. STEADY FLOW CFD PUMP MODEL Table 7.3: The calculation setting used for the steady analysis in Ansys Fluent. Turbulence model SST k − ω Solution methods Pressure- Velocity Coupling Scheme SIMPLE Spatial Discretization Gradient Least Square Cell Based Pressure Second Order Momentum Second Order Upwind Turbulent Kinetic Energy Second Order Upwind Specific Dissipation Rate Second Order Upwind Mixing plane Averaging method Area Under-Relaxation 0.05 Interpolation Points 200 7.4 Discussion of the Model The model is in general an efficient way to get a performance prediction, and useful for design iterations. The model does not include the dynamic effects of the impeller moving in relation to the guide vane. This results in a constant blade torque and a constant effect of the guide vane at a given flow rate. It is possible to reduce the mesh dependency of the solution by increasing the mesh resolution, this would, however, increase the computation time and the gained accuracy would have little impact on the design process. The system is normally tested in an experimental set-up for the final performance evaluation it is therefore more interesting to run a transient analysis, to capture the dynamic effects, than to improve the mesh resolution. The flow through the pump is dynamic, and the relative position of the guide vane compared to the impeller blade causes fluctuations in the pump performance. It is therefore possible that the steady state simplification is presenting a local efficiency extreme. A transient analysis is therefore conducted in order to achieve a more accurate time averaged pump performance. CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 41 CHAPTER 7. STEADY FLOW CFD PUMP MODEL This page is intentionally left blank. 42 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 8 Transient Flow CFD Pump Model The unsteady flow CFD model is used to make a more detailed analysis of the flow through the pump. The time averaged performance calculated using an unsteady flow analysis (a transient analysis) is more accurate than that of the steady state analysis. The transient analysis set-up is presented in figure 8.1. A similar set-up has been used to simulate an axial waterjet pump in [Bulten, 2004] and [Bulten, 2007]. The turbulent flow models used in these analyses are respectively a standard k−ω and a standard k−ε model. The SST k − ω turbulent flow model used in this thesis should have a higher accuracy than both methods (see section 5.2). Figure 8.1: Unsteady flow analysis set-up. The set-up is constructed using the computational domains presented in figure 7.2. The impeller domain is copied four times and the guide vane domain seven times in order to create the full pump domain. 43 CHAPTER 8. TRANSIENT FLOW CFD PUMP MODEL 8.1 The Computational Grid The grid used for the steady analysis is the base of the transient computational grid. The grid is constructed by copying and rotating the impeller and guide vane grid to construct a mesh covering the full pump volume. The grid is constructed in this manner in order to avoid meshing problems. Rolls-Royce has previously experienced problems when meshing blades in more than one radial direction, this method of copying the mesh is therefore used to ensure a good mesh with properties similar to that of the steady mesh. As the grid used is the same as used in the steady analysis the simplified grid de- pendency study is still, to some extend, valid. The grids are combined and fused using Ansys Fluent, the final computational grid is shown in figure 8.2. Figure 8.2: The figure visualises the mesh used for the transient analysis of the unsteady flow through the pump. 8.2 Boundary Conditions The boundary conditions are stated in table 8.1. They are very similar to the ones used in the steady analysis. The 5. boundary condition from 7.2 is no longer needed as the full 44 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 8. TRANSIENT FLOW CFD PUMP MODEL computational grid is modelled and the mesh containing the impeller is actual rotating around the flow axis. The rotation of the impeller grid creates the time dependency of the computation as the relative position of the impeller blades compared to the guide vanes is time dependent. Table 8.1: Boundary conditions. 1. Walls and blades No slip condition. 2. Free-flow pipe Slip condition. 3. Impeller blade inlet Velocity inlet 4. Guide vane outlet Pressure outlet 8.3 Calculation Settings The main calculation settings used for the transient analysis in Ansys Fluent is sum- marised in table 8.2. Here the main difference from the steady flow analysis is the use of a second order implicit scheme to model the time stepping in the SIMPLE solver. The rotation of the impeller mesh is handled by a mesh interface (A fluent function handling the information transfer between independent grids) between the guide vane outlet and the impeller inlet. Table 8.2: The calculation setting used for the transient analysis in Ansys Fluent. Turbulence model SST k − ω Solution methods Pressure- Velocity Coupling Scheme SIMPLE Spatial Discretization Gradient Least Square Cell Based Pressure Second Order Momentum Second Order Upwind Turbulent Kinetic Energy Second Order Upwind Specific Dissipation Rate Second Order Upwind Transient Formulation Second Order Implicit Mesh Interfaces impeller outlet - guide vane inlet CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 45 CHAPTER 8. TRANSIENT FLOW CFD PUMP MODEL 8.4 Multiphase Flow Model The mixture flow model, presented in section 5.2, is used to model cavitation in the pump. The cavitation model is based on a transient analysis and follows the same settings as the transient analysis with some added configurations presented in table 8.3. The model is sensitive and the computation diverges easily, the analysis is therefore started with very small time steps and gradually increased until a similar time step as that of the transient model is used. 8.4.1 Settings Table 8.3: The calculation setting used for the transient multiphase analysis in Ansys Fluent. Changes from table 8.2 is marked with talic. Turbulence model SST k − ω Multiphase model Mixture Phases Phase 1 - Primary Phase Water-liquid Phase 2 - Secondary Phase Water-vapour Vaporization pressure 2.3 kPa Bubble Number Density 106 Cavitation model Schnerr Solution methods Pressure- Velocity Coupling Scheme SIMPLE Spatial Discretization Gradient Least Square Cell Based Pressure Second Order Momentum First Order Upwind Volume Fraction First Order Upwind Turbulent Kinetic Energy Second Order Upwind Specific Dissipation Rate Second Order Upwind Transient Formulation Second Order Implicit Mesh Interfaces impeller outlet - guide vane inlet 46 CHALMERS - Shipping and Marine Technology, Master Thesis 2014:302 CHAPTER 8. TRANSIENT FLOW CFD PUMP MODEL 8.5 Discussion of the Model The unsteady model produces a more accurate prediction of the performance and the cavitation properties of the pump than the steady flow analysis. The model makes it possible to analyse the variation of the pressure on the blades, thereby giving a more real- istic evaluation of the cavitation properties. The cost of the computation is significantly higher compared to the steady analysis, and the analysis is therefore only conducted for the final concept design. The mesh from the steady state analysis is used and the grid dependency study is assumed to cover the use in the transient analysis. The grid does however react differently when used in the transient analysis, a separate grid dependency study should therefore be conducted at a later stage. The grid is however estimated to be sufficiently independent for the performance analysis in this thesis, based on the steady state grid dependency study and comparisons with gird us