Mechanical study of the regulation system of a Kaplan turbine blade

Treball de Fi de Grau Grau en Tecnologies Industrials i Anàlisi Econòmica (GTIAE) Mechanical study of the regulation system of a Kaplan turbine blade Bachelor’s Thesis Report June 25, 2024 Author: Antoni López Pérez Supervisor: David Valentín Ruiz Call: July 2024 Escola Tècnica Superior d’Enginyeria Industrial de Barcelona Mechanical study of the regulation system of a Kaplan turbine blade pag. 1 Abstract The Kaplan turbine, a key technology within hydroelectric power plants, is renowned for its adaptability to varying water flow conditions and its efficiency in generating power. This study focuses on the mechanical behavior of the regulation system of a Kaplan turbine blade, which plays a crucial role in maintaining optimal performance and grid frequency stability. The study employs Ansys Workbench software to conduct a stress analysis of the turbine’s regulation system. The simulation aims to identify critical points and stress concentrations that could lead to system failure. A specific focus is placed on the forces required to actuate the piston mechanism that adjusts the turbine blades, as well as the resulting stress distributions within the system components. Initial results indicate that a substantial force is necessary to move the piston, highlighting potential areas of mechanical strain. The simulation identifies the bottom pin of the link part as a critical stress point due to the combined effects of mechanical strain and friction. The findings of the study are expected to contribute to the development of more robust and reliable hydroelectric turbines, supporting the broader goal of sustainable energy generation. pag. 2 Antoni López Pérez Resum La turbina Kaplan, una tecnologia clau dins les centrals hidroelèctriques, és coneguda per la seva adaptabilitat a les condicions variables de flux d’aigua i per la seva eficiència en la generació d’energia. Aquest estudi es centra en el comportament mecànic del sistema de regulació de les pales d’una turbina Kaplan, que juga un paper crucial en el manteniment del rendiment òptim i l’estabilitat de la freqüència de la xarxa. L’estudi utilitza el programari Ansys Workbench per realitzar una anàlisi de tensions del sistema de regulació de la turbina. La simulació té com a objectiu identificar punts crítics i concentracions de tensió que podrien provocar una fallada del sistema. Es presta especial atenció a les forces necessàries per actuar el mecanisme del pistó que ajusta les pales de la turbina, així com a les distribucions de tensió resultants dins dels components del sistema. Els resultats inicials indiquen que es necessita una força substancial per moure el pistó, destacant les possibles àrees de tensió mecànica. La simulació identifica el passador inferior de la part de l’enllaç com un punt crític de tensió a causa dels efectes combinats de la tensió mecànica i la fricció. S’espera que els resultats de l’estudi contribueixin al desenvolupament de turbines hidroelèctriques més robustes i fiables, recolzant l’objectiu més ampli de generació d’energia sostenible. Mechanical study of the regulation system of a Kaplan turbine blade pag. 3 Resumen La turbina Kaplan, una tecnología clave dentro de las centrales hidroeléctricas, es conocida por su adaptabilidad a las condiciones variables de flujo de agua y por su eficiencia en la generación de energía. Este estudio se centra en el comportamiento mecánico del sistema de regulación de las palas de una turbina Kaplan, que juega un papel crucial en el mantenimiento del rendimiento óptimo y la estabilidad de la frecuencia de la red. El estudio utiliza el software Ansys Workbench para realizar un análisis de tensiones del sistema de regulación de la turbina. La simulación tiene como objetivo identificar puntos críticos y concentraciones de tensión que podrían provocar una falla del sistema. Se presta especial atención a las fuerzas necesarias para accionar el mecanismo del pistón que ajusta las palas de la turbina, así como a las distribuciones de tensión resultantes dentro de los componentes del sistema. Los resultados iniciales indican que se necesita una fuerza sustancial para mover el pistón, destacando las posibles áreas de tensión mecánica. La simulación identifica el pasador inferior de la parte del enlace como un punto crítico de tensión debido a los efectos combinados de la tensión mecánica y la fricción. Se espera que los resultados del estudio contribuyan al desarrollo de turbinas hidroeléctricas más robustas y fiables, apoyando el objetivo más amplio de generación de energía sostenible. pag. 4 Antoni López Pérez Mechanical study of the regulation system of a Kaplan turbine blade pag. 5 Contents Abstract 1 Resum 2 Resumen 3 List of figures 7 1 Introduction 8 1.1 Motivation......................................... 8 1.2 Stateoftheart....................................... 9 1.3 Objectives ......................................... 9 2 Theoretical background 11 2.1 Hydroelectric power plants . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11 2.2 Types of hydropower plants . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11 2.3 Typesofturbines ..................................... 12 2.4 TheKaplanturbine.................................... 14 2.4.1 Description of the turbine . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 2.4.2 Runner blade regulation mechanism . . . . . . . . . . . . . . . . . . . . . . 15 2.5 Frequencyregulation................................... 16 3 Methodology 18 3.1 Numericalanalysis .................................... 18 3.2 AnsysWorkbench..................................... 18 3.2.1 Description of the software . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 3.2.2 Workbench setup options . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 3.3 Simulation development process . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 3.4 Fatigueanalysis...................................... 25 4 Case study 28 4.1 Geometrydefinition ................................... 28 4.2 Workbenchsetup ..................................... 30 5 Analysis of the obtained results 39 6 Difficulties encountered in the simulation process 46 7 Planning 47 8 Economic assessment 48 9 Environmental assessment 49 10 Social and gender equality assessment 50 11 Conclusions 51 References 52 pag. 6 Antoni López Pérez List of Figures 1 Scheme of an impoundment hydropower plant. Source: [1] ............ 12 2 Scheme of a run-of-river (or diversion) power plant. Source: [1] .......... 12 3 Representation of a Francis turbine. Source [2] .................... 13 4 Diagram of the water flow in a Kaplan turbine. Source: [1] ............. 13 5 Diagram of a Pelton turbine. Source: [3] ........................ 14 6 Picture of a real model of a Kaplan turbine. Source: [4] ............... 14 7 Kaplan turbine guide vanes regulation mechanism. Source: [5] .......... 15 8 Blade regulation system in a Kaplan turbine. a) Maximum opening. b) Maximum closing. Source: [6] ................................ 16 9 Element types that can be used in the Finite Element Method. Source: [7] . . . . 18 10 Solidworks model of the simple slider-crank geometry used. ............ 21 11 Ansys Workbench environment: geometry linked with "Static Structural" analysis. 21 12 Definition of the translational joint. ........................... 22 13 Definition of one of the revolute joints. ......................... 22 14 Visual representation of the used mesh. ........................ 23 15 Definition the displacement boundary condition. ................... 23 16 Display of the Von-Mises stress results. ........................ 24 17 Display of directional displacement of the runner. .................. 24 18 Example of stress loading over a 24h period. Source: [8] .............. 25 19 Example of a Rainflow counting algorithm matrix represented in 3D. Source: [8] 26 20 Example of a S-N curve. Source: [8] .......................... 27 21 Solidworks model of the whole Kaplan turbine geometry. .............. 28 22 Solidworks model of the Kaplan turbine geometry after a first simplification. . . 29 23 Solidworks model of the Kaplan turbine geometry after completely simplifying it. 29 24 System in maximum closing position (left) and maximum opening position (right). 30 25 Bonded contacts with the base of the regulation system. ............... 31 26 Other bonded contacts between the blade and internal connection parts. ..... 31 27 Defined contacts of the pins and pin covers. Bonded contact (left) and frictional contact (right). ...................................... 32 28 No separation contact definition between the pins and the link lateral bars. . . . . 33 29 Frictional contacts at the link lateral bars. ....................... 33 30 Joint used to fix the system to the ground. ....................... 34 31 Translational joint that allows the piston to move vertically. ............. 34 32 Revolute joint that allows the blade to rotate. ..................... 35 33 Definition of the gravity. ................................. 35 34 Connection of external data files to the main analysis. ................ 36 35 Rigid transformations applied to the imported pressure distributions. ....... 36 36 Imported pressure on the pressure side. ........................ 37 37 Imported pressure on the suction side. ......................... 37 38 Displacement condition applied on the top surface of the piston. .......... 38 39 Correct movement check for the final simulation: undeformed figure. ....... 39 40 Correct movement check for the final simulation: total deformation. ........ 39 41 Von-Mises stress distribution results. .......................... 40 42 Von-Mises stress distribution in the top pin cover. .................. 41 43 Von-Mises stress distribution in the bottom pin. ................... 42 44 S-N curve of Ansys’ structural steel. Source: Ansys Workbench. .......... 43 Mechanical study of the regulation system of a Kaplan turbine blade pag. 7 45 Von-Mises stress distribution in the bottom pin for a past simulation using bonded contacts. .......................................... 43 46 Piston displacement and Von-Mises stress over a set of friction coefficient values. Source: Own. ....................................... 44 47 Gantt diagram of the project development. Source: Own. .............. 47 pag. 14 Antoni López Pérez For high-head, low-flow situations, an impulse turbine is usually suitable. The most known and used impulse turbine is the Pelton turbine. A Pelton turbine has free jets discharging water directly into the buckets of the runner. They are commonly used in very high-head and low flow situations. Figure 5: Diagram of a Pelton turbine. Source: [3] As seen in figure 5, only a part of the turbine is in contact with the water flow. This is because impulse turbines work at atmospheric pressure. Due to this characteristic, they do not require a draft tube. 2.4 The Kaplan turbine 2.4.1 Description of the turbine A Kaplan is a type of water turbine that is especially suited for operating in a low-head, high flow regime. This means that, in practice, it is particularly used in run-of-river hydroelectric plants where large volumes of water are available but the head is relatively low. Figure 6: Picture of a real model of a Kaplan turbine. Source: [4] The design of a Kaplan turbine system has to ensure that the water flow that enters the rotor area is uniform and perfectly axial. This is achieved by means of a spiral shaped inlet pipe. The inlet, however, is also regulated by adjustable guide-vanes, which control the amount of Mechanical study of the regulation system of a Kaplan turbine blade pag. 15 water passing through the turbine and also introduce different amounts of swirl to the flow, making sure that the water hits the rotor at the most efficient angle [15]. Figure 7: Kaplan turbine guide vanes regulation mechanism. Source: [5] The second adjustability mechanism this type of turbine has, is the rotor blade pitch. The blades can be positioned in an almost flat profile (for very low flows) to a high steep angle (for large flows). The blade pitch mechanism also ensures that the angle of attack of the water flow is the optimal. For both adjustability systems, when the water flow is higher, so is the power generated [16]. At the end of the cycle, the outlet water flows through a draft tube especially designed to avoid cavitation, a phenomenon that can cause thorough damage to the turbine structural elements [16]. The main advantage of the Kaplan over other types of turbines is the adaptability derived from the implementation of the both inlet guide-vanes and rotor blades, allowing for a very wide operating range while maintaining high efficiency and, thus, optimal power generation. 2.4.2 Runner blade regulation mechanism As the goal of this project is to study this mechanism, a more in-depth analysis is provided. The runner blade pitch regulation mechanism consists of the geometry shown below: pag. 16 Antoni López Pérez Figure 8: Blade regulation system in a Kaplan turbine. a) Maximum opening. b) Maximum closing. Source: [6] When the piston moves, the blade turns (actually, the four blades at once). This causes generated electricity to vary depending on how open the turbine is to the water flow. In figure 8, two states are represented: on the left, the maximum opening, when the most water flow is allowed to flow through the turbine, increasing the generation and, on the right, the opposite, the maximum closing position. As mentioned before, this mechanism is put in place so that the angle of attack of the blades is optimum regardless of the water flow conditions. The optimum angle of attack in this specific case of a Kaplan turbine refers to the blade pitch angle that maximizes the turbine’s efficiency for a given flow rate and head. This angle ensures that the turbine blades interact with the water flow in the most effective manner, converting the maximum possible kinetic energy from the water into mechanical energy while minimizing losses due to turbulence, cavitation, and drag. The movement of the runner piston to control the blade pitch causes a stress distribution in the whole structure. These stresses are responsible for the failure of the turbine over time, so they are to be studied in depth. An initial hypothesis is that the largest value of this magnitude will be found in the link between the base and the blade section, especially in the link pins. This stress analysis will be done by means of the Ansys Workbench software (see section 3.1.2.). 2.5 Frequency regulation Frequency regulation is a critical component in maintaining the stability and reliability of the electrical power grid. The frequency of the power system has a nominal value (50 Hz in Europe and 60 Hz in North America) which cannot deviate to ensure a proper operation of electrical devices. An imbalance can cause serious consequences, from efficiency losses to the damage and destruction of electrical equipment. The frequency of the grid is related to the amount of power generated, being the “golden rule” that energy supplied must always be equal to the amount of power consumed. If too much power is generated and then fed into the grid, the electrical frequency increases and, if the generated power is not enough to satisfy a high demand, frequency drops [17]. Mechanical study of the regulation system of a Kaplan turbine blade pag. 17 With the increase in renewable energy production, which can vary greatly depending on the weather (and produces, in general, lower amounts of power per plant than conventional power plants), the complexity of managing the grid has increased significantly [18]. A mechanism commonly used to stabilize the grid frequency is Frequency Containment Reserve (FCR), which does so by automatically adjusting the output power of power plants in response to short-term fluctuations. FCR has an almost immediate response when a frequency disturbance does occur (it is activated within seconds after the deviation) in order to bring back the frequency value to its nominal one. FCR acts as a safety net, making sure that deviations are quickly corrected [18]. One of the main functions of hydropower plants is to provide this FCR to the grid as well as more flexibility, as mentioned above. As hydropower consumption increases, however, a problem arises about the event of mechanical failure in the regulation systems of the employed turbines, which are used in a different, more demanding regime than they were originally designed for. pag. 18 Antoni López Pérez 3 Methodology 3.1 Numerical analysis To perform the simulation of the turbine regulation system, the finite element method (FEM) has been used. This method is a numerical technique used as a tool to solve complex problems by breaking down a large, complex system into smaller parts called finite elements. The method then gives an approximate numerical solution as a result of solving partial differential equations on the discretized space. The discretization is achieved by constructing a mesh of the object, thus defining the system in a finite number of points [19,20]. Different element types can be set to create the mesh, being defined by the interpolation function they use. Elements can be classified by shape (e.g. triangular or quadrangular elements), or by the amount of nodes they are defined with (e.g. quad4 or quad8, being 4 or 8 the number of nodes used to define the quadrangular element) [21]. Figure 9: Element types that can be used in the Finite Element Method. Source: [7] A final consideration to be made is the size of the mesh. The finer the mesh, the closer the simulation to the real value but, it also implies that the computational power needed to execute the simulation will be higher. A balance has to be then found in this tradeoff curve between accuracy and computational power. 3.2 Ansys Workbench 3.2.1 Description of the software Ansys Workbench is a software platform that allows the user to validate or test ideas by performing simulations combining all the physic-based tools and products the company Ansys provides [22]. It’s a very versatile and powerful tool due to its extensive capabilities and integrated environment, which easily allows the user to simulate any kind of real life engineering situation. For this project, the “static structural analysis” has been used. This is a type of simulation used to determine the behavior of structures under static loading conditions. Some of the characteristics of this analysis are: •Static loading: the loads applied are considered to be constant, with no change over time Mechanical study of the regulation system of a Kaplan turbine blade pag. 19 or with a dynamic effect so small it can be ignored. •Equilibrium equations: the analysis is based on solving equilibrium equations derived from Newton’s laws of motion, ensuring that the sum of forces and moments on any part of the structure is zero. •Stress and strain computation: the analysis determines the stresses (internal forces per unit area) and strains (deformations per unit length) within the material of the structure. Stress and strain distributions are critical for assessing the structural integrity and performance. From the analysis will be extracted the information regarding the deformations and stresses of the employed geometry, the Kaplan turbine model. This analysis is chosen over “Transient Structural” because loads applied to the system can be regarded as constant during the instant they’re applied and, although a transient analysis could be more thorough and comprehensive, it would imply the use of a huge amount of extra computational power which is not available. 3.2.2 Workbench setup options The workbench software has many different options for a simulation to be as close as possible to the real life situation that it is being studied. 3.2.2.1 Material data The materials being used can be defined. For different simulations, one or more materials can be used and there’s the possibility of creating them inside the software by defining their characteristics, mainly density, Young’s modulus, isotropy and Poisson’s ratio. 3.2.2.2 Contacts The studied geometries are usually complex enough to have more than a single body. Therefore, the contacts between them have to be defined. Every pair of surfaces that are physically connected and belong to different bodies, have to be properly defined, for the simulation to be precise. There are many types, but the most common (and the ones used in this project are the following): •Bonded: two surfaces joined together by a bonded contact are regarded as if they were welded together, with no relative movement between each other. In practice, if two bodies are in a bonded contact, they will kinetically behave as a single body, having the same motion. •Frictional: a frictional contact is set in two rough surfaces physically connected, with relative movement between them. To create this contact, a friction coefficient must be applied, which will indicate how difficult it will be for one of the bodies to move relative to the other. •No separation: when this type of contact is selected, the target and contact surface are tied up for the rest of the analysis. Slide is possible, but the nodes in contact are bonded to the target surface in normal direction [23]. pag. 20 Antoni López Pérez 3.2.2.3 Joints In mechanics, a joint is a connection between two or more rigid bodies that allows some relative motion between them. Joints are fundamental components in mechanical systems like the ones studied in this project, as they enable the movement and interaction of different parts. They can be categorized based on the types of relative motion they allow, including: •Fixed joints: restricts all relative motion between the linked parts. •Revolute joints: restrict all movements except a rotation in one of the axes. •Translational joints: only allow for a translational motion in one of the axes, restricting all the others. Besides this classification, joints can be separated into two different groups depending on the bodies they are connecting. They can connect either body to ground or body to body. 3.2.2.4 Mesh The mesh applied to the geometry can be adapted to suit the project needs as well as possible. The type of element can be chosen, as well as the size. Moreover, special sizing tools can be inserted in order to apply a different mesh to a specific area (usually just changing the mesh element size to refine it at the critical points). Among the available options, a new mesh can be inserted into a body, a face or a previously defined contact. 3.2.2.5 Loads All kinds of loads can be defined as well in the software. A force or a pressure can be applied to a point, surface or body. Not only that, but displacements can be defined as well in both linear and angular domains (i.e. a specific surface has to move exactly 1m). Another option is to define a support, a constraint of a certain set of degrees of freedom. A fixed support, for instance, is an equivalent of the previously mentioned fixed ground-body joint. External loads can also be applied. From the standard earth gravity, to complex pressures extracted from a computational fluid dynamics (CFD) simulation, as the one used in this project. 3.2.2.6 Results display Once the simulation is completed, the results can be shown by inserting different views under the solution section of the menu. These views can be selected to display the results from magnitudes such as deformation and different kinds of stress, for a selection of surfaces or bodies, or for the entire geometry. For the performed simulations, Von Mises stress will be used, since it combines the normal and shear stresses into a single value, making it easier to interpret. The use of Von Mises stress is widely accepted to analyze this kind of simulation, for ductile materials such as steel. Other useful tools to display the results are probes. Probes in structural analysis are usually used to measure changes in position (or angular displacement). Mechanical study of the regulation system of a Kaplan turbine blade pag. 21 3.3 Simulation development process The first step of the project is learning how to correctly use the Ansys Workbench software. In order to do so, a first test has been done to get familiarized with the program. The idea is to create a simple mechanism and analyze it using the Workbench environment. To do so, a simple slider-crank mechanism is used. The following geometry is created in solidworks, and then imported into Workbench. Figure 10: Solidworks model of the simple slider-crank geometry used. Once imported, the “Static structural" analysis has to be created and linked with it. Figure 11: Ansys Workbench environment: geometry linked with "Static Structural" analysis. The next step is to open the model and set up the contacts and joints. All the contacts with the bodies will be frictional and 4 joints will be defined. The first one is a translational joint between the small block and the base one, which will be fixed to the ground. pag. 22 Antoni López Pérez Figure 12: Definition of the translational joint. Then, 3 body to body revolute joints are defined between the base and the short link, the short link with the long link and, finally, the longer link with the small block. These joints can be defined in different ways depending on the geometry. Here, the revolute joint pins have been chosen not to be represented, and the joints are defined by selecting the surfaces that would be in contact with said pins. Figure 13: Definition of one of the revolute joints. Then, the mesh is defined. For this example, the chosen mesh will be rather coarse, since the desired outcome is not a really precise simulation, but to get the knowledge on how to actually perform it. Mechanical study of the regulation system of a Kaplan turbine blade pag. 23 Figure 14: Visual representation of the used mesh. Next, loads have to be applied. First, the base is fixed to the ground and then, the load that will cause the system to move. Among the available options, a linear force or displacement can be applied to the runner, or a moment or angular displacement to one of the revolute joints. Figure 15: Definition the displacement boundary condition. In this case, a linear displacement has been chosen for simplicity, since simulations with boundary conditions such as displacements are solved more easily by the software. Finally, the simulation is run and the results are shown. Inserting the Von Mises stress view, the program displays the following information: pag. 30 Antoni López Pérez tional processes, while still maintaining the accuracy of the analysis. The next thing worth mentioning about the simulation used is the initial angle of the blade. As mentioned before, the system has two extreme positions, maximum closing position and maximum opening position. Figure 24: System in maximum closing position (left) and maximum opening position (right). Both geometries contain the same elements and the only variation between them is the angle of the blade, with the rest of the system moving accordingly. Specifically, the blade has a variation of 35º, which is the maximum total arc swept by the blade. Along the simulation process, both geometries will be used. 4.2 Workbench setup The first thing to define will be the material properties. Since the real material the system is made out of is steel, a good approximation will be to use one of the predetermined Ansys Workbench materials: structural steel. This is a steel with generic properties that can be adapted to many different uses. Some of its more important mechanical properties are found in table 1. Material Property Value Density 7850.0 kg/m3 Young’s modulus 200 GPa Poisson’s ratio 0.30 Tensile ultimate strength 460 MPa Tensile yield strength 250 MPa Table 1: Basic material properties of Ansys’ structural steel. The next step is to define the contacts. Starting off with the basic bonded contacts, the following are set up: Mechanical study of the regulation system of a Kaplan turbine blade pag. 31 Figure 25: Bonded contacts with the base of the regulation system. The first set of contacts is between the base and the piston and the base and the screw. These two are bonded pairs since they can be regarded as a single body, they don’t move with respect to each other. In the case of the screw-base contact, in reality it is put in place by means of a nut, which has been neglected in this analysis due to the possibility of defining such contact. Figure 26: Other bonded contacts between the blade and internal connection parts. Next, in figure 26, more bonded contacts are defined. As seen in the pictures, these parts are designed with the idea of being assembled using screws and nuts, but, as in the previous case, they have been eliminated from the model. The bonded contact substitutes these connections. Moving on to the link between the base and the blade section, many contacts have to be carefully pag. 32 Antoni López Pérez defined, since this is the more complex part of the system (regarding the simulation creation and the following analysis). First, a bonded contact has to be created between the external surface of the pin and the internal surface of the cover. The external surface of said cover has to be able to rotate with respect to the screw with a specific frictional coefficient and, thus, a frictional contact is defined. Figure 27: Defined contacts of the pins and pin covers. Bonded contact (left) and frictional contact (right). For this and every frictional contact, a friction coefficient of 0.6 is applied [25]. The friction coefficient depends on the materials of both involved surfaces so, since every surface is made out of the same structural steel under the same conditions, the coefficient of friction can be considered to be always the same. Next, a no separation contact is created between the link bars and the extreme of the pin. This contact will prevent the parts from separating but will allow some sliding between them, as mentioned in previous sections. Mechanical study of the regulation system of a Kaplan turbine blade pag. 33 Figure 28: No separation contact definition between the pins and the link lateral bars. To end up with the link parts, frictional contacts are defined between the lateral bars’ interior faces and the pin and screw faces that are in contact with them. Figure 29: Frictional contacts at the link lateral bars. It should be noted that all the contacts defined for the second pin and for the other side of the link are analogous to the ones shown in the pictures above. The next step is to define the joints, starting off with a fixed one between the ground and the pag. 34 Antoni López Pérez middle part. This part will not move at all and act as a reference point. Figure 30: Joint used to fix the system to the ground. A translational joint is also defined between the middle part and the piston. Figure 31: Translational joint that allows the piston to move vertically. To define a joint like this one, the reference system has to be taken into account. By default, the creation of this joint creates as well its own secondary reference coordinate system, and allows longitudinal movement along the X axis of such reference. In case the definition doesn’t match the real movement of the joint, it has to be changed. The last joint is the one that allows the rotation of the blade. To do so, a revolute joint is defined between the ground and the ring on top of the cylindrical piece that connects with the blade. For this joint, the reference system has to be taken into account, in a similar manner as the previous example. In this case, what needs to be determined is the axis of rotation of the joint. Mechanical study of the regulation system of a Kaplan turbine blade pag. 35 Figure 32: Revolute joint that allows the blade to rotate. The contact should ideally be defined with the middle part but its geometry is not perfectly round shaped, so the joint cannot be correctly defined. However, since that part is fixed to the ground, the same result is achieved by creating a body-ground joint. Once all contacts and joints have been correctly defined. The mesh has to be created. The default element size is 0.3872 m which is really high, especially for the areas where the stress concentration will be higher. Since most parts of the system will have negligible stresses, the idea would be to have a general coarser mesh with an element size of the order of the default one (slightly shorter to improve precision) and then create a refinement of the critical areas. However, after multiple unsuccessful attempts (see section 6), it was decided to have just a general mesh with higher definition (element size 0.03m), sacrificing a lower computational power for simplicity and for the simulation to be able to work. The following step is to define the loads and boundary conditions that affect the system. First, standard Earth gravity is applied, since it will always have some effect. Figure 33: Definition of the gravity. Afterwards, the pressure on the blade is applied. When the turbine is generating power in standard operating conditions, it will always be underwater, thus being under the effect of the pag. 36 Antoni López Pérez pressure it generates. The value of this pressure has been provided by the director and was computed on a separate study by means of a computational fluid dynamics (CFD) simulation of the same turbine. The imported pressure values are the ones that the blade would have in maximum opening position. Thus, that specific geometry will be used to better represent the actual situation. To apply it to the current simulation, two new pressures have to be defined and applied to the geometry of the blade, one for the pressure side (the upper surface of the blade) and another for the suction side (the lower surface). These pressures will be imported using the external data option and then connected to the setup of the static structural analysis. Figure 34: Connection of external data files to the main analysis. The pressure distributions are supposed to be defined on top and bottom of the blade, respectively. But, as they come from another simulation, some linear transformations have to be made to place them correctly. Basically, the origin location can be moved by changing its coordinates along the three main axes, as well as its orientation, which can be changed by applying a specific rotation on a certain axis. After trying out multiple combinations of these rigid transformations, the final results are the ones shown in figure 35. Figure 35: Rigid transformations applied to the imported pressure distributions. Mechanical study of the regulation system of a Kaplan turbine blade pag. 37 The representation of the pressures on the blade look as follows: Figure 36: Imported pressure on the pressure side. Figure 37: Imported pressure on the suction side. The last boundary condition to be defined is the one that will cause the piston to move, causing in turn the blade to rotate. This condition can be set up as a force / pressure on the piston or as a displacement. The latter will be chosen for the simplicity of the computations and for some useful properties it possesses. For instance, a special probe can be created to measure the force needed so that the displacement boundary condition holds. Also, a displacement is more easily controlled: if a force is applied it’s harder to predict at first how the system will behave, or even if the magnitude is reasonable. By using a displacement condition, the piston will always move reasonably, as we can expect from the real life system. pag. 38 Antoni López Pérez Figure 38: Displacement condition applied on the top surface of the piston. As seen in figure 38, the displacement is defined on the top surface of the piston (any surface with the same orientation would also be right). The displacement is defined as a vector since the only position change required is the displacement in the Z axis (the vertical one). Once every load and restriction is applied, the simulation can be run. Mechanical study of the regulation system of a Kaplan turbine blade pag. 39 5 Analysis of the obtained results The main results of the project are the simulation itself and the stress analysis. To see if the simulation works, a first step is to check whether, once a nonzero displacement is applied, the rest of the system moves accordingly. Applying a displacement of -0.2 m in the Z axis (the piston moves 200 mm downwards), the system moves as shown in figure 40. Figure 39: Correct movement check for the final simulation: undeformed figure. Figure 40: Correct movement check for the final simulation: total deformation. The displayed results correspond to a total deformation view, including movement and strain. In this case, however, the variations correspond mostly to deformation by movement. The center of the blade and the fixed part of the system are represented in dark blue, which make sense since they don’t move. pag. 46 Antoni López Pérez 6 Difficulties encountered in the simulation process The process of building the simulation from the ground has been difficult due to some challenges encountered that have caused the need to run uncountable variations of the simulation to find the correct set of specifications that would make it work. After all this process, here is a list of some of the challenges that have been overcome to get to the final result. •Definition of the boundary conditions of the link: the link that joins the base of the regulation system and the blade section has many different parts that are in contact and that move with respect to each other, so the contacts and joints definition is very sensitive in this area, since an error may cause the simulation to fail. Many tests were carried out with smaller sets of parts to make sure that the movement between them was correctly defined. Also, some settings that in principle should have worked, didn’t or simply consumed too much computational power, creating never ending simulations. •Time consuming simulations: performing finite element simulations can be very time consuming. This has been a constraint all along the process since, if the computer is carrying out the simulation, it cannot work on anything else (workbench related) simultaneously. The real problem, though, have been simulations that took a very long time to get executed (up to three hours) and then failed, having caused a huge time loss. •Adjusting location of imported pressure: as mentioned before, pressure distribution values from another simulation have been used, creating the need of being placed correctly over and under the blade. To do so, a long manual process of trial and error was done to get the position as close as possible to the real one. The results were, however, successful. •Results display misrepresentation: the results display options are usually accurate but, in certain cases they can lead to very misleading conclusions. During one of the final simulations that were carried out, the total deformation was so low (very close to zero) that even the tiniest deformation was represented as huge. The link bars were shown to deform almost to the point of bending inwards for a situation where they shouldn’t have moved at all. Fortunately, this issue was spotted and disregarded in time not to change many things that, in the end, were correctly set up. Mechanical study of the regulation system of a Kaplan turbine blade pag. 47 7 Planning The project has been developed according to the different stages and tasks shown in the Gantt diagram below. The parts in blue are already completed at the current date (June 25th), and the ones in orange are yet to be done. The project started on February 9th and is considered to end on July 10th, the day of the final presentation. Figure 47: Gantt diagram of the project development. Source: Own. As seen in the diagram, the first part consisted on doing some preliminary research on the topic of the project, mainly on the functioning principles of Kaplan turbines and hydroelectric power plants in general. It is also included in this phase the more in-depth documentations, as in reading the most important scientific papers related to the topic. The next phase is the getting familiarized with the Ansys Workbench environment part. Here is included the documentation on the program (explanations, tutorials, etc), as well as the first test conducted (explained in section 3). The longest task is the development of the final simulation, which was the complex. Result extraction started before the completion of the final simulation because during the process some interesting conclusions were extracted. The final tasks are the elaboration of the report (which ends in week 20) and the preparation of the final presentation (which is set to finish at the presentation day). pag. 48 Antoni López Pérez 8 Economic assessment To economically assess the project, the cost of different items that have been a part of it have to be analyzed: •Software licences: in this project Ansys Workbench and Solidworks have been used. The Ansys license has a different price depending on the needed working packages. In the case of the ones used in this project, the licese price is 22,000 $/year [26] which, with the current EUR/USD exchange rate (1.0725 USD/EUR), is 20,512.82 €/year. The solidworks license cost is 3495 €/year [27]. •Electricity cost: the total working time of this project has been of 360h. It can be considered that during that entire time electricity has been consumed to power the computer used. The laptop consumption is of 50W [28] so, if it has been used for 360h, the total consumption is 18 kWh. Also, a complementary computer has been used to perform the simulations and the time it has been working can be regarded as being the same of the laptop. A bigger computer (also executing some power consuming simulations) has a consumption of 400 W [28] so, its total consumption is 144 kWh. The total electricity consumed is 168 kWh. The mean price of electricity during the period the project has been developed in, is 99.142 €/MWh [29], number obtained by computing the mean value of the prices from February 2024 to June 2024. The total cost of electricity is, therefore, an amount of 16.66 €. •Labour: the last significant cost to be analyzed is labour. For 360h, with a rate of 15 €/h (value extracted from the school’s thesis guide), the total labour cost is 5400 €. Adding up the different terms, the total cost of the project has been of 29,424.48 €. Considering the corresponding 21% VAT, the total cost considering taxes is 35,603.62 €. Mechanical study of the regulation system of a Kaplan turbine blade pag. 49 9 Environmental assessment For the environmental assessment of the project have to be considered the elements involved in the development process that have an environmental impact. Overall, the only thing that could have a significant effect on the environment is the electricity consumed. As mentioned in the previous section, the amount of electricity consumed has been computed by taking into account the hours of use of both computers used. To recall the values, a laptot has been used that has consumed 18 kWh, and an external computer has been used to performed the simulation which has consumed 144 kWh. The total consumption is 168 kWh. Every energy consumed has a CO2 emission associated due to the electricity generation process. In Spain, every kWh of electricity consumed is associated with the emission of 0.246 kg of CO2 [30]. This implies that, due to the electricity consumed during the develompent of the project, 41.328 kg of CO2 have been emitted. This is equivalent as the CO2 absorbed by two trees as they fully grow (as mentioned in the school’s thesis guide). Despite the fact that the environmental impact could be reduced (by performing least simulations, for instance), it is a reasonable value, especially since only electricity is consumed and no any extra materials that could have a significantly worse impact. The project itself could, however, have a futur very positive impact, since the correct application of the results and use of the simulation to analyze the turbines, could lead to a better and more effective use, thus producing more renewable energy and preventing emissions associated with fossil fuel electricity generation to occur. pag. 50 Antoni López Pérez 10 Social and gender equality assessment Throughout the development of the project, the focus has always been on its scientific and technical aspects, while any relation with people that can lead to any kind of discrimination by social status or gender has been completely negligible. Regarding the scientific papers used, all evaluations and decisions have been grounded solely in scientific and technical criteria as well. This deliberate focus ensures that assessments are based exclusively on the quality and merit of the work itself, without any influence from the gender, social status, or personal characteristics of those involved. Even though everything created by someone is, by definition, somewhat subjective, the author has tried to focus as much as possible on science and results, excluding from the project any personal bias or prejudice. The report has been written with the intention of using an inclusive and non-sexist language. Finally, to try to provide a deeper analysis the team that has developed the project can be assessed. The team consists of the author and the supervisor, both of whom are men. This result is, however, not significant since the population sample is so small (only two people). A further study could be derived from this conclusion, though, on the amount of men currently working as professors at the school in contrast with the amount of women, as well as the percentage of male students in scientific and technical related bachelors. This topic is, however, out of the scope of this analysis. Mechanical study of the regulation system of a Kaplan turbine blade pag. 51 11 Conclusions Throughout this project, the runner blade regulation system of a Kaplan turbine has been studied by means of a numerical analysis simulation. The importance of this topic lies on the increasing consumption and demand of hydroelectric power in the entire world, due to the impact fossil fuel generated electricity have on the environment. Specifically, the Kaplan turbine is used to help regulate the grid frequency and the increase in their use can lead to failure in their regulation systems. A numerical simulation has been created using Ansys Workbench to perform a stress analysis on the regulation system. The simulation has been proven to work correctly and has yield some interesting results. To start moving the piston, a force of 188.38 kN has to be applied (753.52 kN if the four blades are considered). A force at least equal to this one has to be applied to put the piston in the desired position, thus rotating the blade to increase the turbine’s efficiency. Regarding the stress, the critical point is found in the bottom pin of the link part: In this pin, due to the strain caused by the force applied and the friction between the different pieces, the stress concentration is the maximum. Therefore, this is the area most likely to cause failure if too much stress is caused. The stress found in the pin depends on the force applied, the friction coefficient of the material and the displacement of the piston. In the simulation environment, huge variations in stress can be found if the type of contact between the lateral bars of the links and the pins are applied. This happens because, for different contacts, different restrictions are defined and some of them are responsible for a higher stress value. High concentrations of stress are also found in the top pin cover. Despite these stresses being disregarded as a singularity, they need to be monitored in future simulations, to further analyze the critical conditions of the system. The maximum stress in the pin is 51.67 MPa, a value that, using an S-N curve of the material, is found to be in the infinite life section. Although this result could be considered plausible due to the long lifespan of the turbines, a more in-depth analysis should be conducted by correctly applying the Rainflow-counting algorithm. Finally, it is worth noting that, now that the simulation is created, the regulation system that has been studied can be analyzed in different working conditions. This means that, if a change in the operation of the turbine is forecast, it can be analyzed following the steps defined in this project to predict whether the turbine will fail or not. pag. 52 Antoni López Pérez References [1] U.S. Department of Energy. Types of hydropower turbines, 2024. Accessed: 2024-06-10. URL: https://www.energy.gov/eere/water/types-hydropower-turbines. [2] Berat Kavurmaci, Kutay Celebioglu, Selin Aradag, and Yigit Tascioglu. Model testing of francis-type hydraulic turbines. Measurement and Control, 50:70–73, 04 2017. doi:10.1177/ 0020294017702284. [3] Felix Ishola, Oluwaseun Kilanko, Timilehin Sanni, Adelakun Adebiyi, Dunmininu Adegoke, and A. Inegbenebor. Design and performance analysis of a model pico size pelton wheel turbine. International Journal of Civil Engineering and Technology, 10:727–739, 05 2019. [4] ElProCus. Kaplan turbine, 2024. Accessed: 2024-06-17. URL: https://www.elprocus. com/kaplan-turbine/. [5] Julian Somberg, Prabakaran Saravanan, Hari Vadivel, Kim Berglund, Yijun Shi, Jan Ukonsaari, and Nazanin Emami. Tribological characterisation of polymer composites for hydropower bearings: Experimentally developed versus commercial materials. Tribology International, 162:107101, 05 2021. doi:10.1016/j.triboint.2021.107101. [6] David Valentín, Alexandre Presas, Mònica Egusquiza, Jean-Louis Drommi, and Carme Valero. Benefits of battery hybridization in hydraulic turbines. wear and tear evaluation in a kaplan prototype. Renewable Energy, 199:35–43, 2022. URL: https: //www.sciencedirect.com/science/article/pii/S0960148122012927,doi:10.1016/j. renene.2022.08.117. [7] Springer. Hydropower plants: A review, 2024. Accessed: 2024-06-17. URL: https:// link.springer.com/chapter/10.1007/978-981-16-5655-2_73. [8] XFLEX HYDRO. Xflex hydro: Making flexible hydropower a reality, 2024. Accessed: 2024- 06-25. URL: https://www.xflexhydro.com/. [9] European Commission. Hydropower, 2024. Accessed: 2024-06-05. URL: https://energy. ec.europa.eu/topics/renewable-energy/hydropower_en. [10] Fundación Endesa. Central hidroeléctrica, 2024. Accessed: 2024-06-05. URL: https://www.fundacionendesa.org/es/educacion/endesa-educa/recursos/ centrales-renovables/central-hidroelectrica. [11] Enel Green Power. Advantages of hydroelectric energy, 2024. Accessed: 2024- 06-05. URL: https://www.enelgreenpower.com/learning-hub/renewable-energies/ hydroelectric-energy/advantages. [12] Dr. M. S. Hebbal and Mukunda Dabair. Static structural, modal and harmonic analysis of alloy car wheel rim using ansys workbench. International Journal of Engineering Research & Technology (IJERT), 8(7), 2019. [13] Repsol. Hydropower plant, 2024. Accessed: 2024-06-10. URL: https://www.repsol.com/ en/energy-and-the-future/future-of-the-world/hydropower-plant/index.cshtml. Mechanical study of the regulation system of a Kaplan turbine blade pag. 53 [14] U.S. Department of Energy. Types of hydropower plants, 2024. Accessed: 2024-06-10. URL: https://www.energy.gov/eere/water/types-hydropower-plants. [15] Renewables First. Kaplan turbines - hydropower learning centre, 2024. Accessed: 2024-06-05. URL: https://renewablesfirst.co.uk/renewable-energy-technologies/ hydropower/hydropower-learning-centre/kaplan-turbines/. [16] Testbook. Kaplan turbine, 2024. Accessed: 2024-06-05. URL: https://testbook.com/ mechanical-engineering/kaplan-turbine. [17] Energuide. Why does the electricity grid have to stay in balance?, 2024. Accessed: 2024-06-06. URL: https://www.energuide.be/en/questions-answers/ why-does-the-electricity-grid-have-to-stay-in-balance/2136/. [18] Nano Energies. Frequency control reserve (fcr), 2024. Accessed: 2024-06-06. URL: https: //nanoenergies.eu/knowledge-base/frequency-control-reserve-fcr. [19] Wikipedia contributors. Finite element method, 2024. Accessed: 2024-06-07. URL: https: //en.wikipedia.org/wiki/Finite_element_method. [20] SimScale. Finite element method: Applications of fea, 2024. Accessed: 2024-06- 07. URL: https://www.simscale.com/blog/what-is-finite-element-method/ #applications-fea. [21] FreeCAD. Fem element types, 2024. Accessed: 2024-06-08. URL: https://wiki.freecad. org/FEM_Element_Types. [22] ANSYS. Ansys workbench, 2024. Accessed: 2024-06-09. URL: https://www.ansys.com/ products/ansys-workbench. [23] Yasin Çapar. Contact types and behaviours in structural analysis. https://yasincapar. com/contact-types-and-behaviours-in-structural-analysis/, 2024. Accessed: 2024- 06-21. [24] Power Technology. Power plant profile: Vogelgrun, france. https://www. power-technology.com/data-insights/power-plant-profile-vogelgrun-france/, 2024. Accessed: 2024-06-21. [25] The Engineering ToolBox. Friction coefficients, 2011. Accessed: 2024-22-05. URL: https: //www.engineeringtoolbox.com/friction-coefficients-d_778.html. [26] Vondran Legal. How much does an ansys software license cost, n.d. Accessed: 2024-06-24. URL: https://www.vondranlegal.com/ how-much-does-an-ansys-software-license-cost. [27] CIMworks. Precios solidworks 3dexperience, n.d. Accessed: 2024-06-24. URL: https: //www.cimworks.es/precios-solidworks-3dexperience/?gad_source=1&gclid= Cj0KCQjwsuSzBhCLARIsAIcdLm6JnMiHhaZ1gyG_CSIHvJeCyVYl5rG1cjZI0IiCGnF1iSm-y_ XLFg4aAhNuEALw_wcB. [28] EnergySage. How many watts does a computer use, n.d. Accessed: pag. 54 Antoni López Pérez 2024-06-24. URL: https://www.energysage.com/electricity/house-watts/ how-many-watts-does-a-computer-use/. [29] Precio de la Luz. Precio por meses, n.d. Accessed: 2024-06-24. URL: https:// preciodelaluz.com/precio-por-meses. [30] Energreen Spain. ¿qué cantidad de co2 se previene con el uso de energía solar fotovoltaica en españa?, n.d. Accessed: 2024-06-24. URL: https://energreenspain.com.