CFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE
|
|
- Kelly Campbell
- 5 years ago
- Views:
Transcription
1 CFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE 1st Author name : SHIVAKUMAR VASMATE, 2nd Author name : KAMALADEVI ANANDE. 1 Department of Mechanical Engineering, India 2 Department of Civil Engineering, India ABSTRACT Steam Turbines play a vital role in power generation as a prime mover which converts kinetic energy of steam into mechanical energy. Many of the utility steam turbines is the combination of three cylinder construction i.e. High pressure cylinder in which pressure is maximum with minimum specific volume and so blade height is minimum, Intermediate pressure cylinder in which pressure is intermediate and so is the blade height and finally low pressure cylinder which has a minimum pressure level and maximum specific volume and hence maximum blade height. Generally, IP Steam turbine consists of 12 stages; combination of 1-7 stages and 8-12 stages which are divided by the use of the extraction strip. A typical Intermediate Pressure cylinder module is chosen to carry out the project work. The flow in a Turbine blade passage is complex and involves understanding of energy conversion in three dimensional geometries. The performance of the turbine depends on the efficient conversion with minimum amount of flow losses. To improve the performance it is essential to identify the losses generating mechanism and study their influence and effects on performance. The objective of the project is to carry out the CFD analysis of a typical IP utility turbine module considering the hub/shroud sealing between the stages which account for leakage losses. To achieve the above objective we need to model separately the bladed region and attach the hub/shroud seal region to it by General Grid Interface. The flow domain and mesh generation for seal area needs to be accurate to get the correct interface with blades. IDEAS software is used for geometric modeling, CFX-TURBOGRID software is used for meshing the blade region, ICEM-CFD software is used for meshing the hub/shroud region of the seals and CFX is used for physics definition and solving the problem. Initially the analysis is carried out for the 8th stage, subsequently for the combined 8-12 stages. The results are compared with two dimensional (2D) analysis calculations and found. Keywords-Steam turbine, Hub/shroud, General Grid Interface (GGI), IDEAS software, CFX TURBO-GRID software, ICEM-CFD software, CFX software Page 21
2 I. Introduction BHEL is manufacturing a wide variety of turbines over the last 50 years to meet India s growing need for power. Steam turbine plays a vital role in power generation as a prime mover, which converts Kinetic Energy of steam to Mechanical Energy. Many of the utility steam turbines are of three cylinder constructions i.e. High pressure cylinder in which pressure is maximum with minimum specific volume and so blade height is minimum, Intermediate pressure cylinder in which pressure is intermediate so the blade height is intermediate and Low pressure cylinder which has a minimum pressure level & maximum specific volume and hence LP cylinder blade height is maximum. A typical Intermediate pressure Turbine of utility steam turbine is chosen to carry out the CFD analysis. The analysis requires solving of fluid problem in bladed region. This can be done in three approaches, Analytical, Experimental and Numerical. Analytical methods which assume a continuum hypothesis are more suited for simple problems and are not suited for complex fluid flow problems. Experimental methods are suited for complex fluid flow problems but the expenditure for carrying out the analysis is high. The other limitation is that the determination of the fluid characteristics in the interiors becomes complex and difficult. Hence, Numerical approach is more feasible approach for analysis of a particular design because it overcomes the limitations of the two methods and it gives a close approximate for complex form of fluid problems too. Numerical approach involves discretization of the governing mathematical equations gives numerical solutions for the flow problems. The analysis is carried out by identifying the flow domain. The domain is modeled, discretized and governing equations are solved using commercially available software. The results are post processed and compared with 2 dimensional program results which were experimentally verified. A. Elements of Steam Turbine: The bladed region of Steam Turbine consists of the following as shown in Fig 1 1. Stationary Blades. 2. Moving Blades. 3. Labyrinth Seals. Fig1. Elements of Steam Turbine. Page 22
3 B. Aerofoil Blades: An aerofoil blade is a streamlined body having a thick, rounded leading edge and a thin trailing edge in order to achieve a high lift-drag ratio. Its maximum thickness occurs somewhere near the midpoint of the chord. Both the stationary and Rotating blades should be designed such that it should be capable of obtaining the desired pressure drop and turning towards the tangential direction between the driving surface and trailing surface of the vane passage, so that the flow comes out of the stationary blade with a desired velocity both in magnitude and direction. The exit flow will have high velocity with a high tangential component. Thus the flow enters axially in the stationary as well as the moving blades and both the tangential force and torque exerted by the fluid jet on the following rotating blade row depends on the change in the tangential velocity of the fluid. The blade with respect to turbine axis and blade nomenclature is shown in Figure 2 and Figure 3 respectively. Fig 2.blade with respect to turbine axis. Fig 3. blade nomenclature. Page 23
4 C. Labyrinth Seals: The provision of seals is necessary to minimize the leakage whenever there is a clearance between a moving and a stationary part with pressure difference across the clearance. In a steam turbine seals are provided at the two turbine ends where the shaft is taken out of the casing, at the clearance between the diaphragm and the rotor of an impulse stage and on the blade tips when provided with shrouds. Mostly the labyrinth and strip type of seals are used in the turbo machines. The number of strips used and their arrangement depends upon the pressure difference across the clearance and the basic construction arrangements used for sealing the diaphragm are shown in figure 4 and these are generally known as Labyrinth seals. The flexible type of labyrinth seals used on diaphragms of the high pressure stages are as shown. Tip seals to the turbine stage in the CFD models are used for the more accurate stage performance predictions. Fig 4. : Flow Domain at Labyrinth Seal II. Methodology A. Problem Solving Approach in CFD: The basic steps involved in solving any CFD problem are as follows: 1. Identification of flow domain. 2. Geometry construction or Component Modeling. 3. Grid generation. 4. Specification of boundary conditions and initial conditions. 5. Selection of solver parameters and convergence criteria. 6. Results and post processing. The IP Utility Steam Turbine is modeled and analysis is carried out by following steps Page 24
5 1. Identification of Flow Domain: Before constructing grid, it is required to understand the exact flow domain properly. The flow domain in the case of Steam Turbine consists of blade path (both Stationary and Rotating blades fixed to casing and rotor respectively), Labyrinth seals, and steam inlet & outlet. It is therefore required that before going ahead with 3D modeling and grid generation, the common interfaces should be clearly defined between each blade in each stage and seals. The software that is used for generating the geometry and meshing is decided based on nature and complexity of the geometry. For axi-symmetry bladed geometry, the data for hub, shroud and blade profiles are obtained from 2D drawing and subsequently grids are generated using Turbo-Grid software. Though the stage consists of Stationary and Rotating blades, but to get the flow developed to the upstream of the hub a small passage is added and similarly to the downstream of the shroud the flow domain is extended up to some distance, so that realistic boundary conditions can be given at the inlet and outlet surfaces. The boundary wall is the region where no slip condition exists and the velocity gradually increases and reaches to mainstream velocities. That means, velocity gradient exists there and that region close to the boundary wall should have fine grids to capture the boundary wall effects. 2. Geometrical Modeling: In order to analyze the flow and to evaluate the performance, basically three steps are required as follows: 1. Modeling of components. 2. Grid generation. 3. Analysis. 4. As the flow domain consists of blade and seal passages, the modeling is carried out as described below: 1.1. Geometrical Model of Blades: The blade of the Utility IP Steam Turbine is of cylindrical type and blade extends between hub and shroud surfaces. The geometry of blade is extracted from blade profile co-ordinates are shown in figure 5.1 and figure 5.2, given in the form of suction side and pressure side points, which are located along the radial positions of the blade. Page 25
6 Fig 5.1: 8th Stage Guide Blade Fig 5.2: 8th Stage Moving Blade The point data is arranged in order to obtain blade profiles from hub to shroud. IDEAS software is used to generate the solid model, and generally we will be saving the points data in ASCII (.curve) file format for convenience of grid generation of blades directly in ANSYS TurboGrid Software. This process requires some programming skills which have been done in Microsoft Excel sheet using some formulae. 1.2 Geometrical Model of Seals: Labyrinth seals are attached at the hub and shroud surface of the blades to reduce the leakage flow. Modeling of seals has been done in IDEAS by extracting the data from the AutoCAD drawing is shown in figure 6. A typical cross-section drawing is shown below for guide blade. By extruding the seals in either of the directions then the solid model of the seal with the required length is obtained and is shown in figure 6.1. Flow domain Strips Fig 6 Two Dimensional views of Seals Page 26
7 Figure 6.1. Fluid model of the Seals (Hub & Shroud) 2 Grid Generation of Blades using CFX-TurboGrid: The flow inside a Steam turbine passes through the bladed and seal passages, which can be described as periodic passages. Geometrically these passages are rotationally periodic about its axis of rotation. For the CFD analysis, it is assumed that the flow is also rotationally periodic in these passages. Therefore, the flow computation can be made in one of the periodic passage while applying periodic boundary conditions at periodic interfaces. For the purpose of flow domain discretization, one blade passage is considered for 3D-grid generation. The tool used for grid generation is CFX-TURBOGRID software package for the stator and rotor blade passages. Input to this software is given by three Data files namely, hub.curve, shroud.curve, and profile.curve. These files contain the hub, shroud and profile curve data files in global Cartesian coordinates or cylindrical form. Page 27
8 Input Format for Turbo Grid CFX-Turbo grid requires three input data files (profile, shroud and hub) to define the path and blade geometry. Hub Data File The hub curve runs upstream to downstream and must extend of the blade leading edge. The hub data file contains the hub curve data points in Cartesian form and downstream of the blade trailing edge. The profile points are listed, line-by-line, in free format ASCII style in order from upstream to downstream. These data points are used to place the nodes on the hub surface, which is defined as the surface of revolution of a curve joined by these points. Shroud Data File The shroud data file contains the shroud curve data points in Cartesian or cylindrical form the shroud curve runs upstream to downstream and must extend upstream of the blade leading edge and downstream of the blade trailing edge the points are listed, line by line in free format ASCII style in order from upstream to downstream. These data points are used to place the nodes on the shroud surface, which is defined as the surface of revolution of a curve joined by these points. Example: Considering XZ Plane with X as Axis of Rotation is shown in figure 7. Shroud.Curve Hub. curve Hub.curve Shroud.Curve Fig 7: Hub Curve and Shroud Curve Page 28
9 Profile Data File: The profile data file contains the blade profile curves in Cartesian or cylindrical form. The profile points are listed, line-by-line, in free format ASCII style in a closed loop surrounding the blade. The blade profiles should lie on a surface of revolution to facilitate transformation to m-prime, theta conformal space. A minimum of two blade profiles are required, one which lies exactly on the hub surface and one which lies exactly on the shroud surface. The profiles must be listed in the file in order from hub to shroud. Multi bladed geometries are handled by placing multiple blade profile definitions in the same profile. Example for Profile.curve: # profile # profile Single blade fluid Passage Fig 8: Single bladed Passage after using profile.curve Page 29
10 The first step is to check whether the blade profile data obtained from solid model is intersecting hub and shroud curves or not. We use CFX-Turbogrid intersect option for this purpose. Using this option, we have to see that blade profile must lie on the surface of revolution of hub and shroud as shown in fig 8. Turbo grid intersecting capability can convert an existing set of blade profiles that does not necessarily lie on the surface of revolution into one that can be used in a CFXTurbogrid template. Next step is generating grid. Among the various templates available in turbogrid, Multi Block Grid template as shown in figure 9 is used. By the way of adjusting control points in figure 10 a good quality hexahedral grid can be generated. Flip topology is used to correct negative grid volume due to left-handed system. The Create command not only creates grid but also calculates and displays the minimum and maximum skew angle in the grid and the node at which it occurs. The View command in the GUI window can be used to see the different views of the grid like Cartesian view, Meridional view and blade-to-blade view as shown in figure 13. Shroud.curve Profile Curve Hub.Curve Fig 9: Template of 3D Blade in Turbo-Grid In the above template shown in figure 9 is a 3D blade in Turbo-Grid, the right side view shows the blade-to-blade view of the blade and the left view shows the mesh statistics of the blade. Page 30
11 Trailing edge Control Periodicity Control Topology - H-Grid and O-Grid Leading edge Control Points Control Nodes Fig 10: Adjusting the control points at the Leading Edge & Trailing Edge Shroud surface Hub surface Fig11. Circumferential View of Guide Blade Surfaces Fig12. G8 Guide Blades periodically arranged throughout the circumference Page 31
12 The mesh generated by adjusting the control points as shown in Figure 10 and correspondingly Circumferential view of guide blade surfaces & Periodical arrangement of blades throughout the circumference which differ for different stages are shown in Figures 11 and 12. A Cartesian view is also in figure 13. Cartesian View Fig13. Views for 8th Stage Guide Blade The following parameters were considered to check the quality of the grids: Skew angle: It is defined as the internal angle of the octahedron. Ideally, all the angles should be equal to 90 degrees to get a perfect orthogonal grid. However, for practical purposes, the grid is considered to be of high quality if the minimum skew angle is not lower than 15 degrees and the maximum skew angle is not greater than 165 degrees. Grid volume: Negative volume meant overlapping of adjacent grids, which would lead to errors in solver. Care was taken to ensure that there was no negative volume in the grids. Aspect ratio: It is defined as the ratio of the longest side to the shortest side. Its minimum value is 1. For good quality grid creation, the maximum aspect ratio should be less than 200. Page 32
13 The mesh is generated for the stator and rotor blades with the total number of nodes, maximum and minimum skew angle and aspect ratio obtained from TURBOGRID are given in Table 1. TABLE 1: MESH DATA FOR COMPONENTS OF 8th STAGE BLADES S.No Number Component Number of Aspect Hexa Ratio Nodes Elements (Max) of Orthogonality angle (Min) 1 Stator Blade (G8) 2 Rotor Blade (M8) 5.4 Seals Meshing using ICEM-CFD:In a Steam Turbine Labyrinth or strip type of seals are invariably used. The flow domain of the seals is modeled in IDEAS from the 2D drawings and exported into ICEM CFD to generate the mesh. Before generating the hexahedral-mesh the geometry should be repaired in order to get no negative volumes and to get the better quality of the mesh. It is a semi-automated meshing module which present the rapid generation of multi-block structured or unstructured hexahedral volume meshes. In case of hexa meshing the structured volume meshes will be obtained. Blocks can be interactively adjusted by splitting it to the underlying CAD geometry and fitted internal or external, O-grids can be generated by the system automatically. The figure 14 and figure 15 are shown below the seal geometry and mesh generated using ICEM-CFD software. Page 33
14 G8 Seals (Hub and Shroud) G8 Seals with Hexa Mesh Fig 14. Seal Geometry and Mesh Generated for Guide blade M8 Seals (Hub & Shroud) M8 Seals with Hexa Mesh Fig 15. Seal Geometry and Mesh Generated for the Moving Blade Page 34
15 Above figure is hexahedral structured mesh for eighth stage moving blade (M8) generated in Ansys ICEM-CFD software. The lower part is called Hub and the upper part is known as Shroud. This is obtained by blocking, splitting, associating the points, curves etc; in order to get the mesh with required quality. The total number of nodes, maximum and minimum skew angle and aspect ratio obtained from ICEM-CFD are given in Table 2. TABLE 2: MESH DATA FOR 8th STAGE SEALS (HUB AND SHROUD) S.No Component Number of Number of Nodes Aspect Volume Hexa Ratio (Min ) Elements (Max) 1 G8 Seals 68,096 58, M8 Seals 71,864 60, ANSYS CFX: CFD analysis is carried out to understand the flow through the turbine, predict the pressure distribution and velocity profiles on the blades and predict the various losses. Ansys CFX-11 software tool is used for analysis purpose. The Analysis is carried out using CFX-Pre, CFXSolver and CFX-Post modules. Specification of boundary conditions and initial conditions: Specification of boundary condition of simulation is done in CFX-Pre processing. The files with the extensions:.grd,.gci,.bcf of Guide and Moving blades, also the files with having.cfx5 extension of seals of a IP utility steam turbine module are copied into a new folders separately and this grid file are read into pre-processing model of CFX-11 software. The complete softwares flow chart is shown below in figure 16. Page 35
16 IDEAS or MODELLING BLADES & SEALS AUTO CAD CFX TURBO_GRID BLADES GRID (MESH) GENERATION ANSYS ICEM_CFD SEALS PRE PROCESSING CFD ANALYSIS SOLVING ANSYS CFX 11.0 POSTPROCESSING Fig 16 SOFTWARES FOR COMPLETE CFD ANALYSIS Page 36
17 III Result and Discussion A. Results: The analysis is carried out in two stages. First, initially the analysis is carried out for the 8th stage and later combined analysis for all the 5 stages has been carried out. The stage analysis has been carried out for the turbine stages with the constant mass flow and it consists of stator, rotor, and seals. The various performance parameters like pressure, temperature distribution and velocity profiles on the blades, isentropic efficiencies, Power have been computed using the CFX Macros and with the help of Mollier Chart. As the eight stages consisting of Guide blade, Moving blade with a stage interface between the blades is simulated, and the solution is obtained with high resolution convergence up to 1e-5.The analysis is carried out with seals for 8th stage. The results obtained are discussed below: 1. Flow and performance parameters for 8th stag with seal: CFX-PRE Physics Definition (Stage8) Shroud Counterroating Wall Blade-Shroud Interface G8 Blade Periodicity M8 Blade Outlet G8 Guide Blade G8 Blade Inlet Inlet G8M8 Blade Stage Interface Blade-Hub Interface Hub Rotating wall Fig17. Boundary conditions for 8th Stage with Seals In the pre processing the following fluid domains and boundary conditions are shown in figure17 and specified for the eight stage analysis. 1. Simulation 2. Domains G8 blade & Seals M8 blade & Seals 3. Boundary Conditions: Inlet : steady state : Fluid type : 8th Guide blade with hub & shroud seals : 8th Moving blade with hub & shroud seals : Guide blade inlet Page 37
18 Outlet Inlet Mass Flow Inlet Static Temperature Wall Outlet Static Pressure Rotational Speed Reference pressure 4. Fluid Properties: : Moving blade outlet : kg/sec : K : smooth : bar : rpm : 0 bar Working Fluid Dynamic Viscosity Thermal Conductivity 5. Rotation Axis : Steam5 (Dry steam) : e-6 Pa s : W/m. ºc : X - Axis 6. Turbulence Model: Turbulence Model : Standard k-epsilon Model Heat transfer Model : Total Energy 7. Interface between Guide and Moving Blade: Type Frame Change Option 8. Pitch Change: : Fluid -Fluid : Stage Interface(G8M8 Blade stage interface) Option: Specified Pitch Angle Pitch angle side 1: Pitch angle side 2: B. Run the solver monitor. The solver is allowed to run till the required convergence is obtained in figure 18 Fig18. Solver run convergence. Page 38
19 C. POST PROCESSING: 1. Results which are obtained from the CFX macro for the Eighth stage User Input Inlet Region G8 blade inlet Outlet Region M8 blade outlet Blade Row Region M8 blade Default Reference Radius [m] Number of Blade Rows 115 Machine Axis X Rotation Speed [rev min^-1] Gamma 1.3 Reference Pressure 0 [Pa] 2. Mass Averages Quantity Inlet Outlet Ratio (Out/In) Temperature K K Total Temperature K K Pressure e+006 kg m^ e+006 kg m^ s^-2 s^-2 Total Pressure e+006 kg m^ e+006 kg m^ s^-2 s^-2 Page 39
20 3. Results Torque (one blade row) kg m^2 s^-2 Torque (all blades) kg m^2 s^-2 Power (all blades) e+006 kg m^2 s^-3 Total-to-total isen. efficiency Total-to-static isen. efficiency Streamline and vector plots for various parameters have been given for better understanding of flow through the stages. The Pressure Contour shows the pressure variation across the stage. It is clear from the Pressure Contour that the pressure drop occurs across the stage. The pressure is high at the beginning of the stage, decreases across the stage and is low at the exit of the stage. The Pressure Contour is useful to see the variation of pressure across the stage and modify the design if required to get uniform pressure drop. The Velocity Vector Plot shows the velocity variation across the stage is shown in figure 19. It can be seen from the Velocity Contour Plot that the velocity is minimum at the entry of the guide blade and reaches maximum at the exit of guide blade. Similarly for the moving blade also the velocity is minimum at the entry and maximum at the throat. Thus the velocity changes for each blade from minimum at entry to maximum at the throat. The Velocity Streamline Plot is useful to note the streamline motion of the Steam through the Stage. The Streamline motion is very useful to determine the proper flow of the steam through the stage. The proper design of the stage should have the continuous streamline motion of the Steam without any discontinuity. The Velocity Vector Plot is useful to draw the velocity triangles of the stage. The power output of the stage depends upon the velocity triangles. Thus the velocity vector is an important plot to decide the design efficiency of the stage. It is very important design the stage to get the required power output so the velocity vector plot is good indicator of the design of the stage. The Pressure Contour, Mach number Contour, Velocity Streamline and Velocity Vector Plots for 8 Stage with seals are shown below. th 4. Plots for 8th Stage with Hub & Shroud seals: Page 40
21 Fig19. 8th stage streamline vector plot Fig20. 8th stage Pressure contour plot Page 41
22 Fig21. 8th stage Temperature Streamline plot Fig22. 8th Stage Mach number Streamline plot Velocity Vector Profiles Above Mid-Span Below Mid-Span Fig23. 8th stage Velocity vector plot Page 42
23 5. Discussions: Streamline, vector and contour plots for various parameters have been given for better understanding of the flow through the stages. The variation of pressure across the stage is seen in Fig 20, it is a pressure contour plot which is a series of lines linking points with equal values of a given variable pressure. It is shown in the figure that the pressure goes on decreasing from entry to exit of the stage. At the entrance the maximum of bar is observed and a minimum of bar is obtained at the exit is obtained. The Contour plot for the variation of temperature across the 8th stage is shown in Fig 21. From the figure it is clear that the temperature is decreasing from the entry to the exit. At the entrance the temperature is maximum around K, and at the exit the temperature is minimum of K. Fig 22 shows the variation of Mach number across the 8th stage with seals. From the figure it is obvious that Mach number is increasing from the entry to exit and minimum Mach number of the order of occurred at the entrance of the guide blade and a maximum of is occurred at the interface of the guide blade and moving blade. Fig 23 shows the variation of the velocity across the eighth stage. This vector plot, which is a collection of vectors drawn to show the direction and magnitude of a vector variable on a collection of points are defined by arrows. From the figure it is obvious that the velocity is minimum at the entrance which is of 7.51 m/sec and maximum at the interface and at the exit of the stage which is around m/sec. 6. Comparison of CFD values and 2D Values: The CFD analysis results are compared with 2D program output. The program output is verified experimentally. The comparison chart of 2D values and CFD values for 8th stage are shown in the table 3. The values obtained show that the CFD values are closer to 2D program and are within the acceptable limits. Table3. Comparison of CFD values and 2D values. STAGE 8 WITH SEALS Description Temp inlet Temp outlet Unit 2D value CFD Value K K Page 43
24 Pressure inlet Bar Pressure outlet Bar Output Power MW CFX software provides a macro which computes the values of Steam properties like pressure, temperature, and enthalpy at Guide &moving blade inlet& exit. In addition to the above the torque on moving blades and power developed by the stage is also calculated. 7. Combined analysis: The combined analysis is carried out for the subsequent 5 stages consisting of large number of elements 17, 34,379 nodes with many General Grid Interfaces and stage interfaces with multiple frames of reference. IBM Cluster computing server with P615 processor is used to obtain the solution for the simulation using 4 processors with 2GB RAM each. The solution is converged with 1e-5 with high resolution. The results are as below. 7.1Flow and performance parameters for combined 5 stages with seals: Inlet Outlet: Average Static Pressure Fig24. Boundary conditions of Combined 5 Stage. 7.2 Run the solver monitor. Page 44
25 The solver is allowed to run till the required convergence is obtained in figure 25. Fig 25. Solver run convergence. 7.2 Plots for Combined 8-12 Stages With seal Fig26. Pressure Contour Plot in Pascal (pa) Page 45
26 The variation of pressure across the stage is seen in Fig26, which is a Pressure Contour Plot with series of lines linking stages with equal values of a given variable pressure. The variable values can quickly be associated with the colored regions of the plot. It is shown in the figure that the pressure goes on decreasing from entry to exit of the stage. At the entrance the maximum of bar is observed and a minimum of bar is obtained at the exit. Fig27: Temperature Contour Plot in Kelvin (K) The contour plot for the variation of temperature across 5 stages is shown in Fig 27. The assumption of steady state flow is assumed when a streamline is created, even with a transient simulation. From the figure it is clear that the temperature is decreasing from the entry to the exit. At the entrance the temperature is maximum around K and at the exit the temperature is minimum of K. Fig28 Velocity Streamline Plot in m/sec Page 46
27 Fig 28 shows the variation of the velocity streamline across the different stages. Here, the streamlines goes on decreasing as the stages passes, it is because of not proper alignment of the blades accurately as needed around its periphery. Fig 28 Mach number contour Plot Fig 28 shows the variation of Mach number contour plot across 5 stages. From the figure it is obvious that Mach number is increasing from the entry to exit and minimum Mach number of the order of occurred at the entrance of the guide blade and a maximum of is occurred at the throat of the guide blade and moving blade. Fig29 Velocity vector contour plots Page 47
28 Above Figure 29 shows the variation of the velocity across the each stage in the combined 5 stages. This a vector plot, which is a collection of vectors drawn to show the direction and magnitude of a vector variable on a collection of points and are defined by a location. From the figure it is obvious that the velocity is minimum at the entrance which is of m/sec and maximum at the throat of the stage which is around m/sec. 8. Comparison of CFD and 2D Experimental Values: The CFD analysis results are compared with 2D program output. The program output is verified experimentally. The comparison chart of 2D values and CFD values for 5 stages are shown in the table 4. The values obtained show that the CFD values are closer to 2D program and are within the acceptable limits. Table 4: Comparison of 2D value and CFD Value Stage 8 with Seals Description Units 2D Value CFD Value Mass Flow Rate Inlet Kg/s Temperature Inlet K Pressure Outlet Bar Specific Enthalpy Inlet KJ/kg Power MW Stage 9 with Seals Description Units 2D Value CFD Value Mass Flow Rate Inlet Kg/s Temperature Inlet K Pressure Outlet Bar Specific Enthalpy Inlet KJ/kg Power MW Stage 10 with Seals Description Units 2D Value CFD Value Page 48
29 Mass Flow Rate Inlet Kg/s Temperature Inlet K Pressure Outlet Bar Specific Enthalpy Inlet KJ/kg Power MW Stage 11 with Seals Description Units 2D Value CFD Value Mass Flow Rate Inlet Kg/s Temperature Inlet K Pressure Outlet Bar Specific Enthalpy Inlet KJ/kg Power MW Stage 12 with Seals Description Units 2D Value CFD Value Mass Flow Rate Inlet Kg/s Temperature Inlet K Pressure Outlet Bar Specific Enthalpy Inlet KJ/kg Power MW VI. Conclusions CFD study was carried out for evaluating the performance of a utility Steam Turbine IP Module. The flow in a turbine blade passage is complex and involves understanding of energy conversion in three dimensional geometries. The performance of turbine depends on efficient energy conversion and analyzing the flow path behavior in the various components IP Steam Turbine. Page 49
30 The CFD analysis of the turbine flow path helps in analyzing the flow and performance parameters and their effects on performance parameters like temperature, pressure and Power output. The Intermediate Pressure turbine consisting of 5 stages with cylindrical profiles used for stationary and moving blades. The blades are also designed with sealing strips between stationary parts and rotating parts to reduce leakage losses. The flow path of the turbine with blades and seals is modeled and meshed using different software s like IDEAS, ANSYS-ICEMCFD, ANSYS-TURBOGRID, etc. The mesh for the blade region is generated separately with ANSYS-TURBO-GRID and mesh for the seals are generated from ANSYS-ICEM-CFD and attached by General Grid Interface. The analysis is carried out for a single stage initially and subsequently for all the combined 5 stages. The combined analysis consists of large number of elements 17,34,379 nodes with many General Grid Interfaces and stage interfaces between multiple frames of reference. IBM Cluster computing server with P615 processor is used to obtain the solution using 4 processors with 2GB RAM each. The solution is converged with 1e-5 with high resolution. The results are analyzed for mass flow rates, temperature and pressure distributions on blades, power developed by stage and isentropic efficiency of the stage. The results are compared with TwoDimensional program validated by experimentally and found to be in agreement with the 2D analysis. The CFD analysis of the Intermediate Pressure turbine module has helped in predicting the turbine performance and comparing with experimentally verified values. V. References 1. C.W. Haldeman, R.M. Mathison; Aerodynamic and Heat Flux Measurements in a SingleStage Fully Cooled Turbine Part II, Journal of Turbomachinery, vol. 130/021016, April X.Yan, T.Takinuka; Aerodynamic Design Model Test and CFD Analysis for a Multistage Axial Helium Compressor, Journal of Turbomachinery, ASME paper,vol. 130/031018, July Arun K.Saha, Sumanta Acharya, Computations of Turbulent Flow and Heat Tansfer Through a Three-Dimensional Nonaxisymmetric Blade Passage, Journal of Turbomachinery, ASME paper, Vol. 130/031008, July Horloc, J.H., The Thermodynamics Efficiency of the Field Cycle, ASME paper, Vol. no. 57.A.44, Computational Fluid Dynamics, the basics with applications 6. Fluid Mechanics and hydraulic machines - John D. Anderson. Jr - Dr. R. K. Bansal 7. Numerical heat transfer and Fluid Flow - Suhas V. Patankar 8. Steam Turbine Theory and Practice - W. J. Kearton Websites: Page 50
31 Page 51
Introduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationNASA Rotor 67 Validation Studies
NASA Rotor 67 Validation Studies ADS CFD is used to predict and analyze the performance of the first stage rotor (NASA Rotor 67) of a two stage transonic fan designed and tested at the NASA Glenn center
More informationTurbocharger Design & Analysis Solutions. Bill Holmes Brad Hutchinson Detroit, October 2012
Turbocharger Design & Analysis Solutions Bill Holmes Brad Hutchinson Detroit, October 2012 Agenda ANSYS overview ANSYS TurboSystem Blade row solutions The ANSYS Transformation methods An example: turbocharger
More informationRAPID DESIGN AND FLOW SIMULATIONS FOR TUBOCHARGER COMPONENTS
EASC ANSYS Conference 2009 RAPID DESIGN AND FLOW SIMULATIONS FOR TUBOCHARGER COMPONENTS Authors Dipl.-Ing. Jonas Belz Dipl.-Ing. Ralph-Peter Müller CFDnetwork Engineering CFturbo Software & Engineering
More informationWebinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines
Webinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines 14.07.2015 Dipl.-Ing. Jan Hesse Jan.hesse@cfx-berlin.de CFX Berlin Software GmbH Karl-Marx-Allee 90 A 10243 Berlin
More informationVerification of Laminar and Validation of Turbulent Pipe Flows
1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan
More informationNUMERICAL SIMULATION OF FLOW FIELD IN AN ANNULAR TURBINE STATOR WITH FILM COOLING
24 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES NUMERICAL SIMULATION OF FLOW FIELD IN AN ANNULAR TURBINE STATOR WITH FILM COOLING Jun Zeng *, Bin Wang *, Yong Kang ** * China Gas Turbine Establishment,
More informationNUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV)
University of West Bohemia» Department of Power System Engineering NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) Publication was supported by project: Budování excelentního
More informationAdvanced Turbomachinery Methods. Brad Hutchinson ANSYS, Inc. Industry Marketing
Advanced Turbomachinery Methods 1 Brad Hutchinson ANSYS, Inc. Industry Marketing Presentation Overview 1. Turbomachinery challenges 2. ANSYS TurboSystem 3. 2 Blade row fluid dynamics solution methods Available
More informationTurbomachinery Applications with STAR-CCM+ Turbomachinery Sector Manager
Turbomachinery Applications with STAR-CCM+ Fred Mendonça Fred Mendonça Turbomachinery Sector Manager An Integrated Solution The applications of the software seem to be infinite. The user-friendly A single
More informationUsing Multiple Rotating Reference Frames
Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More informationUsing Multiple Rotating Reference Frames
Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationEstimation of Flow Field & Drag for Aerofoil Wing
Estimation of Flow Field & Drag for Aerofoil Wing Mahantesh. HM 1, Prof. Anand. SN 2 P.G. Student, Dept. of Mechanical Engineering, East Point College of Engineering, Bangalore, Karnataka, India 1 Associate
More informationCFD Simulation of a dry Scroll Vacuum Pump including Leakage Flows
CFD Simulation of a dry Scroll Vacuum Pump including Leakage Flows Jan Hesse, Rainer Andres CFX Berlin Software GmbH, Berlin, Germany 1 Introduction Numerical simulation results of a dry scroll vacuum
More informationRevolve 3D geometry to display a 360-degree image.
Tutorial 24. Turbo Postprocessing Introduction This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing
More informationNumerical and theoretical analysis of shock waves interaction and reflection
Fluid Structure Interaction and Moving Boundary Problems IV 299 Numerical and theoretical analysis of shock waves interaction and reflection K. Alhussan Space Research Institute, King Abdulaziz City for
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University
More informationFlow Field Analysis of Turbine Blade Modeling Based on CFX-Blade Gen
Flow Field Analysis of Turbine Blade Modeling Based on CFX-Blade Gen Liguang Wang 1, 2, a, *, Zhijun Li 1, 2, b, Yu Wang 1, 2, c, Baolin Liu 1, 2, Qin Zhou 1, 2 1 School of Engineering and Technology,
More informationCFD Simulation of a Dry Scroll Vacuum Pump Including Leakage Flows
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2016 CFD Simulation of a Dry Scroll Vacuum Pump Including Leakage Flows Jan Hesse CFX Berlin
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationAxisymmetric Viscous Flow Modeling for Meridional Flow Calculation in Aerodynamic Design of Half-Ducted Blade Rows
Memoirs of the Faculty of Engineering, Kyushu University, Vol.67, No.4, December 2007 Axisymmetric Viscous Flow Modeling for Meridional Flow alculation in Aerodynamic Design of Half-Ducted Blade Rows by
More informationEnhancement of a large injection system for steam turbines
GE Oil & Gas Leonardo Nettis, GE Oil & Gas Enzo Imparato, GE Oil & Gas Lorenzo Cosi, GE Oil & Gas DOWNSTREAM TECHNOLOGY SOLUTIONS PRODUCTS & SERVICES Enhancement of a large injection system for steam turbines
More informationCFD Post-Processing of Rampressor Rotor Compressor
Gas Turbine Industrial Fellowship Program 2006 CFD Post-Processing of Rampressor Rotor Compressor Curtis Memory, Brigham Young niversity Ramgen Power Systems Mentor: Rob Steele I. Introduction Recent movements
More informationModeling Evaporating Liquid Spray
Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the
More informationCFD Modeling of a Radiator Axial Fan for Air Flow Distribution
CFD Modeling of a Radiator Axial Fan for Air Flow Distribution S. Jain, and Y. Deshpande Abstract The fluid mechanics principle is used extensively in designing axial flow fans and their associated equipment.
More informationCFD Simulations of Flow over Airfoils:
CFD Simulations of Flow over Airfoils: An Analysis of Wind Turbine Blade Aerodynamics By: John Hamilla, Mechanical Engineering Advisor: Maria-Isabel Carnasciali, Ph.D. Abstract Wind turbines are rapidly
More informationNovember c Fluent Inc. November 8,
MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without
More informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationPotsdam Propeller Test Case (PPTC)
Second International Symposium on Marine Propulsors smp 11, Hamburg, Germany, June 2011 Workshop: Propeller performance Potsdam Propeller Test Case (PPTC) Olof Klerebrant Klasson 1, Tobias Huuva 2 1 Core
More informationSimulation of Turbulent Flow around an Airfoil
1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew
More informationSimulation of Flow Development in a Pipe
Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,
More informationNUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING
Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)
More informationNon-Newtonian Transitional Flow in an Eccentric Annulus
Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent
More informationMcNair Scholars Research Journal
McNair Scholars Research Journal Volume 2 Article 1 2015 Benchmarking of Computational Models against Experimental Data for Velocity Profile Effects on CFD Analysis of Adiabatic Film-Cooling Effectiveness
More informationSimulation of Laminar Pipe Flows
Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & Engineering
More informationNUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT
Int. J. Chem. Sci.: 14(2), 2016, 1148-1156 ISSN 0972-768X www.sadgurupublications.com NUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT S. KALIAPPAN, M. D. RAJKAMAL and D. BALAMURALI
More informationProceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA
Proceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA IMECE2011-65058 THE EFFECT OF BLADE LEAN, TWIST AND BOW ON
More informationModeling External Compressible Flow
Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras
More informationHexa Meshing. Defining Surface Parameters for the Mesh Defining Edge Parameters to Adjust the Mesh Checking mesh quality for determinants and angle
4.2.6: Pipe Blade Overview This tutorial example uses the Collapse function to create a degenerate topology in a Conjugate Heat transfer problem around a blade located in the center of a cylindrical pipe.
More informationUse of CFD in Design and Development of R404A Reciprocating Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2006 Use of CFD in Design and Development of R404A Reciprocating Compressor Yogesh V. Birari
More informationCFD MODELING FOR PNEUMATIC CONVEYING
CFD MODELING FOR PNEUMATIC CONVEYING Arvind Kumar 1, D.R. Kaushal 2, Navneet Kumar 3 1 Associate Professor YMCAUST, Faridabad 2 Associate Professor, IIT, Delhi 3 Research Scholar IIT, Delhi e-mail: arvindeem@yahoo.co.in
More informationOptimization of Hydraulic Fluid Parameters in Automotive Torque Converters
Optimization of Hydraulic Fluid Parameters in Automotive Torque Converters S. Venkateswaran, and C. Mallika Parveen Abstract The fluid flow and the properties of the hydraulic fluid inside a torque converter
More informationCo-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine
Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Benoit Bosc-Bierne, Dr. Andreas Spille-Kohoff, Farai Hetze CFX Berlin Software GmbH, Berlin Contents Positive displacement compressors
More informationA Comparative CFD Analysis of a Journal Bearing with a Microgroove on the Shaft & Journal
Proceedings of International Conference on Innovation & Research in Technology for Sustainable Development (ICIRT 2012), 01-03 November 2012 182 A Comparative CFD Analysis of a Journal Bearing with a Microgroove
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationCFD Analysis of conceptual Aircraft body
CFD Analysis of conceptual Aircraft body Manikantissar 1, Dr.Ankur geete 2 1 M. Tech scholar in Mechanical Engineering, SD Bansal college of technology, Indore, M.P, India 2 Associate professor in Mechanical
More information8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH
8. BASIC TURBO MODEL WITH UNSTRUCTURED MESH This tutorial employs a simple turbine blade configuration to illustrate the basic turbo modeling functionality available in GAMBIT. It illustrates the steps
More informationAdvances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist
Advances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist Usage From Across the Industry Outline Key Application Objectives Conjugate
More informationCFD Study of a Darreous Vertical Axis Wind Turbine
CFD Study of a Darreous Vertical Axis Wind Turbine Md Nahid Pervez a and Wael Mokhtar b a Graduate Assistant b PhD. Assistant Professor Grand Valley State University, Grand Rapids, MI 49504 E-mail:, mokhtarw@gvsu.edu
More informationISSN(PRINT): ,(ONLINE): ,VOLUME-1,ISSUE-1,
NUMERICAL ANALYSIS OF THE TUBE BANK PRESSURE DROP OF A SHELL AND TUBE HEAT EXCHANGER Kartik Ajugia, Kunal Bhavsar Lecturer, Mechanical Department, SJCET Mumbai University, Maharashtra Assistant Professor,
More informationHYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM
HYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM Krzysztof Denus CTD Technology ñ Ing. Buro Denus Colin Osborne Concepts NREC 1. INTRODUCTION The impeller
More informationFirst Steps - Ball Valve Design
COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to
More informationPressure Drop Evaluation in a Pilot Plant Hydrocyclone
Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Fabio Kasper, M.Sc. Emilio Paladino, D.Sc. Marcus Reis, M.Sc. ESSS Carlos A. Capela Moraes, D.Sc. Dárley C. Melo, M.Sc. Petrobras Research Center
More informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
More informationReliability - Based Robust Design Optimization of Centrifugal Pump Impeller for Performance Improvement considering Uncertainties in Design Variable
Reliability - Based Robust Design Optimization of Centrifugal Pump Impeller for Performance Improvement considering Uncertainties in Design Variable M.Balamurugan Assistant Professor, Government College
More informationModeling Evaporating Liquid Spray
Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow
More informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationESTABLISHMENT OF AN OPEN 3D STEAM TURBINE FLUTTER TEST CASE
Paper ID: ETC2017-315 Proceedings of 12th European Conference on Turbomachinery Fluid dynamics & Thermodynamics ETC12, April 3-7, 2017; Stockholm, Sw eden ESTABLISHMENT OF AN OPEN 3D STEAM TURBINE FLUTTER
More informationAccurate and Efficient Turbomachinery Simulation. Chad Custer, PhD Turbomachinery Technical Specialist
Accurate and Efficient Turbomachinery Simulation Chad Custer, PhD Turbomachinery Technical Specialist Outline Turbomachinery simulation advantages Axial fan optimization Description of design objectives
More informationInvestigation of mixing chamber for experimental FGD reactor
Investigation of mixing chamber for experimental FGD reactor Jan Novosád 1,a, Petra Danová 1 and Tomáš Vít 1 1 Department of Power Engineering Equipment, Faculty of Mechanical Engineering, Technical University
More informationTutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow
Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat
More informationSimulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach
Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach Dipl.-Ing. (FH) Günther Lang, CFDnetwork Engineering Dipl.-Ing. Burkhard Lewerich, CFDnetwork
More informationComparison of Classic and Finned Piston Reciprocating Linear Air Compressor Using COMSOL Multiphysics
Comparison of Classic and Finned Piston Reciprocating Linear Air Compressor Using COMSOL Multiphysics M. Heidari*, P. Barrade, and A. Rufer LEI, École Polytechnique Fédérale de Lausanne, Lausanne, Switzerland
More informationKeywords: CFD, aerofoil, URANS modeling, flapping, reciprocating movement
L.I. Garipova *, A.N. Kusyumov *, G. Barakos ** * Kazan National Research Technical University n.a. A.N.Tupolev, ** School of Engineering - The University of Liverpool Keywords: CFD, aerofoil, URANS modeling,
More informationSimulation and Validation of Turbulent Pipe Flows
Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,
More informationSolved with COMSOL Multiphysics 4.0a. COPYRIGHT 2010 COMSOL AB.
Journal Bearing Introduction Journal bearings are used to carry radial loads, for example, to support a rotating shaft. A simple journal bearing consists of two rigid cylinders. The outer cylinder (bearing)
More informationSimulation of Turbulent Flow around an Airfoil
Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan
More informationResearch and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (2), Quach Thi Son (2)
GSJ: VOLUME 6, ISSUE 6, JUNE 018 116 Research and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (), Quach Thi Son () (1) Institute for hydro power and renewable
More informationHYDRODYNAMIC MODELLING STUDY OF A ROTATING LIQUID SHEET CONTACTOR
Eleventh International Conference on CFD in the Minerals and Process Industries CSIRO, Melbourne, Australia 7-9 December 2015 HYDRODYNAMIC MODELLING STUDY OF A ROTATING LIQUID SHEET CONTACTOR Christopher
More informationAshwin Shridhar et al. Int. Journal of Engineering Research and Applications ISSN : , Vol. 5, Issue 6, ( Part - 5) June 2015, pp.
RESEARCH ARTICLE OPEN ACCESS Conjugate Heat transfer Analysis of helical fins with airfoil crosssection and its comparison with existing circular fin design for air cooled engines employing constant rectangular
More informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
More informationApplication of Wray-Agarwal Turbulence Model for Accurate Numerical Simulation of Flow Past a Three-Dimensional Wing-body
Washington University in St. Louis Washington University Open Scholarship Mechanical Engineering and Materials Science Independent Study Mechanical Engineering & Materials Science 4-28-2016 Application
More informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationMOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND
MOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND A CYLINDRICAL CAVITY IN CROSS FLOW G. LYDON 1 & H. STAPOUNTZIS 2 1 Informatics Research Unit for Sustainable Engrg., Dept. of Civil Engrg., Univ. College Cork,
More informationCFD Analysis for the Cooling Vent in Automobile
International Journal for Ignited Minds (IJIMIINDS) CFD Analysis for the Cooling Vent in Automobile Vijay Kumar M a, Dr. Basawaraj b & Dr. B R Shridhar c a Asst Prof, Department of Mechanical, S.E.A.C.E.T,
More informationFLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER
FLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER Chao Xu, Cees Bil, Sherman CP. Cheung School of Aerospace, Mechanical and Manufacturing Engineering, RMIT University Keywords: Twin counter-rotating
More informationSpeed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester
Speed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Content ANSYS CFD Introduction ANSYS, the company Simulation
More informationVolute Optimization Workflow
Volute Optimization Workflow Volute design optimization with CAESES, Grid Pro, and TCFD Mattia Brenner Head of Sales Europe FRIENDSHIP SYSTEMS AG brenner@friendship-systems.com Samuel E James Director
More informationTutorial 2. Modeling Periodic Flow and Heat Transfer
Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as
More informationSimulation of Turbulent Flow over the Ahmed Body
1 Simulation of Turbulent Flow over the Ahmed Body ME:5160 Intermediate Mechanics of Fluids CFD LAB 4 (ANSYS 18.1; Last Updated: Aug. 18, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim, Maysam Mousaviraad,
More informationInfluence of Geometric Scaling on Linear Cascade Aerodynamic Performance
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 00 (2014) 000 000 www.elsevier.com/locate/procedia APISAT2014, 2014 Asia-Pacific International Symposium on Aerospace Technology,
More informationNumerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien
Fachtagung Lasermethoden in der Strömungsmesstechnik 8. 10. September 2015, Dresden Numerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien Numerical Investigations of Wind
More informationDEMONSTRATION OF THE DESIGN OF A FIRST-STAGE AXIAL-FLOW COMPRESSOR BLADE USING SOLID MODELING THROUGH A CLASSROOM PROJECT
DEMONSTRATION OF THE DESIGN OF A FIRST-STAGE AXIAL-FLOW COMPRESSOR BLADE USING SOLID MODELING THROUGH A CLASSROOM PROJECT Breon Williams, Brandon Howard, Xiaoqing Qian and Z.T. Deng, Alabama A&M University
More informationTransition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim
Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon
More informationSimulation of Turbulent Flow in an Asymmetric Diffuser
Simulation of Turbulent Flow in an Asymmetric Diffuser 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 3 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University of Iowa C.
More informationNon Axisymmetric Hub Design Optimization for a High Pressure Compressor Rotor Blade
Non Axisymmetric Hub Design Optimization for a High Pressure Compressor Rotor Blade Vicky Iliopoulou, Ingrid Lepot, Ash Mahajan, Cenaero Framework Target: Reduction of pollution and noise Means: 1. Advanced
More informationAnalysis of an airfoil
UNDERGRADUATE RESEARCH FALL 2010 Analysis of an airfoil using Computational Fluid Dynamics Tanveer Chandok 12/17/2010 Independent research thesis at the Georgia Institute of Technology under the supervision
More informationStudy on the Design Method of Impeller on Low Specific Speed Centrifugal Pump
Send Orders for Reprints to reprints@benthamscience.ae 594 The Open Mechanical Engineering Journal, 2015, 9, 594-600 Open Access Study on the Design Method of Impeller on Low Specific Speed Centrifugal
More informationGEOMETRY MODELING & GRID GENERATION
GEOMETRY MODELING & GRID GENERATION Dr.D.Prakash Senior Assistant Professor School of Mechanical Engineering SASTRA University, Thanjavur OBJECTIVE The objectives of this discussion are to relate experiences
More informationCFD design tool for industrial applications
Sixth LACCEI International Latin American and Caribbean Conference for Engineering and Technology (LACCEI 2008) Partnering to Success: Engineering, Education, Research and Development June 4 June 6 2008,
More informationDESIGN OPTIMIZATION OF AN AXIAL FLOW COMPRESSOR FOR INDUSTRIAL GAS TURBINE
DESIGN OPTIMIZATION OF AN AXIAL FLOW COMPRESSOR FOR INDUSTRIAL GAS TURBINE Nilesh P. Salunke 1, S. A. Channiwala 2, Juned A. R. A 3 1 Research Scholar, SVNIT, Surat, Gujarat, India 2 Professor, Department
More informationSIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING.
SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. M.N.Senthil Prakash, Department of Ocean Engineering, IIT Madras, India V. Anantha Subramanian Department of
More informationOPTIMIZATION OF AXIAL HYDRAULIC TURBINES RUNNER BLADES USING HYDRODYNAMIC SIMULATION TECHNIQUES
Scientific Bulletin of the Politehnica University of Timisoara Transactions on Mechanics Special issue The 6 th International Conference on Hydraulic Machinery and Hydrodynamics Timisoara, Romania, October
More informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
More informationDesign, Modification and Analysis of Two Wheeler Cooling Sinusoidal Wavy Fins
Design, Modification and Analysis of Two Wheeler Cooling Sinusoidal Wavy Fins Vignesh. P Final Year B.E.,Mechanical Mepco Schlenk Engineering College Sivakasi,India P. Selva Muthu Kumar Final year B.E.,
More informationPerformance Analysis of an After Cooler Used In High Power Engine Using CFD
International OPEN ACCESS Journal Of Modern Engineering Research (IJMER) Performance Analysis of an After Cooler Used In High Power Engine Using CFD M. Safraaj Salaamer 1, Dr. K. S. Amirthagadeswaran 2,
More informationFlow and Heat Transfer in a Mixing Elbow
Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and
More informationSupersonic Flow Over a Wedge
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge
More information