MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 93 CFD Analysis of 3-D Flow for Francis Turbine Manoj Kumar Shukla Lecturer, KNPC, Jabalpur (MP), India (Email: mksmact@gmail.com) Prof. Vishnu Prasad Professor, Problem Oriented Research Laboratory, MANIT, Bhopal (MP), India Rajeev Jain HOD, Mechanical Engineering Department, KNPC, Jabalpur (MP), India S.N. Shukla General Manager, R&D Division, Kirloskar Brothers Limited, Pune, India Abstract: Computational Fluid Dynamics (CFD) analysis is very useful tool for predicting hydraulic machinery performance at various operating conditions. For designers, prediction of operating characteristics performance is most important task. All theoretical methods for predicting the performance merely gives a value, and one is unable to determine the root cause for the poor performance. Due to the development of CFD code, one can get the performance value as well as observe actual behaviour of flow in the domain. Analysis and variation of performance can be find out by using CFD analysis. In the present work 3-Dimensional (3-D) real flow analysis is done for experimentally tested turbine and the characteristics of prototype turbine were predicted in actual operating regimes. Aim of the work is validation of CFD results with the experimental output.the operating conditions considered are in accordance with that, where actual prototype turbine is to be installed. Flow structure inside the machine is analysed and it showed the scope of improvement in the design (for example casing tip portion). Results obtained by Computational tool were very close to experimental results. This provides confidence on Computational tools. Present paper elaborates model selection for prototype turbine, details of methodology used, visualization of results in CFX-post & then validation of Computational results. Keywords: Computational fluid dynamics (CFD), francis turbine, Efficiency, Head, Unit discharge, unit speed, unit power, pressure, unit discharge, specific speed, flow parameter. I. INTRODUCTION Among all hydraulic turbine machines used for energy conversion, vast operating regime of Francis turbine enables it to be used for varying range of small to large hydro power plant. This makes Francis turbine most popular and hence it is used in maximum number of hydro power plants. In order to develop a reliable machine for this highly demanding operation, the behaviour of the flow in the entire turbine regime has to be predicted by a reliable computational method like CFD which is very economical method. The prediction of prototype turbine performance in actual prevailing conditions is very important for engineers. In order to know the feasibility of the turbine, it is essential to project the results in advance. Since turbines are tailor made as per the requirement of the prevailing site conditions, a unique performance prediction has to be made for a separate turbine. This can be done either by theoretical methods, experimental methods or by computational method (i.e. CFD). Among all methods CFD stands its unique importance, since by this method study of the flow inside turbine space can be made. Flow pattern in intricate portions of the component can also be analysed and variation of the results can be known with the varying conditions. CFD method consumes less money, less gestation period in comparison to the experimental method which requires model fabrication and test rig set up. CFD approach is a combination of numerical technique and computational power. With the help of CFD technique even complex flow pattern inside hydraulic turbine parts can be analysed in detail and modifications can be implemented. It can be used for increasing the efficiency by making necessary modification in the design of hydraulic turbine and checking relevancy of alternate optimizatimised design before the turbine is finally manufactured. However in order to check the reliability of selected optimized design, validation of the results is to be done with experimental results. CFD technique has lead to significant enhancement in efficiency of hydraulic turbine. CFD can also be used to check efficiency of alternate design of hydraulic turbine for optimization before final testing is done. To improve reliability of CFD technique, validations of results are required with experimental results. In present work Francis turbine considered with Horizontal axis. CFD analysis is done on varying working conditions and tabulations of results are done to get the clear picture of changes in the results. In the present paper emphasis is given on predicting the turbine performance in actual condition for a prototype turbine and then to validate the results. Hydraulic turbine which is considered for validation of results is a actual turbine which is to be manufactured and installed at the site. For this turbine head and discharge available are known. With the help of these known quantities other necessary parameters for study like power available, specific speed, diameter of runner, unit speed, unit power and scale ratio are calculated. These quantities are useful for final modelling of prototype hydraulic turbine components. Feasibility of working turbine at actual
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 94 condition is checked for development of high performance product by research engineering. Visual flow pattern around turbine space is obtained by solving continuity and momentum equation with the help of computational fluid dynamics to study fluid flow properties. The losses in various parts of the turbine at critical regions of turbine are also investigated. The performance prediction and assessment are well validated by many investigators for hydraulic turbine. II. GEOMETRIC MODELLING, BOUNDARY CONDITIONS & COMPUTATIONAL PARAMETERS Geometric Modelling Pro-E Software is used for the generation of model which is further imported in ANSYS ICEM for mesh generation. After properly meshing the geometry physical to use the most appropriate mesh. CFX-11 includes the following features: An advanced coupled solver, which is both reliable and robust. Full integration of problem definition, analysis and results presentation. An intuitive and interactive setup process, using menus and advanced graphics. The unstructured tetrahedral mesh is generated in ANSYS ICEM CFD software for all domains which are later assembled for further study. The accuracy of solution is greatly affected by the size of elements [Guoyi Peng et al(2002)]. Francis turbine design consists of 18 stay vanes, 18 guide vanes and 13 runner vanes. Casing and draft tube are also considered as per original dimensions to be manufactured. Therefore the simulated design consists assembly of casing, runner and draft tube as our interest is to get complete performance of the prototype turbine. Each component is modelled separately and then assembled to get the complete assembly through proper interfaces. Mesh with scale factor 1.2 is used for importing to ANSYS CFX Pre. 3D real flow simulation analysis is done for experimentally tested Francis turbine using ANSYS CFX 11 software. The rotational speed of runner is specified, stay vane and guide are kept at frozen state. All inner boundary of turbine space are considered smooth with no slip. Table 1: Summary of mesh data Domain part No. of No. of Type of nodes elements element Casing 204447 1605723 Tetrahedron (including stay vanes & guide vanes) Runner 98741 382088 Tetrahedron Draft tube 121845 35961 Tetrahedron Boundary Conditions The inlet and outlet boundary conditions are to be specified for each run and the accuracy of solution depends on the location and manner, these conditions are specified. Magnitude of mass flow rate and direction are specified at the casing inlet as inlet boundary condition and reference pressure is specified at outlet of draft tube as outlet boundary condition. In present analyses, the mass flow rates as 7305 Kg/s at 80.93 mm guide vane opening (GVO) is given as inlet boundary conditions at stay vane inlet. Guide vane opening considered for the present case is 80.93 mm (75.2 % wrt full guide vane opening) which is near peak efficiency regime. Full Guide vane opening is 107.6 mm. The static pressure as 0 Pa is specified as outlet boundary condition at the draft tube outlet. The reference pressure is taken as 1 atmosphere i.e.105 Pa. The rotational speed of runner is specified as 600 rpm as per guide vane opening. The stay vane, guide vane and draft tube domains are taken as stationary. The shear stress transport (SST), k e turbulence model has been used and the walls of all domains are assumed to be smooth with no slip. Computational flow parameters Computational analysis provides pressure and velocity distribution across whole turbine region in the form of pressure and velocity profile. Head, discharge and efficiency variations are computed for the presentation of results. Losses in various domains are calculated on the basis of pressure difference at inlet and outlet boundary of domains. Various formulae used for computation of different parameters are given below: Specific speed Ns = NÖP/H 5/4 Available power Unit speed Unit discharge Unit discharge P = r g Q H N 11 = ND / ÖH Q 11 = Q / D 2 ÖH Q 11 = P 11 / (9810*Efficiency) Unit power P 11 = P / D 2 H 3/2 Pressure Pr = r g H (Head loss) domain H loss = (Pr inlet Pr outlet ) / 9810 H avilable = (Inlet Pressure casing - Outlet Pressure draft tube )/9810 Total head loss H total loss = H 1 loss + H 2 loss + H 3 loss +.. H n loss (For n number of domains) Turbine efficiency h exp. = H available *100 / (H available - H loss )
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 95 Table 2: Turbine specification Turbine model Francis Turbine Shaft alignment Horizontal Axis Ns of turbine 266.19 m-kw Model selected F280 Desired P generator output 3000 kw Rated head available 48 m Desired P turbine output 3142 kw Rated flow 7.25 m3/s Rated N of turbine 600 rpm Prototype runner diameter 1.01 m Model runner diameter 0.35 m Scale up ratio 2.88 Site elevation EL 143 m Turbine overload 10 % Prated site condition where prototype turbine is to be installed. For the selection of prototype turbine, first of all model turbine is selected (satisfying specification as per Table 2) which is homologous to the prototype turbine. Based on these data, efficiency of prototype turbine is calculated. Also all the parameters are calculated for the prototype turbine based on the selected model. For present study conditions available at the actual site conditions are given in Table 2. The integrated and cross sectional view of assembled hydro turbine is shown in Figure 2 and Figure 3. III. METHODOLOGY OF WORK Complete process comprised from AutoCAD drawing to the CFX post covers following steps: As per the selection of model, drawings for prototype turbine is made by scaling up model drawings 3-D model of all the parts (as per the scaled up geometry) is made in Pro-E. Modelled figures are imported in ANSYS ICEM for mesh generation. The volume occupied by the fluid is divided into discrete cells (the mesh). Meshed part are then taken to CFX-pre to define the physical condition prevailing. The boundary conditions are defined. The equations are solved iteratively by running CFX Solver to get the results. Analysis and visualization of the resulting solutions. Validations of results are done. Figure 2: Assembled Francis Turbine Figure 3: 3-D Assembled Francis Turbine Figure 1: Algorithm for validation of results IV. SELECTION OF TURBINE The selection of model turbine is made according to the specific speed calculated for that turbine. Specific speed is calculated on the basis of head and discharge available at the Figure 4: Assembled 3D Cross-sectional view of Turbine
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 96 V. EXPERIMENTAL INVESTIGATION Experimental tested results of turbine at reduced scale (CRED-KBL) are projected w.r.t. model whose specific speed resembles with the prototype turbine. The geometrical specifications of experimentally tested Francis turbine model are given in Table 2. There is a vast number of iterations available depending upon the guide vane opening of the turbine. Initially for best guide vane opening results are calculated which are tabulated in the Table 2. These Data are obtained by scaling up the models results of various parameters obtained after conducting the experimental wind tunnel testing. Runner diameter of prototype turbine is calculated satisfying the specifications mentioned in Table 1, depending upon the diameter of prototype turbine, scale ratio is calculated. Respective model drawings are scaled up as per scale up ratio. Obtained results for prototype turbine are tabulated in Table 3. An iterative method is used to find that optimum efficiency can be obtained when diameter of runner is 1010 mm which is duty point. For duty point and rated turbine speed of 600 rpm, value of N11 is 87.50. Head and efficiency variations wrt discharge for prototype turbine are shown in Figure 5. For broader visualisation of results, experimental and CFD investigation is done at design and off-design points. Table 3: Experimental results of prototype Sl. N 11 P 11 h exp. H Pr. P Q Q 11 No. % (m) (Pa) (kw) (m3/s) 1 70 9.00 89.00 74.95 735221.46 5956.75 9.10 1.03 2 80 9.30 92.80 57.38 562903.93 4123.57 7.89 1.02 3 87.5 9.28 93.10 47.97 470541.74 3144.74 7.18 1.01 4 90 9.22 93.00 45.34 444763.60 2864.98 6.93 1.01 5 100 8.70 89.50 36.72 360258.52 1975.06 6.13 0.99 Figure 5: Variation of head & efficiency wrt discharge of prototype turbine Axis of turbine Type of draft tube Model head Specific speed of turbine Runner diameter Table 4: Model details No. of runner blades 13 No. of guide vanes 18 PCD of guide vanes No. of stay vanes 18 vertical elbow tube 28 m 266.19 m-kw 0.35 m 0.40 m Best efficiency 92.10 % N 11 at best efficiency point 83.8 P 11 at best efficiency point 8.85 Figure 5: Meshed casing domain Figure 6: Runner model
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 97 and draft tube domain are 204447, 98741, and 121845 respectively. The tests were carried out for different head and flow rate across the turbine. Qualitative results of the test are given in the form of Figures 8, 11, 12 and 13. Computational results obtained are given in Table 5 and compared with experimental results in Table 6. Table 5: Computational results Figure 7: Draft tube mesh Properties are defined in CFX pre and after running solver final results are visualized and analysed in CFX post. CFX-11 is a general purpose Computational Fluid Dynamics (CFD) code, combining an advanced solver with powerful pre and post-processing capabilities. The next-generation physics pre-processor, CFX-Pre, allows multiple meshes to be imported, allowing each section of complex geometries to use the most appropriate mesh. VI. RESULTS AND DISCUSSIONS The numerical simulation is done in ANSYS CFX 11. Experimental results are shown in Table 2 which are obtained by scaling up the results of model turbine as per the scale ratio of 2.88. For prototype turbine available head and discharge for which turbine will operate maximum period of time is known quantity from the detailed project report (Table 1). Rotational speed of turbine is taken as the rated speed i.e. 600 rpm, specific speed calculated is 266 m-kw with the help of which runner diameter is calculated as 1010 mm, N 11 and P 11 is also computed with these results. Generator efficiency is assumed to be 95.50% which is fairly good in this case. The experimental results for prototype turbine are obtained by projecting the results of homologous model turbine in proportion to the computed scale ratio. Then efficiency of prototype turbine is calculated at rated head of 48 m and rated flow of 7.25 m 3 /s, subsequently efficiency of turbine at other unit speeds are also computed to get broader visualization of operation of turbine at design and off design operating regimes. Experimental results for prototype turbine are tabulated in Tables 5 and 6. It is well known that all these parameters could be combined to unit quantities to carry out data reduction. This approach is followed to present the results. The assembly of turbine considered here comprised of Casing, Stay vane, Guide Vane, runner and Draft tube (shown in Figures 5, 6 and 7 respectively).three number of domains are made viz. casing domain (Stationary), runner domain (Rotating) and draft tube domain (Stationary). As the dimension of whole assembly is big, therefore meshing of the domains are done separately and then merged together. Number of grid points in casing domain, runner domain Sl. N 11 Loss (m) Total Head No. Casing Runner Draft Losses Developed Tube (m) (m) 1 70.00 2.336 4.464 1.360 8.160 68.84 2 80.00 0.499 3.751 0.015 4.265 57.34 3 87.50 0.347 2.485 0.342 3.175 49.42 4 90.00 0.192 2.154 0.678 3.024 45.92 5 100.00 1.490 2.091 0.692 4.273 40.05 Table 6: Computational & Experimental Results Sl. N 11 Head (m) Efficiency (%) No. H exp. H cfd h exp. h cfd 1 70 74.95 68.84 89.00 88.15 2 80 57.38 57.34 92.80 92.56 3 87.5 47.97 49.42 93.10 93.58 4 90 45.34 45.921 93.00 93.41 5 100 36.72 40.05 89.50 89.33 In the calculation of experimental efficiency of prototype turbine step factor taken by moody's formula is 1%. Computational results show increase in efficiency at design point wrt experimental results. However at off design point there is variation in efficiency with both methods. Possible reason for this increase in efficiency is the change in the tip portion design of the casing. Change in casing tip portion improves passage of water from casing to runner inlet. The best efficiency point is obtained when head is made available near 48 m and Guide vane opening of 75.2%. Losses in various domains are shown in table 5, which shows that optimum losses occur when unit speed of turbine is near 87.5.This supports that for efficient and optimum performance of turbine unit speed of turbine should be near 87.5 and accordingly other factors should be decided for the design of prototype turbine. Streamline flows are shown indicating maximum turbulence in the runner which is converted into head loss. Runner is the major component of turbine for energy conversion, therefore runner part plays critical role for deciding the efficiency of turbine. Table 5 illustrates losses occurring in casing, runner and draft tube domains. For this casing tip portion design was modified to make smooth entrance of flow which resulted
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 98 in the slight increase of efficiency. This approach can be further studied which can be a part of optimization process. Experimental and computational efficiency of turbine is fairly matching which indicates the robustness of the method followed as shown in Table 6. The blade loading chart is showing pressure variation in mid span of runner blade from leading edge (LE) to trailing edge (TE). Cavitation is another important design aspect for Turbine. Turbine should be free from cavitation effect. To know whether our Turbine design is free from cavitation effect, we should know pressure distribution on two sides of blades. This can be done by plotting Blade loading of runner at different span location i.e. 66.7% span. Blade Loading from Leading edge to trailing edge is shown in the Figure 12. Static pressure (Guage) is gradually decreasing at every span location and there is no abrupt changes observed. As they are not falling below the vapour pressure of water, we can conclude that they are free from cavitation. Figure 9: Variation head & discharge Different sets of operating points were selected to get the performance characteristics of the actual turbine to be made. Experimental and Computational results are compared in the Figures 9 & 10. Since head is calculated after computational investigation for design and off design points, therefore comparative study is made between head, discharge and efficiency off turbine. The scatter in the experimental data was relatively small and hence a trend line was used to represent the curve using a polynomial series. Results obtained from the solver are used to get the real picture inside the geometry and to know the velocity and pressure variations across the whole domain. Graphs shows that the results obtained by CFD are fairly matching with the results obtained from the experimental data. Points where variation occurs is due to the extra losses in the domains, which should be minimized. Figure 10: Variation efficiency & discharge Figure 8: Pressure contour in casing domain Figure 11: Blade Loading from Leading edge to trailing edge
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 99 From Tables 5 and 6 it is seen that for maximum efficiency total losses is minimum. Pressure contour and velocity contour shown in Figure 12 and 13 respectively describes the flow structure inside various components of francis turbine. Velocity profile from Figure 12 inside the turbine assembly indicates that casing and runner domain has smooth velocity profile whereas as soon as water enters draft domain velocity starts decreasing and profile becomes non uniform. Similarly from Figure 13 it becomes clear maximum energy conversation takes place inside the casing domain where pressure is highest and as water moves further its pressure decreases gradually. The best operating regimes, losses and flow pattern can be investigated from the calculated flow parameters of numerical simulation. Thus it can be concluded that CFD simulation can be used for investigating the actual performance of prototype turbine, to get possible sources of improvement in the design geometry with cost effective technique in lesser time. Validation of results done by this method will lead to become very good source of optimization technique for hydraulic turbine performance. Results from experimental evaluation and Simulation performed at different unit speed range for optimum guide vane opening and at rated speed of runner 600 rpm. Results show that optimum turbine performance at actual site will occur when the unit speed of turbine is near 87.5 working under a head of 48 m and accordingly other parameters are available. On the basis of computational results design analysis of prototype turbine can be done accordingly. Figure 12: Velocity Streamlines pattern across whole Domain Figure 13: Pressure contours across whole Domain VII. CONCLUSIONS The paper brought out the validation of experimental results with the computational investigation. The maximum efficiency regime indicated by both approaches is nearly same. Reason for slight difference of efficiency computed by experimental and computational method can be because of instrumental and human errors in experimental testing and also due to discretisation of domains and solution of deferential equations in computational methods. The total computed losses are observed to be minimum at best operating point. Hence the results obtained are fairly matching, however streamline flow in some reasons have more turbulence which is due to occurrence of losses. Difference in results at off peak conditions between experimental and computational
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 100 results is due to error in discretising the governing equations and flow domain. Losses not considered very precisely. There can be human and instrumental error in experimental calculations. Prediction of turbine performance by CFD gives the idea to know the flow behaviour inside the turbine model and get the information about the intricacy of flow pattern, since the flow inside the turbine in actual is very complicated. CFD results gives the qualitative information. It provides the tool to simulate the flow conditions with different geometries in lowest possible time, thus providing reduction in design analysis and yet developing robust technology along with aiding in reducing gestation period. H = Net head (m) NOMENCLATURE Q = Discharge through turbine (m 3 /s) N = Rotational speed of turbine (rpm) h = Mass density of water (kg/m 3 ) g = Gravitational acceleration (m/s 2 ) P = Turbine power (kw) P rated = Power output of turbine at rated condition (kw) P generatoroutput = Power output of generator (kw) EL = Elevation level wrt mean sea level. PCD = Pitch circle diameter (mm) N 11 = Unit speed Q 11 = Unit discharge P 11 = Unit power Pr. = Pressure (Pa) H exp. = Head by experimental testing (m) H cfd = Head by CFD testing (m) h exp. = Efficiency obtained by experimental testing h cfd = Efficiency obtained by CFD testing ACKNOWEDGEMENTS Author would like to express sincere gratitude towards all related to MANIT, Bhopal and KBL Pune, for continuous encouragement and cooperation made available to do the associated paper work. REFERENCES [1] Kirloskar Brothers Limited Data for Francis turbine model, Corporate Research and Engineering Division (CRED-KBL), Pune, India. [2] Maulana Azad National Institute of Technology, Project Reports on Turbine Testing Problem Oriented Research Laboratory (Fluid Mechanics and Hydraulic Mechanics Lab) Bhopal, India. [3] P. Krishnamachar, Dr. V.V. Barlit (Russia), M.M. Deshmukh, Manual on Hydraulic Turbine (MANIT, Bhopal). [4] Guoyi Peng, Shuliang Cao, Masaru Ishizuka, Shinji Hayama (2002); Design optimisation of axial flow hydraulic turbine runner: Part II-Multiobjective Constrained Optimzation Method, International Journal for Numerical Methods in Fluids, Vol. 39, Issue 6, pp. 533-548. [5] Guoyi Peng (2005): A practical combined combined computation method of mean through-flow for 3D inverse design of hydraulic turbine machinery blades, ASME Journal of fluid engineering. [6] V. Prasad, CFD approach for design optimization and validation for axial flow hydraulic turbine, Indian J of Eng and Materials Sciences, Vol. 16, August 1999, 229-236. [7] Bernard M., Maryse P., Robert M. and Anne. M. G., Proc. ASCE Water Power Conference, Las Vegas, USA 1999. [8] Peng G., Cao S., Ishizuka M. and Hayama S., Int. J. Numer Methods Fluids, 39(6) (200) 533-548 [9] Daniel B, Romeo R., and Sebastian M, Proc. Int. conf. on CSHS03, Belgrade, (2003) 29-36. [10] Liplej A., Proc. Inst. Mech. Eng., Pt. A. J. Power and Energy, 218 (2004) 43-50. [11] Guoyi P., J. Fluids Eng., 27 (2005) 1183-1190 [12] C.A.J. Fletcher, Computational Techniques for Fluid Dynamics Vol. 1, Springer Pub. 1991. [13] Lewis RI, Turbo machinery performance analysis (Arnold, Londan), 1996. [14] CFX 11, User Manual, Ansys Inc. 2004. [15] Liplez A., Proc. Inst. Mech. Eng., Pt. A. J. Power and Energy, 218 (2004) 43-50. [16] Guoyi P., J. Fluids Eng., 27 (2005) 1183-1190. [17] Shukla M., CFD Analysis of 3-D flow and it's validation for francis turbine, 34th National Conference on FMFP, BIT Mesra (2007) 732-737. [18] Wu J., Shimmel K., Tani K., Niikura K. and Sato J. J., Fluid Engg., 127(2007) 159-168. [19] Rao, V. Shrinivas, Tripathi, S.K. (2007): Role of CFD analysis in hydraulic design optimization of hydro turbines, Proceeding of National Seminar on CFD-The 3rd Dimension in Flow Analysis & Thermal Design, Bhopal(India), pp.196-201. [20] Vishnu Prasad; V.K. Gahlot, P. Krishnamachar (2009) CFD approach for design optimization and validation for axial flow hydraulic turbine, Indian Journal of Engineering and Material Sciences, pp. 229-236.