See discussions, stats, and author profiles for this publication at: https://www.researchgate.

net/publication/259264538

CFD analysis of 3-D flow for Francis turbine

Article · January 2011

CITATIONS READS
15 4,939

4 authors, including:

Manoj Kumar Shukla Rajeev Jain

12 PUBLICATIONS 371 CITATIONS 52 PUBLICATIONS 1,226 CITATIONS

SEE PROFILE SEE PROFILE

All content following this page was uploaded by Rajeev Jain on 06 January 2014.

The user has requested enhancement of the downloaded file.

MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 93
ISSN No. 2230 – 7699 © MIT Publications

CFD Analysis of 3-D Flow for Francis Turbine

Manoj Kumar Shukla Rajeev Jain
Lecturer, KNPC, Jabalpur (MP), India HOD, Mechanical Engineering Department,
(Email: mksmact@gmail.com) KNPC, Jabalpur (MP), India

Prof. Vishnu Prasad S.N. Shukla

Professor, Problem Oriented Research Laboratory, General Manager, R&D Division,
MANIT, Bhopal (MP), India Kirloskar Brothers Limited, Pune, India

Abstract: Computational Fluid Dynamics (CFD) analysis is very requirement of the prevailing site conditions, a unique
useful tool for predicting hydraulic machinery performance at performance prediction has to be made for a separate turbine.
various operating conditions. For designers, prediction of This can be done either by theoretical methods, experimental
operating characteristics performance is most important task. methods or by computational method (i.e. CFD). Among all
All theoretical methods for predicting the performance merely
methods CFD stands its unique importance, since by this
gives a value, and one is unable to determine the root cause for
the poor performance. Due to the development of CFD code, method study of the flow inside turbine space can be made.
one can get the performance value as well as observe actual Flow pattern in intricate portions of the component can also
behaviour of flow in the domain. Analysis and variation of be analysed and variation of the results can be known with
performance can be find out by using CFD analysis. the varying conditions. CFD method consumes less money,
less gestation period in comparison to the experimental
In the present work 3-Dimensional (3-D) real flow analysis is
done for experimentally tested turbine and the characteristics method which requires model fabrication and test rig set up.
of prototype turbine were predicted in actual operating regimes. CFD approach is a combination of numerical technique and
Aim of the work is validation of CFD results with the computational power. With the help of CFD technique even
experimental output .The operating conditions considered are complex flow pattern inside hydraulic turbine parts can be
in accordance with that, where actual prototype turbine is to be analysed in detail and modifications can be implemented.
installed. Flow structure inside the machine is analysed and it It can be used for increasing the efficiency by making
showed the scope of improvement in the design (for example necessary modification in the design of hydraulic turbine
casing tip portion). Results obtained by Computational tool were and checking relevancy of alternate optimizatimised design
very close to experimental results. This provides confidence on
before the turbine is finally manufactured. However in
Computational tools. Present paper elaborates model selection
for prototype turbine, details of methodology used, visualization order to check the reliability of selected optimized design,
of results in CFX-post & then validation of Computational validation of the results is to be done with experimental results.
results. CFD technique has lead to significant enhancement in
efficiency of hydraulic turbine. CFD can also be used to check
Keywords: Computational fluid dynamics (CFD), francis turbine,
efficiency of alternate design of hydraulic turbine for
Efficiency, Head, Unit discharge, unit speed, unit power, pressure,
unit discharge, specific speed, flow parameter. 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
I. INTRODUCTION considered with Horizontal axis. CFD analysis is done on
Among all hydraulic turbine machines used for energy varying working conditions and tabulations of results are done
conversion, vast operating regime of Francis turbine enables to get the clear picture of changes in the results.
it to be used for varying range of small to large hydro power In the present paper emphasis is given on predicting the
plant. This makes Francis turbine most popular and hence it turbine performance in actual condition for a prototype turbine
is used in maximum number of hydro power plants. In order and then to validate the results. Hydraulic turbine which is
to develop a reliable machine for this highly demanding considered for validation of results is a actual turbine which
operation, the behaviour of the flow in the entire turbine is to be manufactured and installed at the site. For this turbine
regime has to be predicted by a reliable computational method head and discharge available are known. With the help of
like CFD which is very economical method. The prediction these known quantities other necessary parameters for study
of prototype turbine performance in actual prevailing like power available, specific speed, diameter of runner, unit
conditions is very important for engineers. In order to know speed, unit power and scale ratio are calculated. These
the feasibility of the turbine, it is essential to project the results quantities are useful for final modelling of prototype hydraulic
in advance. Since turbines are tailor made as per the turbine components. Feasibility of working turbine at actual
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 94
ISSN No. 2230 – 7699 © MIT Publications

condition is checked for development of high performance Boundary Conditions

product by research engineering. Visual flow pattern around The inlet and outlet boundary conditions are to be specified
turbine space is obtained by solving continuity and momentum for each run and the accuracy of solution depends on the
equation with the help of computational fluid dynamics to location and manner, these conditions are specified.
study fluid flow properties. The losses in various parts of the Magnitude of mass flow rate and direction are specified at
turbine at critical regions of turbine are also investigated. The
the casing inlet as inlet boundary condition and reference
performance prediction and assessment are well validated by
pressure is specified at outlet of draft tube as outlet boundary
many investigators for hydraulic turbine.
condition.
II. GEOMETRIC MODELLING, BOUNDARY CONDITIONS In present analyses, the mass flow rates as 7305 Kg/s at
& COMPUTATIONAL PARAMETERS 80.93 mm guide vane opening (GVO) is given as inlet
boundary conditions at stay vane inlet. Guide vane opening
Geometric Modelling considered for the present case is 80.93 mm (75.2 % wrt full
Pro-E Software is used for the generation of model which guide vane opening) which is near peak efficiency regime.
is further imported in ANSYS ICEM for mesh generation. Full Guide vane opening is 107.6 mm. The static pressure as
After properly meshing the geometry physical to use the most 0 Pa is specified as outlet boundary condition at the draft
appropriate mesh. CFX-11 includes the following features: tube outlet.
• An advanced coupled solver, which is both reliable and The reference pressure is taken as 1 atmosphere i.e.105 Pa.
robust. The rotational speed of runner is specified as 600 rpm as per
• Full integration of problem definition, analysis and guide vane opening. The stay vane, guide vane and draft tube
results presentation. domains are taken as stationary. The shear stress transport
(SST), k – e turbulence model has been used and the walls
• An intuitive and interactive setup process, using menus
of all domains are assumed to be smooth with no slip.
and advanced graphics.
The unstructured tetrahedral mesh is generated in ANSYS Computational flow parameters
ICEM CFD software for all domains which are later Computational analysis provides pressure and velocity
assembled for further study. The accuracy of solution is distribution across whole turbine region in the form of
greatly affected by the size of elements [Guoyi Peng et pressure and velocity profile. Head, discharge and efficiency
al(2002)].
variations are computed for the presentation of results. Losses
Francis turbine design consists of 18 stay vanes, 18 guide in various domains are calculated on the basis of pressure
vanes and 13 runner vanes. Casing and draft tube are also difference at inlet and outlet boundary of domains. Various
considered as per original dimensions to be manufactured. formulae used for computation of different parameters are
Therefore the simulated design consists assembly of casing, given below:
runner and draft tube as our interest is to get complete
performance of the prototype turbine. Each component is Specific speed Ns = NÖP/H5/4
modelled separately and then assembled to get the complete Available power P=rgQH
assembly through proper interfaces. Mesh with scale factor
1.2 is used for importing to ANSYS CFX Pre. 3D real flow Unit speed N11= ND / ÖH
simulation analysis is done for experimentally tested Francis Unit discharge Q11= Q / D 2ÖH
turbine using ANSYS CFX 11 software. The rotational speed
Unit discharge Q11= P11 / (9810*Efficiency)
of runner is specified, stay vane and guide are kept at frozen
state. All inner boundary of turbine space are considered Unit power P11= P / D2H 3/2
smooth with no slip. Pressure Pr = r g H
Table 1: Summary of mesh data (Head loss) domain H loss
= (Pr inlet – Pr ) / 9810
outlet

Domain part No. of No. of Type of Havilable = (Inlet Pressure casing

- Outlet Pressure draft tube
)/9810
nodes elements element
Total head loss
Casing 204447 1605723 Tetrahedron
Htotal loss = H1 loss + H2 loss + H3 loss + .. Hn loss
(including stay
vanes & guide (For n number of domains)
vanes)
Turbine efficiency
Runner 98741 382088 Tetrahedron
Draft tube 121845 35961 Tetrahedron hexp. = Havailable*100 / (Havailable - Hloss)
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 95
ISSN No. 2230 – 7699 © MIT Publications

Table 2: Turbine specification site condition where prototype turbine is to be installed. For
the selection of prototype turbine, first of all model turbine is
Turbine model Francis Turbine selected (satisfying specification as per Table 2) which is
Shaft alignment Horizontal Axis homologous to the prototype turbine. Based on these data,
efficiency of prototype turbine is calculated. Also all the
Ns of turbine 266.19 m-kW
parameters are calculated for the prototype turbine based on
Model selected F280 the selected model. For present study conditions available at
Desired P generator output 3000 kW the actual site conditions are given in Table 2.
Rated head available 48 m The integrated and cross sectional view of assembled hydro
Desired P turbine output 3142 kW turbine is shown in Figure 2 and Figure 3.
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

III. METHODOLOGY OF WORK

Complete process comprised from AutoCAD drawing to the
CFX post covers following steps:
Figure 2: Assembled Francis Turbine
• 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 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
ISSN No. 2230 – 7699 © MIT Publications

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 Figure 5: Variation of head & efficiency wrt
optimum efficiency can be obtained when diameter of runner discharge of prototype turbine
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 Table 4: Model details
efficiency variations wrt discharge for prototype turbine are
shown in Figure 5. For broader visualisation of results, Axis of turbine vertical
experimental and CFD investigation is done at design and Type of draft tube elbow tube
off-design points.
Model head 28 m
Table 3: Experimental results of prototype Specific speed of turbine 266.19 m-kW
Sl. N11 P11 hexp. H Pr. P Q Q11 Runner diameter 0.35 m
No. % (m) (Pa) (kW) (m3/s) No. of runner blades 13
1 70 9.00 89.00 74.95 735221.46 5956.75 9.10 1.03 No. of guide vanes 18
2 80 9.30 92.80 57.38 562903.93 4123.57 7.89 1.02 PCD of guide vanes 0.40 m
3 87.5 9.28 93.10 47.97 470541.74 3144.74 7.18 1.01
No. of stay vanes 18
4 90 9.22 93.00 45.34 444763.60 2864.98 6.93 1.01
Best efficiency 92.10 %
5 100 8.70 89.50 36.72 360258.52 1975.06 6.13 0.99
N11 at best efficiency point 83.8
P11 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
ISSN No. 2230 – 7699 © MIT Publications
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

Sl. N11 Loss (m) Total Head

No. Casing Runner Draft Losses Developed
Tube (m) (m)
Figure 7: Draft tube mesh
1 70.00 2.336 4.464 1.360 8.160 68.84
Properties are defined in CFX pre and after running 2 80.00 0.499 3.751 0.015 4.265 57.34
solver final results are visualized and analysed in CFX post. 3 87.50 0.347 2.485 0.342 3.175 49.42
CFX-11 is a general purpose Computational Fluid Dynamics
(CFD) code, combining an advanced solver with powerful 4 90.00 0.192 2.154 0.678 3.024 45.92
pre and post-processing capabilities. The next-generation 5 100.00 1.490 2.091 0.692 4.273 40.05
physics pre-processor, CFX-Pre, allows multiple meshes to
be imported, allowing each section of complex geometries to Table 6: Computational & Experimental Results
use the most appropriate mesh.
Sl. N11 Head (m) Efficiency (%)
VI. RESULTS AND DISCUSSIONS No. Hexp. Hcfd hexp. hcfd
The numerical simulation is done in ANSYS CFX 11.
Experimental results are shown in Table 2 which are obtained 1 70 74.95 68.84 89.00 88.15
by scaling up the results of model turbine as per the scale 2 80 57.38 57.34 92.80 92.56
ratio of 2.88. For prototype turbine available head and 3 87.5 47.97 49.42 93.10 93.58
discharge for which turbine will operate maximum period of
4 90 45.34 45.921 93.00 93.41
time is known quantity from the detailed project report
(Table 1). 5 100 36.72 40.05 89.50 89.33
Rotational speed of turbine is taken as the rated speed i.e.
600 rpm, specific speed calculated is 266 m-kW with the help In the calculation of experimental efficiency of prototype
of which runner diameter is calculated as 1010 mm, N11 and turbine step factor taken by moody's formula is 1%.
P11 is also computed with these results. Generator efficiency Computational results show increase in efficiency at design
is assumed to be 95.50% which is fairly good in this case. point wrt experimental results. However at off design point
The experimental results for prototype turbine are obtained there is variation in efficiency with both methods. Possible
by projecting the results of homologous model turbine in reason for this increase in efficiency is the change in the tip
proportion to the computed scale ratio. Then efficiency of portion design of the casing. Change in casing tip portion
prototype turbine is calculated at rated head of 48 m and rated improves passage of water from casing to runner inlet. The
flow of 7.25 m3/s, subsequently efficiency of turbine at other best efficiency point is obtained when head is made available
unit speeds are also computed to get broader visualization of near 48 m and Guide vane opening of 75.2%. Losses in various
operation of turbine at design and off design operating domains are shown in table 5, which shows that optimum
regimes. Experimental results for prototype turbine are losses occur when unit speed of turbine is near 87.5.This
tabulated in Tables 5 and 6. It is well known that all these supports that for efficient and optimum performance of turbine
parameters could be combined to unit quantities to carry out unit speed of turbine should be near 87.5 and accordingly
data reduction. This approach is followed to present the other factors should be decided for the design of prototype
results. The assembly of turbine considered here comprised turbine.
of Casing, Stay vane, Guide Vane, runner and Draft tube Streamline flows are shown indicating maximum turbulence
(shown in Figures 5, 6 and 7 respectively).Three number of in the runner which is converted into head loss. Runner is the
domains are made viz. casing domain (Stationary), runner major component of turbine for energy conversion, therefore
domain (Rotating) and draft tube domain (Stationary). As the runner part plays critical role for deciding the efficiency of
dimension of whole assembly is big, therefore meshing of turbine. Table 5 illustrates losses occurring in casing, runner
the domains are done separately and then merged together. and draft tube domains. For this casing tip portion design
Number of grid points in casing domain, runner domain 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
ISSN No. 2230 – 7699 © MIT Publications

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 Figure 9: Variation head & discharge
they are not falling below the vapour pressure of water, we
can conclude that they are free from cavitation.
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 Figure 10: Variation efficiency & discharge
domains, which should be minimized.

Figure 11: Blade Loading from Leading edge

Figure 8: Pressure contour in casing domain to trailing edge
MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 99
ISSN No. 2230 – 7699 © MIT Publications

From Tables 5 and 6 it is seen that for maximum efficiency can be used for investigating the actual performance of
total losses is minimum. Pressure contour and velocity contour prototype turbine, to get possible sources of improvement in
shown in Figure 12 and 13 respectively describes the flow the design geometry with cost effective technique in lesser
structure inside various components of francis turbine. time. Validation of results done by this method will lead to
Velocity profile from Figure 12 inside the turbine assembly become very good source of optimization technique for
indicates that casing and runner domain has smooth velocity hydraulic turbine performance.
profile whereas as soon as water enters draft domain velocity Results from experimental evaluation and Simulation
starts decreasing and profile becomes non uniform. Similarly performed at different unit speed range for optimum guide
from Figure 13 it becomes clear maximum energy conversation vane opening and at rated speed of runner 600 rpm. Results
takes place inside the casing domain where pressure is highest show that optimum turbine performance at actual site will
and as water moves further its pressure decreases gradually. occur when the unit speed of turbine is near 87.5 working
The best operating regimes, losses and flow pattern can be under a head of 48 m and accordingly other parameters are
investigated from the calculated flow parameters of numerical available. On the basis of computational results design
simulation. Thus it can be concluded that CFD simulation 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 also due to discretisation of domains and solution of deferential

The paper brought out the validation of experimental results equations in computational methods. The total computed losses
with the computational investigation. The maximum are observed to be minimum at best operating point.
efficiency regime indicated by both approaches is nearly same. Hence the results obtained are fairly matching, however
Reason for slight difference of efficiency computed by streamline flow in some reasons have more turbulence which
experimental and computational method can be because of is due to occurrence of losses. Difference in results at off
instrumental and human errors in experimental testing and peak conditions between experimental and computational
 MIT International Journal of Mechanical Engineering Vol. 1 No. 2 Aug 2011, pp 93-100 100
ISSN No. 2230 – 7699 © MIT Publications

results is due to error in discretising the governing equations Reports on Turbine Testing” Problem Oriented Research
and flow domain. Losses not considered very precisely. There Laboratory (Fluid Mechanics and Hydraulic Mechanics Lab)
can be human and instrumental error in experimental Bhopal, India.
calculations. Prediction of turbine performance by CFD gives [3] P. Krishnamachar, Dr. V.V. Barlit (Russia), M.M. Deshmukh,
the idea to know the flow behaviour inside the turbine “Manual on Hydraulic Turbine” (MANIT, Bhopal).
model and get the information about the intricacy of flow [4] Guoyi Peng, Shuliang Cao, Masaru Ishizuka, Shinji Hayama
pattern, since the flow inside the turbine in actual is very (2002); “Design optimisation of axial flow hydraulic turbine
complicated. CFD results gives the qualitative information. runner: Part II-Multiobjective Constrained Optimzation
It provides the tool to simulate the flow conditions with Method”, International Journal for Numerical Methods in
different geometries in lowest possible time, thus providing Fluids, Vol. 39, Issue 6, pp. 533-548.
reduction in design analysis and yet developing robust [5] Guoyi Peng (2005): “A practical combined combined
technology along with aiding in reducing gestation computation method of mean through-flow for 3D inverse
period. design of hydraulic turbine machinery blades”, ASME Journal
of fluid engineering.
NOMENCLATURE [6] V. Prasad, “CFD approach for design optimization and
validation for axial flow hydraulic turbine”, Indian J of Eng
H = Net head (m)
and Materials Sciences, Vol. 16, August 1999, 229-236.
Q = Discharge through turbine (m 3/s)
[7] Bernard M., Maryse P., Robert M. and Anne. M. G., Proc.
N = Rotational speed of turbine (rpm) ASCE Water Power Conference, Las Vegas, USA 1999.
h = Mass density of water (kg/m3) [8] Peng G., Cao S., Ishizuka M. and Hayama S., Int. J. Numer
g = Gravitational acceleration (m/s 2) Methods Fluids, 39(6) (200) 533-548
P = Turbine power (kW) [9] Daniel B, Romeo R., and Sebastian M, Proc. Int. conf. on
CSHS03, Belgrade, (2003) 29-36.
Prated = Power output of turbine at rated condition (kW)
[10] Liplej A., Proc. Inst. Mech. Eng., Pt. A. J. Power and Energy,
Pgeneratoroutput = Power output of generator (kW) 218 (2004) 43-50.
EL = Elevation level wrt mean sea level. [11] Guoyi P., J. Fluids Eng., 27 (2005) 1183-1190
PCD = Pitch circle diameter (mm) [12] C.A.J. Fletcher, “Computational Techniques for Fluid
N11 = Unit speed Dynamics” Vol. 1, Springer Pub. 1991.
Q11 = Unit discharge [13] Lewis RI, Turbo machinery performance analysis (Arnold,
P11 = Unit power Londan), 1996.

Pr. = Pressure (Pa) [14] CFX 11, “User Manual, Ansys Inc.” 2004.

Hexp. = Head by experimental testing (m) [15] Liplez A., Proc. Inst. Mech. Eng., Pt. A. J. Power and Energy,
218 (2004) 43-50.
Hcfd = Head by CFD testing (m)
[16] Guoyi P., J. Fluids Eng., 27 (2005) 1183-1190.
hexp. = Efficiency obtained by experimental testing
[17] Shukla M., “CFD Analysis of 3-D flow and it's validation for
hcfd = Efficiency obtained by CFD testing francis turbine”, 34th National Conference on FMFP, BIT
Mesra (2007) 732-737.
ACKNOWEDGEMENTS [18] Wu J., Shimmel K., Tani K., Niikura K. and Sato J. J., Fluid
Author would like to express sincere gratitude towards all Engg., 127(2007) 159-168.
related to MANIT, Bhopal and KBL Pune, for continuous [19] Rao, V. Shrinivas, Tripathi, S.K. (2007): Role of CFD analysis
encouragement and cooperation made available to do the in hydraulic design optimization of hydro turbines, Proceeding
associated paper work. of National Seminar on CFD-The 3rd Dimension in Flow
Analysis & Thermal Design, Bhopal(India), pp.196-201.
REFERENCES [20] Vishnu Prasad; V.K. Gahlot, P. Krishnamachar (2009) “CFD
[1] Kirloskar Brothers Limited “Data for Francis turbine model”, approach for design optimization and validation for axial flow
Corporate Research and Engineering Division (CRED-KBL), hydraulic turbine”, Indian Journal of Engineering and
Pune, India. Material Sciences, pp. 229- 236 .
[2] Maulana Azad National Institute of Technology, “Project

View publication stats