International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014

ISSN 2250-3153

CFD Analysis of Pelton Runner

Amod Panthee*, Hari Prasad Neopane**, Bhola Thapa**
*

Turbine Testing Lab, Department of Mechanical Engineering, School of Engineering, Kathmandu University, Dhulikhel, Nepal
**
Department of Mechanical Engineering, School of Engineering, Kathmandu University, Dhulikhel, Nepal

Abstract- This paper presents Computational Fluid Dynamics (CFD) analysis of Pelton turbine of Khimti Hydropower in Nepal. The
purpose of CFD analysis is to determine torque generated by the turbine and pressure distributions in bucket for further work on
fatigue analysis. The CFD analysis is carried out on model size Pelton runner reduced at 1:3.5 scale to minimize computational cost
and time. The operating conditions for model size runner is selected in accordance with IEC 60193 and IEC 1116. The paper describes
the methods used for CFD analysis using ANSYS CFX software. 3 buckets are used to predict the flow behavior of complete Pelton
turbine. k- and SST turbulence model with interphase transfer method as free surface and mixture model is compared in the paper.
The pressure distribution is found maximum at bucket tip and runner Pitch Circle Diameter (PCD). The torque generated by the
middle bucket is replicated over time to determine total torque generated by Pelton turbine.
Index Terms- Pelton turbine, Computational Fluid Dynamics (CFD), Similitude, Turbulence Model, Torque

I. INTRODUCTION

omputational Fluid Dynamics (CFD), is a branch of fluid dynamics which uses numerical methods and algorithms to solve fluid
flow problems. Reduction of time and cost to predict the model behavior in real environment is key advantage of CFD analysis.
However, the CFD analysis results should be analysed and validated before the model is accepted [1].
ANSYS CFX and ANSYS Fluent are the commercial CFD codes available. The main difference between these is the way solvers
integrate the flow equations and solution strategies. CFX uses finite volume elements to discretize the domain. Contrarily, Fluent
utilizes finite volumes. They are both control volume based solvers, which ensures conservation of flow quantities. The CFD analysis
of Pelton turbine in the paper is carried out using ANSYS CFX [2].
The Pelton turbine is a good choice in situation where the volume flow is small relatively to head. The paper describes the CFD
analysis of scaled Pelton turbine of Khimti Hydropower in Nepal. The purpose of CFD analysis of model Pelton turbine is to
determine the pressure distribution in the Pelton bucket which shall be used for fatigue analysis of Pelton runner with two different
bucket geometry, with and without fillet at root section, as shown in figure 1. The design geometry of bucket was changed during
welding repair and runner failure occurred after 10000 hours of operation [3]. In addition, the torque generated by the turbine is
determined in the paper.

With fillet between

splitter and runner disc

Without fillet between

splitter and runner disc

(a) Before Repair

(b) After Repair
Figure 1. Runner geometry before and after repair
II. METHODOLOGY
The methodology used for CFD analysis of Pelton turbine is shown in Figure 2. The 3D model of Pelton turbine was created with
reference to Khimti Hydropower. The rotating domain and stationary domain for CFD analysis was modeled using PRO/Engineer and
ANSYS Design Modeler respectively. The model size runner was selected considering laboratory test facility and IEC 60193 test
requirements. The numerical methods and boundary conditions were defined in ANSYS CFX and the numerical results were
computationally and analytically validated. The torque was calculated and computationally valid pressure distribution was exported
for fatigue analysis.

www.ijsrp.org

International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014
ISSN 2250-3153
Rotating Domain
(PRO/Engineer)

3D Modelling of Pelton Turbine

(With reference to Khimti Hydropower)

(Meet the requirements for Experimental Test)

Laboratory Test
Facility

Numerical Methods

CFD Analysis using ANSYS CFX

Boundary Conditions

Analytical Solution

Analysis of the Numerical Results

Mesh Dependent Test

IEC 60193

Selection of Model Size Runner

Stationary Domain
(ANSYS Design
Modeler)

Export computationally valid pressure

distribution for fatigue analysis

Figure 2. Methodology for CFD analysis

III. 3D MODELING OF PELTON TURBINE

2D contour plot of Pelton bucket was used to model 3D Pelton runner for CFD analysis. Each contour lines were exported using
AutoCAD and imported in PRO/Engineer software to build 3D model, shown in Figure 3. Figure 4 shows the selected Pelton bucket
for CFD analysis. Half bucket was selected for analysis since the Pelton bucket is symmetric about the splitter. This reduces the total
time for computational analysis [4].

Figure 3. 3D Model of Pelton Turbine

Figure 4. Selected Pelton Bucket for CFD Analysis

IV. SELECTION OF MODEL SIZE RUNNER

Scaled runner has been selected to reduce the computational cost and considering the future prospects of verifying the CFD result at
Turbine Testing Lab, Kathmandu University. The laboratory test facility and minimum requirements for model test of hydraulic
turbines mentioned in IEC 60193 and IEC 1116 has been used to obtain hydraulic similitude conditions between the model and
prototype. The turbine data for prototype is shown in Table 1.
A kinematically similar turbine is obtained when the model and prototype are geometrically similar and ratio of their fluid velocity
and peripheral velocity is equal. A complete similarity is achieved when the Reynolds number is equal between the model runner and
prototype in addition to kinematic similarity. These conditions are satisfied when the speed number is equal in both the turbines [5].
Therefore, equations 1 3 are used to determine the hydraulic similitude conditions [6].

Equation 1
Equation 2

Equation 3

Besides, minimum requirements for model Pelton turbine as stated in IEC 60193 and hydraulic similitude conditions, shown in
Table 2, and the laboratory test facility available at Turbine Testing Lab, shown in table 3, are used to determine the appropriate
operating conditions for model Pelton turbine, shown in Table 4 [6] [7].

www.ijsrp.org

International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014
ISSN 2250-3153

Table 1: Turbine Data: Prototype

Parameter
Unit
Pitch Circle Diameter mm
Number of Buckets
Number of Nozzles
Head (H)
m
Discharge (Q)
m3/s
Rotational Speed
RPM
Table 3: Laboratory Constraint
Parameter
Unit
Head
Open System
m
(H)
Closed System m
Discharge (Q)
m3/s
Torque (T)
Nm

Value
1400
22
2
660
2.15
600

Value
30
150
0.5
2000

Table 2: Hydraulic Similitude Conditions

Parameter
Unit
Speed Number
Speed Factor
Flow Factor
Minimum Reynolds Number
Minimum Hydraulic Specific Energy J/Kg
Minimum Bucket Width
mm

Value
0.076
10.44
0.014
2 106
500
80

Table 4: Selected Model Turbine Operating Condition

Parameter
Unit
Value
Head (H)
m
53.9
Discharge (Q)
m3/s
0.05
Pitch Circle Diameter (PCD)
mm
400
Scale Factor
1:3.5

V. MESHING
Stationary and rotating domain was discretized separately using ANSYS Meshing. The stationary domain, shown in Figure 5 (a),
consists of two regions, water and air flow region. Water flow region is of prime interest while discretizing the stationary domain.
Sweep method was used in core region of water while inflation method was used in boundary region of water and air [8]. The mesh in
stationary domain consisted of structured hexahedral type mesh. Figure 5 (b), (c) shows the mesh in stationary domain.
Water Flow Region

Air Flow Region

(a) Stationary Domain

(b) Mesh
Figure 5: Stationary Domain

(c) Nozzle Region

Bodies of Influence

(a) Rotating Domain

(b) Mesh

(c) Bucket surface and Inlet

Figure 6: Rotating Domain

www.ijsrp.org

International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014
ISSN 2250-3153

Automatic type of meshing method was used in rotating domain due to complex geometry of the bucket. The rotating domain was
divided into three region of interest where fine mesh was created. A body of influence method was used in inlet and outlet region of
the bucket, and the bucket surface meshed using inflation method, shown in Figure 6 (a) [8].
VI. NUMERICAL ANALYSIS
The governing equations of viscous flow are based on conservation of mass, momentum and energy which are langrangian in
nature. The governing equations are expressed using equations 4 6 [9].
Conservation of Mass:

Equation 4

Conservation of Momentum:

Equation 5

Conservation of Energy:

Equation 6

The numerical analysis of CFD in Pelton turbine consists of incompressible fluid flow that reduces the conservation of mass and
momentum to equation 7 8 respectively. In addition, the temperature effect is negligible during the analysis. Therefore, conservation
of energy is ignored during analysis [9].
Equation 7
Equation 8
The standard k- model is extensively used due to its excellent performance. But, it shows poor performance in unconfined flow
regions where the boundary is curved, and in rotating and swirling flows. Similarly, the Wilcox model does not require wall damping
functions and it is robust in near wall regions. However, its robustness is decreased due to sensitivity in free stream region. SST model
is the hybrid model which used the Wilcox model in near wall region and standard k- model in the fully turbulent region. A
comparative study of turbulence model has been carried out using k- and k- based SST model separately in the paper [10].
The domain type for both the rotating and stationary domain was defined fluid. Air and water, both at 25 0C, with continuous fluid
morphology was used in analysis. The fluid model was selected as homogeneous model with standard free surface model. The
interface compression level was set to 2 to produce better convergence. Shear Stress Transport (SST) type turbulence model has been
used with automatic wall function. The surface tension model has been set as continuum surface force with primary fluid as water.
Interphase transfer model was studied separately using free surface and mixture model. The initial conditions for the fluid volume
fractions was defined 1 and 0 for air and water respectively. Since there is no pressure difference between the inlet and the outlet, the
reference pressure was set to 1 atmosphere. And the domain motion option was set to rotating and stationary for rotating and
stationary domain respectively. The symmetry boundary condition was applied in the middle plane diving the turbine into two
sections. Smooth wall with no slip conditions was applied in the bucket wall.

VII. RESULTS AND DISCUSSION

The CFD analysis was carried out using k- and SST model separately using mixture model and free surface model as interphase
transfer method, as shown in Table 5. The simulation failed to converge using k- turbulence model. However, SST model converge
for both mixture and free surface interphase models. This is due to the fact that k-e model has poor performance in unconfined flow
where the boundary is curved. But, SST model uses k- and Wilcox model in fully turbulent and near wall region respectively.
Table 5: Convergence Vs. Turbulence Model and Interphase Transfer
Mesh dependent test was carried out to computationally
Mixture Model
Free Surface Model
validate the result in seven different mesh sets. The total
K E Model
Failed
Failed
number of nodes was varied from 0.75 million to 4.3
SST Model
Converged
Converged
millions. Figure 7 shows the mesh dependent test using
SST model using mixture model and free surface model as interphase transfer method. It was found that the results are better when
using free surface model [11].
The pressure distribution in middle bucket was exported from ANSYS CFX, shown in Figure 8. It was found that the pressure
peaks are obtained at bucket tip and PCD of runner. The pressure peak in bucket tip is due to flow disturbance when jet strikes bucket
tip. It is obvious to obtain the pressure peak at runner PCD since the Pelton runner are designed such that it would convert most of the
hydraulic energy to mechanical energy when the jet strikes the runner PCD [12]. The water volume fraction with velocity index and
pressure distribution in Pelton bucket is shown in Figure 9.
The torque generated by the runner can be predicted by using the torque data produced by middle bucket. A single torque data is
replicated over time calculating the frequency of bucket during rotation, using equation 9. The calculated frequency for the model
turbine is 0.0045 seconds. Figure 10 shows torque generated by different buckets and total torque produced by Pelton turbine. The
comparison of computational torque with analytical solution obtained using equation 10 showed that mechanical efficiency of the
www.ijsrp.org

International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014
ISSN 2250-3153

turbine is 82.5%.
Max. Pressure (Pa) 1000

Max. Pressure (Pa) 1000

200
180
160
140
120

Mixture Model
Free Surface Model

100
80
0

4
6
Mesh Set

160
140
120
100
80
60
40
20
0

at runner PCD
at bucket tip

10

20

39

58

77

96

115

Time Steps

Figure 7: Maximum Pressure Vs. Mesh Set

Figure 8. Maximum Pressure Vs. Time Steps

(a) At bucket tip

(b) At Runner PCD

Figure 9: Water Volume Fraction above 0.75 (left) and Pressure Contour in Pelton bucket (right)
90

Torque (Nm)

70
50
30
10
-100.005

0.01

0.015

0.02

0.025

0.03

0.035

Time (s)
Bucket 1

Bucket 2

Bucket 3

Bucket 4

Bucket 5

Total Torque

Figure 10. Torque generated by buckets over time

www.ijsrp.org

International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014
ISSN 2250-3153

Equation 9
Equation 10

VIII. CONCLUSION
The CFD analysis of scaled Pelton turbine of Khimti Hydropower was performed using ANSYS CFX software. The scale factor
for selected model turbine was 1:3.5. Scaling of the turbine reduces computational time and cost. The time and cost in CFD analysis of
Pelton turbine is also reduced by selecting 3 buckets to predict the behavior of complete turbine. The result showed that SST model is
robust turbulence model to conduct CFD analysis of Pelton turbine. In addition, free surface interphase transfer method gives better
result than mixture model. It was found that peak pressure is obtained at bucket tip and PCD of runner. The pressure distribution in
each bucket surface was exported using monitor tool in ANSYS CFX for further analysis on fatigue of Pelton turbine. The torque
results obtained from the single bucket can be replicated over time to predict the total torque transferred by the Pelton turbine. The
torque results obtained from CFD showed that the model Pelton turbine has efficiency of 82.5%.
REFERENCES
[1] A. Sharma, P. Sharma, A. Kothari, Numerical Simulation of Pressure Distribution in Pelton Turbine Nozzle for the Different
Shapes of Spear, International Journal of Innovations in Engineering and Technology, Vol 1, Issue 4, December 2012.
[2] ANSYS User Guide, Version 14.0, 2011
[3] A. Panthee, B. Thapa, H. P. Neopane, Quality Control in Welding Repair of Pelton Turbine, Proceedings in 3rd Asia Pacific Forum
of Renewable Energy (AFORE), Jeju, Korea, November 4 7, 2014
[4] L. Souari, M. Hassairi, Numerical Simulation of the Flow into a Rotating Pelton Bucket, International Journal of Emerging
Technology and Advanced Engineering, Vol. 3, Issue 2, February 2013.
[5] United States Department of Interiors Bureau of Reclamation (USBR), Hydraulic Model Testing, Denver, Colorado, 1980.
[6] International Electro-technical Commission, IEC 60193, Hydraulic turbines, storage pumps and pump turbines Model
Acceptance Tests, 1999.
[7] International Electro-technical Commission, IEC 1116, Electromechanical Equipment Guide for Small Hydroelectric Installations,
1992.
[8] ANSYS Modeling and Meshing Guide, Version 14.0, 2011.
[9] ANSYS CFX Modeling Theory, Version 14.0, 2011.
[10] L. E. Klemetsen, An Experimental and Numerical Study of Free Surface Pelton Bucket Flow, MSc Thesis, Norwegia University
of Science and Technology, 2010.
[11] D. Jost, P. Menzar, A. Lipej, Numerical Prediction of Pelton Turbine Efficiency, IOP Conference Series: Earth and
Environmental Science, Vol. 12, 2010.
[12] A. Perrig. F. Avellan, j. L. Kueny, M. Farhat, E. Parkinson, Flow in Pelton Turbine Bucket: Numerical and Experimental
Investigations, Transactions of the ASME 128 (2006).
AUTHORS
First Author Amod Panthee, MS by Research Student, Turbine Testing Lab, Department of Mechanical Engineering, School of
Engineering, Kathmandu University, Dhulikhel, Nepal, email: amodpanthi@ku.edu.np
Second Author Associate Professor Hari Prasad Neopane, PhD, Department of Mechanical Engineering, School of Engineering,
Kathmandu University, email: hari@ku.edu.np
Third Author Professor Bhola Thapa, PhD, Department of Mechanical Engineering, School of Engineering, Kathmandu
University, email:bhola@ku.edu.np
Correspondence Author Amod Panthee, amodpanthi@ku.edu.np, amodpanthi@gmail.com, +977-9841551828

www.ijsrp.org