1. NUMERICAL SIMULATION OF FLOW THROUGH
RADIAL IMPELLERS AND EVALUATION OF THE
SLIP FACTOR
by
Hassan Adel Talaat El-Sheshtawy
A Thesis Submitted to the
Faculty of Engineering at Cairo University
in Partial Fulfillment of the
Requirements for the Degree of
MASTER OF SCIENCE
in
MECHANICAL POWER ENGINEERING
FACULTY OF ENGINEERING, CAIRO UNIVERSITY
GIZA, EGYPT
2014
2. NUMERICAL SIMULATION OF FLOW THROUGH
RADIAL IMPELLERS AND EVALUATION OF THE
SLIP FACTOR
by
Hassan Adel Talaat El-Sheshtawy
A Thesis Submitted to the
Faculty of Engineering at Cairo University
in Partial Fulfillment of the
Requirements for the Degree of
MASTER OF SCIENCE
in
MECHANICAL POWER ENGINEERING
Under the Supervision of
Prof. Mohamed G.
Khalafallah
Professor
Principal Adviser
Dr. Abdel-Naby M.
Ahmed
Assistant Professor
Adviser
Dr. Ahmed I. Abd
El-Rahman
Assistant Professor Mech
Adviser
Mechanical Power Engineering, Faculty of Engineering, Cairo University
FACULTY OF ENGINEERING, CAIRO UNIVERSITY
GIZA, EGYPT
2014
3. NUMERICAL SIMULATION OF FLOW THROUGH
RADIAL IMPELLERS AND EVALUATION OF THE
SLIP FACTOR
by
Hassan Adel Talaat El-Sheshtawy
A Thesis Submitted to the
Faculty of Engineering at Cairo University
in Partial Fulfillment of the
Requirements for the Degree of
MASTER OF SCIENCE
in
MECHANICAL POWER ENGINEERING
Approved by the
Examining Committee
Prof. Mohamed G. Khalafallah
Professor, Thesis Main Advisor
Prof. Moustafa Abd Elhamed Rezk
Professor, Mech. Power Eng. Dept., Faculty of Engineering, Cairo University, Member
Prof. Ahmed Maged Ahmed Mohamed
Professor, Mech. Power Eng. Dept., Faculty of Engineering - Shoubra, Benha University, Member
FACULTY OF ENGINEERING, CAIRO UNIVERSITY
GIZA, EGYPT
2014
4. Engineer: Hassan Adel Talaat El Sheshtawy
Date of Birth: 30 / 07 / 1988
Nationality: Egyptian
E-mail: haelsheshtawy@gmail.com
Phone: 01282637989
Registration Date: 01 / 10 / 2010
Awarding Date: / /
Degree: Master of Science
Department: Mechanical Power Engineering
Supervisors:
Prof. Dr. Mohamed G. Khalafallah
Dr. Abdel-Naby M. Ahmed
Dr. Ahmed I. Abd El-Rahman
Examiners:
Prof. Dr. Mohamed G. Khalafallah
Prof. Dr. Moustafa Abd Elhamed Rezk
Prof. Dr. Ahmed Maged Ahmed Mohamed (Benha University)
Title of Thesis:
NUMERICAL SIMULATION OF FLOW THROUGH RADIAL IMPELLERS AND
EVALUATION OF THE SLIP FACTOR
Key Words:
Centrifugal pumps, Computational Fluid Dynamics, Slip factor, Hydraulic efficiency,
Impeller, Splitters
Summary:
The present work reports a three-dimensional computational fluid dynamics (CFD) analysis of the
flow through a centrifugal pump. The simulation is done using ANSYS/CFX commercial code.
Results from the simulation are in good agreement with the pump performance curve particularly
around the design point. Slip factor was calculated from the numerical results and compared with
known mathematical models. The effect of adding splitters and increasing number of blades on slip
factor, produced head and pump efficiency was studied. It was found that by increasing the number of
blades or splitter length, the slip factor improved. However, the resulting hydraulic efficiency did not
show a corresponding improvement due to the incurred hydraulic losses.
5. Acknowledgment
I am heartily thankful to my advisors, Prof. Mohamed G. Khalafallah, Dr. Abdel-Naby M.
Ahmed and Dr. Ahmed I. Abd El-Rahman , whose encouragement, guidance and support
from the initial to the end, enabled me to complete this thesis. Also, thanks are due to my
dad and mom for their supports
Lastly, I offer my regards and blessings to all who supported me in any respect during
the completion of this research.
v
11. 3.8 CPU-time versus the generated number of elements . . . . . . . . . . . . . 34
3.9 Comparison of numerical model head and the flow rate with the pump per-
formance curve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
4.1 The meridional velocity patterns through the passage at mid span of impeller
at Q/QBEP=1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37
4.2 Static head through the passage at mid span of impeller at Q/QBEP=1. . . . 38
4.3 3-D Streaming of flow field, and a contour plane of velocity at midspan of
four blades impeller at flow rate Q/QBEP=1. . . . . . . . . . . . . . . . . . 39
4.4 Slip factor versus flow coefficient at based on CSL. . . . . . . . . . . . . . . 41
4.5 Different span location . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42
4.6 Different span location at meridional view . . . . . . . . . . . . . . . . . . 42
4.7 The local slip factor between two blades at the tip at different cross section. 43
4.8 The slip factor and the flow coefficient at different number of blades using
CFD calculations and compared to Qiu’s model Eq 1.6. . . . . . . . . . . . 44
4.9 Slip factor at BEP at different number of blades . . . . . . . . . . . . . . . 45
4.10 The effect of adding four-splitters to the four-bladed impeller on the slip
factor. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45
4.11 Pump efficiency for different number of blade. . . . . . . . . . . . . . . . 46
4.12 Normalized head for flow different number of blades. . . . . . . . . . . . . 47
4.13 Pump efficiency for different splitter lengths. . . . . . . . . . . . . . . . . 48
4.14 Normalized head for different splitter. . . . . . . . . . . . . . . . . . . . . 49
B.1 The main dimensions of the impeller in CFTurbo . . . . . . . . . . . . . . 61
B.2 The meridional plane view in CFTurbo . . . . . . . . . . . . . . . . . . . . 62
B.3 The setup GUI in CFTurbo . . . . . . . . . . . . . . . . . . . . . . . . . . 63
B.4 The exporting GUI in CFTurbo . . . . . . . . . . . . . . . . . . . . . . . . 63
xi
12. List of Symbols and
Abbreviations
Mathematical Symbols
β1 Blade inlet angle.
β2 Exit blade angle.
β2 Flow exit angle.
˙m Mass flow rate, [ kg/s].
C
Se
Solidity or chord to space ratio.
ω Angular velocity[rad/s].
φ The volute casing tongue angle.
σ Slip factor, American definition.
σ Slip factor, European definition.
θ Wrap angle.
b2 Impeller width at exit .
b4 Volute casing width at exit .
BEP Best efficiency point.
xii
13. C Absolute velocity, [m/s].
Cm2 Meridional velocity at exit .
CSL Slip velocity.
Cu2 Theoretical whirl velocity.
D2 Impeller outer diameter.
D4 Outer diameter of volute casing .
DS Impeller shaft diameter .
FC2 Exit flow coefficient.
HS The slip Head [m].
Hth The theoretical head [m].
m Meridional distance on the Z-R plane.
N Revolutions per minute.
PS Pressure side.
Q Volume flow rate [m3/s] .
S2 Pitch at the blade exit.
SS Suction side.
t Blade thickness.
U Peripheral speed.
Z Number of blades.
PDE Partial differential equation .
xiii
14. This thesis is dedicated to my mother, father,
and my beloved family.
xiv
15. Abstract
THE aim of this work is to study the slip phenomenon in centrifugal pumps. Flow sim-
ulation can give better understanding of flow behavior through radial impellers. The
present study is directed towards evaluating slip factor and its effect on pump performance
through the use of Computational Fluid Dynamics (CFD). A commercial software (ANSYS
- CFX) is used to perform the present simulation of which is validated using the performance
data of a four-bladed centrifugal pump. The pump geometry is first generated, discretized
then simulated. The frozen rotor technique is used to model the interaction between the
rotor and stator. The validated model is used to evaluate the slip factor and compare the
results with available mathematical models. The effect of varying number of blades and
adding splitters on slip factor and pump performance is studied.
The results show that the evaluated slip factor is in reasonable agreement with some of
the available mathematical models. The generated head increases as slip factor increases.
Adding splitters increase the predicted head, while adding more blades decreases the gener-
ated head. On the other hand, splitters addition and increasing the number of blades lead to
less hydraulic efficiency due to relatively greater friction losses.
Keyword : Centrifugal pumps, Computational Fluid Dynamics, Slip factor, Hydraulic
efficiency, Impeller, Splitters
1
16. Chapter 1
Introduction
1.1 Introduction
Slip phenomenon in turbomachines takes place due to the inability of the fluid to faithfully
follow the guiding blades. The characteristic curves and performance of centrifugal pumps
are greatly affected by the way in which the fluid exits the impeller to the volute casing. The
direction of the flow depends on how the fluid follows the blade turning angles, and varies
with location in the span-wise direction. The slip factor, in radial impeller, is a measure
of such flow deviation and is defined in terms of the exit whirl velocity. Slip occurs when
the blades fail to perfectly guide the flow, causing the flow to deviate at the impeller exit
with a mean relative angle β2 less than the blade exit angle β2 , as shown in Fig.1.1. This
results in a slip factor less than unity, significant reduction in the work done on the fluid,
and consequently, the pump head is dramatically influenced.
2
17. C`u2
Cu2
β`2 β2
Cm2
U2
C2
W2
Cm2/tanβ`2 CSL
W2 `
C2`
Figure 1.1: Actual (solid line) and theoretical (dashed line) exit velocity triangles
The effect of slip coefficient on head and flow rate (H-Q) curve is shown in figure
1.2. The theoretical head of a pump is represented by Eq 1.1, where all terms except Q is
constant, thus it can be represented by linear relation Eq (1.1), but due to losses shown in
Fig 1.2, the relation of H-Q curve does not behave like linear, and indicates also that the
head decreases due to slip Eq 1.2.
Hth =
Cu2 U
g
=
U2
2
g
−
U2Q
gπD2b2
cotβ2 (1.1)
Hs = σ Hth (1.2)
3
18. Figure 1.2: Slip losses in H-Q curve of centrifugal pump
Keeping this in mind, the slip in radial impeller depends on various parameters, such as
the pump flow rate, the number of blades and the blade geometry. Although increasing the
number of blades helps reduce the flow deviation in the impeller exit, it may also promote
blockage in the flow channels. Therefore, a careful study on the effect of the number of
blades on the slip coefficient, developed head and pump efficiency is considered in this
work.
In this study we perform a three-dimensional Computational Fluid Dynamics (CFD)
simulation of fluid flow through a centrifugal pump using the commercial software ANSYS-
CFX. This simulation is used to evaluate the slip factor and compare the results with avail-
able mathematical models. A parametric study on the effect of varying number of blades
and splitters on slip and the effect of this on pump performance is also done.
In this chapter we review previous research work. Section 1.2 reviews the available
mathematical models for this phenomenon. Section 1.3 reviews computational studies while
section 1.4 sets the objective of this thesis.
4
19. 1.2 Slip factor mathematical models review
The slip factor is defined in terms of the well known expression of the slip velocity (CSL),
according to Stodola [19] :
σ = 1−
CSL
U2
= 1−
π sin(β2 )
Z
(1.3)
Busemann [7] was the first to develop a theoretical framework for the estimation of the
slip velocity and the calculation of the slip factor for several blade angles and number of
blades. The results were plotted as a function of the inlet-to-outlet radius ratio and indi-
cated constant slip behavior zone at small ratios followed by a sharp reduction at higher
values of the inlet-to-outlet radius. Wiesner [22] presented a general review of the various
prediction methods, developed for the calculation of basic slip factors, applicable for cen-
trifugal impellers. He concluded the first part of his work by supporting the validity of the
classical theoretical method of Busemann [7]. Wiesner carefully explored the Busemann
experimental results and proposed a simpler empirical expression for slip factor estimation
which reads.
σ = 1−
sinβ2
Z0.7
(1.4)
Although limited by the impeller inlet-to-outlet radius ratio, Wiesner’s values showed
a more accurate fit to the Busemann test data. Weisner then carried out extensive compar-
isons of slip factors, with test data, reported in literature for over than 60 different impeller
geometries and further demonstrated its high potential in describing the slip phenomenon.
That is why the Wiesner model is currently representing the most widely-used method for
centrifugal impellers.
Backstrom [5] derived a unified correlation for the slip factor assuming a single relative
eddy (SRE) centered on the rotor axis in his fluid dynamic model. He ignored other mech-
anisms affecting the slip phenomenon such as the blade turning angle and the flow-induced
wakes, and proposed a model to calculate the magnitude of the recirculating flow caused
by the relative eddy. He argued that the eddy-induced slip velocity is dependent on the
blade solidity and defined the slip factor in terms of the normalized slip velocity, following
the work of Wiesner [22] as shown in Eq. 1.5. In his trial to unify the previously derived
5
20. formulas for the slip factor, Backstrom compared his results with other attempts to demon-
strate its feasible replacement; however, his model lacks generality and does not show any
dependence on the pump flow rate.
σ = 1−1/[1+5(cosβ2 )0.5
(C/Se)] (1.5)
The work of Backstrom [5] was then followed by an experimental investigation of the
effect of flow rates on slip factors in centrifugal pumps, presented by Memardezfouli and
Norbakhsh [12]. They evaluated the existing prediction methods by comparing their results,
using five different industrial pumps, with the theoretical slip factors, such as those defined
by Wiesner [22] and Stodola. [19]. They found good agreement at the pump best-efficiency
point “or, design-point”, whereas a significant divergence was found at off-design condi-
tions, specifically at low-flow-rates operating regimes. Memardezfouli and Norbakhsh [12]
further defined the local slip factor and illustrated its non-uniform distribution in the blade-
to-blade passage. A relative decrease in the local slip factor was noticed, while moving
across the streamlines from the blade pressure side to the blade suction side. Although
inconsistent, their values for the mean slip factors at the impeller exit showed clear depen-
dence on the flow rates and the number of blades.
Qiu et al [14] were the first to consider the influence of the variable pump flow-rate in
their derivation for a unified slip factor. Qiu et al [14] distinguished the mechanism con-
trolling the flow behavior, and thus the slip factor, within the impeller and at the impeller
exit into three components. The first component represented the radial “Coriolis” effect, ev-
ident for typical radial impellers. The second contribution accounted for the blade-turning
rate(dβ
dm) characterizing the extra loading from the streamline curvature, while the third com-
ponent, the rate of change the fluid density and passage width to meridional space(dρb
dm )
described the weak effect of the passage width variation on the back flow and wakes gener-
ation and it can be neglected. Qui et al defined their slip factor in terms of the slip velocity
normalized by the rim rotor speed as shown in Eq 1.6
σ = 1−
CSL
U2
= 1−
Fπ cosβ2b sinγ2
Z
−
Fs2φ2
4cosβ2b
(
dβ
dm
)2 +
Fφ2s2sinβ2b
4ρ2b2
(
dρb
dm
)2 (1.6)
6
21. Furthermore, their model was validated for several case studies including an industrial
pump with actual turning rate (dβ
dm) 4.94 [m−1]. An adjustable fitting parameter F=0.6 was
needed to obtain a good match with the test data. Qui et al also compared their slip re-
sults with corresponding values, calculated using other prediction methods, but specifically
indicated a close agreement with the Weisner [22] model as shown in Eq. 1.4. For more
information about mathematical slip factor equations and how to use it see Appendix A.1
1.3 Previous CFD work on centrifugal impellers
Bacharoudis et al [4] investigated various parameters affecting the pump performance and
the energy consumption. The impeller outlet diameter, the blade angle and the blade number
are the most critical. The outlet blade angle of a laboratory centrifugal pump were changed
to show its effect on the performance . The impeller has six untwisted blades backward
facing and the trailing edge angles β2=20, 30 and 50◦ . The volute of the centrifugal pump
is of rectangular section with rounded corners was used to make this parametric study. As
the outlet blade angle increases the performance curve becomes smoother and flatter for the
whole range of the flow rates. When the pump operates at off-design conditions, the per-
centage increase in the head, due to the increase of the outlet blade angle, is larger for high
flow rates and becomes smaller for flow rates relative to nominal capacity of Q/QN <0.65.
Moreover, at high flow rates, the increase of the outlet blade angle causes a significant im-
provement of the hydraulic efficiency.
Spence and Amaral-Teixira [18] focused on a high energy, double entry double volute
pump. Due to the high energies involved these pumps tend to suffer more from pressure
pulsations than single entry pumps. Their study was concerned with using pressure pulsation
information to increase the pump life and reduce noise and vibration levels. The centrifugal
pump with a double entry, double volute type with 6 backwards curved blades was used in
simulation.
Three flow rates were investigated and the pulsations were extracted at 15 different
locations covering important pump regions. Pressure pulsations and performance character-
istics both in terms of non dimensional values and percentage contributions were studied,
which will assist understanding of the pump behavior and the effect of the cut water gap,
the snubber gap, and sidewall clearance as shown in Fig1.3.
7
22. Figure 1.3: Geometric factor locations within the pump [18].
In general, the cut water gap and vane arrangement are the two strongest influences on
the pressure pulsation, with the snubber gap and sidewall clearance being considerably less
important. A numerical study on the pulsating flow at the tongue region for a conventional
centrifugal pump was investigated by Raúl Barrio et al [6]. The study focuses on the relation
between the pressure pulsations and the fluctuating velocity field. An investigation is pre-
sented on the unsteady flow behavior near the tongue region of a single-suction volute-type
centrifugal pump. The vibration and noise levels of pumps must not exceed certain criti-
cal values, and so the fluid–dynamic perturbations at fBP (the blade-passing frequency)can
represent an important performance limitation.
The simulations were performed for five flow rates corresponding to about 20%, 60%,
100%, 120% and 160% of the nominal flow rate. The leakage through the impeller–tongue
gap showed pulsations that increased with flow rate up to about 30% for the 160% flow
rate. Remarkable fBP pulsations were obtained for the flow exiting the impeller through
specific angular intervals at both sides of the tongue edge. It was found that the peak-to-
peak pulsation of the net flow rate provided by the pump always remained below 0.3%.
8
23. Shojaeefard et al.[17]. A numerical simulation for a 3-D flow in a centrifugal pump
along with the volute for a viscous fluid. They found that by increasing the blade outlet
angle, and the passage width, the pump efficiency decreases at part load, but increases to the
highest level at the best efficiency point.
Sun-Sheng et al [20] studied the effect of splitters on the performance of hydraulic
centrifugal pump at different flow rates 50%, 80%, 100% and 120% of Best Efficiency
Point(BEP). A splitter blade with 50% shorter than the original blade has been used. It has
been found that the splitter blade increases the head.
Asuaje et al [3] presented a numerical simulation of a centrifugal pump using com-
mercial packages CFX-TASC flow and CFX. A quasi-unsteady simulation has been used to
solve impeller and volute casing. The velocity and pressure field were calculated at different
flow rates, for different relative positions of the impeller-volute tongue at the best efficiency
point. The results indicated the existence of non-uniform pressure distributions, causing
a fluctuating radial thrust, and unsymmetrical flow distributions which induces the partial
appearance of cavitation within the blade passage.
A simulation of fluid flow through shrouded impeller with six twisted blades and exit
blade angle of 23◦ was reported by Cheah et al[9] . Different flow rates were specified
ranging from 0.45 QBEPto 1.45 QBEP . They concluded that at design point the internal flow
or velocity vector is very smooth along the blade, However flow separation occurs at leading
edge due to non-tangential inflow conditions. A strong flow recirculation at center of the
impeller and stall region occurs through the passage when operated at off-design.
A computational fluid dynamics (CFD) simulation, of the flow field in centrifugal mixed
- flow impellers was reported by Huang et al [16]. They considered the effect of the mass
flow rate, the blade exit angle, the blade wrap angle and the blade number. They defined the
slip factor in terms of exit flow angle where angles measured with radial direction as shown
in Eq. 1.7. which is based on Busemann mathematical model [7].
σ = 1−[(tanβ2 −tanβ2 )
Cm2
U2
] (1.7)
For simulation and comparison purposes, Huang et al’s simulation considered the ge-
ometry of Eckardt [11]“rotor A” impeller. Huang et al showed that the onset of slip occurs
close to the exit section at a normalized camberline distance at which the departure of flow
9
24. streamlines from the blade guidance becomes significant. The calculated total pressure ra-
tio and slip factor were successfully compared to Eckardt [11] results. Their slip factor
exhibited a slight rise with the increase of the mass flow rate.
1.4 Objectives
Due to the scarcity of computational fluid dynamics in slip factor calculation, it’s necessary
to introduce this work. This work numerically simulates the flow field through the radial
impeller and the volute casing of a typical centrifugal pump, and calculates the resulting slip
factor. It also studies the effect of flow rate, number of blades and splitters on the generated
slip. The geometry processing of both parts is first presented, along with detailed meshing
procedures. The steps to achieve these objectives are:
1. Setup a numerical model of the pump.
2. Validate this model using available pump performance data.
3. Use the validated model to calculate the slip factor.
4. Compare the results with available slip factor mathematical models.
5. Perform a parametric study to evaluate the effect of number blades and splitters on
slip and pump performance.
10
25. Chapter 2
Geometry and meshing of the
pump
2.1 Introduction
In this chapter, the pump geometry and its discretization procedure are introduced. Detailed
dimensions of all pump components, including impeller, volute casing and blade profiles are
mentioned in section 2.2. Section 2.3 explains the meshing procedure for grid generation.
2.2 Geometry of centrifugal pump
In the present work, an industrial centrifugal pump is selected for computational modeling
and simulation purposes. To generate the pump geometry, the CFturbo[8] is used for this
purpose to generate the shape of both of the impeller and the volute casing, for more de-
tails see AppendixB. The impeller is defined by a fourth-order polynomial profile obtained
graphically by the program. The impeller is trimmed on outer edge and has a wrap angle(θ)
of 124 degrees as shown in Fig.2.2.
The selected profile leads to exit blade angles of 74.5, 74.1 and 73.7, measured from the
radial direction according to program definition as shown in Fig.2.2, at the hub, midspan and
shroud sections. The blade solidity is estimated to be 0.968, 0.970 and 0.983 at the hub, the
midspan and the shroud sections, respectively. The main dimensions of the pump geometry
11
26. are indicated in table 2.1. The volute casing is the part of the centrifugal pump at which the
velocity is decelerate and to increase the head. There are a lot of empirical methods by which
volute casing can be designed [13], The cross section of the volute casing is Trapezoidal.
The main dimensions of the volute are shown in table.2.2. The volute has a tongue angle
φ=28.9 as shown in Fig.2.5. The pump design is then passed to the ANSYS 14.5 software
package, where the BladeGen program is used for the three-dimensional blade generation
Fig.2.4. The spiral developed is shown in Fig.2.4 - 2.5. The all elements of centrifugal pump
are shown in Fig.2.6
Figure 2.1: The impeller and volute casing width
12
27. Figure 2.2: The main angles of the pump
Table 2.1: The main dimensions of the impeller
Z t[mm] b2 [mm] D2[mm] Ds[mm] β2 β1
4 4 29.5 360 177 72.5◦ 70◦
13
28. Figure 2.3: Cross section view of the volute casing
Figure 2.4: Spiral developed area
14
30. Table 2.2: Main dimensions of volute casing
D4 [mm] b4 [mm] φ
396.9 51 28.9◦
A splitter is a blade of shorter length situated half distance between two original blades. It’s
length is stated as a percentage of the original blade length. It is situated on the rotor as
shown in Fig. 2.7. In the present study 30%, 50% and 70% splitters were used.
(a) Passage of blade and splitter 50% (b) 3-D view for blade and splitter
Figure 2.7: Blade and splitter geometry at case of 50% splitter
2.3 Meshing techniques and procedures
The next step is to generate the grid or mesh, so that the governing equations can be solved
on these grids. In general, there are two types of grids, structured and unstructured. In
structured grids, a uniform layout of grid is used, while in unstructured grids, an arbitrary
layout of grid is generated. Information about the grid layout must be provided.
Structured grid comes in many different types: H-grids, O-grids, C-grids, J-grids, L-grids,
and H/J/C/L grids. An O-grid will have lines of points where the last point wraps around
and meets the first point. Thus, we have some grid lines that looks like the letter ’O’. A C-
grid will have lines of points in one direction which are shaped roughly like the letter “C”.
16
31. An H/J/C/L grids type means that the grid type could be any or all of these grids depending
on the geometry under consideration [2]. The unstructured grid can be composed of any
kind of polygon (for 2-D) or polyhedral (for 3-D). The basic element shapes accepted by all
unstructured CFD codes are typically triangles and tetrahedrals. Most of the CFD codes can
treat hybrid grids as composed of triangles and quadrangles, or either tetrahedrals, prisms,
pyramids and hexahedral. In contrary of structured grids which are difficult to design and
extensive to deal with, the unstructured grid are generated quickly by commercial softwares.
Compared with structured grids, the use of unstructured grids leads to an increase of the
CPU time due to slow work conversion.
2.3.1 Grid generation
In the present work, ANSYS TurboGrid is used to create high-quality hexahedral mesh
while preserving the underlying geometry, allowing for accurate and fast CFD analy-
sis.TurboGrid product is an integral part of the software tools from ANSYS for rotating
machinery within the ANSYS® Workbench. It’s a meshing tool that is specialized for CFD
analyses of turbomachinery blade rows, which is used to make structure mesh for Impeller.
Figure 2.8: H/J/C/L Topology for Blade
The structured H/J/C/L grid topology for a 3-D impeller blade is chosen for grid gener-
ation, as shown in Fig.2.8. The unstructured grid topology is applied in the volute casing.
Figures 2.9a and 2.10 show the 2-D impeller grid and the corresponding 3-D version, re-
spectively.
17
32. (a) Complete 2-D Impeller mesh (b) Shape of Impeller with 70% splitter of the blade
length, and mesh at span equal 0.5
Figure 2.9: Different impeller meshes
Figure 2.11 shows a cross sectional of the cut complete pump (i.e. rotor and stator, rep-
resented by the volute casing). The rotor grid is quadrilateral while the volute casing is
composed of tetrahedral type. General Connection Interface (GCI) is used to link the nu-
merical information between the rotor and the stator.
2.3.2 Grid examination
It is important to check the quality of the structured mesh which affects the accuracy of the
CFD simulation such as face angle, and the Edge length Ratio. The face angle is defined as
the angle between the two edges of the face that touch the node, and the Edge length Ratio
is the ratio of the longest edge of a face divided by the shortest edge of the face for each
face [2]as shown in table. Automatic mesh chech was carried by ANSYS Turbo-grid which
shows the percentage error according to structured mesh limits as shown in Fig. 2.12
18
33. Figure 2.10: 3-D impeller mesh
Figure 2.11: The cross section area of meshed impeller and volute casing
19
34. Table 2.3: Grid quality check for the impeller
Runs Number of elements Min face angle Max face angle Max edge length ratio Min element size
1 7248 12.218 173.024 414.86 9.23854e-7
2 68588 13.462 170.446 300.651 2.52410e-9
3 116072 15.982 169.931 120.651 3.1105e-10
4 134600 16.7 169.224 100.167 3.19324e-11
5 366485 18.41 165.5143 99.345 3.12324e-12
6 873673 19.67 164.897 97.551 5.37924e-12
Figure 2.12: Structured mesh statistics [1]
Parameters such as skewness, and the aspect ratio are used to check the quality of un-
structured mesh. The value of aspect ratio tends to one is better. Each element has a value
of skewness between 0 and 1. The skewness is classified in two ways, EquiAngle skew and
EquiSize skew. The smaller value of equiAngle skew and equisize skew are more acceptable
close to zero. It is also important to verify that all of the elements in mesh of the impeller
and the volute casing have positive area/volume otherwise the simulation in the solver is not
possible. Table 2.4 shows the check on the volute casing mesh.
20
35. Table 2.4: Grid quality check for the volute casing
Runs Number of elements Skewness Aspect ratio Min element size
1 396011 0.75 3.16 1.5673e-3
2 573440 0.632 2.924 2.5674e-4
4 242520 0.531 2.865 4.5764e-5
3 722244 0.341 2.032 3.7845e-6
5 1310008 0.272 1.865 1.5673e-7
6 1607212 0.223 1.657 3.6789e-7
21
36. Chapter 3
Numerical modeling and
solution procedure
3.1 Introduction
Numerical modeling of centrifugal pump for CFD simulation using commercial softwares
such as ANSYS-CFX follows a standard procedure. First the pump geometry is constructed.
Detailed dimensions of all pump components, including impeller, volute casing and blade
profiles should be all available. Second, the constructed geometry is discretized into 3-D
finite volumes suitable for solving the governing Navier-Stokes and turbulence models equa-
tions. Third, appropriate boundary conditions are setup in the solver to allow for a specific
solution to certain case. Fourth, the appropriate solver is chosen together with appropriate
solution procedure parameters that can obtain a converged solution. Fifth, Converged results
are compared against known data to check the validity of the obtained solution. Sixth, if the
numerical model is validated, it can be trusted to perform other required calculations. The
first two objectives were introduced in chapter 2. This chapter is dedicated for introducing
the details of the third to the sixth steps stated above.
Section 3.2 introduces the governing equation and turbulence modeling. Section 3.3
introduces the discretized finite volume equations and the type of control volume which
is being used with appropriate methods of handling pressure in the momentum equations.
22
37. Section 3.4 introduces the convergence criteria. Section 3.5 introduces boundary condi-
tions.Section 3.6 introduces the grid independence study. Section 3.7 introduces the model
validation procedure. The results of the validated model are presented in the next chapter.
3.2 Governing equations and turbulence models
3.2.1 The general transport equations
The continuity equation for steady incompressible flow:
∂Ui
∂xi
= 0 (3.1)
The momentum for steady incompressible flow:
∂
∂xi
(ρUiUj) = −
∂ p
∂xi
+
∂
∂xj
(µSij)−
∂
∂xj
(ρuiuj) (3.2)
where Sijis the strain - rate tensor
uiuj = −νt(
∂Ui
∂xj
+
∂Uj
∂xi
)−
2
3
kδij (3.3)
3.2.2 The turbulence model equations
The present study considers the commonly used k-ε equations for turbulence modeling. In
the k-ε model the transport equations for the turbulent kinetic energy, k, and the dissipation,
ε, are solved. For incompressible flow the equations read [21]
∂(Uik)
∂Xi
=
∂
∂Xi
[(ν +
νt
σk
)
∂k
∂Xi
]+Pk −ε (3.4)
∂(Uiε)
∂Xi
=
∂
∂Xi
[(ν +
νt
σε
)
∂ε
∂Xi
]+
ε
k
(cε1Pk −cε2ε) (3.5)
Where Pk is the production term and νt is the turbulent viscosity, which are expressed
as [21]
23
38. Pk = νt(
Ui
∂Xi
)2
(3.6)
νt = cµ
k2
ε
(3.7)
Coefficients cµ , cε1 , cε2 , σk and σε in Eqs.3.4 - 3.7 are empirical constants, and the
default values in ANSYS CFX (presented in table3.1) are used.
Table 3.1: Constants for the standard k-ε model.
Constants Values
cµ 0.09
cε1 1.44
cε2 1.92
σk 1
σε 1.3
Turbulence intensity refers to the turbulence level, as defined by Eqs. 3.8 - 3.10. In
turbomachinery, the value of turbulence intensity at inlet typically falls in the range of 5-
20% according to ANSYS documentation, and [9]
I ≡
v
V
(3.8)
v =
1
3
(v 2
x +v 2
y +v 2
z ) (3.9)
V = V2
x +V2
y +V2
z (3.10)
3.3 Finite volume method
3.3.1 Numerical techniques
In order to solve the governing equations stated above, they should be projected on the pump
mesh using appropriate numerical transformation techniques. The numerical discretization
24
39. is a transformation of the partial differential equations (Navier-Stokes equations )to what
is known as numerical analogue (algebraic equations of PDE). Various techniques are used
for numerical discretization. This section introduces, a preview of the finite volume method
(FVM) for numerical discretization, and discusses the parameters affecting the computa-
tional effort and solution accuracy. The usefulness reason of using FVM lies in its general-
ity, its conceptual simplicity and its ease of implementation for arbitrary grids, structured as
well as unstructured. The FVM preserves conservativeness.
ANSYS-CFX solver is a commercial software package that uses the finite volume
method to solve the governing equations. It’s a cell-vertex-based coupled solver, which
consumes considerable amount of time and memory but leads to accurate results, specially
complex geometries. In the coupled algorithm equation for all flow variables as solved si-
multaneously for a given cell, and the process is then repeated for all cells. this reduces the
number of iteration necessary for convergence, as shown in the Fig.3.1
Figure 3.1: Flow chart for the coupled solution algorithm[21]
This approach involves discretization of the spatial domain into finite control volumes
using a mesh. The governing equations are integrated over each control volume, such that
the relevant quantities (mass, momentum, energy, etc.) are conserved in a discrete sense
for each control volume. Many discrete approximations developed for CFD are based on
25
40. series expansion approximations of continuous functions (such as the Taylor series). The
order-accuracy of the approximation is determined by the exponent on the mesh spacing or
time step factor of the largest term in the truncated part of the series expansion.
In the present simulation, the advection term is treated using the High Resolution
scheme which is a combination of upwind and central differencing[1, 21], while the diffu-
sion term is discretized using the central difference scheme[21]. The turbulence equations
are discretized using the first order upwind scheme.
3.3.2 Pressure-velocity coupling
CFX is a fully coupled solver and so the pressure-velocity coupling is inherent in the so-
lution procedure[21]. Its main feature is to avoid decoupling of adjacent cells. Here, all
three momentum equations and the pressure equation are the same matrix and they solved
together. It does not need the pressure velocity coupling as it’s being taken care of in the
matrix solution. Coupled solvers consumes more time per iteration and use more memory
as the matrix gets bigger, however they usually converge much faster, specially for the non
linear terms.
The Rhie and Chow[15] algorithm is an interpolation for pressure velocity coupling for
co-located unstructured grid and curvilinear structured grid and gives appropriate coupling
between pressure and velocities nodal values. This special pressure–velocity coupling pre-
vents the checker-board pressure effect (i.e. spurious oscillations in the solution) and it is
available in ANSYS-CFX [1]. The Rhie and Chow’s interpolation practice is to obtain the
cell face velocity ue as in Fig.3.2, according to
Ue =
UP +UE
2
+
1
2
(dE +dP)(PP −PE)−
1
4
dp(pW −PE)−
1
4
dE(Pp −PEE) (3.11)
26
41. Figure 3.2: Collocated arrangement[21]
The first term on the right hand side of 3.11 is the average of the velocities straddling
face e. We assume constant values for d everywhere and write Rhie and Chow’s interpolated
face velocity Ue follows:
Ue =
UP +UE
2
+
d
4
[4(Pp −PE)−(PW −PE)−(Pp −PEE)] (3.12)
therefore,
Ue =
Up +UE
2
+
d
4
∂3 p
∂X3
(3.13)
This shows that Rhie and Chow’s pressure interpolation practice involves the addition
of a third-order pressure gradient term. Since the remainder of the method is at best second-
order accurate, this addition does not compromise the solution accuracy. Its beneficial effect
is to provide damping of the spurious oscillations due to the co-located arrangement, so it
is called a pressure smoothing term or added dissipation term. The damping is caused
by the restored linkage between the pressure differences across the control volume faces
and the face velocities, which appear in the continuity equation. The source term of the
latter equation is the mass unbalance, which, in a constant density flow, involves differences
between the cell face velocities, so the addition of a third-order pressure gradient term to
each of these velocities is equivalent to adding a fourth-order pressure gradient term to
their differences in the resulting pressure correction equation. CFX applies a co-located
arrangement along with the Rhie-Chow model [15, 10].
27
42. 3.3.3 General Connection
The General connection [1] is a powerful way to connect regions together. It can be used to
connect non-matching grids in our case the mesh between the rotor and stator as shown in
Fig. 3.3a, and connect the interface between a rotor (moving) and stator(fixed) ( i.e a frame
change at the interface ) Fig. 3.3b.It also enables the data transfer between periodic pairs
as the simulation proceeds through the application of the ANSYS CFX frozen-rotor frame-
change model. In this model, the frame of reference is changed but the relative orientation
of the components across the interface is fixed. It is worth to mention that this model is
limited to steady flows. The frozen-rotor model is fully described in the ANSYS User
Documentation [1].
(a) The frame change and pitch change
(b) Different mesh connection
Figure 3.3: General connection cases[1]
28
43. 3.3.4 Partitioning of solution on local machine
The present simulation runs are carried out on hp Pavilion g4 (Intel®Core™ i7-3632QM
CPU@2.2 HZ), number of cores is eight. The number of iterations required to obtain a con-
verged solution ranged from 700 to 1000. Partitioning is the process of dividing the domain
into a number of ‘partitions’ each of which may be solved on a separate processor core thus
reducing the computational effort. Several partitioning methods have been developed, in
this simulation we use MeTiS algorithms which is a set of serial programs for partitioning
graphs, partitioning finite element meshes, and partitioning finite volume meshes. it gener-
ates the best partitions with respect to the size of the overlap regions between the partitions.
grids containing periodic pair boundary conditions are handled much more efficiently by
MeTiS than the other partitioning techniques.
3.4 Convergence and false time incrementation
In its strict mathematical sense, convergence is the ability of a set of numerical equations to
represent the analytical solution of a problem, if such a solution exists. Equally, a process is
stable if the equations move towards a converged solution such that any errors in the discrete
solution do not swamp the results by growing as the numerical process proceeds.
The solver will stop when it reaches the specified maximum number of iterations un-
less convergence is achieved sooner within the specified limits of the residuals. Here, the
convergence criteria settings include the specification of the maximum number of iterations
to 1000 and the residuals to 1.x10−4. The type of residual calculation is set to root mean
square (RMS):
RMS =
∑i R2
i
n
(3.14)
In the present steady-state solution, the following three conditions are satisfied. First, the
acceptable RMS error values of the residuals are reduced to 10−4, while the imbalances
in the governing equations are set less than 1%. The evolution of the total pressure in the
centrifugal pump is also monitored as the simulation proceeds to steady-state solution, as
shown in Fig.3.4.
29
44. Figure 3.4: Total pressure rise in the centrifugal pump at different time step
The ANSYS CFX employs the so-called false transient algorithm, in which a false
timescale is used to move the solution towards the final answer, thus, decreasing the con-
vergence time [21][1]. The selection of an appropriate time-step size is essential in order
to obtain good convergence rates for simulation. If the time step is too large the resulting
convergence behavior will be bouncy and a smaller time-step size should be attempted. In
our simulation, the initial time-step size is automatically selected by ANSYS CFX solver
[1], using available information regarding the domain size, flow physics, and the boundary
conditions. However, slow convergence is observed as the number of time steps exceeds
1000.
This is then followed by the specification of more appropriate time scales, in accordance
with the impeller angular speed of N=1450 rpm, in the range of
10
N to 60
N . The preliminary
investigation motivates the use of the current time-step 60
N in the rest of this thesis. For
instance, the residuals in the mass and momentum equations are indicated in Fig. 3.5
30
45. Figure 3.5: Residuals_RMS at time step=60
N
. The residuals are shown to fall below 1.x10−8 within a maximum number of time
steps of about 700.
3.5 Boundary conditions
Accurate specification of the boundary conditions is important and most-influencing in com-
putational fluid dynamics simulations. The inlet boundary condition is set as a total inlet
atmospheric pressure, whereas the outlet boundary condition is set as a constant mass flow
rate. This ensures robust setup for the boundary conditions[1], because the outlet mass
flow typically allows a natural velocity profile to develop based on the upstream conditions.
The no slip and the no penetration boundary conditions at the solid walls are applied to the
external surfaces of the blades, the hub, and the shrouds.
It is unreasonable to numerically model the pump entire domain as it contains periodi-
cally repeated flow regimes between each two successive blades. Instead, we concentrate on
31
46. a representative control volume and impose appropriate boundary conditions at its bound-
aries, as illustrated in Fig. 3.6. A 3-D computational domain that consistently surrounds one
complete blade in the peripheral direction is selected while retaining equivalent flow inlet
and exit sections in the radial direction. To ensure that the enclosed domain behaves as a
representative part of the entire impeller, rotationally periodic boundary conditions are en-
forced on the control volume surfaces in the peripheral direction. This approach also allows
us to reduce the computational effort.
Figure 3.6: Rotationally periodic boundary condition imposed on one blade passage with
50% splitter included
3.6 Grid independence study
In the aim of reducing the influence of the generated grid sizes on the obtained solution,
the present attempt is considered. Six different grid sizes are generated and the dependence
of the simulated head on the total resulting number of elements is investigated. The total
number of elements ranges from 4x105 to two millions. The study is carried out using the
four-bladed impeller with a measured flow rate and head of 260 m3/h and 38 m, respectively.
Figure 3.7 shows the numerical results of the generated head using different grid sizes. It
is noticed that as the total number of elements increases from 4x105 to 6x105, the head
32
47. jumps from 35.75 m to 37.25 m. A slower rate of increase follows using larger number of
elements, indicating sufficient number of computational points.
Figure3.8 shows the consumed CPU time in terms of the total number of elements used
in five of the above simulation runs. Using fewer number of grid elements yields to lesser
computational effort, as expected. The CPU-time increases almost linearly within the appli-
cable range of the number of elements. Therefore, a suitable grid size with a corresponding
number of elements of about one million is selected according to the presented results.
0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 2
x 10
6
35
35.5
36
36.5
37
37.5
38
Total number of element
HCFD
(m)
Figure 3.7: Influence of grid size selection on the pump numerical head
33
48. 0.642 0.8383 1.1162 1.6765 1.9737
x 10
6
0
1
2
3
4
5
Total number of element
CPU−Time(hr)
Figure 3.8: CPU-time versus the generated number of elements
3.7 Model validation
To validate the numerical model, the characteristic curve of the pump (H-Q curve) is con-
sidered for comparison purpose. Computations are carried out using K-ε turbulence model.
Shojaeefard et al. [17] noticed that the K-ε turbulence model yields better agreement with
the experimental data. Figure.3.9 compares the present numerical results of the H-Q curve
with the corresponding test data. Good agreement is found in the range of normalized flow
rate between 0.8 and 1.2, while the maximum relative error is found to be 4%. For relatively
high and low flow rates, the difference between the numerical and actual results increases
up to about 13%. Such discrepancy may be attributed to the inability of numerical model to
catch the proper flow behavior in the low and high flow-rate regimes where flow separation
is highly expected.
34
49. 0.6 0.8 1 1.2 1.4 1.6
0.7
0.8
0.9
1
1.1
1.2
1.3
1.4
Q/QBEP
H/H
BEP
Actual performance
K−ε
Figure 3.9: Comparison of numerical model head and the flow rate with the pump perfor-
mance curve
35
50. Chapter 4
Results
4.1 Introduction
In this chapter we present the results of the CFD simulations. The simulations are done for
an industrial pump that has a performance curve available. The pump develops a flow rate
of 260 m3/h and a head of 38 m at the Best Efficiency Point (BEP). The first step was to
study the flow characteristics in terms of meridional velocity and developed head. Second
the slip factor is evaluated and compared with some mathematical models. Third, the effect
of increasing number of blades and splitters insertion on pump performance are introduced.
Section 4.2 introduces the results of developed meridional velocity and pressure in the
basic pump case. Section 4.3 presents the results of slip factor calculations. Section 4.4
presents the effect of increasing number of blades and splitters insertion on slip factor. Sec-
tion 4.5 presents the effect of increasing number of blades and splitters insertion on pump
hydraulic efficiency.
4.2 Flow field investigation
Figure 4.1 shows the dependence of both the meridional velocity and the static head on the
normalized passage width at three different radial locations, 25%, 50% and 81% “stream-
wise direction”, as indicated in Figs. 4.1a and 4.2a
36
51. (a) Meridoinal velocity between two blades
0 0.2 0.4 0.6 0.8 1
−1
0
1
2
3
4
5
Normalized pitch
Meridionalvelocity[m/s]
25%
50%
81%
SS PS
(b) Meridoinal velocity at different radial stations
Figure 4.1: The meridional velocity patterns through the passage at mid span of impeller at
Q/QBEP=1.
37
52. (a) Static head between two blades
0 0.2 0.4 0.6 0.8 1
−5
0
5
10
15
20
25
30
Normalized pitch
StaticHead[m]
25%
50%
81%
SS PS
(b) Static head at different radial stations
Figure 4.2: Static head through the passage at mid span of impeller at Q/QBEP=1.
38
53. Here, the number of blades is z=4. The shown results are for a plane half-way between
the hub and the shroud at the best efficiency point. In the neighborhood of the blade suction
side, The distributions are nearly captured with a peak of 4.4 m/s at 25% radial location as
seen in Fig. 4.1b. In Figure 4.1b the velocity values are the highest at 25% away from the
blade inlet then gradually decreases as the flow moves toward the blade exit because of the
widening cross-sectional area of the flow passage. A corresponding increase in the static
head is seen in Fig. 4.1. The existence of the recirculating eddy flow near the pressure side
is evident and its effect on the meridional velocity and static head is clear. The influence of
the induced eddies is minimal near the exit section.
This is clearly seen for the 81% line shown in Fig. 4.1b near the pressure side where the
meridional velocity has increased substantially compared to the 25% and 50% profiles.
To help illustrating the eddy motions within the impeller passage, the flow streamlines
are represented in Fig.4.3, together with a contour plot of the velocity magnitude, in a plane
located midway between the hub and the shroud, while operating at the best efficiency point.
Figure 4.3: 3-D Streaming of flow field, and a contour plane of velocity at midspan of four
blades impeller at flow rate Q/QBEP=1.
The number of blades is z=4. The incoming flow is shown to separate right behind the
leading edge on top of the pressure side. The portion occupied by the wakes increases to
39
54. block about thirty percent of width and then gradually shrinks allowing the main flow to
refill the whole domain at the exit section.
4.3 Slip factor calculations
To calculate the slip factor, a post processing MatLab program was written to use the values
of the velocity components Cu2, and Cm2 , together with the exit flow angle β2, see Appen-
dices A.2-A.3, to evaluate the slip velocity and the slip factor at the blade tip “exit section”.
We pursue this using the definition of the slip factor given by
σ = 1−
CSL
U2
(4.1)
CSL = U2 −Cu2 −
Cm2
tanβ2
(4.2)
To further investigate the model validity, the present slip factor, assuming four blades,
is calculated at the best efficiency point and compared with some mathematical models, as
indicated in table 4.1.
Table 4.1: The slip factor with different correlation compared with numerical results at BEP
Z Stodola Backstrom Eckardt Qui et al Wiesner Numerical
4 0.7638 0.7275 0.8146 0.515 0.6288 0.58264
The slip factor at the best efficiency point was found to be 0.58 which is closer to the
Qui et al model [14] with a relative error of about 11.6 % and the Wiesner model [22] with
a relative error of about 8%. The variation of the slip factor with the flow coefficient is
presented in Fig. 4.4. A linear reduction in the slip factor is found in the range of flow co-
efficient from about 0.075 to about 0.105. Consistent results, but under-predicted by11.6%,
are indicated by the Qui et al model in the same range of flow coefficient, but error increase
by increasing flow coefficient than 0.105.
40
55. 0.08 0.09 0.1 0.11 0.12 0.13
0.35
0.4
0.45
0.5
0.55
0.6
0.65
0.7
Flow coefficient
Slipfactor
Present work
Qui et al
Wiesner
BEP flow
coefficient
Figure 4.4: Slip factor versus flow coefficient at based on CSL.
This is possibly because of the incorporated three dimensional analyses and the k-ε
turbulence model, adopted to model the physical flow behavior in typical centrifugal im-
pellers. Generally, the effect of flow rate is represented by the second component of Eq.1.5,
in which the blade-turning rate causes extra loadings due to streamline curvature. The larger
the amount of flow rate, the less-controlled the guidance to the working fluid and the smaller
slip factor. In this particular run (z=4) , the slip factor varies from 0.6 at FC2=0.075 to 0.41
at FC2=0.127.
Furthermore, the local slip factor is calculated according to Eq. 4.3 and evaluated at
three different span locations along the tip section, specifically, 0% span (hub), 50% span
and 100% span (shroud), as illustrated in Fig.4.5 - 4.6.
σ = 1−
U2 −Cu2i − Cm2i
tanβ2
U2
(4.3)
41
56. Figure 4.5: Different span location
Figure 4.6: Different span location at meridional view
The variation of the local slip factor as a function of the normalized passage width
(pitch), evaluated at the tip section, is then plotted in Fig. 4.7.
42
57. 0 0.2 0.4 0.6 0.8 1
0.2
0.3
0.4
0.5
0.6
0.7
0.8
0.9
1
Normalized pitch
Localslipfactor
Hub
Mean
Shroud
SS PS
Figure 4.7: The local slip factor between two blades at the tip at different cross section.
Consistently with our understanding of the flow behavior near the boundaries, the local
slip factor exhibits a remarkable increase at the hub section as compared to those values es-
timated at the mean section because of higher fluid guidance near the solid walls. Moreover,
the comparison reveals relatively lower slip factor at the 100%-span plane, corresponding to
the top section. This is due to the fact that, in our particular model, the pump is un-shrouded.
It is concluded that a shrouded impeller would help improving the respective slip factor.
4.4 Effect of number of blades and splitters on slip
factor
In these simulation runs, the number of blades is further increased to study the effect of
increasing the number of blades on the flow slippage, while retaining the original impeller
geometry and an equal range of the imposed flow rate. Specifically, six, eight, ten and
twelve blades are now considered. In principle, using fewer numbers of blades would result
in lesser slip factors because of the compliant guidance, the fluid exhibits between each
43
58. two successive blades. It is seen that as the number of blades is increased, the slip factor
increases. However, increasing the number of blades from 10 to 12 showed slight reduction
near the BEP and slight improvement at higher flow rates.
Figure 4.8: The slip factor and the flow coefficient at different number of blades using CFD
calculations and compared to Qiu’s model Eq 1.6.
This is reflected in Fig. 4.8 that shows the variation of slip factor with number of blades
at BEP. It is seen that as the number of blades increases the slip factor increases reaching a
maximum of about 0.69 after which remains almost constant. This specifies the achievable
limit, in terms of guidance, through the increase of the number of blades. Eq. 1.6 defines the
three main factors affecting the slip in centrifugal impellers. The contribution of the number
of blades is obvious in the second term, of the right hand side; justifying the above effect
of the number of blades on the slip behavior. However, because of the existence of other
factors, such as the blade turning rate, the slip factor saturates at about 0.69.
The effect of adding a 30 %, 50 %, 70 % spanwise splitters is also examined in Fig. 4.10.
It is clear that adding splitters improves slip factor as seen for the 30 % and 50 % splitters.
Increasing the splitter length to 70 % does not improve the slip factor significantly specially
at the BEP. Thus the 50 % splitter length could be considered the optimum splitter length
for the pump under study.
44
59. 4 5 6 7 8 9 10 11 12
0.5
0.55
0.6
0.65
0.7
0.75
Number of blades
Slipfactor
Figure 4.9: Slip factor at BEP at different number of blades
0.06 0.08 0.1 0.12 0.14 0.16
0.4
0.5
0.6
0.7
0.8
Flow coefficient
Slipfactor
Without splitter
30% Splitter
50% Splitter
70% Splitter
Figure 4.10: The effect of adding four-splitters to the four-bladed impeller on the slip factor.
45
60. 4.5 Effect of number of blades and splitters on head
and hydraulic efficiency
Figures 4.11 and 4.12 show that as the number of blades increases, both the head and hy-
draulic efficiency decrease. This means that although improving slip due to increasing the
number blades, the head would have increased, but the frictional losses wasted this improve-
ment . As a consequence of the reduction in head, the hydraulic efficiency decreased. This
means that although improving slip due to increasing the number blades, the head would
have increased, but the frictional losses wasted this improvement .
0 0.5 1 1.5 2
30
40
50
60
70
80
Q/QBEP
Pumpefficiency%
Z=4
Z=6
Z=8
Z=10
Z=12
Figure 4.11: Pump efficiency for different number of blade.
46
61. 0 0.5 1 1.5 2
0
0.2
0.4
0.6
0.8
1
1.2
1.4
1.6
Q/QBEP4
Headratio(H/HBEP4
)
Z=4
Z=6
Z=8
Z=10
Z=12
Figure 4.12: Normalized head for flow different number of blades.
As a consequence of the reduction in head, the hydraulic efficiency decreased. Fig-
ures 4.13 and 4.14show that increasing the splitter length leads to increasing head especially
for the 50% splitter.
47
63. 0 0.5 1 1.5 2
0.8
1
1.2
1.4
1.6
Q/QBEP4
Headratio(H/HBEP4
)
Without splitter
30% Splitters
50% Splitters
70% Splitters
Figure 4.14: Normalized head for different splitter.
How- ever the decrease in hydraulic efficiency is slight compared to adding whole
blades. This shows that adding splitters improved slip, the same as adding blades did, but
since the frictional losses in the whole blades were much higher than those in the splitter
case. Thus, we conclude that for the pump under consideration adding a 50% splitter could
increase the pump head by about 10% at the BEP with minimal reduction in pump hydraulic
efficiency.
49
64. Chapter 5
Summary and Future Work
5.1 Summary
Numerical simulation of flow through a centrifugal pump was carried out to study the be-
havior of the flow through the impeller and to evaluate the slip factor as function of the flow
rate, number of blades and splitter insertion. It was shown that the computational results are
in good agreement with the pump performance curve data in the neighborhood of the best
efficiency point but is in fair agreement with it near the neighborhood of the low and high
flow rates. Overall slip factor was found to change linearly with flow coefficient in a similar
way as the expression by Qui et al [14] .
The effect of increasing the number of blades up to ten was found to increase the slip
factor reaching saturation at about 0.69. Also, insertion of 30% and 50% splitters increases
slip factor. However a 70% splitter does not improve the slip factor any more. The effect of
splitter insertion and increasing the number of blades on both developed head and hydraulic
efficiency have been examined. The effect of splitter insertion was to increase the developed
head. The effect of increasing the number of blades was to decrease the head developed.
It is clear that there is a contrast between the increase in head due to splitter insertion and
the decrease in head due to more blades insertion although both of them do the same thing
of improving flow guidance. The reason for this is that improving flow guidance increases
the slip factor which in turn increases developed head, however the higher incurred friction
50
65. losses due to blades insertion offsets the improvement due to better guidance. In both cases,
the hydraulic efficiency decreases due to the increased friction losses.
5.1.1 Recommendations for future work
This work can be extended by evaluating slip phenomena in different machines and under
different operating conditions. So this work can be extended to:
1. Slip evaluation in mixed flow pumps
2. Slip evaluation for compressible flow machines such as compressors.
51
66. Appendix A
Appendix
A.1 Slip factor relations
A.1.1 The slip model single relative-eddy (SRE)
σs= 1-∇W
U = 1- 1
(1+F( C
Se
))
Where
F(Solidity coefficient)=F0(cos(β2))0.5
F0=5, C
Se
= (1−RR)
2π cosβ2b
A.1.1.1 SRE approximate equation
σ = 1−0.8π cosβ2
Z
A.1.2 Stodola equation
σs = 1− π cos(β2)
Z
A.1.3 Wiesner equation
σs = 1−
√
cosβ2)
Z0.7
52
67. A.1.4 Stanitz equation
σs = 1− 0.63π
Z0.7
A.1.5 USF Equation
σs=1-Fπ cosβ2 sinγ2
Z2
- FS2φ2
4cosβ2b
(dβ2
dm )2 +Fφ2S2 sinβ2
4ρ2b2
(dρb
dm )2
where (dβ2
dm )2=(β2−β1)
Ccosζ
(Assume linear distribution of the blade angle along the chord)
Cslip= C2mδ
(cosβ2b)2
δ=F cosβ2b
4cosζ
(S
C)∆β
where ∇β is chamber angle, and ζ is stagger angle
S2 = πD2
Z
A.1.6 Eck equation
σs=1- 1
(1+4
Z(1−RR)
2πcosβ2
)
A.1.7 calculation of head
H=
Pexit,t−Pinlet,t
ρg [m]
where Pexit,t, Pinlet,l is area average pressure at exit at trialling edge, area average pres-
sure at leading edge
A.2 Matlab code used to calculate this empirical re-
lations at different conditions
53
68. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% S l i p c o e f f i c i e n t f o r c e n t r i f u g a l pump Using data
%from excel s h e e t which i s e v a l u a t e d from ANSYS CFX.
% This code i s used to e v a l u a t e the s l i p f a c t o r f o r the
%most i m p o r t a n t r e l a t i o n s and compare i t
%with the CFD−s l i p f a c t o r .
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% F i r s t l y you shoud e x t r a c t a l l below
%unkowns in Execl s h e e t and a d j u s t i t s
%l o c a t i o n in the code according to your s h e e t
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
c l c
c l e a r a l l
filename = ’ z =4. xlsx ’ ;
% you can change the name of Execel s h e e t ac c o r in g to your s h e e t name
s h e e t = 1;
q1= ’AI2 ’ ; %(z )
q2= ’AS2 ’ ; %(D2)
q3= ’AO2’ ; %(beta2 )
q4= ’AN2’ ; %(beta1 )
q5= ’AT2 ’ ; %(RR)
q8= ’AL2 ’ ; %(( r )
q9= ’AJ2 ’ ; %(C) %
q10 ( t )= ’ ’; q11 = ’AM2’ ; %(cs )
q12 = ’AK2’ ; %(M)
q20 = ’AU2’;%( b2 )
q6= ’AF7’;%( f i )
q13 = ’N7’;%( ca2=c222 )
q14 = ’R7’;%( c22=cu2 )
q15 = ’U7’;%(H)
q16 = ’AC7’;%( u22 )
q17 = ’AA7’;%( u11 )
54
69. q19 = ’AG7’;%(Q)
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%All t h e s e v a r i a b l e s should be c o n t a i n e d in
% the Excel s h e e t
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
z= x l s r e a d ( filename , sheet , q1 ) ;
% Number of blades
D2= x l s r e a d ( filename , sheet , q2 ) ;
%Diameter a t e x i t in [mm]
beta2 = x l s r e a d ( filename , sheet , q3 ) ;
%Exit blade angle
beta1 = x l s r e a d ( filename , sheet , q4 ) ;
%I n l e t blade angle
RR= x l s r e a d ( filename , sheet , q5 ) ;
%Radius Ratio
f i = x l s r e a d ( filename , sheet , q6 ) ;
%flow c o e f f i c i e n t
g2 =33;
% m e r i d i o n a l i n c l i n a t i o n angle
r = x l s r e a d ( filename , sheet , q8 ) ;
%s t a g g e r angle
C= x l s r e a d ( filename , sheet , q9 ) ;
%chamber l i n e in [mm]
t = 4 . 5 ;
% t h i c k n e s s a t the blade t r a i l i n g edge in [mm]
cs= x l s r e a d ( filename , sheet , q11 ) ;
% space to chord r a t i o
M= x l s r e a d ( filename , sheet , q12 ) ;
% Meridonal l e n g h t in [mm]
C222= x l s r e a d ( filename , sheet , q13 ) ;
% Meridonal v e l o c i t y in [m/ s ]
55
70. C22= x l s r e a d ( filename , sheet , q14 ) ;
% V e lo c it y t h e t a in [m/ s ]
H= x l s r e a d ( filename , sheet , q15 ) ;
% Head r i s e in [m]
u22= x l s r e a d ( filename , sheet , q16 ) ;
%p e r p h e r a l speed a t e x i t in [m/ s ]
u11= x l s r e a d ( filename , sheet , q17 ) ;
%p e r p h e r a l speed a t i n l e t in [m/ s ]
e t =0.9 ;
%Volumatric e f f i c i e n c y
Q= x l s r e a d ( filename , sheet , q19 ) ;
% Volume flow r a t e in [m3/ s ]
D2= x l s r e a d ( filename , sheet , q2 ) ;
% blade e x i t diameter in [m]
b2= x l s r e a d ( filename , sheet , q20 )
%i m p e l l e r e x i t width
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% S l i p c o e f f i c i e n t using S t a n i t z
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
a =1 −((0.63* pi ) / z )
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% S l i p c o e f f i c i e n t using Stodola e q u at i on
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
c=1−(( pi * cos ( beta2 * pi / 1 8 0 ) ) / z )
%% S l i p c o e f f i c i e n t using Wiesner e q ua t io n
w=1−(( s q r t ( cos ( beta2 * pi / 1 8 0 ) ) ) / ( z ^ 0 . 7 ) )
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% S l i p c o e f f i c i e n t using SRE
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
F1=5*( cos ( beta2 * pi / 1 8 0 ) ) ^ 0 . 5 ;
M=( f i *(1−RR) ) / ( 2 * pi * cos ( beta2 * pi / 1 8 0 ) ) ; %>C/ S
SRE=1 −(1/(1+( F1 *( cs ) ) ) )
56
71. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% S l i p USF Equation
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
s2 =( pi *D2 ) / z;% s2 : p i t c h a t the blade e x i t
F2=1−(( s i n ( pi / z ) ) * ( s i n ( ( ( pi / z )+ beta2 )* pi / 1 8 0 ) ) * ( cos ( beta2 * pi / 1 8 0 ) ) *
( s i n ( g2* pi /180))) −(( t ) / ( s2 * cos ( beta2 *180/ pi ) ) ) ;
u1 =(( F2* pi * cos ( beta2 * pi /180)* s i n ( g2* pi / 1 8 0 ) ) / z ) ; %Radial Term
d2 =(( beta2−beta1 )* pi / 1 8 0 ) / ( 1 1 4 . 6 4 3 ) ;
u2 =(( F2* s2 * f i ) / ( 4 * cos ( beta2 * pi / 1 8 0 ) ) * d2 ) ;
USF=1−u1−u2
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% CFD s l i p f a c t o r
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
A=(C222* tan ( beta2 * pi / 1 8 0 ) ) / u22 ; B=(( u11*C22)+H ) / ( u22*u22 ) ;
s l i p =1−A−B Cmth2=Q/ ( pi *D2*b2*1e −6);
Cuth2=u22−(Cmth2 / ( e t * tan ( beta2 *180/ pi ) ) ) ;
s l i p 2 =C22 / Cuth2
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% Output f i g u r e
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
u i t a b l e ( ’ Data ’ , ( [ a c w E SRE USF s l i p s l i p 2 ] ) , ’ColumnName ’ ,
{ ’ S t a n i t z ’ , ’ Stodola ’ , ’ Wiesner ’ , ’ECK’ , ’SRE’ , ’USF’ , ’ S l i p ( F ) ’
, ’ S l i p (W) ’} , ’ P o s i t i o n ’ , [10 150 500 1 0 0 ] ) ;
A.3 Matlab code used to draw velocity triangles at
inlet and exit sections of radial impeller, both
with and without slip
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%
57
72. % This code i s used to draw the e x i t v e l o c i t y t r i a n g l e s
% which are c a l u a l a t e d from
% the above codes f o r d i f f e r e n t r e l a t i o n s and compare
% i t with CFD s l i p f a c t o r
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% you shoud f i l l the GUI data which are
% U1 , Ca1 , Cu1 , U2 , Ca2 , Cu2 th , Cu2 ac , s c a l e
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
c l e a r
c l c
a= i n p u t d l g ({ ’ u1 ’ , ’ ca1 ’ , ’ cu1 ’ , ’ u2 ’ , ’ ca2 ’ , ’ cu2Th ’ ,
’cu2Ac ’ , ’ scale ’} , ’ i n p u t d a t a ’ , 1 ) ;
f i g u r e s u b p l o t 221
% s u b p l o t 221 %
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%%%%% s c a l e =5; %% Scale of draw
[1 mm = 5 m/ s ]
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
[1 mm = 5 m/ s ] x1= str2num ( a { 1 } ) ;
%[m/ s ]
y1= str2num ( a { 2 } ) ;
%[m/ s ]
z1= str2num ( a { 3 } ) ;
%[m/ s ]
put value x2=str2num ( a { 4 } ) ;
%[m/ s ]
put value y2=str2num ( a { 5 } ) ; %[m/ s ]
z2=str2num ( a {6});%[m/ s ]
put value z t =str2num ( a {7});%[m/ s ]
s=str2num ( a { 8 } ) ;
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
% I n l e t v e l o c i t y t r i a n g l e
58
73. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
x=x1 / s ; y=y1 / s ;
p l o t ( [ 0 , z1 , x ,0] ,[0 , − y , 0 , 0 ] , ’ LineWidth ’ , 3 )
a x i s ([ −5*x max ( 1 . 5 * x , 1 . 5 * z1 ) −1.5*y 0.5* y ] )
Alpha1=90−( atan ( z1 / y )*180/ pi ) ;
beta1 =( atan ( y / ( x−z1 ) ) * ( 1 8 0 / pi ) ) ; %i n s i d e ( pump )
x l a b e l ( ’ s c a l e in mm’ )
y l a b e l ( ’ s c a l e in mm’ )
t i t l e ( ’ Veocity t r i a n g l e a t i n l e t ’ )
g r i d on
%f i g u r e %Exit v e l o c i t y t r i a n g l e s with s l i p
s u b p l o t 222
x2=x2 / s ;
y2=y2 / s ;
z2=z2 / s ;
z t = z t / s;%cu2 a c t u a l
p l o t ( [ 0 , z2 , x2 ,0] ,[0 , − y2 , 0 , 0 ] , ’ r ’ , ’ LineWidth ’ , 3 )
Alpha2=90−( atan ( z2 / y2 )*180/ pi ) ;
beta2 =( atan ( y / ( x2−z2 ) ) * ( 1 8 0 / pi ) ) ; %T h e o r i t i c a l e x i t blade angle
beta3 =( atan ( y / ( x2−z t ) ) * ( 1 8 0 / pi ) ) ; %e x i t s l i p e x i t blade angle
a x i s ([ −5*x2 max ( 1 . 5 * x2 , 1 . 5 * z2 ) −1.5*y2 0.5* y2 ] )
x l a b e l ( ’ s c a l e in mm’ )
y l a b e l ( ’ s c a l e in mm’ )
t i t l e ( ’ Veocity t r i a n g l e a t exit ’ )
hold on
p l o t ( [ 0 , zt , x2 ,0] ,[0 , − y2 ,0 ,0] , ’ − − ’ , ’ color ’ , ’ b ’ , ’ LineWidth ’ , 3 )
s l =abs ( z2 / z t )
t e x t ( 0 , 0 . 3 * y , [ ’ alpha2 = ’ , num2str ( Alpha2 ) , ’ degree ’ ] , ’ FontSize ’ , 1 1 )
t e x t ( 0 , 0 . 4 * y , [ ’ beta2 = ’ , num2str ( beta2 ) , ’ degree ’ ] , ’ FontSize ’ , 1 1 )
g r i d on
f i g u r e s u b p l o t ( 2 , 1 , 1 ) ;
p l o t ( 1 : 1 0 ) ;
59
74. s u b p l o t 212
u i t a b l e ( ’ Data ’ , [ Alpha1 beta1 Alpha2 beta2 beta3 s l ] , ’ColumnName ’ ,
{ ’ Alpha1 ’ , ’ Beta1 ’ , ’ Alpha2 ’ , ’ Beta2Th ’ , ’ Beta2act ’ , ’ s l i p f a c t o r ’} ,
’ P o s i t i o n ’ , [50 50 500 1 0 0 ] ) ;
60
75. Appendix B
Appendix
B.1 Design steps
B.1.1 Main dimensions
The main dimensions menu item is used to define main dimensions of the impeller such as
ds, dh,d2, and b2 as shown in FigB.1.
Figure B.1: The main dimensions of the impeller in CFTurbo
61
76. B.1.2 Meridional contour
The design of the meridional contour is the second important step for the impeller design.
Graphical elements can be manipulated not only by the computer mouse per drag and drop
but also by using context menus as shown in FigB.2.
Figure B.2: The meridional plane view in CFTurbo
B.1.3 Setup
Some basic settings were specified, such as flow rate, head at best efficiency point, rota-
tional speed You can add splitter, and shrourd in this step. Design a shrouded (closed) or
unshrouded (open) impeller. For an unshrouded impeller you have to define the tip clearance
as shown in Fig.B.3
62
77. Figure B.3: The setup GUI in CFTurbo
B.1.4 Exporting data
The design of impeller and volute casing are exported in standard file formats or for several
CAE applications as shown in FigB.4.
Figure B.4: The exporting GUI in CFTurbo
63
78. References
[1] ANSYS (2013): ANSYS CFX - Reference Guide. ANSYS, 12th edn.
[2] ANSYS (2013): ANSYS Turbogrid. ANSYS, 12th edn.
[3] Asuaje, Miguel; Farid Bakir; Smane Kouidri; Frank Kenyery; and Robert Rey (2010):
Numerical modelization of the flow in centrifugal pump: volute influence in velocity
and pressure fields. International Journal of Heat and Fluid Flow, 31(6):1113 – 1118.
[4] Bacharoudis, E.C.; A.E. Filios; M.D. Mentzos; and D.P. Margaris (2008): Parametric
study of a centrifugal pump impeller by varying the outlet blade angle. The Open
Mechanical Engineering Journal, 9(6):49–61.
[5] Backstroms, Theodor W Von (2006): A unified correlation for slip factor in centrifugal
impellers. Journal of Turbomachinery, 128(1):1–10.
[6] Barrio, Raul; Jorge Parrondo; and Eduardo Blanco (2010): Numerical analysis of the
unsteady flow in the near-tongue region in a volute type centrifugal pump for different
operating points. Computers and Fluids, 39(5):859 – 870.
[7] Busemann, A. (1928): Das Forderhohenverrhaltnis radialer kreiselpumpen mit
logarithmisch-spiraligen schaufeln. In: Z.Angew.Math.Mech. pp. 32–74.
[8] CFturbo (2012): CFturbo User manual. CFturbo, 9th edn.
[9] Cheah, K. W.; T. S. Lee; S. H. Winoto; and Z. M. Zhao (2007): Numerical Flow
Simulation in a Centrifugal Pump at Design and Off-Design Conditions. International
Journal of Rotating Machinery, 2007(Article ID 83641, 8).
64
79. [10] Date, A. W. (1996): Complete pressure correction algorithm for solution of incom-
pressible navier stokes equations on a nonstaggered grid. Numerical Heat Transfer,
Part B: Fundamentals, 29(4):441–458.
[11] Eckardt, D. (1980): Flow field analysis of radial and backswept centrifugal impellers.
In: 25th ASME Fluids Engineering Conference. p. 7.
[12] Memardezfouli, Mohamad and Ahmad Nourbakhsh (2009): Experimental investiga-
tion of slip factors in centrifugal pumps. Experimental Thermal and Fluid Science,
33(5):938–945.
[13] Mikhaial, S.; A. M. Mobarak; and M. G. Khalafallh (2007): Turbomachineres princi-
ples and Application. Cairo university, 1st edn.
[14] Qiu, Xuwen; David Japikse; Jinhui Zhao; and Mark R. Anderson (Apr 25 2011):
Analysis and validation of a unified slip factor model for impellers at design and off-
design conditions. Journal of Turbomachinery, 133(4):9.
[15] RHIE, C. M. and W. L. CHOW (1983): Numerical study of the turbulent flow past an
airfoil with trailing edge separation. AIAA, 21(11):1525–1532.
[16] Shengqin, HUANG; LIU Zhenxia; LU Yaguo; YAN Yan; and LIAN Xiaochun (2008):
Validations of some slip factor models for mixed-flow impellers. In: ASME Fluids
Engineering Conference. p. 7.
[17] Shojaeefard, M.H.; M Tahani; M.B. Ehghaghi; M.A. Fallahian; and M. Beglari (2012):
Numerical study of the effects of some geometric characteristics of a centrifugal pump
impeller that pumps a viscous fluid. Computers and Fluids, 60(0):61–70.
[18] Spence, R. and J. Amaral-Teixeira (2009): A {CFD} parametric study of geometrical
variations on the pressure pulsations and performance characteristics of a centrifugal
pump. Computers and Fluids, 38(6):1243–1257.
[19] stodola, A. (1945): Steam and gas turbine. McGraw-Hill Book co.
65
80. [20] Sun-Sheng, Yang; Kong Fan-Yu; Fu Jian-Hui; and Xue Ling1 (2012): Numerical
research on effects of splitter blades to the influence of pump as turbine. International
Journal of Rotating Machinery, 2012(Artical ID 123093):9.
[21] Versteeg, H. K. and W. Malalasekera (2007): An introduction to computional fluid
dynamics. Pearson Education Limited.
[22] Wiesner, F.J. (1967): A review of slip factors for centrifugal impellers. pp. 558–572.
66
