�
CFD study of a pump trip in a pump-check valve system
Elin Eriksson
����������������������
����������������
������������
�������
behavior of the centrifugal pump and swing check valve. In existing cal- culation tools, the system and components are modeled in one dimension along the axis of the piping with the Relap5 code. There exist models for swing check valves and centrifugal pumps, but the models are insufficient for accurate prediction of pressure wave phenomenons. In two previous Master Thesis projects performed by D.Bragmark and E.Boqvist, the dy- namic behavior of a centrifugal pump and a swing check valve in transient flow have been investigated using CFD (Computational Fluid Dynamics).
The model of the centrifugal pump from the previous thesis work by D.Bragmark was improved by including leakages and flow correcting ge- ometries that had been removed as well as surface roughness. Both a centrifugal pump and a swing check valve have been investigated during a pump trip event. One dimensional simulations in Relap5 suggested that the pump is not noticeably affected by the valve closing before the valve is completely closed. Due to this, the centrifugal pump and the swing check valve were simulated separately during the pump trip. The CFD code Ansys Fluent as well as the one dimensional code Relap5 are used to simulate the pump during the pump trip. The swing check valve was simulated in the two CFD codes Ansys Fluent and Star-CCM+.
The pump trip simulated in Relap5 showed similar characteristics as the pump trip simulation in Ansys Fluent. The main difference was that the Relap5 pump rolls out faster that the CFD pump, i.e the impeller of the pump comes to a stop faster. This means that the pump model in Relap5 is conservative, i.e it overestimates the loads in the system. The valve simulation in the two different CFD codes showed close to identical re- sults. For further valve simulations the Star-CCM+ code is preferred due to more convenient dynamic mesh method and geometry handling. If the approximation of separate simulation proves to be accurate, the pump trip simulation of the valve could be used efficiently in future develop- ment. It is hard to take measurements of the valve during a pump trip and therefore no experimental values were available.
The valve model used in Relap5 is a newly developed model and might not
be fully tested yet. For further used one should make sure that the model
is properly tested. A better estimate of the surface roughness would be
desirable for further use of the CFD models.
a day I was not happy to arrive at the office. I also thank FS Dynamics for giving me the opportunity to perform my master thesis at their Solna office.
A special thank you to my two supervisors Ori Levin and Fady Ishaq, for lending me your time and for discussing my problems with me, without their help I would not have come this far. I thank them also for our weakly meetings and for the help with Relap5 and the CFD codes. A thank you also to Emil Boqvist and David Bragmark for lending me your expertise when no one else knew the answers.
A thank you to Ber¨ akningsgruppen for funding the thesis and lastly I
would like to thank KSB for allowing me to work with their real model
of the centrifugal pump as well as their experimental data to compare my
models to.
Contents
1 Introduction 8
1.1 Background . . . . 9
1.2 Problem description . . . . 10
1.3 Aim . . . . 10
1.4 Published work . . . . 11
2 Theory 13 2.1 The Realizable k − ε model . . . . 15
2.2 Wall functions . . . . 16
2.3 Surface roughness . . . . 17
2.4 Impeller rotation . . . . 18
2.5 Valve closing . . . . 19
2.6 Homologous curves . . . . 19
2.7 Mesh motion . . . . 19
2.8 Dimensionless valve variables . . . . 20
3 Method 21 3.1 Geometry . . . . 24
3.1.1 Pump . . . . 24
3.1.2 Valve . . . . 26
3.1.3 Pump system . . . . 27
3.1.4 Pump-valve system . . . . 27
3.2 Mesh . . . . 28
3.2.1 Pump . . . . 28
3.2.2 Pump system . . . . 29
3.2.3 Pump-valve system . . . . 30
3.2.4 Valve . . . . 30
3.3 Pump . . . . 31
3.3.1 Numerical set up . . . . 31
3.3.2 Boundary conditions . . . . 31
3.3.3 Impeller motion . . . . 31
3.3.4 Sensitivity Study . . . . 32
3.3.5 Reproducing pump curves . . . . 32
3.4 Pump trip . . . . 33
3.4.1 Numerical setup . . . . 33
3.4.2 Boundary conditions . . . . 33
3.4.3 Impeller motion . . . . 33
3.4.4 Sensitivity study . . . . 34
3.4.5 Pump trip Relap5 . . . . 34
3.5 Pump trip with open valve . . . . 34
3.5.1 Numerical setup . . . . 34
3.5.2 Boundary conditions . . . . 34
3.5.3 Impeller motion . . . . 34
3.5.4 Sensitivity study . . . . 34
3.5.5 Pump trip with valve Relap5 . . . . 35
3.6 Dynamic valve closing . . . . 35
3.6.1 Numerical setup . . . . 35
3.6.2 Boundary conditions . . . . 36
3.6.3 Disc motion . . . . 36
3.6.4 Relap5 . . . . 36
4 Result 37 4.1 Pump . . . . 37
4.1.1 Sensitivity study . . . . 37
4.1.2 Reproducing pump curves . . . . 40
4.2 Pump trip . . . . 41
4.3 Pump trip with open valve . . . . 43
4.3.1 Relap5 . . . . 43
4.3.2 CFD . . . . 44
4.4 Dynamic valve closure . . . . 45
5 Discussion 46 5.1 Method . . . . 46
5.2 Result . . . . 48
5.2.1 Reproducing pump curves . . . . 48
5.2.2 Pump trip . . . . 48
5.2.3 Pump trip with valve . . . . 49
5.2.4 Dynamic valve closing . . . . 49
6 Conclusion 50
A Sensitivity study pump trip B Pump trip UDF
C Dynamic valve UDFs
D Relap5 pump trip with dynamic valve code
List of Figures
1 A typical centrifugal pump. Image from Bragmark [1]. . . . 8 2 The valve model with disc in closed position. Image from Bo-
qvist [2]. . . . 8 3 The experimental setup from the experiment performed by KSB.
The static pressure was measured in four points, two diameters from both inlet (p
M 1) and outlet (p
M 2) [1]. Image from Brag- mark [1]. . . . 21 4 The Homologous curves representing (a) Pressure head and (b)
impeller torque used in the Relap5 simulations. . . . 22 5 The dimensionless coefficients defined in (a) (42), (43) and (b)
(44) obtained by simulating the valve in Star-CCM+ with fixed valve disc for varying opening angles and constant mass flow rate. 23 6 A cross section of the meshed (a) old pump geometry [1] and (b)
new, full pump geometry. Notice the leakage clearances at the inlet and below the impeller at the shaft. The moving mesh zone is highlighted with red. . . . 24 7 A zoom in on the cross section of the leakage clearances at (a)
the inlet and (b) the shaft as well as (c) one of the two stabilizing geometries at the inlet . . . . 25 8 A side view of the valve showing opening angle, rotation center,
center of mass and the distance between the two later. Image obtained from Boqvist [1]. . . . 26 9 The geometry used in the pump trip simulations. . . . 27 10 The geometry used in the pump trip with open valve simulations. 27 11 The leakage clearance at the inlet consists of two walls, i.e. inner
and outer part of the circle. This part is connected to the rest of the fluid zone by interfaces at the top and bottom of the clearance. 28 12 A stationary rotation of the impeller with the entire pump ge-
ometry is compared to the previous thesis at nominal flow with regard to (a) pressure head normalized by nominal pressure head
∆H
Rand (b) impeller torque normalized by nominal impeller torque τ
R. The flow rate is normalized by the nominal flow rate Q
R. There is no surface roughness applied, hence the 0 µm no- tation. The dashed line between the Bragmark simulation points is an interpolation of the simulated data. . . . 37 13 Pump simulations were performed with surface roughness 600
µm, 100 µm and 30-45 µm defined in table 9 at Q=190m
3/h. The resulting impeller moment and pressure head of these simulations are compared to the previous thesis results and to experimental values. (a) Pressure head normalized by nominal pressure head
∆H and (b) the impeller torque normalized by nominal impeller torque τ
Rare shown. The flow rate is normalized by the nominal flow rate Q
R. The dashed line between the Bragmark simulation points is an interpolation of the simulated data. . . . 38 14 A comparison of the result of pump simulations at nominal flow
rate with meshes P1 and P2, defined in table 6. . . . 39
15 The normalized experimental pump curves for head rise and im- peller moment are compared to the result of simulations at the four flow rates Q = 0, 60, 120, 190 m
3/h. In the simulations the surface roughness is set to 25 µm for all surfaces in contact with the fluid. The mechanical loss has been added to the moment.
The curves are normalized by nominal values ∆H
R, τ
Rand Q
Rof head rise, impeller torque and volumetric flow rate. . . . 40 16 The pump trip simulations in Fluent and Relap5 are compared
for (a) pump head, (b) impeller moment, (c) volumetric flow rate and (d) radial velocity of the impeller. . . . 41 17 A comparison between taking away the motor torque in one
timestep (sharp) and over ten time steps (smooth) in Ansys Flu- ent for (a) pump head, (b) impeller moment, (c) volumetric flow rate and (d) radial velocity of the impeller. . . . . 42 18 The Resulting flow rate from the Relap5 pump trip simulations
are shown. The three simulations include the piping system in figure 10 without valve, with fully open valve and with dynami- cally closing valve. The deviation of the closing valve simulation starts when the valve is completely closed. . . . 43 19 Pump trip simulations without valve and with valve implemented
in both Ansys Fluent and Relap5 are compared for (a) pump head, (b) impeller moment, (c) volumetric flow rate and (d) the radial velocity of the impeller. o.p stands for only pump and w.v stands for with valve. . . . 44 20 The dynamic valve closing simulated in both Star-CCM+ and
Ansys Fluent. The result of the simulations are represented by (a) the total pressure drop over the valve, (b) the moment on the disc produced by pressure and viscous forces, (c) The volumetric flow rate and (d) the opening angle θ of the disc over time, also simulated in Relap5 with both new valve model and original valve model. . . . 45 21 Surface roughness 25 µm and 45 µm implemented in Ansys Flu-
ent are compared for (a) pump head, (b) impeller moment, (c) volumetric flow rate and (d) the radial velocity of the impeller. . 22 Meshes P3 and P4 implemented in Ansys Fluent are compared
for (a) pump head, (b) impeller moment, (c) volumetric flow rate and (d) the radial velocity of the impeller. . . . 23 Pump trip with time step 0.0002 and 0.00046 implemented in
Ansys Fluent are compared for (a) pump head, (b) impeller mo- ment, (c) volumetric flow rate and (d) the radial velocity of the impeller. . . . 24 The designed UDF and the Ansys Fluent 6DOF solver imple-
mented in Ansys Fluent are compared for (a) pump head, (b)
impeller moment, (c) volumetric flow rate and (d) the radial ve-
locity of the impeller. . . .
List of Tables
1 Definition of the near wall regions [8]. . . . . 16
2 The definition of the different homologous curves used to model the pump in Relap5. . . . 22
3 Pump values . . . . 25
4 Scaled valve values . . . . 26
5 Clearance mesh . . . . 29
6 Pump meshes used in various simulations . . . . 29
7 Valve meshes used in a sensitivity study . . . . 30
8 Solution settings in Ansys Fluent. . . . . 31
9 Surface roughness . . . . 32
10 Solution settings in Ansys Fluent and Star-CCM+. L-S is an ab- breviation of Least Squares and p-v is an abbreviation of pressure- velocity. . . . 36
11 Comparison between simulation and experimental pressure head and moment results. The experimental value at nominal flow of the impeller moment is 113 Nm and of the head rise 25.7 m. . . . 38
12 The result of the leakage clearance sensistivity study. . . . 39
13 Comparison between simulation, experimental and previous sim- ulation pressure head and moment results. . . . 40
14 Result of sensitivity study of valve mesh with stationary disc. . . 43
Nomenclature
α
RRotational speed at nominal operation [rpm or rad/s]
δ
ijKronecker delta
µ Dynamic viscosity [Pa·s]
µ
tTurbulence viscosity [m/s]
ν Local kinematic viscosity [m
2/s]
ω Rotational velocity of impeller [rad/s or rpm]
ρ Density [kg/m
3] τ Torque [Nm]
τ
RImpeller torque at nominal operation [Nm]
τ
wWall shear stress [kg/(m·s
2)]
τ
bBuoyancy torque [Nm]
τ
f rFriction torque [Nm]
τ
hHydraulic torque [Nm]
τ
totTotal torque on the valve disc [Nm]
τ
wWeight torque [Nm]
τ
wexternal torque [Nm]
θ Opening angle of valve disc [deg]
ε Dissipation rate of turbulence kinetic energy [m
2/s
3]
C
MCoefficient that expresses the ratio between measured torque and torque calculated from the measured static pressure difference [-]
C
qDimensionless flow coefficient [-]
D
impImpeller diameter [m]
e internal energy [J]
f Force [N]
g Gravitational accelleration [m/s
2] H Pressure head [m]
h Height [m]
H
RPressure head at nominal flow [m]
I Moment of inertia [kg·m
2]
K Pressure loss coefficient [-]
k Turbulent kinetic energy [m
2/s
2] K
sRoughness height [m]
K
s+Dimensionless roughness height [-]
L Length scale [m]
L
dLength of valve disc torque arm [m]
m Mass [kg]
p Static pressure [Pa]
Q Volmetric flow rate [m
3/s or m
3/h]
Q
RNominal flow rate [m
3/h]
r Distance from rotation axis [m]
R
CGDistance from rotation axis to center of gravity [m]
Re
cReynolds number for centrifugal pump [-]
U Mean velocity of fluid [m/s]
u Velocity of fluid [m/s]
u
0Velocity fluctuations [m/s]
U
∗Dimensionless velocity [-]
u
τFriction velocity [m/s]
W Work [J]
y
+Dimensionless wall distance [-]
1 Introduction
In this master thesis two components common in nuclear piping systems will be studied, a centrifugal pump and a swing check valve. Both components have been studied in previous thesis work, thus this will be a continuing and connecting work. Figure 1 shows a typical centrifugal pump and figure 2 shows the geometry of the swing check valve when the valve is closed.
Figure 1: A typical centrifugal pump. Image from Bragmark [1].
Figure 2: The valve model with disc in closed position. Image from Boqvist [2].
1.1 Background
FS Dynamics has a well-developed cooperation with Swedish and Finnish nu- clear power industry where FS Dynamics contributes with experience and deep theoretical knowledge within various simulations. The nuclear power plants are required to verify that piping systems can withstand the loads that the systems are exposed to. Due to this, it is of high interest to investigate the behavior of a centrifugal pump and a swing check valve during a pump trip.
The centrifugal pump is one of the most common pumps and has been used to transport fluid for over a decade. The centrifugal pump is a thoroughly tested and robust device. When the pump is operating, the fluid is sucked from the suction side in to the pump at the center of the impeller, the impeller eye.
The pressure of the fluid is increased from inlet to outlet, or from suction to pressure side. This is done by transforming mechanic energy to kinetic energy through the rotating impeller. The fluid is accelerated along the impeller blades by the centrifugal force and thus transforming kinetic energy into pressure and this results in a higher pressure at the pressure side than at the suction side.
The fluid flow inside a pump is a three dimensional, turbulent flow which is often complicated to analyze. [3].
Losses in a centrifugal pump can be divided into two main groups; hydraulic- and mechanical losses. Among mechanical losses we have losses in bearings and in the shaft seals. The mechanical losses cause the power consumption to rise since they give a resisting torque. Bearing life, which is dependent of axial, radial and hydraulic thrust can also affect the mechanical losses [4].
The hydraulic losses contain flow friction, mixing, recirculation, incidence, impeller friction and leakage. The impeller friction will lead to a higher power consumption due to its resisting torque, leakage leads to a reduced flow through the pump and the rest of the hydraulic losses cause a lower head rise [3].
pressure-to-suction leakage flows in shrouded centrifugal pumps also substan- tially contribute to the fluid induced rotor dynamic forces. These forces inversely proportional to the clearance between impeller and casing [5], from here on ref- erenced by leakage clearances.
Reverse flow can occur in the pipe system due to for example a pipe rupture or a pump trip. It is not desirable to have back flow since it might damage the pump and other components. This can be prevented by having check valves build in to the pipe system. Although back flow can still occur, it will be restricted by the check valve. There are a number of different check valves available, for example swing, lift and tilting disc. The most represented type in the nuclear industry, which is also the type that causes the most failures is the swing check valve. This valve is beneficial since it gives a low pressure loss compared to other mentioned models, has a simple design and comes in many different sizes.
One drawback of the swing check valve is that it is known to have one of the longest closing times, which may increase the maximum back flow compared to other valve types.
Today’s method of obtaining preliminary results is to simulate the system in
1D along the axis of the piping. The nuclear system code Relap5 (Reactor
Excursion and Leak Analysis Program) developed at Idaho National Labora- tory for the U.S Nuclear Regulatory Commission in the 1980s is one of the most widely used 1D codes in the nuclear industry. An interesting question is weather the code is conservative or not, i.e. if the code overestimates loads in the system. A new model of the swing check valve has recently been created for Relap5 by W.Baltyn [6]. The new valve model can be used with different calculation models for the hydraulic torue data. The model of interest for this thesis work is a model called the cmcq model [7]. The new valve model is an empirical model, but one should have in mind that it has not been completely tested yet. One of main the problems with the original swing check valve model in Relap5 is that it is known to close too fast.
In this Thesis, the centrifugal pump and swing check valve will be simulated in 3D using the CFD (Computational Fluid Dynamics) codes Ansys Fluent 16.2 ans Star-CCM+ 11.2. CFD is the analysis of system including fluids, heat transfer and associated phenomenons through computer aided simulation. CFD codes are structured around numerical algorithms that can solve fluid problems and it can be advantages to experiments since it can shorten development time and costs [8].
A model of the pump created by David Bragmark [1] will be used together with an existing model of the swing check valve created by Emil Boqvist [2].
1.2 Problem description
Pressure waves can be caused by e.g. valve operations, pump trips, pipe break and steam collapse. Therefore it is of interest to investigate the behavior of the centrifugal pump and swing check valve. In existing calculation tools, the sys- tem and components are modeled in one dimension along the axis of the piping with the Relap5 code. There exist models for swing check valves and centrifugal pumps, but the models are insufficient for accurate prediction of pressure wave phenomenons. In two previous Master Thesis projects, the dynamic behavior of a swing check valve and a centrifugal pump in transient flow have been investi- gated using CFD. The idea of the present Master Thesis is to model a centrifugal pump and a swing check valve with appropriate boundary conditions to study the scenario of a pump trip and how the pump rolls out as well as how the valve closes during this event.
1.3 Aim
An existing pump model is to be improved by including losses that have not
yet been considered. The aim of the project is to simulate a pump trip scenario
both with 1-dimensional (1D) modeling and 3-dimensional (3D) CFD analysis
and compare the results. The main focus will be to see how the centrifugal
pump impeller rolls out and how the swing check valve closes. It is of high
interest to see how the one dimensional calculations compare to CFD and if the
one dimensional calculations are conservative as well as if valve and pump can
be simulated separately without making a too rough of an estimate.
1.4 Published work
This Master thesis is a continuing work of David Bragmarks thesis [1] regarding a centrifugal pump during a water hammer event. The same centrifugal pump will be used in this project. In Bragmark [1] a valve closure was modeled in Ansys Fluent 16.0 by decreasing the mass outflow of the pump, which was set as the outlet boundary condition. Both transient and stationary simulations were performed, where the simulation was stationary with regard to the mass outflow.
A mesh with 2 prism layers was used, although more prism layers could give better results. two turbulence models were tested, the realizable k − ε and the SST k − ω model. The SST k − ω model was found to be more mesh dependent than the realizable k − ε model. The resulting pressure head and moment of the 3D simulation did not quite match the experimental values from the pump manufacture. The pressure head curve had a percentage error between 3-4%
and the moment curve had a percentage error between 3-16% when compared to experimental data. The deviation from the experimental curves could be due to ignoring some losses from motor to pump.
URANS equations together with the two equation k − ε turbulence model were found by S.R.Shah et.al. [9] to be appropriate and considered to give a good es- timation of the overall performance of the centrifugal pump. The typical errors of the result using this approach was found to be below 10 % of the experimen- tal values. The study concludes that the impeller has been extensively studied, while the volute of the centrifugal pump is a field with few studies, and thus studies in this field may be promising for pump performance. Although CFD is promising in many regards, it is still recommended to compare the result of CFD simulations to experimental results.
In an article written by Wen-Guang Li [10] the impact of the surface roughness, viscosity and design of the impeller was investigated by CFD computation. The quantities were investigated using the CFD code Ansys Fluent. The standard k − ε model was used in the CFD computations to evaluate turbulent stresses.
Non-equilibrium wall functions were applied to include stress on the walls of the pump. Water and three different oils with varying viscosity were used to investigate the importance of viscosity. The sand roughness height 0, 50 and 100 µm were used to investigate importance of surface roughness. The roughness coefficient in Fluent was set to 0.75. It was concluded that the results for the performance of the CFD simulation were qualitative compared to observations.
In an article from 2007 by R. Spence and J. Amaral-Teixeira [11] a model of
the complete geometry of a double inlet centrifugal pump, including the leakage
from pressure to suction side. The simulations were performed in 3D using CFX-
TASCflow which is a Navier-Stokes code. In the article, it was concluded that
previous studies had suggested that the area where the leakage flow meets the
inlet flow requires careful modeling. It was also suggested that the grid design
was improved by grid interfaces in complex regions having one-to-one connec-
tions. Scalable wall functions were used in the model. The study resulted in a
successful model of the entire geometry. The largest pressure pulsations were
found at the impeller outlet and the CFD-analysis agreed well with experimen-
tal results at most locations.
A doctoral thesis by Eskil Storteig [12] suggests that leakage from pressure to suction side through the seal in a centrifugal pump can be important for pump performance. In the article the importance of the geometry of the seals are investigated. It was concluded that inlet and exit conditions of seals affect both seal leakage and rotor dynamic coefficients to some extent. The clearance was modeled with a grid of square cells. For clearances between 0.0031 and 0.10 mm the number of layers for the minimum clearance was set to 8. For clearance 0.15, 0.20 and 0.40 the number of layers were set to 18, 25 and 40 respectively.
In a former thesis paper by Emil Boqvist [2] a swing check valve was inves- tigated. The swing check valve investigated was used to transport pressurized water to a reactor tank. The aim of the project was to simulate both stationary and transient cases to later improve a 1D model. Two important parameters when investigating the fluids impact on the disc are the torque on disc and mass flow. The turbulence model used in the final simulation was the Realizable k − ε model and sclalable wall functions were used for wall treatment. The valve was tested for different deaccelerations of the flow and it was found that the closing time varies with the deacceleration. It was also found that back flow occurs before the valve is completely closed. There were however noticeable differences in torque on the disc for different turbulence models for the steady state simu- lations and the turbulence models were not tested for the transient simulations.
There were no experimental values available for determining which turbulence model was best suited for the CFD simulations. A model of the same swing check valve is also available in Star-CCM+, although there are no sensitivity studies performed on this model and the existing mesh is currently to coarse.
In an article written by A. R. D. Thorley [13] a review of check valves un-
der transient flow conditions is made. In this paper it is stated that the systems
that are most at risk are those with pumps that deliver high pressure heads. If
a pump is protected with a badly fitted check valve it can result in problems
with check valve slam, line vibration and failure. A basis for valve dynamic
response from measurements taken under laboratory conditions has been cre-
ated. The use of this basis is most efficient in pipeline designs when used in
non-dimensional representation of the important terms.
2 Theory
Centrifugal pumps are used to increase the pressure of a fluid for it to be trans- ported to a higher level. The process that takes place when the fluid passes through the pump can be assumed to be adiabatic, since the heat exchange between the fluid and the surroundings is so small that it can be neglected. We can also assume that the external leakage is negligible, since this is normally very small. For the described case, the energy equation for stationary flow per pumped unit mass according to
W = e
o− e
i+ p
o− p
iρ + c
2o− c
2i2 + g(h
o− h
i), (1) where W is the work performed by the pump, e
iand e
oare the inlet and outlet internal energy, p
iand p
oare the inlet and outlet static pressure, g is the gravitational acceleration, h
iand h
oare the inlet and outlet heights and c
iand c
oare the inlet and outlet absolute velocity.
It is desirable that as much as possible of the work added by the electric motor results in an increase of static energy in the fluid, since internal energy is hard to utilize. An increase of internal energy would increase the temperature of the fluid and is considered to be a loss [14]. The increase of pressure head is thus the useful part of the fluids change of state and is defined by
∆H = p
o− p
iρg + c
2o− c
2i2g + h
o− h
i. (2)
When the Reynolds number of a flow rises above the critical Reynolds number, the flow goes from the laminar to turbulent regime. The flow goes from be- ing smooth and predictable, to containing random and chaotic motions. The reynolds number in the centrifugal pump can be defined by
Re
c= ρnD
2impµ , (3)
where n is revolutions per second, D
impis the diameter of the impeller and µ is the dynamic viscosity of the fluid. The flow in a centrifugal pump is in the turbulent region since the Reynolds number in the volute is Re
c∼ 10
6, which is in the turbulent region [1].
The governing equations needed to model the turbulent flow, written in Einstein notation, are the continuity equation
∂u
i∂x
i= 0 (4)
and Navier-Stokes equations
∂u
i∂t + u
j∂
∂x
ju
i= 1 ρ f
i− 1
ρ
∂p
∂x
i+ 1 ν
∂
2u
i∂x
j∂x
i, (5)
where f
iare the external forces, p is the static pressure, u is the velocity of
the fluid and ν is the local kinematic viscosity. The fluctuations in a turbulent
flow are always in 3D and makes the flow costly to describe. We need to apply
numerical methods and turbulence models to predict the flow. When using CFD, the finite volume method (FVM) is used, where the fluid is discretized on to a grid of control volumes that contain the flow variables. To account for the turbulence, velocity and other flow properties are divided into fluctuating and mean values e.g
u = U + u
0, (6)
where u is the velocity of the fluid, U is its mean value and u
0its fluctuations (also applicable on f
i, p,...). This method is called Reynolds decomposition. We consider time averaging the fluctuating properties u = U + u
0and v = V + v
0defined by
hu
0i = hv
0i = 0 hU i = U h ∂u
∂s i = ∂U
∂s h Z
udsi = Z
U ds (7) hu + vi = U + V huvi = U V + hu
0v
0i huV i = U V hu
0V i = 0.
The time average of the governing equations (5) and (4) used together with (7) can be written
∂u
i∂x
i= ∂U
i∂x
i= 0 (8)
and
∂U
i∂t + U
j∂
∂x
jU
i= 1 ρ
F
i− ∂P
∂x
i+ ∂
∂x
j2µS
ij− ρhu
0iu
0ji
, (9)
where F
iare the external forces and S
ij= 1
2
∂U
ix
j+ ∂U
j∂x
i(10) is the mean strain rate tensor. The last term in (9) is the Reynolds stress R
ij= −ρhu
0iu
0ji. In 1877 Boussinesque proposed that the Reynolds stress is proportional to the rates of deformation, that is
− ρhu
0iu
0ji = 2µ
tS
ij− 2
3 ρkδ
ij, (11)
where µ
tis the turbulent viscosity and k =
12hu
0iu
0ji is the turbulence kinetic energy [8].
To numerically model the RANS equation (9) it can be beneficial to write the pressure on the form
P = ˜ P + ρ
0g
ix
i(12)
where ρ
0is a reference density and ˜ P is a non-physical pressure variable. Thus (9) can be written
∂U
i∂t + U
j∂
∂x
jU
i− 1 ρ
∂
∂x
j2µS
ij− ρhu
0iu
0ji = 1 ρ
F
i− ∂P
∂x
i= 1
ρ
F
ext+ ρg − ∂P
∂x
i= 1 ρ
F
ext+ g(ρ − ρ
0) − ∂P
0∂x
i, (13)
where F
extare the average external forces excluding gravity. If the reference
density is set equal to the constant density it may improve convergence [15] [16].
The k − ε equations are based on mechanisms that affect the turbulent kinetic energy. The standard k − ε model has two model equations, one for turbulence kinetic energy k, and the second for dissipation rate ε. The standard k−ε model is empirically based on the understanding of relevant fluid processes, since the exact k − ε equations contain many unknown parameters and constants. This model can be used for a large number of turbulent applications, but is not well suited for rotating flows or flows with large adverse pressure gradients. For the standard k − ε model the turbulent viscosity is defined by
µ
t= ρC
µk
2ε , (14)
where C
µ= 0.09 [15].
2.1 The Realizable k − ε model
The realizable k − ε model differes from the standard k − ε model in two important ways,
First C
µin the turbulent viscosity is not a constant.
Second The transport equation for the dissipation rate ε is derived from an exact equation for transport of mean square vorticity fluctuation.
The term realizable means that the model satisfies certain mathematical con- straints on the Reynolds stress which is consistent with turbulent flows. The standard k − ε model does not satisfy these constraints and is therefore not realizable. The transport equation for k in the realizable k − ε model is defined by
∂k
∂t + ∂ku
jx
j= 1 ρ
∂
∂x
jµ + µ
tσ
k∂k
∂x
j+ G
k+ G
b− ρε + Y
M+ S
k(15) and the transport equation for ε is defined by
∂ε
∂t + ∂εu
jx
j= 1 ρ
∂
∂x
jµ + µ
tσ
ε∂ε
∂x
j+
ρC
1Sε − ρC
2ε
2k + √
νε + C
1εε
k C
3εG
b+ S
ε. (16)
G
krepresents the generation of turbulence kinetic energy due to mean veloc- ity gradients, G
brepresents the generation of turbulence kinetic energy due to buoyancy and Y
Mis the contribution of fluctuating diliation due to compress- ibility. C
2and C
1εare constants, S
kand S
εare user defined source terms and C
3εis the degree of which the dissipation rate is affected by the buoyancy. C
3εcan be defined by
C
3ε= tanh | u
⊥u
k|, (17)
where u
kis the velocity component parallel to the gravitational vector and u
⊥is the velocity component perpendicular to the gravitational vector [15]. The turbulent viscosity is defined by
µ
t= ρC
µk
2ε (18)
as in the standard k − ε model. The difference is in the definition of C
µwhich follows
C
µ= 1
4.04 + √
6 cos φ (19)
where
φ = 1
3 cos
−1√
6W
, W = s
ijs
jks
ki˜
s
3, ˜ s = √
s
ijs
ji(20) and
s
ij= 1 2
∂u
j∂x
i+ ∂u
i∂x
j. (21)
The constants in the model are set to [15]
C
1ε= 1.44, C
2= 1.9, σ
k= 1.0, σ
ε= 1.2. (22)
2.2 Wall functions
Semi empirical formulas called wall functions can be used to model the flow near the wall when that region is not resolved. Instead of resolving the near wall region, wall functions bridge the viscous sublayer between the wall and the log layer, without having to modify the turbulence model to consider the presence of the wall. The dimensionless wall distance and friction velocity are defined by
y
+= u
τy
ν , u
τ= r τ
wρ (23)
where τ
wis the wall shear stress and y is the wall distance. When y
+of the first wall adjent cell is below 15 the solution gradually deteriorates and the accuracy of the solution is not be maintained [15].
Table 1: Definition of the near wall regions [8].
Layer Region
Viscous sublayer y
+< 5 Buffer layer 5 < y
+< 30 Log-layer 30 < y
+< 500
The three near wall regions are defined in table 1. In the log layer the law of the wall for mean velocity is used, which is defined by
U
∗= 1
κ ln y
++ B (24)
where κ = 0.4187, B = 5.4494 and
U
∗= U
u
τ. (25)
The layer closest to the wall is the viscous sublayer. In this layer the dimen- sionless velocity is related to y
+by
U
∗= y
+. (26)
In the buffer layer it can be hard to determine an equation for the dimensionless velocity [8]. Ansys Fluent’s standard wall function uses (24) when y
∗> 11.225 and (26) when y
∗< 11.225. Note that in Ansys fluent,
y
∗= ρC
µ1/4k
1/2Pτ
w/ρ (27)
is used instead of y
+in (26) and (24), where k
Pis the turbulence kinetic energy at the wall-adjacent cell centroid. These two variables are approximately equal in equilibrium turbulent boundary layers [15].
Scalable wall functions are chosen to get consistent results when the grid refinement is arbitrary and can be used when y
∗< 11.225 to avoid deterioration of the standard wall functions. For the case when y
∗> 11.225 the scalable wall function is equal to the standard wall function. The limiter
˜
y
∗= y
lim∗if y
∗lim> y
∗y
∗otherwise (28)
where y
∗lim= 11.225. ˜ y
∗will be used instead of y
∗[15], when using scalable wall functions.
2.3 Surface roughness
The surface roughness affects the drag on the walls and can therefore have a considerable effect on the flow, depending on the non-dimensional roughness height,
K
s+= ρK
sU
∗µ , (29)
where K
sis the roughness height in meters. In Ansys Fluent [15], surface roughness heights are divided into three regimes:
Hydraulic smooth: K
s+≤ 2.25, Transitional: 2.25 < K
s+≤ 90, Fully rough: 90 < K
s+.
The hydraulic smooth region is considered to be negligible, while the importance of the roughness height increases in the transitional region and having full effect in the fully rough region. The wall roughness is added to the simulation through the law-of-the-wall modified for roughness [15]
U
∗= 1
κ ln y
++ B − ∆B. (30)
In the three regions, the constant ∆B [15] [16] takes the values
∆B = 0 (31)
in the hydraulic smooth region,
∆B = 1
κ ln K
s+− 2.25
87.75 + C
sK
s+sin{0.4258(ln K
s+− 0.811)} (32) in the transition region and
∆B = 1
κ ln(1 + C
sK
s+) (33)
in the fully rough region.
2.4 Impeller rotation
When the pump is tripped the driving torque from the motor driving the im- peller rotation will be set to zero. Thus only the torque arising from fluid and mechanical losses will be present. The mechanical losses can be considered con- stant with rotational speed, while the fluid forces will vary with both mass flow rate and rotational speed. The moment of inertia is the resistance of a body against change in rotation rate and depends on how the mass is distributed around the rotational axis. The moment of inertia, I
φaround axis φ is calcu- lated by
I
φ= Z Z Z
r
2dm (34)
where r is the orthogonal distance from the axis and dm = ρdV [15]. If we perform a dimension analysis of the mass and moment of inertia we get
[m] ∼ [ρ]L
3, [I] ∼ [m] · L
2∼ L
5, (35) where L is the length scale. Since the density of the material will not be affected by scaling, the moment of inertia scales with L
5, according to (35).
Given the torque around the rotation axis on the impeller from the fluid, the radial acceleration of a rigid body rotation can be then calculated by
˙
ω = τ
i/I
xx, (36)
where I
xxis the moment of inertia around the x-axis and τ
iis the torque around the rotation axis on the impeller. The rotational velocity of the impeller can then be calculated by [15]
ω(t) = Z
tt0
˙
ω dt. (37)
Given the rotational velocity of the impeller, the impeller passing frequency f
ip, i.e. the frequency of impeller blades passing a fixed point, can be calculated by
f
ip= 6ω
2π , (38)
since there are 6 impeller blades in the centrifugal pump we will use in the
present work.
2.5 Valve closing
The torque that controls the position of the valve disc is a sum of the torques caused by the weight of the disc τ
w, the buoyancy of the disc τ
b, friction at the hinge pin τ
f rand the surrounding fluid τ
h. It might also exist external torque τ
e, thus the total torque can be written
τ
tot= τ
w+ τ
b+ τ
f r+ τ
h+ τ
e. (39) The total torque can also be written
τ
tot= I
Aθ ¨ (40)
where I
Ais the inertia moment around axis A and ¨ θ is the angular acceleration of the disc [2]. I
Acan be calculated by (34) by letting r be the distance from axis A.
2.6 Homologous curves
To simulate the pump trip in the 1D code Relap5, homologous curves need to be provided to describe the behavior of the pump. Homologous curves in Relap5 are described by the dimensionless variables
α = ω ω
R, v = Q Q
R, h = H H
Rand β = τ τ
R, (41)
where α
R, H
R, Q
Rand τ
Rare the values of rotational speed, head, flow rate and torque at nominal operation. The relationship between the four parameters defined in (41) are displayed in a four quadrant representation. For a full pump representation, all four parameters need to be represented for both positive and negative values [17].
2.7 Mesh motion
In this thesis, three types of mesh motions will be used, dynamic mesh with smoothing, layering and overset mesh.
Smoothing retains the original cells and only moves cell common nodes. It is therefore suitable for boundaries with small deformations [15].
Layering allows cells to compress or expand. In this case, the mesh may only consist of hexahedra and prism cells. If a cell is too compressed/expanded the cell will merge with the neighboring cell/split into two cells. This method is useful when having large movements [15].
Overset is a dynamic mesh option that is available in Star-CCM+. This
method used overlapping meshes and is useful when working with moving
bodies. It does not require mesh modification after initialization. The
solutions in the overlapping mesh zones are interpolated, the cell size of
the two meshes should thus be similar [16].
2.8 Dimensionless valve variables
To model the swing check valve in Relap5 the cmcq model [7] presented in W.Baltyn [6] is used. This model needs measurement data from stationary experiments, or in our case simulations. To use this model three dimensionless variables are needed for different opening angles with stationary flow. The first variable is the coefficient that expresses the ratio between measured torque and torque calculated from the measured static pressure difference. This coefficient is calculated by
C
M= τ
HA∆pL
d, (42)
where τ
His the hydraulic torque, A is the seat area of the disc, ∆p is the pressure drop over the valve and L
dis the length of the torque arm. The second variable is a flow coefficient defined by
C
Q= s
ρQ|Q|
2∆pA
2, (43)
where Q is the volumetric flow rate. Finally, the third coefficient is a loss coefficient that can be written
K = 1
C
Q2. (44)
To model the valve, a model called the sr model [18] could also be used.
This model requires measurements from transient experiments or simulations
to calculate the necessary variables.
3 Method
In an experiment performed on the centrifugal pump by KSB, the static pressure of the fluid was measured at four points around the wall of the pipe, all four points the same distance from the inlet/outlet. The measurements were taken two diameters from the inlet and two diameters from the outlet. The mean value of these measurements was considered to be the static pressure at that point.
The total pressure was calculated by (2), assuming no height difference between the measurements, that is h
i= h
o. In figure 3 we can see the experimental setup of the experiment performed by KSB. To mimic the experiment and get a model close to reality, the pressure head produced by the pump was obtained by calculating an area weighted average of the static pressure at the inlet and outlet of the pump. The average of the static pressure was calculated two diameters from the inlet and two diameters from the outlet. The total pressure was calculated by (2) assuming h
i= h
o. Since the flow is assumed to be incompressible, the absolute velocity is calculated from the volumetric flow rate and cross sectional area by u = Q/A.
Experimental values provided by KSB were also used to produce the ho- mologous variables defined in (41). These variables were used to model the pump in Relap5. Since there were no experimental measurements for back flow through the pump, some values had to be estimated for the homologous curves.
The estimations were based of the experimental values together with results from articles by Jung Yoon, Tae-Ho Lee, Hwi-Seob Park [19] and I.K Madni, E.
Cazzoli [20].
Figure 3: The experimental setup from the experiment performed by KSB. The
static pressure was measured in four points, two diameters from both inlet (p
M 1)
and outlet (p
M 2) [1]. Image from Bragmark [1].
The curves presented in figure 4 are the homologous curves that were used to model the pump in Relap5. The six curve types HAD, HVN, HAN, BAD, BVN and BAN are defined in table 2 with α, h, v and β defined in (41).
Table 2: The definition of the different homologous curves used to model the pump in Relap5.
Curve x-axis y-axis quadrant
HVN α/v h/v
21st
HAD v/α h/α
22nd
HAN v/α h/α
21st
BVN α/v β/v
21st
BAD v/α β/α
22nd
BAN v/α β/α
21st
-1 -0.5 0.5 1
v/α or α/v 0.5
1
h/α2 or h/v2
HAN HVN HAD
(a)
-1 -0.5 0.5 1
v/α or α/v 0.5
1
β/α2 or β/v2
BAN BVN BAD
(b)
Figure 4: The Homologous curves representing (a) Pressure head and (b) impeller
torque used in the Relap5 simulations.
The pressure difference over the valve was measured directly in total pressure drop, by calculating the surface average of the total pressure at inlet and outlet.
The input variables (42) - (44) were calculated for 7 different disc opening angles between minimum and maximum angle using a CFD model, the valve model later defined for Star-CCM+. The values were taken from steady state solutions with fixed valve positions. This was done since there were no experimental values available. The values of the coefficients for completely closed valve were estimated.
0 20 40 60
angle [deg]
0 0.5 1 1.5 2
[-]
Cq
CM