scispace - formally typeset

Journal ArticleDOI

A CFD study on the mechanisms which cause cavitation in positive displacement reciprocating pumps

01 Mar 2015-Journal of Hydraulic Engineering-Vol. 1, Iss: 1, pp 47-59

AbstractA transient multiphase CFD model was set up to investigate the main causes which lead to cavitation in positive displacement (PD) reciprocating pumps. Many authors such as Karsten Opitz [1] agree on distinguishing two different types of cavitation affecting PD pumps: flow induced cavitation and cavitation due to expansion. The flow induced cavitation affects the zones of high fluid velocity and consequent low static pressure e.g. the valve-seat volume gap while the cavitation due to expansion can be detected in zones where the decompression effects are important e.g. in the vicinity of the plunger. This second factor is a distinctive feature of PD pumps since other devices such as centrifugal pumps are only affected by the flow induced type. Unlike what has been published in the technical literature to date, where analysis of positive displacement pumps are based exclusively on experimental or analytic methods, the work presented in this paper is based entirely on a CFD approach, it discusses the appearance and the dynamics of these two phenomena throughout an entire pumping cycle pointing out the potential of CFD techniques in studying the causes of cavitation and assessing the consequent loss of performance in positive displacement pumps.

Topics: Cavitation (57%), Reciprocating pump (53%), Centrifugal pump (51%), Positive displacement meter (51%)

Summary (3 min read)

1. Introduction

  • If one focuses on the sole category of positive displacement (PD) reciprocating pumps one may say that there is a significant shortage of technical literature in this important area.
  • Even though water, in certain operative condition, may be considered incompressible there are periods within the pumping cycle when the inlet and outlet valve are both closed and the compressibility model is required to stabilize the simulation and fulfil the mass continuity equation.
  • In the case of incipient or marginal cavitation, for instance, it is understood [1] that the number of bubbles and their distribution do not seem to be harmful to the pump and, avoiding any operating condition in this range, would result in a uneconomical device.

2. Material and Methods

  • The transient CFD model simulated the entire pumping cycle; the induction stroke, from the Tod Dead Centre position (TDC) to when the plunger reached the Bottom Dead Centre (BDC) position sweeping through the displacement volume, to the delivery stroke when the plunger again reached the TDC position as shown in Figure 1.
  • Figure 3 shows that the displacement volume was created by means of creation of cell layers during the inlet stroke and removal of cell layers during the outlet stroke in the direction of the plunger axis.
  • To make this possible a full hexahedral mesh was chosen for the displacement volume.
  • The spring force was provided to the UDF by means of spring stiffness characteristic curve.
  • The water vapour fraction was initialised as null in all of the volumes and the Singhal et al. cavitation model managed the phase change dynamics according to the pressure field as explained in [11].

2.1 Set up cases

  • A mesh sensitivity analysis was carried out to define the best mesh size and spacing within the opposing needs of achieving good accuracy and keeping the computational time low.
  • To this purpose three mesh sizes were tested; 3, 5 and 6 Million cells overall.
  • The ANSYS-Fluent commercial code was chosen to solve the Reynolds Averaged Navier Stokes (RANS) equations and Table 1 shows a summary of the settings selected.
  • A 12 GB RAM computer with an Intel Xeon W3670 @ 3.2GHz processor was employed for the simulation and the time needed for a single run (1 pumping cycle only) ranged from 3 to 4 weeks.
  • For all cases the inlet and outlet pressure were set as the sum of a constant value, ranging from 0kPa to 100 kPa (depending on the case) and a transient value depending on the mass flow which was automatically calculated every time step by the solver.

3.1 Case 1

  • The chamber pressure fell close to the vapour level and remained fairly constant throughout the temporal range 100°-170° of the inlet stroke.
  • Its trend may be considered linear ascending in the range 17°-105°.
  • Figure 8 and Figure 9 demonstrate the presence of two types of cavitation which occurred simultaneously in the pump chamber.

3.2 Case 2

  • The chamber monitor point pressure during the induction stroke approached the saturation vapour pressure.
  • Figure 8 shows a behaviour of the vapour fraction similar to case 1 but the maximum values estimated by the CFD solver were lower (15%) and remained almost constant over a narrower range (90°-165°).
  • The smaller overall amount of vapour generated implied a smaller delay in valve closing which can be observed in Figure 13(a).
  • Table 3 quantifies the delay of 14.6° and a volumetric efficiency loss within the limit of 3% discussed by John Miller [6].
  • One can assume that case 2 describes a pump operating in the partial cavitating condition in accordance with Karsten Opitz [1], [8].

3.3 Case 3

  • A 5% peak of vapour fraction was present in the gap volume as shown in Figure 8 and occurs at 120° of crank rotation.
  • One may say that on the whole the pressure remained above the vapour limit but locally there were regions affected by low pressure.
  • In this case Figure 8 shows a linear trend which was different with respect to case 1 and 2 where the vapour volume fractions revealed a strongly non-linear behaviour before reaching the maximum.
  • In fact Figure 10 points out that the high velocity in the inlet valve-seat gap volume, as well as the induced localized pressure drop, is a piece of evidence of the flow induced cavitation.
  • The low level of vapour volume fraction resulted in a shorter delay of valve closing and an inlet mass flow rate/time history curve closer to the theoretical one .

3.4 Case 4

  • The chamber minimum pressure remained either generally or locally safely above the vapour limit, the minimum monitor point pressure/time curve ranged around the ambient pressure as shown in Figure 7.
  • Figure 8 shows a flat trend of the vapour volume fraction throughout the pumping cycle.
  • The graph indicates a 1% quantity of the second phase but, rather than water vapour this may be interpreted as the initial non-condensable mass fraction which slightly expanded during the inlet stroke.
  • The model correctly calculated the expansion of that gas providing a minimum variation of its volume fraction.
  • Among all cases this one is the closest to the theory in terms of inlet mass flow as pointed out by Figure 12 and it is affected by the least amount of volumetric efficiency loss ( Table 3).

4. Conclusion

  • A comprehensive transient CFD model of a PD reciprocating pump was created making use of the Ashok Singhal et Al. [11] cavitation model to simulate the device from incipient to full cavitating conditions.
  • The model was capable of simulating the phase change in the three conditions of incipient to full cavitation.
  • In case 1, where the higher second phase generation was observed, the vapour trapped in the vicinity of the inlet valve, at the end of the inlet stroke, kept the pressure close to the vapour level.
  • This paper showed and discussed the two different types of cavitation affecting PD reciprocating pumps which the numeric model identified; flow induced cavitation and cavitation due to expansion.
  • The authors are already working on a test rig to validate the results shown in this paper.

Did you find this useful? Give us your feedback

...read more

Content maybe subject to copyright    Report

A CFD study on the mechanisms which cause cavitation in positive
displacement reciprocating pumps
Aldo Iannetti
1
, Matthew T. Stickland
1
and William M. Dempster
1
1. Department of Mechanical and Aerospace engineering, University of Strathclyde, Glasgow G1 1XJ, UK
Abstract: A transient multiphase CFD model was set up to investigate the main causes which lead to cavitation in positive
displacement (PD) reciprocating pumps. Many authors such as Karsten Opitz [1] agree on distinguishing two different types
of cavitation affecting PD pumps: flow induced cavitation and cavitation due to expansion. The flow induced cavitation
affects the zones of high fluid velocity and consequent low static pressure e.g. the valve-seat volume gap while the cavitation
due to expansion can be detected in zones where the decompression effects are important e.g. in the vicinity of the plunger.
This second factor is a distinctive feature of PD pumps since other devices such as centrifugal pumps are only affected by
the flow induced type. Unlike what has been published in the technical literature to date, where analysis of positive
displacement pumps are based exclusively on experimental or analytic methods, the work presented in this paper is based
entirely on a CFD approach, it discusses the appearance and the dynamics of these two phenomena throughout an entire
pumping cycle pointing out the potential of CFD techniques in studying the causes of cavitation and assessing the
consequent loss of performance in positive displacement pumps.
Key words: Multiphase flows, PD reciprocating pump, cavitation model, expansion cavitation, flow induced cavitation
1. Introduction
The phenomenon of cavitation in pumps is still a
complex problem to study. If one focuses on the sole
category of positive displacement (PD) reciprocating
pumps one may say that there is a significant
shortage of technical literature in this important area.
Concentrating on the numerical analysis literature,
very few CFD works on PD reciprocating pumps
have been made so far, none of them deals with a
comprehensive model of this kind of device
operating in cavitation regimes. The main reason for
the lack of studies dealing with the numerical
analysis of cavitation dynamics in PD pumps is a
consequence of the following reasons:
Over the last decades PD pumps have
gradually become obsolete compared to
_____________________________
Corresponding author: Aldo Iannetti, master, main research
field: fluid dynamics. E-mail: aldo.iannetti@strath.ac.uk
centrifugal pumps on which great effort has
been spent by researchers both in
experimental and numerical analysis. This
was recalled by Herbert Tackett [2] who
identifies the cause of the great popularity of
centrifugal pumps due to the technological
improvement made to them in the last
decades. He also pointed out that, as a
consequence, PD pumps nowadays may be
considered a technically “old” device.
Despite their appearance PD pumps are a
complex device to model and study
particularly by means of CFD. This has led
the few researchers involved in PD pumps
studies to prefer experimental tests over
numerical methods.
The experimental methods, which are the only
techniques utilized so far, usually provide the
analysts with all the difficulties related to how to
take, from the test rigs, crucial information such as

A CFD Study on the mechanisms which cause cavitation in positive displacement reciprocating
pumps
the pressure field, the production rate of water vapour
and the loss of volumetric efficiency. Furthermore
numerical methods have not been feasible for many
years because of the great amount of computational
resources that a complex model, such a pump in
cavitating condition, may need. Herbert Tackett [2]
also explains that there are still many applications
where PD pumps outperform centrifugal pumps
which is the reason why, in the authors’ opinion, in
the next few years a re-evaluation of this old”
device is to be expected. One of the reasons for the
re-evaluation lies in the development of both High
Performance Computational (HPC) systems and CFD
techniques such as multiphase algorithms and
moving meshes which provide the analysts with
advanced numerical tools ready to be employed in
the analysis of fluid dynamics in PD pumps despite
their complexity, will be demonstrated in this paper.
The main feature successfully implemented in the
model developed by the authors, which puts this
work ahead of the previous work such as that carried
out by Ragoth Singh [3], is the simultaneous
coexistence of the following sub-models:
1. Compressibility of water. Even though
water, in certain operative condition, may
be considered incompressible there are
periods within the pumping cycle when the
inlet and outlet valve are both closed and
the compressibility model is required to
stabilize the simulation and fulfil the mass
continuity equation.
2. The valve dynamics model. The inlet and
outlet valves move following the pump
chamber pressure field which in turn
depends on the valves dynamics. To
correctly model a PD pump it is crucial to
provide the solver with a User Defined
Function (UDF) which accounts for the
two-way coupling between the valve
dynamics and the pressure field. As stated
by Stephen Price [4], cavitation strongly
depends on the inertia characteristic of the
valve.
3. Advanced cavitation model. The choice of
the cavitation model is crucial to achieve
reasonably accurate results in the case of
full cavitation conditions because the
analyst must account for the non-
condensable gas mass fraction to predict
pump performance deterioration in the
cavitating conditions. As demonstrated by
H. Ding [5] the amount of non-condensable
gas dissolved in the water affects the
prediction of the minimum Net Positive
Suction Head (NPSH) required in the inlet
manifold to keep the volumetric efficiency
loss above the generally accepted 3% as
recalled by John Miller [6].
The important role of the non-condensable gasses in
cavitation was also pointed out by Tillmann Baur [7]
who carried out an experimental test to demonstrate
the interaction of the gases dissolved in the water on
the bubble dynamics.
Many authors such as Karsten Opitz [8] agree on the
partitioning of the cavitation types into incipient (also
referred to as marginal cavitation), partial and full
cavitation. They are characterized by different
features as described in [8] and it is of crucial
importance, for the designer, to know which
cavitating condition the pump being designed will
operate in. In the case of incipient or marginal
cavitation, for instance, it is understood [1] that the
number of bubbles and their distribution do not seem
to be harmful to the pump and, avoiding any
operating condition in this range, would result in a
uneconomical device. In the case of partial to full
cavitation the damage as well as the loss in
performance may be extremely high and allowing the
pump to operate at that condition would result in
failures and loss of money.

A CFD Study on the mechanisms which cause cavitation in positive displacement reciprocating
pumps
The cavitation phenomenon in PD pumps appears to
be different from the one occurring in centrifugal
pumps. In the latter case cavitation is related to the
low pressure induced by the high velocity which
affects the rotor at certain operational conditions
(flow induced cavitation) while, in the case of PD
pumps, cavitation may depend on the low static
pressure due to the plunger decompression at the
beginning of the inlet stroke as well as on the high
velocity that the flow through the inlet valve may
experience. This was discussed by Karsten Opitz [1].
The work presented in this paper was based on a
transient CFD model of a PD reciprocating plunger
pump to investigate the cavitation dynamics in
incipient to full cavitating conditions and discusses
the rate of production/destruction of vapour in the
vicinity of the plunger, where the flow velocity is
small, and in the volume between the inlet valve and
its seat where the velocities are high and the
Bernoulli’s effect is important.
2. Material and Methods
The transient CFD model simulated the entire
pumping cycle; the induction stroke, from the Tod
Dead Centre position (TDC) to when the plunger
reached the Bottom Dead Centre (BDC) position
sweeping through the displacement volume, to the
delivery stroke when the plunger again reached the
TDC position as shown in
Figure 1. The overall pumping cycle was included
within the range -360° of the reciprocating crank
rotation where (plunger at TDC position) was the
initial time of the induction stroke and 360° (plunger
at TDC position again) was the end of the delivery
stroke. The 3D CAD model of the pump is shown in
Figure 2 and was cleaned up and prepared from the
CAD files used for manufacture for the Boolean
operations which extracted the fluid volumes from
the solid volumes The operation was performed with
both valves in the closed position and the plunger
located in the TDC position (initial simulation
configuration). The fluid volume was then
decomposed into the pattern shown in Figure 3 to
allow the layering moving mesh algorithm [9] to
correctly act during the simulation. Figure 3 shows
that the displacement volume was created by means
of creation of cell layers during the inlet stroke and
removal of cell layers during the outlet stroke in the
direction of the plunger axis. The layers created on
the top of the plunger surface increased the overall
fluid volume during the pumping cycle up to the
displacement volume amount.
Figure 1. PD pump geometry and nomenclature. The displacement volume is swept by the plunger moving from TDC to BDC.
1
3
2
4
5
6
Displacement Volume
Final Plunger position (BDC) 180°
crank rotation
3
7
8
1 Valve
2 Valve seat
3 Conic spring
4 Spring retainer
5 Inlet duct
6 Outlet Duct
7 Pump case
8 Plunger

A CFD Study on the mechanisms which cause cavitation in positive displacement reciprocating
pumps
Figure 2. Generation of the fluid volumes from the 3D CAD model of the pump.
Figure 3. Moving mesh: Decomposition pattern of fluid volumes, the arrows indicate the direction of creation of new mesh layers
when the plunger is moving backwards (induction) and the valve is lifting up
The layers generation rate was a fixed time law
which was automatically calculated by the solver by
providing it with the reciprocating motion parameters
(crank rotational speed and phase, connecting rod
length and crank diameter). The solver utilised the
In-Cylinder motion tool [9] to turn the set of
reciprocating motion parameters into the plunger
position (Figure 4) and speed and thus layer creation
at each time step. To make this possible a full
hexahedral mesh was chosen for the displacement
volume. Figure 3 also shows how the valve lift was
simulated. The fluid volume around the valve (inlet
and outlet) was decomposed into either translating
volumes or expanding volumes. During valve lift, the
valve-seat gap volume was expanded by means of
cell layer creation, the valve upper and lower
volumes were rigidly translate upwards following the
gap layering to keep the valve shape unchanged
during the lift. The two cylindrical volumes on the
top and on the bottom of the valve were compresed
and expanded respectively to keep the volume
continuity and to interface with the pump chamber
static volumes, and vice versa while the valve closed.
It is clear that during the valve motion, although the
mesh changes, there was no increase in the overall
fluid volume due to the motion of the valve. To make
the valve lift possible a full hexahedral mesh was
chosen for all the expanding and contracting volumes
Static mesh
Expanding mesh
Translating mesh
STATIC MESH
Mesh (time 1)
Mesh (time 2)
TRANSLATING MESH
Mesh (t1)
Mesh (t2)
EXPANDING MESH

A CFD Study on the mechanisms which cause cavitation in positive displacement reciprocating
pumps
as they were involved with the layering generation
just like the plunger top surface.
Figure 4. Boundary conditions, plunger displacement
Figure 5: Mass flow adjustable pressure drop for inlet and
outlet boundary conditions.
All expanding volumes, were either cylindrical or
annular shaped to simplify the meshing process and
to permit a full hexahedral mesh. The static volumes
and the translating volumes did not have any mesh
requirements and a tetrahedral mesh was chosen for
them.
Unlike the plunger, the valve layering generation was
self-actuated. The diagram of Figure 6 summarises
how the UDF managed to calculate the amount of
valve lift to apply without any analyst’s external
action. The function at every time step utilised the
pressure field output of the RANS solver to calculate
the overall pressure force on the valve surfaces which
was added to the spring force and then integrated to
assess the valve velocity and displacement which was
utilised by the moving mesh algorithm to update the
valve position for the following time step. The spring
force was provided to the UDF by means of spring
stiffness characteristic curve. The function utilised
the position of the valve at the previous time step to
calculate the spring force to be applied to the valve
force balance for the actual time step.
As mentioned in the introduction, the model was also
equipped with a water compressibility model which
was crucial to fulfil the mass continuity equation at
the times when the inlet and outlet valve were both
closed. The model made the assumption of one way
coupling between the pressure field and the density
field. This means that the pressure field affected the
density field but the density did not affect the
pressure. In this case the density field can be
calculated implicitly without linking the pressure and
density via the energy equation. The assumption is
reasonable when the working fluid is water.
The distinguishing feature and added sub-model
which improved the model presented in this
document from the one discussed in [10] is the
multiphase and cavitation algorithm. A three phase
model composed of water, water vapour and 15 ppm
of non-condensable ideal gas was utilised as the
working fluid. The water vapour fraction was
initialised as null in all of the volumes and the
Singhal et al. cavitation model managed the phase
change dynamics according to the pressure field as
explained in [11]. This cavitation model, also
referred to as the “full” cavitation model, utilises a
simple source term coming from the Rayleigh
equation [12] by omitting the second-order
derivative. It also accounts for the non-condensable
gas effects already mentioned. A mass flow
adjustable pressure was chosen as the boundary
condition for the inlet and outlet pipe. Figure 5 shows
that the solver automatically chose the static pressure
0
0.05
0.1
0.15
0.2
0.25
0 100 200 300
Plunger displacement [m]
Crank rotation [°]
SUCTION
STROKE
DELIVERY
STROKE
0.E+00
1.E+05
2.E+05
3.E+05
4.E+05
0 5 10 15 20 25 30
Delta P [Pa]
Mass flow rate [kg/s]
OUTLET LINE
INLET LINE

Citations
More filters

Journal ArticleDOI
Abstract: To fill the lack of literature in the numerical study of Positive Displacement (PD) pumps in cavitating condition, a comprehensive and transient Computational Fluid Dynamics (CFD) model of a PD pump, simulating the cavitation arising during the suction stroke, was created. The “full” cavitation model was utilised to study its capability on PD pumps cavitation. A set of three plunger speeds were simulated. Using the highest plunger speed an assessment was made of the effect of 1.5, 3, 4.5 and 15 ppm of air mass fraction on pump performance and cavitation. An experimental test rig, replicating the CFD model, was designed and built in order to validate the numerical model and find its weaknesses. CFD modelled, in a consistent way, the fluid dynamics phenomena related to cavitation (chamber pressure approaching the vapour pressure, the vaporization/condensation and the pressure spike occurrence at the end of the suction stroke marking the end of cavitation). On the other hand the CFD pressure trends calculated appeared stretched along the time axis with respect to the experimental data and this highlighted issues in the multiphase and cavitation models: the vaporization/condensation rate calculated by CFD did not follow the real dynamics correctly because the non-condensable gas expansion was overestimated. This was seen when comparing the CFD/experiments where the simulated pressure drop gradient, at the beginning of the suction stroke and the pressure peaks as the valve closed, exhibited a delay in their occurrence. The simulation results were sensitive to the dissolved air mass fraction as the delay depended on the amount of air dissolved in the water. Although the influence of the air mass fraction was considered consistent, the 3 ppm CFD case was the closest to the experiment results whereas the analyst expected the 15 ppm case to be more accurate.

22 citations


Journal ArticleDOI
TL;DR: The comparison between numerical results and the experimental performance curves has confirmed the accuracy of the model and the correct mesh selection in the small gaps and passages of the pump internal geometry and suggested the convenience of the development of a full-unsteady 3D model in the near future.
Abstract: This paper presents the unsteady numerical methodology for the CFD simulation of Air-Operated Diaphragm Pumps. The model reproduces the unsteady displacement of the diaphragm using dynamic mesh techniques and fully resolves the Fluid Structure Interaction (FSI) responsible for the motion of the check valves. The governing parameters have been modified with User Defined Functions (UDFs), using an implicit scheme for the grid motion that guarantees the stability and realizability of the two-dimensional model adopted. The analysis of the instantaneous delivered flow rate, as a function of the discharged outlet pressure, has provided interesting and useful information for the future design of new prototypes. The comparison between numerical results and the experimental performance curves has confirmed the accuracy of the model and the correct mesh selection in the small gaps and passages of the pump internal geometry. The leakage flows, especially in the exhausting valve during the forward stroke, and the ball tapping responsible for instabilities and high-frequency noise during oscillations of the valves has been accurately simulated. At high-delivered pressures, it has been observed a characteristic ripple in the instantaneous flow rate during the deceleration of the diaphragm towards its top-dead-center, associated to a partial re-opening of the exhausting valve. A closer look to the dynamics of the balls has revealed a strong coupling between inlet and outlet check valves. In addition, despite of the remarkable level of accuracy (less than 9% of deviation), the recirculating cells found in the flow fields inside the pump suggest the convenience of the development of a full-unsteady 3D model in the near future.

15 citations


Cites background from "A CFD study on the mechanisms which..."

  • ...The performance of plunger pumps as a function of the crank angle [14], the evaluation of its inlet stroke performance [15] and even cavitation inception [16,17] are some examples of the potentiality of computational modelling....

    [...]


Journal ArticleDOI
TL;DR: A full 3D unsteady numerical model with dynamic meshes is developed to simulate the fluid–structure interaction in the non-returning valves of air-operated diaphragm volumetric pumps, providing a more accurate description of the flow patterns and a superior evaluation regarding the dynamic response of the valves motion.
Abstract: A full 3D unsteady numerical model with dynamic meshes is developed to simulate the fluid–structure interaction in the non-returning valves of air-operated diaphragm volumetric pumps. This new three-dimensional CFD model provides a more accurate description of the flow patterns and a superior evaluation than a previous 2D model, published by the authors, regarding the dynamic response of the valves motion, which are responsible for internal volumetric losses that penalize the overall pump efficiency. Both piston-like and deformable geometries for the prescribed sinusoidal displacement of the membrane have been checked and compared in the modeling, resulting in similar behavior concerning the basic performance of the pump. Standard operation and free-delivery conditions are exhaustively analyzed, confirming more instabilities in the check valves in case of low air-supplied pressures. In particular, the exhausting valve is found to experience severe tapping with repetitive partial closures during the forward stroke due to an intense Fluid–Structure Interaction. On the contrary, the aspirating valve presents much better sealing characteristics with a partial reopening only at the initial moments of the backward stroke. All these numerical evidences have provided useful information for the pump manufacturers concerning the design, selection of materials and maintenance routines, which have been employed for the development of a series of new prototypes.

7 citations


Journal ArticleDOI
Abstract: An advanced transient CFD model of a positive displacement reciprocating pump was created to study its behavior and performance in cavitating conditions throughout the inlet stroke. The "full" cavitation model developed by Singhal et al. was utilized and a sensitivity analysis test on two amounts (1.5 and 15 parts per million) air mass fraction content was carried out to study the influence of the air content in water on the cavitation phenomenon. The model was equipped with user defined functions to introduce the liquid compressibility which stabilizes the simulation and to handle the two-way coupling between the pressure field and the inlet valve lift history. Estimation of the pump performance is also presented in both cases.

6 citations


Cites background from "A CFD study on the mechanisms which..."

  • ...As Iannetti explained in [9], the moving mesh algorithm managed the volume deformation and growth due to the valves lift and the displacement volume increment by means of a transient approach....

    [...]

  • ...The process was already explained by Iannetti [9] for a slightly different geometry but since the basis hypothesis did not change, the pattern is presented again for the attention of the reader in Figure 2....

    [...]

  • ...This was already observed by Iannetti [6] but the influence of the air content on it is still unclear....

    [...]

  • ...User Defined Function to drive the valve motion, how it interfaces to the main numerical solver [6] Initialization (t=0): • Chamber pressure = delivery pressure • Valve lift =0 • Valve spring force = spring preload...

    [...]

  • ...How does it affect the NPSH? The authors choose to carry out the investigation already mentioned by means of the advanced CFD model explained and discussed in [6] that will be briefly recalled in the next sections....

    [...]


Journal ArticleDOI
Abstract: Organic Rankine cycle (ORC) power plants are considered as one of the most promising technologies to generate power from low temperature heat sources such as biomass combustion, industrial waste heat, geothermal heat, and solar thermal energy. A feed pump is a key component of an ORC power plant to circulate the working fluid within the system. Owing to the low boiling temperature of most organic fluids, the feed pumps of ORC power plants are more vulnerable to suffer from cavitation. Cavitation of the organic fluid in the feed pump in an ORC system can degrade the evaporator performance and cause instabilities in the systems’ operation. Properly determining the required net positive suction head or subcooling for the pump is critical for the ORC system design and operation. Thus, this paper presents a systematic review of cavitation models with thermodynamic effect in simulations of cavitating flows. Methods for implementing thermodynamic effect were summarised. The features of the cavitation models were characterised and criticized, and their drawbacks were identified. A number of newly established cavitation models were explained and discussed in detail. Homogeneous mixture cavitation models have advantages such as less computational effort and easier implementation of thermodynamic effect in comparison with fully coupled multiscale models. However, when the thermodynamic effect is considered in the existing cavitation models, the cavitation regimes are not distinguished and applied properly. Nucleation cavitation models for organic fluids in ORC systems should be developed in terms of experimental nuclei profile and non-condensable gas concentration in future.

4 citations


References
More filters

Journal ArticleDOI

2,348 citations


"A CFD study on the mechanisms which..." refers methods in this paper

  • ...This cavitation model, also referred to as the “full” cavitation model, utilises a simple source term coming from the Rayleigh equation [12] by omitting the second-order derivative....

    [...]


Journal ArticleDOI
Abstract: Cavitating flows entail phase change and hence very large and steep density variations in the low pressure regions. These are also very sensitive to: (a) the formation and transport of vapor bubbles, (b) the turbulent fluctuations of pressure and velocity, and (c) the magnitude of noncondensible gases, which are dissolved or ingested in the operating liquid. The presented cavitation model accounts for all these first-order effects, and thus is named as the full cavitation model. The phase-change rate expressions are derived from a reduced form of Rayleigh-Plesset equation for bubble dynamics. These rates depend upon local flow conditions (pressure, velocities, turbulence) as well as fluid properties (saturation pressure, densities, and surface tension). The rate expressions employ two empirical constants, which have been calibrated with experimental data covering a very wide range of flow conditions, and do not require adjustments for different problems. The model has been implemented in an advanced, commercial, general-purpose CFD code, CFD-ACE+

1,187 citations


"A CFD study on the mechanisms which..." refers background or methods in this paper

  • ...[11] cavitation model to simulate the device from incipient to full cavitating conditions....

    [...]

  • ...cavitation model managed the phase change dynamics according to the pressure field as explained in [11]....

    [...]



DOI
01 Jan 2008
Abstract: Product Manager for Union Pump Company, in Battle Creek, Michigan. He has 39 years of experience in the design, application, and maintenance of reciprocating power and direct acting pumps. Prior to Mr. Tackett’s current position in Aftermarket Product Development, he served as R&D Engineer, Field Service Engineer, and new equipment order Engineer, in addition to several positions in Reciprocating Pump Sales and Marketing. He has been a member of ASME since 1991.

26 citations


"A CFD study on the mechanisms which..." refers background in this paper

  • ...Herbert Tackett [2] also explains that there are still many applications where PD pumps outperform centrifugal pumps which is the reason why, in the authors’ opinion, in the next few years a re-evaluation of this “old” device is to be expected....

    [...]

  • ...recalled by Herbert Tackett [2] who identifies the cause of the great popularity of centrifugal pumps due to the technological improvement made to the min the last decades....

    [...]

  • ...E-mail: aldo.iannetti@strath.ac.uk. recalled by Herbert Tackett [2] who identifies the cause of the great popularity of centrifugal pumps due to the technological improvement made to the min the last decades....

    [...]


Book
03 Nov 1987
TL;DR: Pump types Dynamics Net Positive Suction Head Pulsation and Surge Control Pump Design Liquid Ends Expendable Parts Valves Slurry Pumping Parts Wear and Life Applications Instrumentation Theory of Flow in Pipe Appendix Index.
Abstract: Pump Types Dynamics Net Positive Suction Head Pulsation and Surge Control Pump Design Liquid Ends Expendable Parts Valves Slurry Pumping Parts Wear and Life Applications Instrumentation Theory of Flow in Pipe Appendix Index.

24 citations


"A CFD study on the mechanisms which..." refers background or methods in this paper

  • ...As demonstrated by H. Ding [5] the amount of non-condensable gas dissolved in the water affects the prediction of the minimum NPSH (net positive suction head) required in the inlet manifold to keep the volumetric efficiency loss above the generally accepted 3% as recalled by John Miller [6]....

    [...]

  • ...6° and a volumetric efficiency loss within the limit of 3% discussed by John Miller [6]....

    [...]

  • ...Ding [5] the amount of non-condensable gas dissolved in the water affects the prediction of the minimum NPSH (net positive suction head) required in the inlet manifold to keep the volumetric efficiency loss above the generally accepted 3% as recalled by John Miller [6]....

    [...]

  • ...Table 3 quantifies the delay of 14.6° and a volumetric efficiency loss within the limit of 3% discussed by John Miller [6]....

    [...]