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 0°-360° of the reciprocating crank
rotation where 0° (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
Mesh (t1)=Mesh (t2)
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
