ArticlePDF Available

Experimental and numerical investigation of cavitation in marine Diesel injectors

Authors:
  • Accelleron Industries

Abstract and Figures

To further increase the efficienc y and decrease emissions of large two-stroke marine Diesel engines, the understanding of the fuel injection, spray breakup and the resulting combustion plays a vital role. Investigations have shown that the strongly asymmetrically and eccentrically arranged nozzle bores of the fuel injectors can lead to undesirable spray deflections that provoke increased component temperatures, emissions and fuel consumption. In order to investigate the origin of these spray deviations, transparent nozzles have been used to qualitatively visualize the in-nozzle flow under realistic geometrical and fuel pressure conditions. Three different, 0.75 mm diameter, single-hole nozzle geometries that represent typical geometrical characteristics have been used in cavitating nozzle flow experiments. The optical measurement technique Shadowgraphy has been applied to visualize the in-nozzle flow over the complete fuel injection process. The experiments have been performed with Diesel fuel at a rail pressure of 50 MPa with ambient back-pressure and temperature. Impingement measurements have been executed to compare the nozzle performance and validate CFD simulations using URANS with cavitation modeling in order to provide qualitative and quantitative support to the experimental results. The volume of fluid (VOF) method has been applied to simulate the multiphase flow with High Resolution Interface Capturing (HRIC). The cavitation model is based on a flash-boiling method with rapid heat transfer between the liquid and vapor phases. A Homogeneous Relaxation Model (HRM) has been utilized to describe the rate at which the instantaneous quality, the mass fraction of vapor in a two-phase mixture, will approach its equilibrium value. The numerical modeling of the cavitation inside the nozzle bore and the evaluated momentum flux have been compared to the experimental findings and show good agreement for the qualitative comparison of the cavitation patterns and differences of less than 6% for the quantitative momentum flux comparison.
Content may be subject to copyright.
International Journal of Heat and Mass Transfer 169 (2021) 1209 33
Contents lists available at ScienceDirect
International Journal of Heat and Mass Transfer
journal homepage: www.elsevier.com/locate/hmt
Experimental and numerical investigation of cavitation in marine
Diesel injectors
Reto Balz
a , b , , Imre G. Nagy
b , c
, German Weisser
b
, David Sedarsky
a
a
Chalmers University of Technology, Department of Mechanics and Maritime Sciences, Göteborg, Sweden
b
Winterthur Gas & Diesel Ltd., Winterthur, Switzerland
c
National Tech nic al University of Athens, School of Naval Architecture and Marine Engineering, Athens, Greece
a r t i c l e i n f o
Article history:
Received 14 May 2020
Revised 31 October 2020
Accepted 5 December 2020
Keywo rds:
Fuel injection
Cavitation
In-nozzle flow
CFD
Large marine diesel engine
a b s t r a c t
To further increase the efficienc y and decrease emissions of large two-stroke marine Diesel engines, the
understanding of the fuel injection, spray breakup and the resulting combustion plays a vital role. In-
vestigations have shown that the strongly asymmetrically and eccentrically arranged nozzle bores of the
fuel injectors can lead to undesirable spray deflections that provoke increased component temperatures,
emissions and fuel consumption. In order to investigate the origin of these spray deviations, transpar-
ent nozzles have been used to qualitatively visualize the in-nozzle flow under realistic geometrical and
fuel pressure conditions. Three different, 0.75 mm diameter, single-hole nozzle geometries that repre-
sent typical geometrical characteristics have been used in cavitating nozzle flow experiments. The optical
measurement technique Shadowgraphy has been applied to visualize the in-nozzle flow over the com-
plete fuel injection process. The experiments have been performed with Diesel fuel at a rail pressure of
50 MPa with ambient back-pressure and temperature. Impingement measurements have been executed
to compare the nozzle performance and validate CFD simulations using URANS with cavitation modeling
in order to provide qualitative and quantitative support to the experimental results. The volume of fluid
(VOF) method has been applied to simulate the multiphase flow with High Resolution Interface Captur-
ing (HRIC). The cavitation model is based on a flash-boiling method with rapid heat transfer between the
liquid and vapor phases. A Homogeneous Relaxation Model (HRM) has been utilized to describe the rate
at which the instantaneous quality, the mass fraction of vapor in a two-phase mixture, will approach its
equilibrium value.
The numerical modeling of the cavitation inside the nozzle bore and the evaluated momentum flux have
been compared to the experimental findings and show good agreement for the qualitative comparison of
the cavitation patterns and differences of less than 6% for the quantitative momentum flux comparison.
©2021 The Authors. Published by Elsevier Ltd.
This is an open access article under the CC BY-NC-ND license
( http://creativecommons.org/licenses/by-nc-nd/4.0/ )
1. Introduction
1.1. Background
Large two-stroke marine Diesel engines belong to the most effi-
cient internal combustion engines existing and can reach efficien-
cies over 55% [1] . To further decrease emissions and increase the
overall efficiency, the understanding of the fuel injection plays a
crucial role. Development strategies which can maintain highly ef-
ficient combustion while reducing pollutant formation require a
Corresponding author.
E-mail addresses: balz@chalmers.se , reto.balz@wingd.com (R. Balz).
more granular understanding of the mixture preparation, which is
the driving force of in-cylinder combustion.
Due to the large bore of two-stroke marine Diesel engines and
a strong swirl motion of the charged air, multiple fuel injectors are
used and arranged around the single exhaust valve. As a result, the
typical three fuel injectors arranged by 120 °have highly eccentri-
cally and asymmetrically arranged nozzle bores. A typical nozzle
tip that is mounted on the fuel injector is illustrated in Fig. 1 . Note
the five-hole nozzle design where all five nozzle bores face a sim-
ilar direction. This particular nozzle design and the large nozzle
bore diameters limit the usability of research focused on small-
and medium-sized Diesel engines.
Some of the specific issues that affect fuel injection in large ma-
rine Diesel engines have been examined by experiments conducted
https://doi.org/10.1016/j.ijheatmasstransfer.2021.120933
0017-9310/© 2021 The Authors. Published by Elsevier Ltd. This is an open access article under the CC BY-NC-ND license ( http://creativecommons.org/licenses/by-nc-nd/4.0/ )
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
Fig. 1. Illustration of a standard nozzle tip for large two-stroke marine Diesel en-
gine fuel injectors indicating the typically five-hole design of the nozzle bores. Note
that the main body diameter is 15 mm and the nozzle bores have diameters around
1 mm. The nozzle tips are exchangeable and directly mounted on the fuel injectors
(not depicted).
in the constant-volume Spray and Combustion Chamber (SCC) at
Winterthur Gas & Diesel Ltd. (WinGD) [2] . Investigations in the
SCC have shown that the asymmetric and eccentric nozzle layout
of large two-stroke marine Diesel engine fuel injectors has a sig-
nificant influence on spray formation [3,4] . Additionally, CFD sim-
ulations have shown that inhomogeneous fuel velocity profiles in
the nozzle bores induced by geometric cavitation lead to signifi-
cant spray deflections, especially for eccentrically arranged nozzle
bores [5,6] .
To further investigate the in-nozzle flow and how it affects the
spray morphology of large two-stroke marine Diesel engine injec-
tors, experiments have been performed using transparent nozzles
made of polymethyl methacrylate (PMMA). The feasibility of us-
ing PMMA as material to visualize in-nozzle flow has been proven
by countless work over the last years [7–13] . Although different
non-invasive measurement techniques have been proven success-
ful to investigate the in-nozzle flow under real fuel injection con-
ditions, the use of transparent nozzle tips still allows the high-
est spatial and temporal resolutions, especially compared to x-ray
imaging. The flow inside multi-hole marine injectors has previ-
ously been studied optically only using transparent models with
water at a few atmospheres pressure as working fluid [ 7,14 ]. Ya ng
et al. [15] provide an up-to-date and detailed review of the experi-
mental non-intrusive investigations of fuel injector phase changing
flow. In this study, full-scale nozzle diameters and realistic injec-
tion pressures with real Diesel fuel are utilized in order to match
set points for WinGD marine Diesel engines. The design of opti-
cally transmissive injector inserts provides the possibility of pro-
duction nozzle geometry duplication while realistic injection pres-
sures can be applied. This allows the acquisition of optical mea-
surements which provide insights for model development and can
be used for the validation of cavitation modeling results based on
CFD for large marine Diesel engine atomizers.
1.2 . In-nozzle cavitation
Cavitation is the process of formation and consequent collapse
of gaseous bubbles in a liquid under a local decrease in static pres-
sure. Depending on the topology of the vapor structures in the
flow, cavitation occurs in the form of traveling bubbles or vapor
pockets, extending over a partial length of the nozzle bore (cloud
cavitation and sheet cavitation), or supercavitation, when the vapor
region extends over the whole length of the nozzle bore [16,17] .
Hydrodynamic cavitation in fuel injectors develops at high in-
jection rates when the pressure drops below the critical level in-
side the nozzle bore, leading the fuel to evaporate into vapor. Cav-
itation is reported to improve the spray breakup processes [18–
22] . However, undesirable effects on the fuel injection performance
may occur, such as flow instabilities, excessive noise generation,
and erosion, which can cause damage to the injector and nozzles
[23] .
To characterize the flow inside the nozzle, the dimensionless
discharge coefficient providing the ratio between actual and theo-
retical discharge through the nozzle bore is used:
C
D
=
˙
m
actual
˙
m
ideal
(1)
where ˙
m
ideal
is the theoretical mass flow based on Bernoulli’s
equation and ˙
m
actual
the actual, entropy bounded, mass flow
through the atomizer.
2. Experimental methods
2.1. Optically transparent nozzle holder
A transparent nozzle holder (TNH) to be mounted on fuel injec-
tors of large marine Diesel engines has originally been developed
at Chalmers University of Technology [24] and proved to cope with
fuel pressures in the ranges of large two-stroke marine Diesel en-
gines (50 to 80 MPa rail pressure) for a limited number of injec-
tions (usually around 20 to 60 injections before failure). The de-
sign uses transparent nozzles made from PMMA. The thermoplas-
tic has a similar optical refractive index to Diesel (1.49 and 1.4 6
to 1.52 depending on the Diesel mixture, respectively) that allows
visualization of the in-nozzle flow without optical distortions due
to the round shape of the nozzle bore that otherwise would act
as a cylindrical lens. The transparent nozzle is mounted onto the
TNH with rigid metallic clamps that apply an external force onto
the nozzle to suppress the expansion of the PMMA. This clamping
reduces the internal stresses in the PMMA and decreases the fail-
ure probability significantly (see [11] for further information). For
the optically interesting axis, polished sapphire bricks have been
used between the metal clamps and the PMMA nozzle to guaran-
tee maximal optical access while still applying a clamping force on
the plastic.
Fig. 2 illustrates the used TNH. The entire setup can be mounted
on a typical WinGD injector by using the injector mount (e). The
main bore leads the fuel to the PMMA nozzle (k) and the pres-
sure sensor (a). The metallic top-clamps (c) apply force directly
to the PMMA nozzle, while the side-clamps (g) provide stability
via two polished sapphire bricks (h) to maintain optical access.
The PMMA nozzle is also fixed by using two fitting bolts (f) that
connect the sensor-body (b) and the main-body (d) together. The
depicted transparent nozzle (k) is a single-hole, perpendicular de-
sign with a nozzle bore diameter of 0.75 mm. The sensor-body (b)
presented in Fig. 2 holds a pressure transducer that allows mea-
suring the fuel pressure in the main bore of the TNH. The used
piezo-resistive pressure sensor from Kistler (type 4067C20 0 0) has
a natural frequency of over 200 kHz that allows dynamic acqui-
sition of the fuel pressure in the main bore of the nozzles. The
pressure sensor allows accurate data acquisition that is necessary
to investigate cavitation behavior during the quasi-steady-state in-
jection conditions. It is important that the pressure at the main
bore is known during the whole injection process to better under-
stand cavitation fluctuations in the nozzle bore. The measured data
has crucial importance as a boundary condition in CFD simulations
since fuel injectors usually have significant pressure losses.
2.2. Nozzle geometries
Three different single-hole cylindrical nozzle designs have been
chosen based on the realistic five-hole atomizer designs of large
2
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
Fig. 2. Sectional view (i) and top view (ii) illustration of the new transparent noz-
zle holder with pressure sensor (a), sensor-body (b), top-clamps (c), main-body (d),
injector mount (e), fitting bolt (f) side-clamp (g), sapphire brick (h) and transparent
nozzle (k).
two-stroke marine Diesel engine injectors. This simplification has
been chosen to reduce the computational cost for CFD simulations
and to reduce the experimental effort. The application of ve-hole
nozzle bores would complicate the optical access since they are
overlapping in the interesting optical axis and, as a result, would
limit the information about the in-nozzle flow of the nozzle bores
(compare with the original five-hole nozzle tip in Fig. 1 ). Fig. 3
shows geometry projections of the three different nozzle types
adapted for the TNH: isometric, side, and top views. The fuel flow
enters the nozzle main bore from the top, and the pressure sen-
sor is mounted at the bottom side in the isometric projection (see
Fig. 2 for reference). The nozzle N101 represents the most straight-
forward arrangement of the three designs, where the nozzle bore
is located centrally with reference to the main bore and perpen-
dicular to the main bore axis. The nozzle N105 also has a centrally
arranged nozzle bore but with an angle of 75 °. The nozzle N104
has a perpendicular angle as well, but the nozzle bore is 0.8 mm
eccentrically arranged. The nozzle bore and main bore diameters
are identical for all three nozzles and are 0.75 mm and 3.5 mm,
respectively.
2.3. Optical imaging
The TNH is designed to visualize the in-nozzle flow using
a line-of-sight optical measurement technique like Shadowgraph
imaging, where a light source illuminates one side of the trans-
parent nozzle and an imaging system is installed on the other
side. A schematic of the optical setup used is depicted in Fig. 4
where a simplified drawing of the fuel injector (j) together with
the mounted TNH (d) is depicted as well, indicating the propor-
tions. The dashed line indicates the optical axis. The setup used
consisted of a Cavitar Cavilux Smart diode laser (i) emitting at
a center wavelength of 640 nm together with a Questar QM100
far-field microscope (b) and a Photron Fastcam SA5 CMOS high-
speed camera (a). A diffuser plate (e) has been installed in front
of the TNH to guarantee a uniform background illumination. An
Fig. 3. Isometric, side, and top projection of the three different transparent noz-
zle types used. N101: centrically arranged 90 °setup, N105: centrically arranged
75 °setup, and N104: eccentrically arranged 90 °setup. The main bore diameter is
3.5 mm and the nozzle bore diameter is 0.75 mm.
Fig. 4. Schematic of the optical setup used with high-speed camera (a), far-field
microscope (b), mirror (c), transparent nozzle holder (TNH) (d), diffuser plate (e),
focusing lens (f), collimator (g), optical light guide (h), diode laser (i) and injector
(j). The dashed line represents the optical axis. Note that the spray chamber sur-
rounding the TNH is not illustrated.
additional 150 mm plano-convex spherical lens (f) has been used
together with an optical light guide (h) and its matching collima-
tor (g) to focus and concentrate the diode laser emission onto the
diffuser plate in front of the TNH (d). A mirror (c) has been used
to protect the far-field microscope from possible debris in case of
material failure. The field of view of approximately 5 x 5 mm has
been acquired with a resolution of 512 x 512 pixels and a framer-
ate of 20 kHz.
3
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
The use of a pulsed light source with short pulse lengths is nec-
essary to acquire sharp in-nozzle flow images under realistic fuel
pressure conditions. This is due to motion blur that would occur
with a constant light source because of the relatively long expo-
sure times in the range of μs compared to the fuel velocities of a
couple 100 m/s in the nozzle bore.
2.4. Impingement measurements
To quantitatively characterize the different single-hole nozzle
geometries, the spray momentum flux has been measured using
a calibrated piezoelectric force sensor (type 9215a) together with
a charge amplifier (type 5064) from Kistler. The so-called impinge-
ment measurements are further described in [25,26] and use con-
servation of momentum based on the assumption that the spray
impingement area is much smaller than that of the sensor used in
the measurements. Hence, the momentum flux of the spray at the
nozzle bore exit is identical to the force measured on the sensor.
To align the force sensor exactly on the nozzle bore symme-
try axis, three different sensor holders have been manufactured ac-
cording to the different nozzle geometries. The force sensor hold-
ers have been mounted directly on the two top clamps of the TNH
(see Fig. 2 for further details) to minimize the distance between
the nozzle bore exit and the force sensor.
The momentum flux ˙
M
f
can be calculated using Eq. 2 :
˙
M
f
=
A
0
v
2
·ρ·dA (2)
where A
0
is the geometrical area of the nozzle bore exit, and ρand
v the density and velocity of the fluid in liquid or gaseous phase
exiting the nozzle bore.
2.5. Test facility
The experiments have been conducted in the constant-volume
Spray and Combustion Chamber (SCC) at WinGD, where the geom-
etry represents the combustion volume with the piston at top dead
center of an RT-flex50 engine from WinGD’s portfolio. The SCC is
able to operate under realistic engine loads regarding charge pres-
sures, swirl motion, and temperatures. The chamber diameter is
identical to the cylinder bore and measures approximately 500 mm
(more details about the test rig can be found in [2–4,6,27,28] ). The
fuel is pressurized using a standard common-rail system equipped
with an injection control unit (ICU) as used on each cylinder of
the RT-flex engines. The rail pressure has been set to 50 MPa,
which represents a standard value at part load engine operation.
Since only the in-nozzle flow has been investigated for this work,
the back-pressure and gas temperature in the spray chamber have
been set to ambient conditions. Experiments have shown that the
back-pressure and fuel temperature play a less significant role for
the in-nozzle flow cavitation patterns when the pressure differ-
ences are large and the fuel temperatures less than 80 °C [29–31] .
The fuel used is a standard Diesel from Preem AB with the product
code DMK1UA-SE, a density of 815.9 kg/m
3
(at 15
°C), a viscosity of
2.112 mm
2
/s (at 40 °C) and a net heat of combustion of 43.16 MJ/kg.
3. Numerical modeling
3.1. In-nozzle flow CFD simulations
Modeling turbulent cavitating flows is a challenging task be-
cause of the complexity of the phenomenon itself and the highly
dynamic interaction between phases and non-equilibrium ther-
modynamic states. Recent numerical simulations have proven the
applicability of CFD in cavitating flow predictions, thus support-
ing experimental measurements and product development [32–
35] . Most of the published numerical work is limited to small- and
medium-sized engine fuel injectors and due to large geometrical
differences, only insufficiently useful for the validation and opti-
mization of cavitation formation in large marine Diesel engine fuel
injectors.
Several different models have been developed for cavitation
in nozzles. Giussani et al. [36] provide an extensive overview of
numerical modeling approaches of cavitating flows in fuel injec-
tor nozzles. The available methodologies for simulating multiphase
flows can be classified either according to the adaptation of the
multiphase fluid modeling or according to the mass transfer mech-
anism assumed for cavitation. Concerning multiphase modeling in
Diesel fuel nozzles involving cavitation, the most common imple-
mentations are the homogeneous mixture models, the heteroge-
neous multi-fluid models, and the Lagrangian models.
The homogeneous Eulerian flow model has been utilized in
[37,38] with a separate transport equation for the vapor volume
fraction describing the evolution of the cavitation region. It is as-
sumed that all the phases share the same velocity and pressure;;;
the fluid is a continuous mixture of liquid and vapor. Most models
rely on the assumption of thermodynamic equilibrium. The occur-
rence of cavitation is determined based on a cavitation criterion, in
the simplest case, just by means of the local pressure in compar-
ison with the vapor pressure. Dabiri et al. [39] tested this simple
criterion and found that the viscous stress contributes to the size
of cavitating regions significantly and thus leads to earlier cavita-
tion inception [40] .
Multi-fluid Eulerian models [41,42] allow a more detailed de-
scription of the flow compared to the homogeneous model. This
method is characterized by different sets of conservation equations,
one for each phase; thus each phase has its own velocity, temper-
ature, and pressure [43] . However, the two-fluid model is based on
time and space averaged equations and cannot track the interface
explicitly.
When the cavitation level is low and the resulting bubbles are
smaller than the cells in the computational grid, it is possible to
use the Euler-Lagrangian approach. In this approach, each bubble
as product of cavitation is tracked in a Lagrangian frame. Here,
only the liquid is a continuum, while the vapor is the dispersed
phase and is represented by parcels of bubbles. Vapor bubble tra-
jectories are tracked, integrating the Newton equation of motion
for each parcel. Examples of this method applied to nozzle flows
are reported by Giannadakis et al. [44,45] .
The widely-applied sharp interface capturing method Volume
of Fluid (VOF) technique [36,43,46,47] has been chosen to cap-
ture the liquid/gas interface. The model is similar to the homo-
geneous model, where a single momentum equation is calculated
for all phases that interact using the VOF model. The method is
suitable to capture small to large scale deformations and interface
zones as it is an Eulerian-Eulerian method, and therefore, the liq-
uid and vapor are treated in separate phases. The cavity shape is
constantly tracked and updated until the local pressure inside the
cavity reaches the vapor pressure, therefore giving precise and con-
vergent modeling of the cavity-surrounding liquid interface. The
VOF method is able to successfully predict the separation point,
recirculation zone, and reattachment points. Furthermore, the pres-
sure distribution inside the compressible flow is also correctly cap-
tured. The solved transport equation of the vapor fraction predicts
the convection of bubble nuclei or micro-bubbles within the liquid
caused by cavitation. The basic drawback of this approach is the
high numerical grid resolution required to sufficiently resolve the
length and time scales. In this particular study, the VOF method
has been chosen to track the interface of different phases. High
Resolution Interface Capturing (HRIC) [4 8,4 9] has been applied in
the VOF method to avoid artificial effects and to minimize numer-
ical diffusion and compressive character. VOF and HRIC governing
equations can be found in [49,50] .
4
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
3.2. Cavitation model
The numerical representation of cavitation and flash boiling has
been an important area of research due to the difficulties of rep-
resenting their physics by robust and accurate numerical method-
ologies. Schmidt et al. [37] and Giannadakis [44] provide an exten-
sive discussion on various models available. A widely-used Eulerian
approach to simulate cavitation is based on the Rayleigh-Plesset
equation, which describes the growth and collapse of a bubble in
a liquid, assuming no slip between the two phases. This model
is highly dependent on the initial bubble radius and number pa-
rameters, which can be defined by using prior experimental data
data. In [51] , Neroorkar et al. simulated cavitation phenomenon
based on the Homogeneous Relaxation Model (HRM), thus provid-
ing an alternative to the Rayleigh-Plesset equation. In his study,
it has been found that despite the differences between cavitation
(driven by pressure) and flash boiling (driven by temperature as
well), these models are sufficiently similar to suggest that the HRM
can also model cavitation [52,53] . The results have been validated
against geometries experimentally evaluated in [51] and demon-
strated that the model could could correctly reproduce the cavita-
tion in a nozzle. Battistoni et al. [54] , in their study, compared a
mixture model in conjunction with the HRM phase change model
with a multi-fluid model utilizing the Rayleigh bubble dynamics
for phase change, and validated against experimental data. It has
been concluded that from an engineering point of view, the two
models showed good predictive capabilities.
The cavitation model implemented in the commercial soft-
ware Converge has been used for this study. The model is
based on the flash-boiling hypothesis of Shields et al. from 2011
[37,38,55,56] with rapid heat transfer between vapor and liquid
phase. The method represents a similar procedure to cavitation,
where the vapor formation happens through a pressure drop on a
constant temperature level, except that the pressure drop is lower
and there is a temperature elevation in the system. The mass ex-
change between phases is predicted by an HRM, which describes
the process of vapor mass fraction approaching its equilibrium
state. This mass fraction rate is calculated by the formula:
D
x
D
t
=
x x
(3)
where x represents the equilibrium mass of vapor phase, x is the
instantaneous mass, and is the time scale over which x relaxes
to x . For evaporation, E is expressed in Eq. 4 , furthermore the
condensation time scale is described by equation Eq. 5 :
E
= 0
·α0 . 54
·ϕ
1 . 76 (4)
C
= F ·0
·α0 . 54
·ϕ
1 . 76 (5)
where F is the condensation time scale factor with a typical value
of 5E3, meaning that the condensation is 5E3 times faster than
the evaporation under similar conditions. The 0 coefficient is set
to 3.84E-7 s based on validated work from [52,57,58] . The non-
dimensional pressure ratio ϕ, is given by the formula:
ϕ =
p
sat
p
p
c
p
sat
(6)
where p
c means the critical pressure. Further information of the
cavitation model can be found in [50] .
In the flow field, O
2
and N
2
representing the air inside the noz-
zle and the gas state of n-Dodecane as fuel surrogate have been
initialized. The equation of state has been handled by the Redlich-
Kwong cubic equation (shown in Eq. 7 ), while the real gas proper-
ties are calculated as a function of temperature.
p =
RT
v b
a
v
2
+ ubv + wb
2
(7)
Fig. 5. Schematic Figure of CFD domain with applied boundary conditions pre-
sented for nozzle type N101.
Further information of the coefficients can be found in
[50] .
Based on its very similar physical properties compared to the
measured Diesel fuel, n-Dodecane has been utilized as Diesel sur-
rogate.
3.3. Turbulence modeling
RANS and URANS simulations have been popular within the in-
dustry due to time and cost constraints, predicting flows accept-
ably on a macroscopic level. LES, DES, and hybrid RANS/LES ap-
proaches, among other turbulence models, still have high compu-
tational demand but resolve transient large-scale turbulent struc-
tures and provide more detail of the flow [59,60] . Koukouvinis
et al. [61] , in their extensive work, tested several turbulence mod-
els with different cavitation models at many pressure drops and
compared those results to experimental data. They found that
RANS produced less accurate results at low-pressure drops. Edel-
bauer et al. [62] compared RANS and LES of cavitating flows and
concluded that RANS could predict cavitation with reasonably ac-
ceptable accuracy in an operating condition with high-pressure dif-
ference. In the present high-pressure injection study, the Renor-
malization Group (RNG) k turbulence model has been applied.
The model coefficients have been taken from the literature and fol-
low the instructions for cavitating flows in Diesel injectors sug-
gested by Convergent Science. Further information on the turbu-
lence kinetic energy and turbulence dissipation equations can be
found in [50] .
3.4. Numerical setup
The CFD domain with the applied boundary conditions can be
seen in Fig. 5 . The nozzle is modeled as wall boundary. Static pres-
sure derived from the measurements is applied at a fuel tempera-
ture of 323 K at the nozzle inlet. The mass fraction of the entering
fuel is 99.9% of n-Dodecane and 0.1% of air. The turbulent intensity
and length scale are approximated and set to 0.02, and 0.0 0 01 m,
respectively. The nozzle walls are treated as no-slip walls assum-
ing smooth wall conditions. The plenum, which is a constant vol-
ume filled with air, has atmospheric conditions. Here, the out-
flow boundary condition is applied. The turbulent kinetic energy
is specified at a value of 0.02 and the length scale is set to have a
value of 0.0 0 03 m. Together with the wall boundary conditions, the
law of the wall for high-Reynolds number applications is applied.
In the absence of prism layers, the viscous sub-layer of the bound-
5
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
Fig. 6. Grid structure applied in the simulation in case of the nozzle type N101
with a detailed view around the nozzle bore (top).
ary layer cannot be sufficiently resolved; therefore the application
of the wall function is obligatory. The law of the wall approach is
a logarithmic curve fit of the turbulent boundary layer; thus the
tangential componen ts of the stress tensor can be calculated. The
simulation is set to reach a quasi-steady solution at 0.01 s.
3.5. Grid generation
Three different grids have been created for the standard noz-
zle N101 in order to investigate the grid resolution influence on
the computational results. Based on the nozzle bore diameter of
0.75 mm, 40, 35, and 30 cells have been placed in the nozzle
bore, respectively. With the aforementioned nozzle bore resolution,
a base grid size has been calculated for the entire geometry of the
nozzle.
The nozzle bore region has been computed by the so-called
fixed embedding, utilizing a scaling factor of 4 compared to the
chosen base cell size, where a stationary zone has been defined in-
cluding the nozzle bore length, the vicinity of the nozzle bore inlet
and the near nozzle bore region inside the plenum (see Fig. 6 ). The
plenum region has been computed by Adaptive Mesh Refinement
(AMR), where the automated grid refinement cuts the cells by a
scaling factor of four, based on velocity and void fraction sub-grid
criteria. The wall boundaries have been computed by a permanent
grid resolution by keeping the non-dimensional wall distance value
y
+ at 30, which is appropriate in case of high-Reynolds number
turbulent flow applications.
3.6. Solver settings
The transient solver with the full hydrodynamic simulation
mode has been chosen for this application. Both the gas and liq-
uid flow solvers are fully compressible. The Pressure-Implicit with
Splitting of Operators (PISO) algorithm with a tolerance of 0.001
has been used for the pressure-velocity field coupling, while the
momentum, pressure, density, and energy equations have been
taken care of the linear solver method, thus allowing a faster con-
vergence. The time step has been set to be varied between 1E-
10 and 1E-06 s, while the maximum CFL (Courant-Friedrichs-Lewy
condition) number and diffusive CFL number have been chosen to
be lower than 0.25 and 0.5, respectively.
Fig. 7. Avera ged fuel pressure and injector solenoid current for injection duration
of 12 ms. The time origin is triggered start of injection (tSOI).
Fig. 8. Average d momentum flux ˙
M
f of the three different nozzles used over the
injection duration. The time origin is triggered start of injection (tSOI).
4. Results and discussion
4.1. Experimental results
The fuel pressure measured in the main bore of the nozzle
mounted in the TNH and the corresponding normalized current
signal of the injector solenoid are depicted in Fig. 7 . The signals
shown are averaged over 20 injections. The time axis origin is the
triggered start of injection (tSOI). The shift between current and
pressure signal indicates the hydraulic delay due to the needle
movement in the fuel injector. The quasi-steady-state injection pe-
riod has been defined between 5 and 13 ms after tSOI and has
been used to average the pressure, the momentum flux, and the
in-nozzle flow images for comparison with the CFD results. The
depicted pressure curve in Fig. 7 represents the data of the nozzle
type N101. As there is no significant difference in the pressure sig-
nals of the three nozzle types, the pressure curves of the nozzles
N104 and N105 are not depicted for visibility reasons.
The momentum flux data acquired for the three different noz-
zles used is depicted in Fig. 8 . Note the similar curve characteris-
tics compared with the pressure curve shown in Fig. 7 . The pres-
sure and momentum flux results have been averaged over the
quasi-steady-state period of the fuel injection process between 5
and 13 ms after tSOI. The averaged values and the correspond-
ing standard deviations of the pressure measurements are depicted
together with the momentum flux results from the impingement
measurements in Table 1 . The averaged pressure data has been
used for the CFD boundary conditions.
Although the quasi-steady-state period of the pressure and mo-
mentum flux curves show fluctuations, the signal is very stable, as
indicated by the small standard deviations as sown in Table 1 - tt
hose fluctuations originate from the hydraulic high-pressure sys-
tem providing the injector with fuel and are fully reproducible.
6
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 16 9 (2021) 120933
Tabl e 1
Experimentally measured and averaged fuel pres-
sure and momentum flux ˙
M
f together with the
standard deviation for the three different nozzle
types (N101, N104 and N105) investigated.
measurements
avg. pressure N101 [MPa] 38.51 ±1.08
avg. pressure N104 [MPa] 38.98 ±1.04
avg. pressure N105 [MPa] 38.32 ±1.00
avg. ˙
M
f N101 [N] 21.46 ±0.09
avg. ˙
M
f N104 [N] 19.97 ±0.07
avg. ˙
M
f N105 [N] 20.93 ±0.11
Fig. 9. In-nozzle images of nozzle N101. Note that dark areas within the nozzle bore
indicate gaseous flow, i.e., cavitation. Nozzle bore filled with Diesel, but no cavita-
tion flow (i), first sign of cavitation (ii), and following image frames with 50
μs
time interval (iii - vi), and during quasi-steady-state fuel injection at around 8 ms
after tSOI (vii).
The acquired images of the in-nozzle flow have only been in-
tensity adjusted, rotated and cut, to remain the maximal image in-
formation. A series of selected in-nozzle flow images are shown in
Fig. 9 where i) shows the with Diesel fuel filled nozzle bore be-
fore the needle opening, ii) - vi) during needle opening, and vii)
during the quasi-steady-state fuel injection at around 8 ms after
tSOI. The field of view used covers the entire nozzle bore (verti-
cal) of the transparent nozzles and a small area of the nozzle main
bore (horizontal, top of image). Since the refractive index of the
PMMA material and the Diesel fuel used are not perfectly identi-
cal, the main bore and nozzle bore walls are visible at all times
in the images acquired. Therefore, the image before needle open-
ing, as depicted in Fig. 9 i), serves as a reference background. In
the other images shown in Fig. 9 , the additional dark areas repre-
sent gaseous flow, i.e., cavitation. The light is refracted away from
the optical axis due to the phase and consequent refractive index
change and therefore does not arrive on the camera sensor. The
bright areas within the walls of the nozzle bore indicate the liq-
uid fuel flow as the light passes the transparent nozzle with only
slight distortions and arrives on the camera sensor. For comparison
with the CFD results, only the images during the quasi-steady-state
injection period as depicted in Fig. 9 vii) have been used and aver-
aged. However, the images acquired during needle opening ( Fig. 9
ii) - vi)) are quite interesting as well. Image ii) represents the in-
nozzle flow at around 2.1 ms after tSOI (compare with the pres-
sure curve in Fig. 7 ) and shows the first cavitation in the acquired
measurement series. The pressure is still quite low compared to
the maximal pressure achieved roughly 1 ms later. The following
images iii) to vi) are the consecutive frames with 50 μs interval
given by the 20 kHz frame rate of the high-speed camera. The cav-
itation development within these five sequential images is interest-
ing since the cavitation pattern develops to supercavitation in im-
age vi) and then forms back to film and cloud cavitation as shown
in images iii) and vi) [16,63] . This reduction in cavitation intensity
can be traced back to the small pressure fluctuation at the begin-
Fig. 10. Density distribution [kg/m
3
] shown in a vertical section cut in the middle
of the nozzle bore (side view) for the nozzle type N101 (i), while streamlines col-
ored by velocity magnitude [m/s] give the flow path inside the nozzle (ii) taken at
the end of the simulation.
ning of the pressure curve, as depicted in Fig. 7 . Another interest-
ing fact is the very similar supercavitating pattern in image v) and
vii) although the pressure difference with approximately 40 MPa is
extensive (compare with pressure curve in Fig. 7 , image v) acquired
at around 2.25 ms and image vii) at around 8 ms after tSOI).
4.2. CFD in-nozzle flow investigation
A grid sensitivity analysis investigating three different numer-
ical grids has been executed by utilizing the standard nozzle
N101. After reaching a converged quasi-steady solution, the spray
Reynolds number of each mesh type, based on the velocity mag-
nitude values stored in a section 0.05 mm before the nozzle bore,
has been defined. Here, the flow field has been sampled along a
straight line in the nozzle bore cross-section in 50 points. Then,
the grid types have been compared by means of averaged pressure,
density, and velocity fields, as well as by taking the cell gas frac-
tions at the nozzle bore exit. It can be stated that only minor devi-
ations among the test grids could be found. The finest grid predicts
the highest maximum velocity magnitude at the nozzle bore exit,
while the coarsest grid shows a loss in velocity magnitude by ap-
proximately 20 m/s. The average velocity magnitude analyzed at
the same cross-section of the nozzle bore results in very similar
behaviour. Furthermore, the test meshes have been compared by
means of time-averaged Mach number and cell densities stored in
the sampling points. The coarser grid resulted in very similar val-
ues in any investigated physical flow properties to the finest grid
and still having remarkably less computational time. As a result,
the grid spacing of the coarser grid has been utilized for all three
nozzle layouts for further numerical investigations.
Each of the three nozzles has been analyzed individually. A ver-
tical cross-section cutting the nozzle bore exactly in the middle
and visualizing the density distribution inside the nozzle is de-
picted in Fig. 10 i). Note that only the side view of the nozzle ge-
ometry is visualized for visibility reasons. The density distribution
shows not just a separation of flow at the sharp nozzle bore in-
let but also a flow detachment close to the nozzle bore exit can
be seen, which has a pronounced effect on the spray formation.
Regarding the pressure field (not presented here), one can state
that the pressure reduces while entering the nozzle bore, where
the fuel velocity increases according to Bernoulli’s law. The local
pressure at the nozzle bore inlet drops below the vapor pressure of
the fuel at the given temperature level, and additionally, the sud-
den geometrical change invokes immediate cavitation inception.
Streamlines colored by velocity magnitude (see Fig. 10 ii)) show
the path of the fuel inside the nozzle, with a vena contracta rep-
resented by the compressed streamlines after the fuel enters the
7
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 16 9 (2021) 120933
Fig. 11. Density distribution [kg/m
3
] shown in a vertical section cut in the middle
of the nozzle bore (top view) for the nozzle type N104 (i), while streamlines colored
by velocity magnitude [m/s] give the flow path inside the nozzle (ii) taken at the
end of the simulation.
nozzle bore from the main bore. A more pronounced separation
can be seen on the upper side of the nozzle bore, which is ex-
pected since the fuel enters directly from the nozzle main bore in-
let direction and therefore suffering a significant redirection caused
by the geometrical properties of the nozzle.
The cavitating flow simulation results from the eccentric noz-
zle N104 are depicted in Fig. 11 . Note that only the top view of
the nozzle geometry is shown for visibility reasons. The flow field
is described in terms of density distribution (i) and velocity field
(ii) inside the nozzle. The flow enters the nozzle bore through a
significant distortion caused by the sharp inlet formed by the ec-
centrical arrangement. Flow separation inside the nozzle bore on
the nozzle main bore symmetry side occurs, and as a result, a
large recirculation zone is created, which is filled by fuel vapor.
The region extends until the nozzle bore exit, forming a massive
vapor tube inside the nozzle bore and therefore significantly re-
ducing the effective area of the nozzle bore. The eccentric side of
the nozzle bore seems to be undisturbed by the geometry and as
a result, the presence of a remarkably high-velocity zone can be
found. The highly non-uniform velocity magnitude distribution is
an obvious outcome of the nozzle bore eccentricity and the ge-
ometrically induced cavitation. The cavitation zone at the nozzle
bore inlet detaches after approximately a distance of one nozzle
bore diameter and separates from the nozzle bore wall into the
internal region of the nozzle bore. The extended and coherent va-
por zone reaches the nozzle bore exit while vapor bubbles travel
through the flow. This sort of vapor formation is a typical char-
acteristic of string cavitation and supercavitating nozzles [18,64] .
Vapor formation can also be seen at the nozzle bore exit, which
significantly influences the spray formation and causes spray core
deformation.
The CFD results of the angled nozzle N105 are depicted in
Fig. 12 . Note that only the side view of the nozzle geometry is
presented for visibility reasons. The density distribution ( Fig. 12 i)
shows an extended separation zone on the bottom side of the noz-
zle bore initiated by the sudden geometrical change at the nozzle
bore inlet. This zone evolves into the fluid domain, compressing
the velocity streamlines ( Fig. 12 ii) to the upper side of the nozzle
bore, creating an area with high velocities. The upper edge of the
Fig. 12. Density distribution [kg/m
3
] shown in a vertical section cut in the middle
of the nozzle bore (side view) for the nozzle type N105 (i), while streamlines col-
ored by velocity magnitude [m/s] give the flow path inside the nozzle (ii) taken at
the end of the simulation.
Tabl e 2
Summary of the flow properties of the three nozzle types based on the
CFD simulation results.
nozzle types
N101 N104 N105
avg.
v
mag
at orifice [m/s] 296 278 285
avg. Re at orifice [-] 69.9k 65.6k 67.2k
velocity uniformity index U
i [%] 94 89 96
avg. cell gas fraction at orifice [%] 31 30 23
discharge coefficient C
D [-] 0.65 0.62 0.69
momentum flux ˙
M
f [N] 21.06 18.81 21.71
nozzle bore inlet shows a comparably very small depression zone,
which can be identified as cavitation inception at the nozzle bore
inlet; however it does not seem to have a significant effect on the
flow field.
A summary of the nozzle and flow field properties of the CFD
simulation results can be found in Table 2 .
Taking the average velocity magnitude evaluated by the CFD
simulations at the nozzle bore exit (orifice), the standard noz-
zle N101 has the highest velocity and the eccentric nozzle N104
the lowest. Based on these velocities, the corresponding Reynolds
numbers ( Re ) have been defined for all three nozzle geometries,
proving the presence of highly turbulent flow. The velocity mag-
nitude distribution in the vicinity of the nozzle bore exit can be
defined by the velocity uniformity index U
i introduced by Weltens
et al. [65] described in Eq. 8 ,
U
i
=
1 1
2 n
n
i =1
(v
z
v
z
)
2
v
z ·100 (8)
where n is the total number of cells considered, v
i is the axial ve-
locity in the cell and v
z
represents the mean axial velocity. The ve-
locity uniformity index U
i
shows uniform flow velocity distribution
arriving at the nozzle bore exit for the standard and the inclined
nozzles (N101 and N105, respectively) while the eccentric nozzle
N104 stays by a few percentage points behind (see Table 2 for fur-
ther details). Another indicator of the flow uniformity is the void
fraction of phases at the nozzle bore exit. Therefore, averaging of
the gas fraction of cells has been executed using the CFD simula-
tion results. The standard N101 and the eccentric nozzle N104 have
8
R. Balz, I.G. Nagy, G. Weisser et al. International Journal of Heat and Mass Transfer 169 (2021) 120933
Fig. 13. Experimental and simulated momentum flux ( ˙
M
f
) of analyzed atomizer ge-
ometries as function of Reynolds number.
higher gas fraction, while the angled nozzle N105 results in less
gas-phase content just right before entering the plenum. The dis-
charge coefficient C
D gives a good indication of nozzle efficiency,
wherewith the reduced effective nozzle bore area due to cavita-
tion, the value decreases and therefore influences the injected fuel
velocity. The eccentric nozzle N104 provides the lowest discharge
coefficient, while the rest of the nozzles have slightly higher values
(see Table 2 for reference). The momentum flux ˙
M
f
has also been
evaluated from the CFD simulation results as it remains the only
quantitative result to compare directly with the experimental re-
sults. The angled nozzle N105 has the highest momentum flux and
the eccentric nozzle N104 with a significant deviation, the lowest.
4.3. Comparison of experimental and numerical results
Fig. 13 depicts the momentum flux ˙
M
f
from the experiments
and simulations together with their Reynolds numbers ( Re ) evalu-
ated from the CFD simulation results. The experimentally acquired
momentum flux of the three different nozzle types shows error
bars with a span of 5% to illustrate the deviations between ex-
periment and simulation. Although the standard deviation of the
measured and averaged force signals from the impingement ex-
periments were evaluated (see Table 1 ), the errors are likely to
be larger due to observational errors, and hence, a fixed span of
5% was chosen instead of the standard deviation of approximately
only 0.1 N. The simulation results fit the experimental data well for
nozzle type N101 while predicting a slightly lower value for the
eccentric nozzle N104 and a slightly higher value for the angled
nozzle N105. The standard nozzle N101 has the smallest discrep-
ancy with less than -2% compared to the experimentally measured
value.
Fig. 14 , 15 , and 16 show the experimentally acquired in-nozzle
flow images compared to the CFD simulation results. To create CFD
images that are qualitatively comparable to the experimental im-
ages, a time frame has been defined for statistical examination af-
ter the simulation has reached a quasi-steady-state. This allows a
comparison to the outcome of