Experimental and numerical study of a high-pressure waterjet

Abstract

High-pressure waterjet (HPWJ) nozzles are used for cutting or for surface treatment such as cleaning, decoating and deburring. The flow within a HPWJ nozzle is compressible and turbulent due to the high water pressure and velocity. Depending on flow velocity and the geometry of the HPWJ nozzle a multiphase flow of liquid and vapor can occur. Outside of the nozzle, a highly complex turbulent waterjet breakup takes place. In order to increase the breakup length of the waterjet, geometric modifications inside the nozzle are required. On the other hand, wear resistance of a nozzle is highly desirable. In this study, the flow inside of a convergent waterjet nozzle was investigated by means of computational fluid dynamics. For the true geometrical model, µ-CT scans of the studied nozzle were used. A reverse engineering process provided the model of the nozzle. The diameter of the orifice was 0.5 mm and the inlet pressure was at 75 MPa. For the modeling of the multiphase flow, the Volume-of-Fluid (VOF) method was applied. Turbulence is also a major influential factor on the primary breakup and therefore the Large-Eddy-Simulation (LES) method was utilized. Since LES method requires good inlet boundary conditions for producing stochastic components of the velocity field, separate Reynolds-Averaged-Navier-Stokes (RANS) simulations for realistic inlet conditions were performed. The studied nozzle had a flow grid, which is located in front of the convergent part of the nozzle. The influence of the flow grid on the waterjet was investigated both in the simulation and in the experiment. To validate the simulations, the flow rates from the experiment were compared with the simulation. High-speed photography provided the spray angle of the waterjet. The results of this study showed that higher turbulence, which was produced by the cross-shaped flow grid, had a stabilizing influence on the primary breakup of the jet.

Full text

ILASS–Europe 2019, 29th Conference on Liquid Atomization and Spray Systems, 2-4 September 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Experimental and numerical study of a high-pressure waterjet
Oleg Urazmetov*1, Marcel Cadet2, Roman Teutsch2, Christian Schindler3, Sergiy Antonyuk1
1Institute of Particle Process Engineering, Technische Universität Kaiserslautern,
Gottlieb-Daimler-Str. 44, 67663 Kaiserslautern, Germany
2Institute for Mechanical and Automotive Design, Technische Universität Kaiserslautern,
Gottlieb-Daimler-Str. 42, 67663 Kaiserslautern, Germany
3Chair and Institute for Rail Vehicles and Transport Systems, RWTH Aachen University,
Seffenter Weg 8, 52074 Aachen, Germany
*Corresponding author: oleg.urazmetov@mv.uni-kl.de
Abstract
High-pressure waterjet (HPWJ) nozzles are used for cutting or for surface treatment such as cleaning, decoating
and deburring. The flow within a HPWJ nozzle is compressible and turbulent due to the high water pressure and
velocity. Depending on flow velocity and the geometry of the HPWJ nozzle a multiphase flow of liquid and vapor
can occur. Outside of the nozzle, a highly complex turbulent waterjet breakup takes place. In order to increase the
breakup length of the waterjet, geometric modifications inside the nozzle are required. On the other hand, wear
resistance of a nozzle is highly desirable. In this study, the flow inside of a convergent waterjet nozzle was
investigated by means of computational fluid dynamics. For the true geometrical model, µ-CT scans of the studied
nozzle were used. A reverse engineering process provided the model of the nozzle. The diameter of the orifice was
0.5 mm and the inlet pressure was at 75 MPa. For the modeling of the multiphase flow, the Volume-of-Fluid (VOF)
method was applied. Turbulence is also a major influential factor on the primary breakup and therefore the Large-
Eddy-Simulation (LES) method was utilized. Since LES method requires good inlet boundary conditions for
producing stochastic components of the velocity field, separate Reynolds-Averaged-Navier-Stokes (RANS)
simulations for realistic inlet conditions were performed. The studied nozzle had a flow grid, which is located in front
of the convergent part of the nozzle. The influence of the flow grid on the waterjet was investigated both in the
simulation and in the experiment. To validate the simulations, the flow rates from the experiment were compared
with the simulation. High-speed photography provided the spray angle of the waterjet. The results of this study
showed that higher turbulence, which was produced by the cross-shaped flow grid, had a stabilizing influence on
the primary breakup of the jet.
Keywords
high-pressure waterjet nozzle, CFD, VOF, spray, atomization, primary breakup, turbulence.
Introduction
High-pressure waterjet nozzles are widely used in a range of applications. Cutting with a pure HPWJ is limited to
thin and soft materials. In order to cut thicker materials, abrasive particles are commonly mixed to form an abrasive
waterjet [1]. For cleaning purposes, pure HPWJ is usually used [2]. In both cases, a high specific energy per unit
area is desired. Therefore, almost all high-pressure nozzles work in the atomization regime as defined by [3]. Thus,
under the present process conditions, atomization should occur directly at the nozzle outlet, which is not desired. It
is known that the geometry of the nozzle has a significant influence on the waterjet breakup [4]. Many manufacturers
design their nozzles in a special way to avoid a fuzzy jet. Experiments are often difficult due to the small dimensions
of the nozzle, which hinders exact flow measurements, especially inside the nozzle. Stability analysis theories have
been done in the past, but always neglected the flow field within the nozzle [5]. Therefore, numerical simulation of
the flow inside the waterjet nozzle is often the only way to gain knowledge about the physical properties, such as
turbulence values and velocity profiles. The aim of this study is to create a connection between the flow inside the
nozzle and the influence on the atomization of the waterjet.
Theoretical velocity of the high-pressure waterjet flow
Since water becomes compressible at sufficiently high pressure, the error must be checked as to whether the water
can be treated as incompressible or not. The following three equations are used to calculate the velocity of the jet
with water as a compressible liquid [6]. With p as the pressure of water, the equation of state for density is:
ρ = ρ01+ p
nK0n
(1)
Where ρ is density with n as a density exponent and K0 as the reference bulk modulus of water. Together with
equation (1) and Bernoulli’s equation for theoretical velocity vth (2),

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
vth = 2p
ρ (2)
the jet velocity, vj , can be found as [6].
vj = 2nK0
ρ0(1-n)1+ p
nK01-n
-1 (3)
At p = 75 MPa and a constant density of 998.2 kg/m³ equation (2) gives: vth = 387.65 m/s. With compressible density
and values for p = 75 MPa, n=7.15 and K0 = 2.2 GPa (values for n and K0 can be for example found in the online
guide for Ansys Fluent [7].) the jet velocity becomes vj = 384.34 m/s. The difference is small at 75 MPa but becomes
more significant with higher pressure values.
Another important value for nozzle flow is the nozzle discharge coefficient cd. By obtaining the volume flow, the
discharge coefficient can easily be calculated using equation (4).
q
= cdA0vj (4)
where A0 is the area of the nozzle cross section.
Experimental setup
A plunger pump is generating the high-pressure water for the waterjet. The water flows through a hose from the
pump to the nozzle lance. Inside the lance, there is a turbulent flow. Figure 1 shows the experimental setup. A Nikon
d7200 CMOS camera with a Zeiss 50 mm, f/2 lens was used. Pictures were taken in a completely dark room with
a relatively slow shutter speed of 1/15 s. Therefore, only the NANOLITE flash exposed the sensor. The aperture
was set to f/2, which provided good light intensity and a sufficient good depth of field. To keep the spray development
as low as possible, the water tank was covered with a plastic plate.
Figure 1. Experimental setup.
Simulation model
The simulation of the primary breakup is computationally very demanding, because of the high mesh density at the
liquid/gas phase. Therefore, the simulation of the nozzle flow and the high-pressure waterjet were considered
separately. Two simulation models had to be created. The flow inside the nozzle was numerically calculated from
the nozzle lance to the nozzle outlet. The simulation of the high-pressure waterjet consists of a short cylindrical part
(the total length of the nozzle was preserved) of the nozzle and a cylindrical surrounding area in which the jet
breakup was calculated numerically. In order to design the nozzle geometry as realistically as possible, μ-CT scans
were performed and the triangulated surfaces were reconstructed in a reverse engineering process, see Figure 2.
The black box marks the area of interest of the water flow.

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Figure 2. CAD assembly reconstructed from µ-CT scan (Arrow illustrates the direction of flow).
Although the nozzle was labeled as 0.5 mm in diameter, the generated model had 0.49 mm as the nozzle diameter.
The reason for the deviation of both values could originate from the scan, however, the value is still in the tolerance
of the nozzle. The specifics of the used nozzle are summarized in Table 1
Table 1. Geometry of the nozzle
nozzle diameter
cone angle
l/d nozzle
nozzle edge radius
nozzle parameter
0.49 mm
30 degree
2.5
1 mm
Parameters of RANS and LES-VOF simulation
For the simulation of the flow inside the nozzle, a 3D interior volume was extracted from the location, which was
marked by the black box in Figure 2. The extracted volume can be seen in Figure 3. The two colors in Figure 3
indicate the two simulation domains, grey for the RANS simulation and blue for the LES-VOF.
Figure 3. Extracted 3D interior volume (Grey volume: water under high pressure, blue area: air at ambient pressure).
For the RANS simulation, a hybrid mesh was generated with tetrahedral and hexahedron elements, Figure 4. The
cylindrical part of the nozzle was meshed with hexahedron elements. For the more complex geometry, tetrahedral
elements were used. From previous 2D simulations, the inlet edge of the nozzle was examined and no cavitation
was detected with an inlet edge of 1 mm. Therefore, a single-phase simulation was set up. The modeling of the
turbulence effects were carried out with the kω-SST model [8]. For the LES-VOF simulation, the geometry was
reduced to the outlet part of the nozzle and a cylindrical volume in which the waterjet interacts with the quiescent
air was added. The dimensions of the outflow space were simplified; the hexagonal socket was replaced with a
cylinder. As for turbulence modeling the LES was used [9]. The results from RANS simulation were used as
boundary conditions for the LES-VOF.

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Figure 4. Mesh for the RANS simulation on the left side and mesh for the LES-VOF simulation on the right side (Arrow illustrates
the direction of flow, walls are coloured in grey).
The properties of both the RANS and LES-VOF simulations are summarized in Table 2
Table 2. Mesh properties and simulation parameters
RANS
LES-VOF
total cells
2.9·106
12·106
total length of the domain
37 mm
6 mm
total volume of the domain
4.89·10
-7
m³
4.43·10
-8
m³
turbulence model (y+-value)
kω-SST (~35)
LES (~4.5)
boundary conditions
pressure inlet: 75 MPa
pressure outlet: 0 MPa
velocity inlet: velocity. mag., tke and epsilon
pressure outlet: 101325 Pa
fluid
water compressible
water/air incompressible
surface tension
-
73.5·10
-3
N/m
Reynolds/Weber number
2·105/-
2·105/1·106
time step
steady-state
14 ns (implicit)
RANS results
First, the results of the flow inside the nozzle are shown, Figure 5 and Figure 6 show the velocity field of the flow.
For comparison reason, the flow grid was removed. Through the flow grid, there is a local speed increase.
Additionally, the flow grid untwists the flow if there are some swirls present from the inlet boundary condition.
However, the flow grid had no influence on the maximum velocity of the flow at the nozzle exit. In both cases, the
maximum speed of around 385 m/s was reached, which is almost identical to the value calculated with equation
(3). The volume flow rate was in both cases almost identical, around 4.15 l/min. The measurements of the flow rate
with an ultrasonic flow meter fluctuated between 3.67 and 4.33 l/min, while the product data sheet of the
manufacturer indicated the flow under the given conditions with 4.2 l/min. The simulation predicts the experimentally
determined values for the volume flows. With the values for speed and volume flow rate, the discharge coefficient
of cd ≈ 0.96 was determined. Table 3 illustrates the results of the influence of the flow grid. The discharge coefficient
with the flow grid is slightly lower when compared to the nozzle without the flow grid. The reason is that the flow
grid acts as flow resistance. However, the influence is negligibly small, due to the relatively low flow velocity. When
comparing the nozzles with and without the flow grid, it becomes clear that the walls of the flow grid create
turbulence in the flow core as indicated in Figure 7. The results of the RANS simulations are summarized in Table 3.
Table 3. RANS Results
nozzle with flow grid
nozzle without flow grid
mass flow / kg/s
0.0691764
0.0692236
max. velocity / m/s
384.769
384.762
discharge coefficient / -
0.95619
0.95684
max. tke (nozzle outlet) / J/kg
1229
1070.6

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Figure 5. Velocity magnitude inside the nozzle with the flow grid.
Figure 6. Velocity magnitude inside the nozzle without the flow grid.
Figure 7. Contour plots of turbulence kinetic energy (tke).
As next, Figure 8 shows the velocity magnitude and the turbulence kinetic energy on the nozzle outlet for the nozzle
with and without the flow grid. It is noticeable that the turbulence, produced by the flow grid, persists to the nozzle
outlet. In addition, the absolute values for turbulence kinetic energy (tke), close to the wall, are up to 20% higher for
the nozzle with the flow grid. The velocity field was found to be more irregular in the near wall region for the nozzle
with the flow grid.

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Figure 8. Contour plot of velocity magnitude (left side A and B) and turbulence kinetic energy (right side A and B), red areas are
greater than/equal 40 m²/s², at the nozzle outlet (Nozzle type A: flow grid, nozzle type B: no flow grid).
LES-VOF results
As mentioned before, the data from the RANS simulation was used for the LES-VOF simulation as a boundary
condition. To produce stochastic components from steady-state RANS simulation, the spectral synthesizer method
was utilized [10]. The results of the LES-VOF simulations are summarized in Table 4.
Table 4. VOF-LES results
nozzle
with
flow grid
nozzle
without
flow grid
simulation time / µs 21.42 21.42
surface area of iso-
surface of water with
volume fraction of 0.5
/ mm²
26.68 27.55
surface area of
cylinder with diameter
of the nozzle and the
length of the domain
/ mm²
9.24
Figure 9. Normalized area of iso-surface of the waterjet.
From Figure 9 it can be seen that the waterjet is more coherent with the flow grid. We examined the surface of the
waterjet and compared both variations. The iso-surface of the waterjet was related to a cylinder with the diameter
of the nozzle and the same length as the waterjet. The iso-surface of the waterjet with the flow grid has a smaller
area than the waterjet without the flow grid. The difference is around 3.3 %, which is small, but noticeable. This
difference may grow larger if the size of the domain is increased. The smaller surface of the waterjet indicates a
more coherent waterjet. The waterjet without the flow grid shows both, a larger wave formation and more ligaments
and droplets, Figure 11. Both waterjets show the typical wave formation, as also shown in [11]. This wave instability
grows immediately after the nozzle outlet that eventually leads to the formation of ligaments, which are the
precursors of drops. Due to surface forces, a ligament is constricted and a droplet can detach. Thus, the simulation
reproduced the primary atomization qualitatively well. Upon closer examination, small droplets are noticed which
have a high flow velocity. This may be related to the fact that when droplets are only a few grid cells in size, their
physical interaction with the ambient air cannot be calculated correctly.
Figure 10. LES-VOF simulation, waterjet with flow grid installation (iso-surface of water volume fraction 0.5).
0.0
0.5
1.0
1.5
2.0
2.5
3.0
3.5
010 20 30
area of iso
-surface/area of
ideal cylinder /
-
simulation time / µs
without flow grid
with flow grid

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Figure 11. LES-VOF simulation, waterjet without flow grid installation (iso-surface of water volume fraction 0.5).
High-speed photography
For the experimental setup, both the original nozzle with the flow grid and a modified nozzle without the flow grid
were used. The pressure was set up to 75 MPa, the same value as in the simulation. The nozzle outlet from which
the waterjet exits was not visible because the nozzle holder hides it. From the outlet of the nozzle, up until the
waterjet can be seen, there is 9 mm distance. Therefore, the first breakup of the waterjet cannot be seen. The high-
speed photo in Figure 12 shows a waterjet with the flow grid. When compared to nozzle without the flow grid, in
Figure 13, it is noticeable that the nozzle with the flow grid creates a more coherent jet. The jet disintegration takes
place, further downstream for the nozzle with the flow grid. Furthermore, the spray angle is lower for the nozzle with
the flow grid. A low spray angle is required to maximize the specific energy per unit area on the surface of a
component.
Figure 12. High-speed photograph of waterjet from nozzle with flow grid (~125 ns, with NANOLITE fx xenon flash).
Figure 13. High-speed photograph of waterjet from nozzle without flow grid (~125 ns, with NANOLITE fx xenon flash).
Summary
In this study, the flow inside a HPWJ nozzle at 75 MPa was investigated. The waterjet velocity reaches around 385
meters per second according to our simulations, which matches with the theoretical calculation. With a high-speed
photography the dynamics of the waterjet were captured, which revealed a waterjet core surrounded by small
droplets. The breakup of the waterjet takes place shortly after exiting the nozzle, as expected. Investigating the
waterjet in more detail, the simulations showed the typical behaviour of wave instabilities on the surface of the jet.
The instabilities grow, which finally leads to the ligament and droplet development. The effect of a flow grid was
studied which had a beneficial effect on the stability of the liquid core in both the simulation and in the experiment.
From the photos, the stabilizing effect of the flow grid was proven. The spray angle was significantly lower for the
nozzle with the flow grid than for the nozzle without the flow grid. The simulation revealed that the nozzle with the
flow grid produces higher levels of turbulence, which seems to be responsible for the higher stability. The approach
in this study combined steady state RANS simulation results with computationally higher demanding unsteady LES-
VOF simulations.
α ≈ 5°
α ≈ 7.5°

ILASS – Europe 2019, 2-4 Sep. 2019, Paris, France
This work is licensed under a Creative Commons 4.0 International License (CC BY-NC-ND 4.0).
Conclusion and outlook
According to the subdivision of the flow regime as in [3], the operating conditions of the studied HPWJ-nozzle are
in the atomization regime. A liquid core, therefore, should disintegrate shortly after the nozzle outlet. This was
however not the case with the studied HPWJ nozzle, which indicates the presence of additional influences, which
have a positive effect on the disintegration length. Turbulence produced by a flow grid might be responsible for the
stabilization. Therefore, the next step is to investigate other shapes of the flow grid. The stabilizing effect could be
significantly increased. It is also planned to run a LES-VOF simulation with the convergent part of the nozzle and
the corresponding boundary conditions. Moreover, it is planned to study the effect of the turbulence kinetic energy
inside the liquid core more thoroughly. It seems plausible, that higher turbulence inside the liquid core acts as an
additional turbulence viscosity, which stabilizes the jet further downstream. This phenomenon will also be studied
at higher inlet pressures. Although computationally very demanding the LES-VOF approach shows promising
results. The study of high-pressure liquid jets remains a difficult area of research, but it is worth to continue analyzing
the effects in order to understand the influences on the atomization process.
Acknowledgements
This work was funded by the German Research Foundation (DFG) under the project: “Experimentelle und
numerische Untersuchung des Strömungsprozesses von Hochdruckwasserstrahlen und ihrer Interaktion mit
Bauteiloberflächen“, which the authors gratefully acknowledge.
Nomenclature
ρ density [kg m-3]
ρ0 reference density [kg m-3]
p pressure [Pa]
p0 reference pressure [Pa]
K0 bulk modulus [Pa]
vj jet velocity [m s-1]
vth theoretical jet velocity [m s-1]
n density exponent [-]
q
 volume flow rate [m3 s-1]
cd nozzle discharge coefficient [-]
A0 reference area [m2]
tke turbulence kinetic energy [J/kg]
References
[1] M. Hashish, “Visualization of the abrasive-waterjet cutting process,” Experimental Mechanics, vol. 28, no. 2,
pp. 159–169, 1988.
[2] Frenzel L., “WHAT EFFECT DOES WATERJET CLEANING HAVE ON THE SURFACE AND SURFACE
PREPARATION?,” 2007 American WJTA Conference and Expo August 19-21, 2007 Houston, Texas.
[3] Wolfgang von Ohnesorge, “Die Bildung von Tropfen an Düsen und die Auflösung flüssiger Strahlen:
Vorträge der Hauptversammlung in Dresden,” Zeitschrift für angewandte Mathematik und Mechanik, no.
Band 16, Heft 6, pp. 355–358, 1936.
[4] A. Begenir, H. Vahedi Tafreshi, and B. Pourdeyhimi, “Effect of Nozzle Geometry on Hydroentangling Water
Jets: Experimental Observations,” Textile Research Journal, no. 74(2), pp. 178–184.
[5] R. D. Reitz and F. V. Bracco, “Mechanisms of breakup of round liquid jets,” Encyclopedia of Fluid
Mechanics, pp. 233–249, 1986.
[6] T. Susuzlu, A. M. Hoogstrate, and B. Karpuschewski, “Initial research on the ultra-high pressure waterjet up
to 700MPa,” Journal of Materials Processing Technology, vol. 149, no. 1-3, pp. 30–36, 2004.
[7] 7.3.4. Compressible Liquid Density Method. [Online] Available:
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v190/flu_ug/flu_ug_props_co
mp_liq_den_treat.html. Accessed on: Mar. 05 2019.
[8] F. R. Menter, “Two-equation eddy-viscosity turbulence models for engineering applications,” AIAA Journal,
vol. 32, no. 8, pp. 1598–1605, 1994.
[9] J. H. Ferziger and M. Perić, Computational Methods for Fluid Dynamics. Berlin, Heidelberg, s.l.: Springer
Berlin Heidelberg, 2002.
[10] A. Smirnov, S.Shi, I. Celik, “Random Flow Generation Technique for Large Eddy Simulations and Particle-
Dynamics Modeling,” Journal of Fluids Engineering, no. 123, pp. 359–371, 2001.
[11] J. W. Hoyt and J. J. Taylor, “Waves on water jets,” J. Fluid Mech., vol. 83, no. 01, p. 119, 1977.