Numerical Analysis of the Behavior of A New Aeronautical Alloy (Ti555-03) Under the Effect of A High-Speed Water Jet

In this paper, we present a numerical simulation of a water jet impacting a new aeronautical material Ti555-03 plate. The Computational Fluid Dynamics (CFD) behavior of the jet is investigated using a FV (Finite Volume) method. The Fluid–Structure Interaction (FSI) is studied using a coupled SPH (Smoothed Particle Hydrodynamics)-FE (Finite Element) method. The jets hit the metal sheet with an initial velocity 500 m/s. Two configurations which differ from each other by the position (angle of inclination) of the plate relatively to the axis of revolution of the jet inlet are investigated in this study. The objective of this study is to predict the impact of the fluid produced at high pressure and high speed especially at the first moment of impact. Numerical simulations are carried out under ABAQUS. We have shown in this study that the inclination of the titanium alloy plate by 45° stimulates the phenomenon of recirculation of water. This affects the velocity profile, turbulence and boundary layers in the impact zone. The stagnation zone and the phenomenon of water recirculation are strongly influenced by the slope of the plate which gives a pressure gradient and displacement very important between the two configurations. Fluctuations of physical variables (displacement and pressure) prove the need for a noise and vibratory study. These predictions will subsequently be used for the modeling of the problem of an orthogonal cut in a high-speed machining process assisted by high-pressure water jet.


Introduction
The High-Speed Water Jet-Assisted Machining (HSWJAM) consists in projecting a jet of lubricant between the cutting face of the tool and the chip. The lubricant could be generally water. The pressure of the jet can exceed several hundred bars. This high pressure (HP) jet allows more effective lubrication and evacuation of the heat produced during the cutting process, as compared with conventional machining. The high pressure lubrication adds the possibility of breaking chips by a mechanical action of the jet independently of the cutting parameters (Braham-Bouchnak, 2010). The efficiency of the process is conditioned by the choice of the parameters of the jet, namely: the pressure, diameter and inclination of the nozzle (Ayed et al., 2013).  Fig. 2 show an example of a tool during a HSWJAM. The impact of a high-velocity jet on an obstacle is widely studied because of its large applications from household appliances to space technology. The high-velocity water jet is characterized by its many advantages and ease of industrialization (Kaushik et al., 2015). The technology of water jets is now applied in many industrial fields, such as welding, cleaning (turbine, engine parts), decorating process, cutting (metals sheet, plastic), removing materials by abrasive water jet, high-pressure water jet assisted machining (Chizari et al., 2008(Chizari et al., , 2009Mabrouk et al., 2000;Mabrouk and Raissi, 2002;Saxena and Paul, 2007;Ayed et al., 2016). The most used way to produce a high-velocity water jet is forcing a quantity of water through a conver-ging nozzle. By using this method, the water is accelerated and the jet can attain the speed up to 4000 m/s (Hsu et al., 2013). Owing to the strong multi-physics coupling, the numerical modeling of Fluid-Structure Interaction (FSI) is considered very difficult (Kaushik et al., 2015). Recently, Simulations have started to take into consideration of the capability of the water jet technique in different domains. Only a few studies have been focused experimentally and numerically on high pressure water-jet taking into account the FSI problems where the Coupled Eulerian Lagrangian (CEL) method has been used to simulate the FSI (Ayed et al., 2016;Hsu et al., 2013), or by the use of finite elements analyses (FEA) to simulate welding (Chizari et al., 2008), tube forming (Chizari et al., 2009), or else by using the LS-DYNA3D code to understand the decoating process (Mabrouk et al., 2000). The efficiency of the jet is related to the right choice of parameters, so the jet must be controlled in terms of the varying jet speed and mass flow rate. The jet control aims to modify the flow development in relation to a specific application. Other studies focused numerically and experimentally on the CFD behavior of the jet by investigating the velocity profile of the jet water before and after impact and the distribution of the pressure on the target without taking into consideration the (FSI) phenomena (Kaushik et al., 2015;Guha et al., 2011). This study is a part of a research project to understand the HSWJAM of a new Titanium alloy: Ti555-03.
Within this framework, we propose a numerical study with an aim to investigate the behavior of a pure water jet by continuing impact on a metal sheet. In this paper, we propose two numerical models using ABAQUS. The first model is a CFD model using the numerical FV method based on the Eulerian formulation in order to investigate the CFD behavior and solve the transient fluid problem such as the first impact time, velocity profile of the flow and distribution of the pressure on the plate. The second model is a meshfree SPH based on Lagrangian formulation developed to handle and analyze in detail the material behavior under the water jet impingement. By using the above methods, we propose in this study to investigate the influence of the position (angle of inclination 0° and 45°) of the target relative to the axis of the jet nozzle. During the HSWJAM, the chip takes several angular positions with respect to the nozzle axis of the jet. The positions start from 0° to the roll up. In this study, we have chosen 0° where the chip still belongs to the work piece and another intermediary position corresponding to 45°. A convergence study was developed to validate the stability of the numerical results for each model.

Problem formulation
We are going to impact a horizontal plate of Titanium alloy: TI55503 with a pure water jet which has an initial velocity of V e =500 m/s through a nozzle with a diameter D of 0.3 mm. The Target is a sheet of titanium alloy metal Ti555-03 having 6 mm as the length, 1 mm as the width and 3.5 mm the thickness presented in Fig. 3a. These geometrical parameters values correspond to a high-pressure water jet assisted machining applications . In addition, in order to minimize the computation time of CPU. The domain of the jet flow is fixed to h=1.5 mm far from the target. The axis of the nozzle is coaxial with the normal of the target. We propose to study tow con-   I. Ben Belgacem et al. China Ocean Eng., 2019, Vol. 33, No. 1, P. 114-126 115 α figurations of impacting a target. For Configuration 2 the only difference is the incline of the target by =45° from the horizontal level as presented in Fig. 3b.

CFD simulations under ABAQUS
3.1 Numerical model

State equation of water
In this study, the impact time is very short. So the heat exchange and vaporization of water are not considered (Hsu et al., 2013). In Table 1, we present values of the fluid properties used in this computation.
For the hydrodynamic behavior law, we need to associate an state equation of water. In this study, the water is modeled using the linear Hugoniot form of the Mie-Greisen equation of the state which is a relation between the pressure and the volume of a material at a given temperature (Hsu et al., 2013). ABAQUS/Explicit provides a linear U s -U p equation of the state model that can simulate incompressible viscous and in-viscid laminar flow governed by the Navier-Stokes Equation of Motion (ABAQUS 6.14 documentation). The U s -U p form is given by Eq. (1): where, E m is the internal energy per unit mass; is the reference density; is the Grüneisen ratio defined as = 0 ( ), 0 being a material constant; is the nominal volumetric compressive strain; C 0 and s define the linear relationship between the linear shocks velocity, U s and the particle velocity, U p , as follows: Γ The values of these parameters, s and for defining water, were referred from ABAQUS 6.14 documentation. Equation parameters are shown in Table 2.

Equation of the Navier-Stokes and turbulence model
The water is considered as an incompressible and homogenous fluid. The flows of incompressible fluids are governed by the Navier-Stokes equations (Comte Bellot and Bailly, 2003). These equations are written for the mass con-servation, momentum, and energy respectively as follows: where, is the density, u is the displacement, p is the pressure, h is the enthalpy, and is the dissipation function of the viscous effects. The thermal aspect of the problem is not taken into account, so the last equation of the energy conservation is no longer to be considered as long as we assume that the flow is at constant temperature. Therefore, the system of Eq. (2) is reduced as follows: τ where is the viscous stress tensor and it is written as follows: μ where, is the dynamic viscosity of the fluid, I is the unit tensor, and u is the displacement vector.
The nonlinear and non-predictable characters and the existence of a wide range of scales of these equations are the origin of the turbulence phenomena (Comte Bellot and Bailly, 2003). The fluid flow in the current impinging jet study is turbulent due to the large Reynolds number of Re =73500. Therefore, the best turbulence model used in the literature is which can be used for high Re values to deliver acceptable numerical results in a steady flow analysis for higher H/D ratios (Behera et al., 2007) which is equal to 5 in our case. We have used this model of turbulence presented in ABAQUS to handle this phenomenon. It is based on the hypothesis of Boussinesq (Comte Bellot and Bailly, 2003). This model presents two equations. The first will manage the turbulent kinetic energy k. The second will deal with the corresponding dissipation . This model presents three different formulations: standard , the realizable and the RNG . The RNG is the only formulation presented in ABAQUS. The RNG approach, which is a mathematical technique, can be used to obtain a turbulence model similar to by introducing a turbulent viscosity expressed from the turbulent kinetic energy and its dissipation rate as follows (ABAQUS 6.14 documentation): Thus, the two transport equations necessary to evaluate this turbulent viscosity are respectively the transport equation of Note: is the density; is the dynamic viscosity (at 20°C and atmospheric pressure) ε the turbulent kinetic energy k and the equation of the turbulent dissipation . These are given in Eq. (6) (ABAQUS 6.14 documentation): where, is the term for the production of energy; is the shear tensor component; S ij is the stress tensor component; is an empirical constant. Table 3 presents the values of the empirical constants of this model introduced by ABAQUS.

Boundary and initial conditions
ε For the inlet we apply a velocity equal to 500 m/s. A no slip condition is applied on the walls of the studied volume of fluid (VOF) presented in Fig. 4. For the outlets, we assumed an atmospheric pressure. Initial conditions of the value of the turbulent kinetic energy k 0 as well as the turbulent dissipation 0 are given by Eq. (7) (Mahjoub Saïd, 2002).

Mesh and convergence study
The quality of the mesh has a serious impact on the convergence, the precision of the solution and especially on the calculation time. A good quality of mesh is based on the minimization of elements with distortions and on a good resolution. At the end of this convergence study, we will arrive at 244256 linear 4-node tetrahedral elements for the first configuration and 629305 linear 4-node tetrahedral elements for the second configuration.
3.2 Results of the fluid model

Velocity profile
Velocity profile of the water flow at each point in the studied volume after 6×10 -5 s could be decomposed into three different regions (Khan et al., 2011): (1) A free jet region At the outlet of the nozzle, the flow is not significantly influenced by the impact surface and the velocity component is predominantly axial. The distance of the free jet (Z) is equal to 1.24 mm for the horizontal target and 1.23 mm for the inclined target. This result is in accordance with the experimental results published in (Roux et al., 2009) where it is proved that Z=4D. For both configurations (horizontal and inclined target), this zone presents the same velocity profile. Fig. 5 shows the flow of water in the study volume during 3×10 -6 s before impact. The free jet region can be composed of the three zones: • Zone 1 is a core zone having a conical shape. In this region the velocity reaches its maximum value V max =1093 m/s for the horizontal target (Fig. 5) and V max =1101 m/s for the inclined target. The maximum magnitude is supported by the component along the y axis V y .
• Zone 2 is a reorganization zone where the jet starts to develop softly.
• Zone 3 is a zone of established flow, also known as a "developed turbulence zone". Here, the turbulence phenomenon starts to develop significantly.
(2) A region of stagnation The flow properties deviate from those of a free jet. It is the impingement zone where the flow starts to be influenced by the target. It is characterized by a change of the jet ε Table 3 Values of the empirical constants of the k-turbulence model (ABAQUS 6.14 documentation) Note: is the Logarithmic wall law; is the comparison with the jetwake experience; is the comparison with jet-wake experience; is the uniform deformation or shearing; is the isotropic turbulence decay.  α direction with a transition towards a parietal jet due to the deflection of the water after impact. A helical structure is observed when the jet impacts the wall. Also, this region is characterized by a zone of stagnation localized and stabilized by the target. In the case of the angle of target equal to 45°, this zone is no more in the center of the impact zone observed in the horizontal target as shown in Figs. 6a and 6b. In the deflection region, the velocity on the central axis of the jet decreases as the flow approaches the point of stagnation until a zero value is reached at the wall.
(3) A radial jet region This zone known as the wall-jet region is parallel to the wall (Roux et al., 2009;Sodjavi, 2013;Rivière, 2008;Gojon, 2015;Roux, 2011). The principal component of the velocity is radial. The thickness of the boundary layer increases in a radial direction. Turbulence is no longer the same. We speak about the wall turbulence. In this region, the flow is dominated by the wall effects through the viscosity forces. The angle of inclination occurs at the velocity profile especially in the wall zone where the water recirculation phenomenon is also observed. The re-circulated water strikes the inclined plate but with less intensity. The phenomenon of recirculation is observed clearly after 9.002× 10 -6 s of flow of water.

Pressure distribution on the target
During the transient regime, the target supports high stresses in terms of the velocity and pressure due to the first shock wave of the flow. This wave is subsequently the origin of a high vibration rate. This vibration can reach the frequency of resonance of the plate. For the horizontal target, farther away from the center the lower values are obtained until reaching a negative value. This value is equal in the absolute value to the pressure at the center P max (234 MPa).
This phenomenon of depression is in correlation with the sense of the deformation of the target as shown in Fig. 7a. For the inclined target, the distribution of the pressure is shown in Fig. 7b. The pressure reaches a maximum value equal to 392 MPa. Numerically speaking, the mesh and time of the flow were controlled in order to not reach the recirculation of the water. Following a study of the spatial convergence (mesh density) and temporal (flow time) taking into account not reaching recirculation, a flow time of 6.3×10 -6 s was fixed. Fig. 8 presents the curve of the maximum pressure during 6×10 -6 s. It shows the difference between the maximum pressures in the HT and IT. The IT presents a maximum value of the pressure equal to 4 MPa. While, the maximum value of the pressure is about 2.7 MPa for the HT. Indeed, the inclination of the target does not affect the shape of the curve of the pressure versus the time but it influences the magnitude.

Overview of the SPH method
The SPH method is a meshfree particle technique following the Lagrangian formulation. The main strength of  the SPH method is based on the absence of a fixed mesh coming from its Lagrangian nature. Modeling difficulties coming from fluid flow and structural problems presenting large deformation and free surfaces are resolved in a relatively soft way. To model fluid dynamics problems governed by the Navier-Stokes equations, the use of SPH method is a very powerful alternative. The studied flow is represented by a set of particles with predefined material properties, mechanical behavior and initial fields. These particles are interacting with each other in a domain controlled by a smoothing function or a weight function. These discrete particles are used to discretize the continuum partial differential equations governing the studied system. In this regard, the SPH method is quite similar to the FE method. For the calculation of the local density, velocity and acceleration of the fluid, particle-based formulations have been used. Hence, the fluid pressure is calculated from the density using an equation of state (EOS). The particle acceleration is then calculated from the pressure gradient and density. To approximate a variable value at any point in the studied domain, the SPH method uses an evolving interpolation scheme. Thus, this value can be approximated by summing the contributions from a set of neighboring particles. SPH method has some special advantages compared with other numerical methods by using the grid to discretize the problem. The SPH method deals in an easily way with complicated geometries and large high deformation. The implementation of the SPH method in a numerical code is simple. SPH is a fully Lagrangian modeling scheme permitting the discretization of a prescribed set of continuum equations by interpolating the properties directly at a discrete set of points distributed over the solution domain without the need to define a spatial mesh. This is why it presents a robust scheme. The readers may refer to Liu et al. (2010) for more details about the SPH method, techniques, and smoothing function. In this section, the SPH method is used under ABAQUS to model a high pressure round water jet impact-ing a metal sheet in Titanium alloy Ti555-03. The target is modeled by the finite element method.

Numerical models
For both configurations predefined in Section 1 and shown in Table 1, a water column acting as a water source having a diameter D of 0.3 mm and a height of 6 mm was taken. The length of the water jet was fixed to be long enough to obtain a stable flow during that period. The target is a sheet of Titanium alloy metal Ti555-03 having 6 mm as the length, 1 mm as width and 3.5 mm as thickness.

Material modeling
(1) Fluid modeling For the water column the same state equation used in the numerical computation fluid model in Section 3.1.1 is chosen for the SPH model.
(2) Sheet modeling This study handles the numerical investigation of the impact of a Titanium alloy Ti555-03 plate by high-speed water jet. Titanium is often used as alloys. The addition elements stabilize either the phase (alpha element), or the phase (beta-element). The alpha elements increase the phase change temperature contrary to the beta-element (Braham Bouchnak, 2010). The alpha elements are as follows: • Aluminum (Al); • Oxygen (O); • Carbon (C); • Nitrogen (N). The beta elements may be the isomorphic (V, Mo, Nb, Ta) or eutectoid type (Fe, Cr, Mn, Si). The Ti-555-03 is a quasi-beta Titanium alloy developed for the construction of large parts subjected to high mechanical stresses such as aircraft landing gear. It is a variant of the Russian alloy VT22 (Ti-5Al-5V-5Mo-1Cr-1Fe) and an alternative to the alloy Ti-10Al-2V-3Mo. Its mechanical properties are excellent (Braham Bouchnak, 2010). The chemical composition of the Titanium alloy is presented in Table 4.
In Table 5 the mechanical and thermal proprieties are also presented.
The constitutive law of Johnson-Cook and the Johnson-Cook damage model have been chosen to take into account the dynamic behavior of the material. This constitutive law is given in Eq. (9) (Ayed et al., 2016).
where, Term 1 is the isotropic hardening of Ludwik; Term 2 is the sensitivity to the strain rate; Term 3 is the temperature sensitivity; 0 is the reference strain rate; T m is the melting temperature of the material; T a is the ambient temperature. Parameters A, B, n, C and m are constants determined experimentally.
The fracture strain, triaxiality, strain rate and temperature are related by the damage model given in Eq. (10) (Ayed et al., 2016).
where Term 1 is the sensibility of the fracture strain to the triaxiality; is the rate of triaxiality, being the hydrostatic stress and , the von Mises stress; Term 2 is the strain rate; Term 3 is the temperature.
Parameters of this law are presented in Table 6 and  Table 7.

Mesh and conversion to particles
In this modeling part, a hybrid discretization technique has been adopted. The SPH method is adopted for the water source where only a set of nodes is used. As mentioned previously, these nodes are commonly referred to particles or pseudo-particles. Start by meshing the column of water with C3D8R (8-node linear brick, reduced integration, hourglass control) to generate "parent" elements. These "parent" elements will be after that converted to internally generated SPH particles (PC3D elements). By default, one particle is generated per parent element. The number of particles generated per element is controlled by specifying the number of particles to be generated per parent element in isoperimetric direction. The total number of particles generated per element depends on the element type that is being converted. The particles are evenly spaced inside the parent element such that they fill the volume as uniformly as possible. (ABAQUS 6.14 documentation). Since we have selected the C3D8R element types and after the convergence studies, we have fixed the total number of elements in the column of water at 515967. After conversion to particles, we have the total number of particles equal to 13931109. For the Titanium target, it is presented as a shell membrane. We have used a Lagrangian finite elements method to discretize the membrane. Hence the elements type is a 4-node generalpurpose shell, reduced integration with hourglass control, finite membrane strains (S4R). In order to carry out a good convergence study and to highlight the behavior of the target under the first shock wave resulted from the impact of water, the refinement of the mesh has been concentrated towards the center of the target. The total number of elements is fixed at 515967.

Boundary conditions and predefined field
In SPH method, the boundary conditions cannot be applied directly to the generated particles. They are applied to nodes of the parent elements and could not be transferred to the generated particles (ABAQUS 6.14 documentation). An initial velocity field of 500 m/s is applied on the water column. The four edges of the target were fixed as shown in Fig. 9. Moreover, the general contact was used, and the type of the contact domain was chosen.

Numerical results
Analyzing the impact of the high-speed water jet on a solid target requires considering the connected solid mechanics and fluid mechanics theories. This study proposes a method using ABAQUS to simulate the dynamic process of    . 9. Simulation of the high-speed water jet impact on (a) HT and (b) IT after 8×10 -6 s. impact for tow configurations already shown in Table 1.
Simulations are presented in Figs. 10a and 10b.

Horizontal target
(1) Pressure on the target The simulation was extended to a period of 8×10 -6 s from the beginning of the fall of the water column. The distribution of the impact pressure on the surface of the titanium sheet at different moments of the process was investigated as shown in Fig. 11. The color contour represents the magnitude of the pressure. Fig. 11a presents the first moment of impact. In earlier stage, the pressure has a symmetric distribution (Figs. 11b, 11c and 11d) along the y and x axes. In Fig. 11e, the pressure does not present a symmetrical distribution any more. There was a chaotic distribution at the points closer to the sheet limits. The pressure fluctuates as far as the water hits the target. The particles of the fluid are more dispersed on the entire target in a random and unpredictable way. The distribution of the pressure on the target shows the zones of the pressure and depression in an alternate way. At approximately 4.5×10 -6 s, a peak value of the pressure approached just over 0.36 MPa and a peak value of depression approached to -0.54 MPa. This high fluctuation then propagated strongly out to the surrounding areas as a wave. The depression is more approached at the limit of the target as shown in Fig. 11e. This fluctuating response of the target under the water impact could be in consistency with the vibration of the metal sheet. At approximately 8×10 -6 s, Fig.  12 presents the maximum pressure in a radial direction crossing the center of the horizontal target. The evolution of the highest pressure in a radial direction at different points A, B and C is presented in Fig. 13. Point A corresponds to the center of the target. Points B and C are placed at 1.5 mm  I. Ben Belgacem et al. China Ocean Eng., 2019, Vol. 33, No. 1, P. 114-126 and at 5.5 mm respectively from the target. In Fig. 13, the water does not hit the target yet so the pressure keeps a value of zero until 3×10 -6 s corresponding to the moment of the first impact and the beginning of the dynamical process of the impact. In the early stage of the impact, the fluctuation seems smoother in Point A (centre of the target) because the head of the water jet is perfectly flat, which owns the stability of the contact of the water column in the centre unlike the dispersion of water particles becoming more complex in Points B and C. When comparing the evolution of the pressure in Points B and C, a higher fluctuation is observed in Point C but a lower magnitude of the pressure occurred. The water jet will hit the center and the neighboring areas first at higher velocity in the same way but with different magnitudes. This fluctuation of the pressure was also investigated in the numerical study presented in (Lush, 1991).
(2) Stress on the target Fig. 14 shows the Von-Mises stress on the metal sheet at different moments of the simulation from a side view. A high pressure occurs at the center first as shown in Fig. 14a.
This pressure propagates in a symmetrical way to the neighboring areas along the x and y axes (Figs. 14b,14c,14d and 14e). At approximately 5.5×10 -6 s, the stress reaches a maximum value equal to 1.5 MPa in the center of the metal sheet. Investigating the stresses in the targets helps predicting the damage in the structures. The variation of the stress state under the impact may cause the appearance of cracks.
(3) Displacement of the target The maximum displacement reached is 0.0126 mm. Fig.  15 presents the evolution of the maximum displacement magnitudes, U x , U y and U z after 8×10 -6 s. It seems that the main magnitude of the displacement is coming from the displacement U z with a fluctuant way (U x and U y are nearly zero compared with U z ). This could be explained by the vibration of the plate under the water jet along the z axis of the dropped water. From 3×10 -6 s to the end of the simulation the displacement on the HT reaches the maximum value about 0.016 mm.

122
I. Ben Belgacem et al. China Ocean Eng., 2019, Vol. 33, No. 1, P. 114-126 4.3.2 Inclined target (1) Pressure on the target The simulation was extended to a period of 8×10 -6 s from the beginning of the fall of the water column. The distribution of the impact, the pressure on the surface of the inclined plate at different intervals is presented in Fig. 16. During the impact maximum pressure keeps one position located in the center of the metal plate unlike the first configuration. Fig. 16a shows the state at 2.8×10 -6 s, that is when the water jet began hitting the structure. At approximately 4.5×10 -6 s (Fig. 16b), the pressure approached the peak value of just over 0.7 MPa and more approached at the limit of the target. This high pressure then propagated out to the surrounding areas as a wave. In the next period, there was a chaotic distribution of the pressure (Fig. 16c), which may be due to the changing state of the flow before the stability appeared. The distribution of the stagnation pressure is shown in Fig. 16e at 8×10 -6 s. Furthermore, the pressure distribution presents alternative zones of the pressure and depression as far as the jet hits the target. The jet head is not perfectly flat. It could be considered as punctual relatively to the length of the plate due to the 45° angle position of the plate, which means that the points localized in the part of the plate under the Y axis reach their maximum values earlier than other points. The impact pressures at different positions on the plate surface (presented in Fig. 17) in the radial direction are shown in Fig. 18.
The water does not hit the target until 2×10 -6 s corresponding to the moment of the first impact and the beginning of the dynamical process of the impact for Points A, B, C, D, E and F as presented in Fig. 18. A high pressure occurred at the center of the impact zone first and then spread to the localized under the y axis areas very fast. Curves corresponding to Points A and C present at the end of the flow more fluctuations and the peaks of the pressure greater than those prescribed by the curves of Points E and F. This may be explained by the recirculation phenomena observed in the CFD simulation. Fig. 19 shows the distribution of the highest pressure at different points in a radial direction. The maximum pressures in the zone under the y axis are fairly higher than those in the zone above the y axis. This could be related to the turbulence due to the recirculation phenomena which is more important under the y axis.
(2) Stress on the target Fig. 20 shows the Von-Mises stress on the target at different intervals. High stress appears at the center first (Fig.  20a) and then propagates to the zone under the y axis (Figs. 20b and 20c). During impact, the zone localized under the impacted surface is subjected at different states of the stress with relatively low value (Fig. 20d). The variation of the stress state may cause the appearance of star cracks and fa-  I. Ben Belgacem et al. China Ocean Eng., 2019, Vol. 33, No. 1, P. 114-126 tigue effects. Fig. 20e shows that the stress reaches the maximum value equal to 0.18 MPa which corresponds to the stagnation flow.
(3) Displacement on the target Fig. 21 presents the evolution of the displacement components U x , U y and U z after 8×10 -6 s. It seems that the main magnitude of the displacement is coming from the displace-ments U z and U x (U y is nearly zero) unlike the HT where U x does not influence the displacement of the target. The magnitude U takes the maximum value about 0.008 mm at the end of the impact. Fig. 22 presents the magnitude displacement through a radial direction crossing the center of the target for both configurations. It shows that the horizontal target presents the higher displacement and stronger fluctuations compared with the second configuration which presents lower magnitude and smoother fluctuation. Indeed water in the first configuration keeps contact with the target but for the second configuration water finds a way for evacuation faster thanks to the inclination of the target. Fig. 23 presents the maximum displacement versus the time history. The IT shows a smoother shape compared with the HT. The IT presents the maximum value at the end of    the impact equal to 0.008 mm while the HT presents the maximum at about 6×10 -6 s. At the first moment of the impact (3×10 -6 s) a pic of 0.004 mm is shown in the IT. For the HT, the first pic of the displacement of 0.008 mm is observed at 4×10 -6 s. This pic is less acute. This could be explained by the shape of the head of the jet at the first moment of impact. In fact for the HT the head is perfectly flat unlike the IT where the head of the jet is quite punctual due to the inclination of the target. Fig. 24 presents the maximum pressure in radial direction crossing the center for both IT and HT. It shows that the pressure in the centre of the IT is equal to 0.08 MPa while it is a depression equal to about -0.24 MPa for the HT. This gradient of pressure is probably explained by the change of the shape of the stagnation zone previously presented in the velocity profile.

Conclusions
In this paper, numerical simulations of a high velocity water jet impacting a horizontal plate and an inclined plate were carried out under ABAQUS. The plate is a metal sheet of Ti555-03. Its mechanical behavior is handled by the Johnson Cook law. Two points of view are presented for this study. The first one is a CFD study of the jet impacting where it is possible to demonstrate the structure of a free jet and impacting for the two cases of positioning the plate (0°a nd 45°). The second part is devoted to study the FSI by a hybrid method of a finite element modeling for the plate and free mesh method called SPH method to investigate the Von Mises stress, the pressure and the displacement of the target. This result will be useful to investigate and to understand the behavior of a water assistance jet impact during highspeed machining of a Ti555-03 Titanium material in terms of the interaction between the water of assistance and the work piece and tool. Furthermore these results will be useful in a study of tool, workpiece and cutter system.    I. Ben Belgacem et al. China Ocean Eng., 2019, Vol. 33, No. 1, P. 114-126 125