Analysis of Geometric Parameters of the Nozzle Orifice on Cavitating Flow and Entropy Production in a Diesel Injector

Abstract

In this chapter, we investigated the effect of geometric parameters of the nozzle orifice on cavitating flow and entropy production in a diesel injector. Firstly, we analyzed the effect of some parameters of diesel injector such as the nozzle length and the lip rounding on cavitating flow. In the second parts, we studied the entropy production inside the diesel injector in several cases: -single phase and laminar flow,- single phase and turbulent flow and –tubulent cavitating flow. In the last case, the mixture model cupled with k-ε turbulent model has been adopted. The effects of average inlet velocity and cavitation number on entropy production have been presented and discussed. The results obtained show that the discharge coefficient is weakly influenced by the length of the orifice and the radius of the wedge has a large effect on the intensity and distribution of cavitation along the injection nozzle. On the other hand, the study of entropy production inside the diesel injector shows that the entropy production is important near the wall and increases whith increasing the average inlet velocity and pressure injection.

1. Introduction

The fuel flow through injector nozzles affects the spray formation, the atomization phenomenon of the liquid fuel and, therefore, the efficiency of the combustion process and pollutant emission. Modern passenger cars and trucks use higher injection pressures than early models to improve the atomization of fuel in order to reduce soot emission of internal combustion engines. Diesel engine injectors often operate at injection pressures about 2000 bar. The high injection pressure and the abrupt change of the orifice section of the injector allows to have a pressure drop below the saturated vapor pressure and consequently the development of cavitation. Cavitation has a great effect on both the fuel injection process and the performance of an engine. Cavitation generated at the entrance of the orifice affects the fluid flow and the atomization of the injected liquid jet [1, 2, 3]. Cavitation is often observed in pumps, inducers, hydraulic turbines, propellers, fuel injectors, and other fluid devices [4, 5]. However, cavitation has positive effects in some biomedical and industrial applications such as shock wave lithotripsy, water disinfection and organic compounds decomposition, etc. [6, 7].

The study investigation of cavitation phenomenon in the injection orifice is useful even important to control and optimize the atomization process.

The high injection pressure (> 2000 bar), the high speed flow [8] and the small dimensions of the injection nozzle make the studies experimental. In addition, experiments were performed on large-scale and transparent injector configurations to visualize the phenomenon of cavitation [3, 9, 10, 11, 12, 13, 14, 15].

Confronted with experimental difficulties, several theoretical and numerical studies have been developed to study this cavitation problem in a real diesel injector [16, 17, 18, 19, 20, 21, 22]. In a previous study [17], we studied numerically, using the mixing model, the effect of the wall roughness of the orifice injection on the cavitation phenomenon. In another work [23], we studied the effect of inlet corner radius of orifice injection on the flow characteristic and the development of cavitation. We noticed a reduction in the intensity of cavitation when corner radius increases.

The relative risk of erosion of the inner wall of the diesel injector orifice due to cavitation has been studied by [16, 22]. Xue et al. studied the effect of cavitation in a multi-hole injector on the transient flow characteristic in a 3D asymmetric configuration using a two-phase (liquid–vapor) model [21]. The effect of the needle lift was analyzed by these authors. They showed a difference in velocity profile and cavitation within the holes.

Torelli et al. [24] performed a 3D simulation in a five-hole diesel mini-injector to model the internal flow of the nozzle using three types of fuel (full-range naphtha, light naphtha and n-Dodecane). They have show that the cavitation is strongly related to the saturating vapor pressure of different fuel.

In this chapter, we aim to investigate the cavitating flow inside a Diesel injector using the mixture model and taking into account the turbulence. A parametric analysis of the size and the shape of the injector is carried out. The entropy production inside the diesel injector in several cases: -single phase and laminar flow,- single phase and turbulent flow and –tubulent cavitating flow is analyzed. Furthermore, the flow is simulated in the steady state as well as in the unsteady state.

2. Theoretical model

In this mixture model, the fluid (fuel) is composed of three phases: liquid, vapor and non-condensable gases (CO) which the mixture density is given by [25].

$${\rho }_m={\alpha }_v{\rho }_v+{\alpha }_g{\rho }_g+\left(1-{\alpha }_v-{\alpha }_g\right){\rho }_l$$E1

where $\rho$ is the density and α is the volume fraction. The indices l, v and g denote the liquid, vapor and gas phases, respectively.

The mass fraction f_i can be calculated from this equation

$$f_i=\frac{{\alpha }_i\times {\rho }_i}{{\rho }_m}$$E2

The transport equations describing the cavitating flow inside the diesel injector are:

• Navier Stokes equations for the mixture

• k-ε turbulence model

• Transport equation of vapor fraction

2.1 Multiphase model

In this work, the following hypotheses are adopted:

• The mixture is assumed to be single-phase;

• The flow is assumed to be isothermal and incompressible;

• The fluid is Newtonian;

• The gravity force is neglected

The mass conservation equation of the mixture flow is [17]:

$$\frac{\partial }{\partial t}\left({\rho }_m\right)+\nabla .\left({\rho }_m{\overrightarrow{U}}_m\right)=0$$E3

where ${\overrightarrow{U}}_m$ present the velocity of the mixture.

The mixture momentum conservation equation is [17]:

$$\frac{\partial }{\partial t}\left({\rho }_m{\overrightarrow{U}}_m\right)+\nabla .\left({\rho }_m{\overrightarrow{U}}_m\otimes {\overrightarrow{U}}_m\right)=-\nabla p+\nabla .\left[\left({\mu }_t+{\mu }_m\right)\left(\nabla {\overrightarrow{U}}_m+{\left(\nabla {\overrightarrow{U}}_m\right)}^T\right)\right]$$E4

where μ_m is the laminar viscosity of the mixture and ${\mu }_t={\rho }_m{C}_{\mu }\frac{k^2}{\epsilon }$ is the turbulent viscosity. C_μ = 0.09, k is turbulent kinetic energy, ε is the dissipation rate.

It should be noted that the liquid and the vapor have the same velocity ${\overrightarrow{U}}_m$. Since the liquid is incompressible, we obtain $\mathit{div}\left({\overrightarrow{U}}_m\right)=0$. On the other hand, for the steady flow, the continuity equation becomes$\mathit{div}\left({\rho }_m{\overrightarrow{U}}_m\right)=0$.

2.2 k-ε turbulence model

Several experimental investigations have shown that turbulence has a significant effect on cavitating flows (e.g. [26]). Also, [27] studied the sensitivity of the cavitating flows to turbulent fluctuations. For the present computations, we use the standard k-ε turbulence [17, 23]:

$$\frac{\partial }{\partial t}\left({\rho }_{m}k{\overrightarrow{U}}_m\right)+\nabla .\left({\rho }_{m}k{\overrightarrow{U}}_m\right)=\nabla .\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_k}\right)\nabla k\right]+P-\mathit{\rho \epsilon }$$E5

$$\frac{\partial }{\partial t}\left({\rho }_m\epsilon {\overrightarrow{U}}_m\right)+\nabla .\left({\rho }_m\epsilon {\overrightarrow{U}}_m\right)=\nabla .\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_{\epsilon }}\right)\nabla \epsilon \right]+C_{1\epsilon }\frac{ϵ}{k}P-C_{2\epsilon }\frac{{ϵ}^2}{k}$$E6

where P is the production term of turbulent kinetic energy given by:

$$P={\mu }_t\left[\left(\nabla U_m\right)+{\left(\nabla U_m\right)}^{\mathrm{T}}\right]\nabla U_m$$E7

The standard values of the constants are: σ_k = 1.0, σ_ε = 1.3, C_1ε = 1.44 and C_2ε = 1.92 [17].

2.3 Cavitation model

According to [17, 28], the differential equation describing the transport of the vapor fraction is given by

$$\frac{\partial }{\partial t}\left({\rho }_m{ƒ}_v\right)+\nabla .\left({\rho }_m{\mathrm{ƒ}}_v{\overrightarrow{U}}_v\right)={\mathrm{R}}_{\mathrm{e}}-R_c$$E8

Here R_e and R_c denote the evaporation and condensation rates, respectively. The rates R_e and R_c depend on the static pressure and the velocity as well as on the fluid properties. They depend also on the pressure fluctuations generated by the turbulence as well as on the turbulent kinetic energy k.

The following relations are usually adopted to express the rates R_e and R_c [29].

$$R_e=C_e\frac{\sqrt{k}}{\sigma }{\rho }_{\ell }{\rho }_v{\left(\frac{2}{3}\frac{p_v-p}{{\rho }_l}\right)}^{1/2}\left(1-{\mathrm{ƒ}}_v-{\mathrm{ƒ}}_g\right)p\le \mathit{pv}$$E9

$$R_c=C_c\frac{\sqrt{k}}{\sigma }{\rho }_{\ell }{\rho }_v{\left(\frac{2}{3}\frac{p-p_v}{{\rho }_l}\right)}^{1/2}{\mathrm{ƒ}}_v\mathrm{p}>\mathrm{pv},$$E10

where C_e = 0.02 and C_c = 0.01 are calibration constants, f_v and f_g are vapor mass fraction and non-condensable gas mass fraction. The phase-change threshold pressure p_v is estimated from the following equation [17]:

$$p_v=p_{\mathit{sat}}+\frac{p_t}{2}$$E11

where p_sat present the vapor saturation pressure and p_t = 0.39ρ_mk is the turbulence pressure [17]. The above relations show that the evaporation and condensation happen at the vapor pressure p_v and not at the saturation pressure p_sat as in laminar flows. The diffusion phenomenon between phases is neglected.

2.4 Entropy production

Taking into account the following assumptions:

• The slip velocity between the two phases is negligible;

• The diffusion of species through the interface is ignored

The entropy production rate for the mixture is then written [30]:

$${\overline{\dot{P}}}_{\mathit{sm}}=\frac{1}{T}\left({\mathrm{\Phi }}_{\mathit{\mu m}}+{\mathrm{\Phi }}_{\mathit{tm}}+{\mathrm{\Phi }}_{\mathit{Dm}}\right)$$E12

where ${\mathrm{\Phi }}_{\mathit{\mu m}}$ is the average entropy production for the mixture, ${\mathrm{\Phi }}_{\mathit{tm}}$ is the entropy generation due to turbulent shear stress and ${\mathrm{\Phi }}_{\mathit{Dm}}$ is the entropy production due to the turbulent dissipation term.

The mean of the entropy production and the entropy production due to the turbulent shear stress can be written as follows [30]:

$${\mathrm{\Phi }}_{\mathit{\text{effm}}}={\mathrm{\Phi }}_{\mathit{\mu m}}+{\mathrm{\Phi }}_{\mathit{tm}}={\mu }_{\mathit{\text{effm}}}\left[\left(\nabla .⟨{\overrightarrow{U}}_m⟩+{\left(\nabla .⟨{\overrightarrow{U}}_m⟩\right)}^{\mathrm{T}}\right):\nabla .⟨{\overrightarrow{U}}_m⟩\right]$$E13

where ${\mu }_{\mathit{\text{effm}}}=\left({\mu }_m+{\mu }_{t_m}\right)$ is the effective viscosity of the mixture.

In a two-dimensional flow in an injection orifice, the entropy production in cylindrical coordinates (2D) is then written [30]:

$${\overline{\dot{P}}}_{\mathit{sm}}=\frac{{\mu }_{\mathit{\text{effm}}}}{T}\left[2\left({\left(\frac{\partial u_m}{\partial r}\right)}^2+{\left(\frac{u_m}{r}\right)}^2+{\left(\frac{\partial v_m}{\partial z}\right)}^2\right)+{\left(\frac{\partial u_m}{\partial z}+\frac{\partial v_m}{\partial r}\right)}^2\right]+\frac{{\rho }_m\overline{{\epsilon }_m}}{T}$$E14

3. Numerical method and nozzle geometry

To simulate the cavitating flow, the numerical code Fluent was used. This code is based on implicit finite volume scheme. The SIMPLE algorithm [31] is used for the pressure–velocity coupling. Grid generation process for performing finite volume simulations were carried out using GAMBIT (v2.3.16) program available with the commercial code Fluent. A first order implicit temporal discretization and a first order upwind differentiating scheme have been used. All under-relaxation factors range between to 0.2–0.4.

3.1 Nozzle geometry and boundary conditions.

Figure 1 illustrates the nozzle geometry of diesel injector in 2D axisymmetric. The geometric parameters of the nozzle are R₁ = 0.3 mm, R₂ = 0.1 mm and L₁ = 0.5 mm. The transition radius between inlet pipe and orifice is r_c.

Figure 1.

2D-axisymmetric configuration of the diesel injector with boundary conditions.

In this study, a stationary single phase fluid is assumed as initial conditions. Uniform inlet and outlet static pressure were adopted as boundary conditions. A value of k₀ and ε₀ are imposed at the inlet.

3.2 Effect of the grid resolution

the mesh presents an essential parameter in fluid mechanics problems for the convergence of the solution. The existence of an important gradient of the physical (pressure, velocity and vapor fraction) requires a concrete study of the sensitivity of the mesh on the solution. The mesh sensitivity on the solution was studied under the following injection conditions: inlet pressure p_in = 5 bar and outlet pressure p_out = 1 bar.

The mesh grid is adapted several times (six times: see Table 1). In Table 1, n and m represents the number of meshes according to z and r axis in the orifice.

Mesh	0	1	2	3	4	5
n × m	5x30	10x50	15x80	20x110	25x140	30x160

Table 1.

Meshes tested in the simulation.

where n and m are the number of meshes according to z and r axis in the orifice.

The mesh effect on the local field (e.g the pressure field) and on the global coefficient (e.g discharge coefficient) along the wall of the nozzle is presented in Figure 2(a,b). Figure 2(a), indicates the pressure field distribution along the near wall at the orifice for several grids resolutions. It is clear that the local minimum pressure is strongly affected by the mesh size. The local pressure near the wall decrease with mesh size until it reaches a minimum value lower than the vapor saturation pressure.

Figure 2.

Pressure profile near the wall using different mesh and b-mass flow rate and discharge coefficient for several grid resolutions.

In this region, the cavitation phenomenon appears. According to Raleigh-Plesset Equation [32], cavitation is governed by the local pressure. The effect of mesh on the masse flow rate and discharge coefficient is presented in Figure 2b(i & ii). We notice a variation in the discharge coefficient C_d with the mesh. For example, C_d undergoes a variation of 1.6% going from 1 to 4 and then remains constant. Mesh N°3 can be used for simulation.

4. Results and discussions

4.1 Steady flow

In this part, we study the effect of geometric parameters such as L₂/d₂, r_c/d₂ ratios and Reynolds number Re on the cavitation phenomenon in steady state.

4.1.1 Influence of the Nozzle length

The pressure drop in the injector is described by the discharge coefficient C_d that is the ratio of the effective mass flow rate to the theoretical maximum flow rate:

$$C_d=\frac{{\dot{m}}_{\mathit{eff}}}{{\dot{m}}_{\mathit{\text{ideal}}}}$$E15

where ${\dot{m}}_{\mathit{eff}}=\iint {\rho }_m{\overrightarrow{v}}_m.\overrightarrow{\mathit{dA}}$ is the effective mass flow rate and ${\dot{m}}_{\mathit{\text{ideal}}}=\pi R_2^2\sqrt{2{\rho }_l\left(p_{\mathit{\text{in}}}-p_{\mathit{\text{out}}}\right)}$ is the ideal flow rate.

Figure 3 shows the distributions of vapor volume fraction for several nozzle lengths (p_in = 10 bar and p_out = 1 bar). The latter (nozzle lengths) has a significant effect on the cavitation area. The cavitation region decreases when the length of nozzle increases.

Figure 3.

Contour of vapor volume fraction for several nozzle lengths.

We perceive a transition on the cavitation nature from fully developed cavitation (for L₂ = d₂ or 2d₂) to incipient cavitation (for L₂ > 2d₂).

For a length L₂ ≤ 0.6 mm, cavitation still takes place and occupies a large part of the orifice. Cavitation is highly developed in this situation. However for L₂ ≥ 0.6 mm, the cavitation remains very confined. It is useful to also examine the effect of length at high injection pressures and taking into account the presence of the combustion chamber.

Figure 4, shows the discharge coefficient C_d as a function of L₂/d₂ ratio for a nozzle with r_c/d₂ = 0. it is clear that the discharge coefficient varies linearly with the L₂/d₂ ratio. When the L₂/d₂ ratio increases from 2 to 8, we notice a reduction of 13% in C_d. The discharge coefficient is weakly dependent on the length of the orifice which can be explained by the dominance singular pressure losses generated at the entrance over regular pressure drops provoked by wall friction. These results have been shown experimentally [33] and numerically [34].

Figure 4.

Discharge coefficient C_d as a function of L₂/d₂ ratio.

For the low values of Re, we must take into account the linear and singular pressure losses.

4.1.2 Influence of the lip rounding

Figure 5 shows the distribution of the vapor volume fraction for different values of r_c and for inlet pressure p_in = 50 bar and L₂/d₂ = 5. Figure 5 shows the important effect of rc on the creation of cavitation within the injector. When r_c = 0, cavitation develops over almost 1/3 the nozzle length and the cavitation zone extends to the combustion chamber. The cavitation area attached to the wall will be reduced by increasing the r_c radius.

Figure 5.

Distribution of vapor fraction for several radius r_c with inlet pressure p_in = 50 bar and p_out = 1 bar.

In order to study the effect of r_c/d₂ ratio on the flow characteristics, the discharge coefficient is calculated for two values of Reynolds number Re and for L₂/d₂ = 5 (Figure 6).

Figure 6.

Discharge coefficient as a function of rc/d2 ration for Re = 2 × 10³ and Re = 6.8 × 10³.

There are two zones: the first zone for r_c/d₂ < 0.1 and the second zone for r_c/d₂ > 0.1. In the first zone, the coefficient of discharge varies linearly with inlet roundness for the two values of Re.

In the second zone, the discharge coefficient remains constant for any value of r_c/d₂. This result is consistent with the literature [35, 36].

4.2 Transient flow

In this section the transient simulations results are presented. Figure 7 represents the evolution of vapor volume fraction at different times for L₂/d₂ = 5. The inlet corner radius r_c is equal to zero. The injection pressure p_in = 1000 bar and the exit pressure p_out = 50 bar.

Figure 7.

Transient evolution of vapor volume fraction.

The cavitation appears in the vicinity of the sharp edge for a time of the order of 0.6 μs. Then, the cavitation pocket elongates progressively through the orifice and reaches the nozzle exit at t = 3 μs. This result agrees well with the numerical simulation obtained by Dumont et al. [37] in a similar injector and by experimental visualization and measurements Ohrn et al. [33].

Figure 8 depicts the axial profile of the mixture density near the wall at t = 1.5 μs and t = 3.8 μs. Upstream of the corner the fluid is at liquid state.

Figure 8.

Mixture density profile at t = 1.5 μs and t = 3.8 μs near the nozzle wall.

At the sharp edge, the density exhibits an important decrease due to the pressure drop and the appearance of cavitation. In this region, the mixture density contains mainly fuel vapor.

Downstream the corner, the mixture density increases and the vapor fraction decreases, owing to the collapse and the breakup of the cavitation along the orifice.

At the nozzle exit, the cavitation is present for t = 3.8 μs and therefore the mixture density is smaller than the liquid density ρ_l. Thus the spray that leaves the injector and penetrates into the combustion chamber is formed not only by fuel liquid but also by fuel vapor.

4.3 Entropy production

The entropy generation is a measure of the degree of irreversibility. It is a method for optimizing thermal and fluidic systems. It could be agreed for specific applications.

4.3.1 Case of single phase and laminar flow

4.3.1.1 Mesh sensitivity

In this part, we study the effect of the mesh on the axial component of the velocity field. The studied geometry is discretized in n × m meshes of rectangular shape. The calculation is carried out using Ansys software based on the finite volume method.

In order to assess the accuracy of the numerical method, we performed several studies based on systematic mesh refinement until there were negligible changes in the variation of the axial velocity. Table 2 present the different mesh used in this simulation for single phase laminar flow inside the diesel injector and for two Reynold values Re = 381 and 1000, respectively.

Mesh	Mesh number (Re = 381)	Mesh number (Re = 1000)
Mesh 1	61	457
Mesh 2	137	1445
Mesh 3	391	5789
Mesh 4	1453	23156

Table 2.

Mesh used in this simulation.

Figure 9(a,b) shows the axial velocity profile for different mesh and for two Reynolds number Re = 381 and 1000, respectively. From this figure, the axial velocity exhibits oscillations for the first and the second mesh. This oscillation shows that the solution is not stable and that convergence has not yet been achieved. The last mesh (1453 meshes) seems the best since it shows that convergence has indeed been achieved.

Figure 9.

Axial velocity profile for several mesh and for two values of Re = 381 (left) and Re = 1000 (right).

4.3.1.2 Entropy production

Figure 10 shows that the entropy generation increases from zero at the center of the channel to a maximum value on the wall. This trend indicates that the maximum entropy produced on the wall is mainly due to the irreversibility of fluid friction contributed by the wall velocity gradient near top while towards the center of the channel with zero velocity gradient, the generation of entropy due to friction of the fluid.

Figure 10.

Local entropy profile inside the orifice for different values of average inlet velocity v₀ = 0.1, 0.325, 0.55 et 1 mm/s.

The total entropy is obtained by taking the integral of the local entropy over the total volume, given by the following expression:

$$S_{\mathit{tot}}=∰\mathit{SdV}$$E16

Figure 11 illustrates the total entropy as a function of the inlet injection velocity v0. Its clear that the total entropy production varies quadratically with the inlet velocity.

Figure 11.

Evolution of total entropy production as a function of inlet velocity.

The interpolation in Lagrange polynomial of degree 2 of S_tot as a function of inlet velocity $v_0$:

$$S_{\mathit{tot}}\left(\mathit{nW}/K\right)=C_0+C_1\times v_0+C_2\times v_0^2$$E17

where C₀ = 0.0078 nW/K, C₁ = -0.08 nW.s/K.m and C₂ = 10.4 nW.s²/K.m².

4.3.2 Case of single phase and turbulent flow

The same geometry already seen in the previous part will be used in this part. However, the flow will be considered turbulent. The main objective of this study is to simulate the entropy generation within the injector for high injection pressure taking into account the turbulent behavior of the flow. The mathematical model used consists of the Navier–Stokes equations coupled with the k-ε turbulence model taking into account the following assumptions:

• Steady flow;

• Incompressible fluid;

• Newtonian fluid;

• Isothermal flow.

Water with a density ρ = 1000 kg/m³ and a dynamic viscosity μ = 10⁻³ Pa.s is used as a fluid.

For the velocity field and the pressure, the same boundary conditions that will be used previously at the inlet and outlet of the injector. On the other hand, at the level of the walls we use a wall law.

For the k-ε turbulence model, the boundary conditions used are as follows:

• On the axis of symmetry (r = 0)

$$\frac{\partial k}{\partial r}=0\mathit{et}\frac{\partial \epsilon }{\partial r}=0$$E18

• At the inlet

$$l=C_{\mu }\frac{k^{3/2}}{\epsilon }\approx 3.8\%D_h$$E19

$$I=0.16{\left(\mathit{Re}\right)}^{-1/8}$$E20

• At the outlet

$$\overrightarrow{n}.\overrightarrow{\mathit{grad}}k=0,\overrightarrow{n}.\overrightarrow{\mathit{grad}}\epsilon =0$$E21

In order to assess the accuracy of the numerical method, we performed an automatic adaptive mesh refinement. The mesh adaptation is done automatically in areas with a significant gradient (pressure, velocity, turbulent kinetic energy, kinetic energy dissipation rate).

Figures 12–15 illustrate the radial profiles of local entropy within the orifice for different axial positions. Figures 12(a)–15(a) show the radial entropy profiles which arise from dissipation due to the mean flow movement for various inlet velocity u₀ ranging from 10 m/s to 60 m/s. The logarithmic representation of the average viscous dissipation is shown in Figures 12–15. For such a single-phase viscous flow, which is both laminar and turbulent, the viscous dissipation is a function of the velocity gradient. Near the wall vicinity, the velocity gradient has a maximum value. Axially, the local entropy is important at the entrance of the orifice where the velocity gradient is important. We also notice that laminar entropy increases considerably with the inlet volocity.

Figure 12.

Radial entropy profile at different position along the z-axis for inlet velocity v₀ = 10 m/s. (a) Laminar entropie, (b) turbulent entropie et (c) total entropy.

Figure 13.

Radial entropy profile at different position along the z-axis for inlet velocity v₀ = 30 m/s. (a) Laminar entropie, (b) turbulent entropie et (c) total entropy.

Figure 14.

Radial entropy profile at different position along the z-axis for inlet velocity v₀ = 50 m/s. (a) Laminar entropie, (b) turbulent entropie et (c) total entropy.

Figure 15.

Radial entropy profile at different position along the z-axis for inlet velocity v₀ = 60 m/s. (a) Laminar entropie, (b) turbulent entropie et (c) total entropy.

Figures 12(b)–15(b) show the irreversibility due to the Reynolds shear stress resulting from the velocity fluctuation. This irreversibility can also be interpreted as the work done by force in the direction of the flow. From Figures 12(a,b)–15(a,b), we can conclude that the entropy due to shear stress is dominant.

Figures 12(c)–15(c) illustrate the radial profiles of the total local entropy (laminar entropy and turbulent entropy) for different axial positions. As it is clear, the total entropy is important at the level of the constriction zone having a large velocity fluctuation.

Figure 16 show the local entropy distribution inside the orifice for various inlet velocity 10, 30, 50 and 60 m/s, respectively.

Figure 16.

Total entropy distribution for various inlet velocities vo = 10, 30, 50 and 60 m/s. the results are presented in logarithmic decimal scale.

It is clear that the entropy is maximum in the vicinity of the wall at the contraction zone having a large velocity gradient. The greater the injection velocity, the more the irreversibility zone spreads out.

Figure 17 illustrates the total entropy as a function of the inlet injection velocity v₀. Its clear that the total entropy production varies quadratically with the inlet velocity.

Figure 17.

Evolution of total entropy production as a function of inlet velocity.

The interpolation in Lagrange polynomial of degree 2 of S_tot as a function of inlet velocity $v_0$:

$$S_{\mathit{tot}}\left(\mathit{MW}/K\right)=C_0+C_1\times v_0+C_2\times v_0^2$$E22

where C₀ = 0.29 MW/K, C₁ = -0.037 MW.s/K.m and C₂ = 0.0012 MW.s²/K.m².

4.3.3 Case of two-phase turbulent cavitating flow

Our study is based on the same configuration seen in the previous sections to study the entropy generation. In fact, in this part we take into account the effect of cavitation within the orifice of the diesel injector. This will allow us to make an exhaustive study of the topology of the flow associated with the cavitation that has appeared in the injector. For this, we take into account the homogeneous mixture approach for the modeling of two-phase flows. The fluid used in this study is therefore water, the properties of which are illustrated in the following Table 3.

	liquid	vapor
Density (kg/m^3)	1000	0.02558
Dynamic viscosity (kg/m-s)	0.001	1.2610^−6
Surface tension (kg/s^2)	0.0717	—
Vapor pressure (Pa)	3540	—

Table 3.

Water properties.

To analyze entropy generation within the injector, we have studied the effect of the injection pressure. In this case, simulations were carried out for inlet pressure varying between 1.9 bar and 1000 bar and for a fixed downstream pressure of 0.95 bar. Figure 18 illustrates the vapor fraction and local entropy distributions inside the injector for various values of cavitation number K.

Figure 18.

Distribution of vapor fraction (left) and entropy (right) for various cavitation number values.

We notice from Figure 18 (left) that the state of the fluid changes as it enters the orifice and as the injection pressure is increased. The change in the fluid state is due to the cavitation phenomenon that is created for a significant local depression. The 2D results for the vapor fraction show that cavitation is triggered when K ≈ 1.45 confirms the previous results.

In the center of the orifice, the fluid is formed by a dense core of fluid (liquid) and a dispersed phase (vapor), which is analogous to the experimental results of Yan and Thorpe [38]. For high injection pressures, the cavitation zone extends to the outlet leading to the formation of the hydraulic flip.

According to the results of Figure 19 (right) show the local entropy distribution for different K values. It is clear that the entropy generation takes place near the orifice edge with a very high intensity. These results can be explained by the effect that near the wall, the radial component is important. Thus, the low pressure zone essentially gives rise to the formation of bubbles and the recirculation zone is very limited. The velocity gradient in the recirculation zone is very important causing viscous effects. This trend indicates that the maximum entropy produced near the edge of the orifice is mainly due to the irreversibility of fluid friction contributed by the velocity gradient due to the abrupt change of injector section.

Figure 19.

Total entropy production in decimal logarithm as a function of cavitation number K.

For z ≥ D₁, the flow is strongly developed. The turbulent velocity components promote the transfer of momentum between adjacent layers of the fluid and tend to reduce the average velocity gradient and subsequently a decrease in the degree of irreversibility.

Figure 19 shows the evolution of total entropy as a function of the number of cavitation K. These results prove that the degree of irreversibility is proportional to the injection pressure. For high injection pressures, entropy production is important.

5. Conclusion

A numerical simulation of the phenomenon of cavitation in a 2D-axisymmetric configuration of a diesel injector nozzle has been presented. A turbulent mixture model has been adopted to simulate the multiphase flow. The study is carried out in two regimes, namely stationary and transient. The effect of the geometric parameters of the injector (e.g orifice length and the corner radius) on the cavitation phenomenon inside the nozzle has been studied.

Unsteady simulations have also been carried out. The space–time evolution of the vapor fraction is analyzed.

In the other hand, the entropy production inside the diesel injector is analyzed. Firstly, the local entropy distribution in the orifice is studied for a single phase and laminar flow under several average inlet velocity. In the second part, we analyzed the entropy production for a single phase and trubulent flow. In the same way, the effet of average inlet velocity on the entropy production is studied. Finally, the entropy production is studied for two-phase, turbulent and cavitating flow. In this case, the effet of cavitation number on local entropy production in the orifice is analyzed.

The main conclusions from the present study can be summarized as follows:

1. The study shows that the discharge coefficient is weakly influenced by the length of the orifice, especially for high injection pressures. However, the radius of the wedge has a large effect on the intensity and distribution of cavitation along the injection nozzle.

2. It appears that the spray leaving the orifice and entering into the combustion chamber contains liquid and vapor. Hence, the cavitation is expected to have an effect on the atomization and the combustion processes.

3. The entropy production is important near the wall and increases whith increasing the average inlet velocity.

4. The turbulent entropy production dominates over laminar entropy production for a single phase and trubulent flow.

5. The maximum local entropy production is localized near the wall at the entrance of the orifice.

6. The numerical results shows the increase of total entropy generation by increasing the injection pressure.