CFD analysis of jet flows ejected from different nozzles

Nozzles are widely used to control the rate of flow, speed, direction, mass, shape and pressure of the stream in connection with many different engineering applications. This paper presents the performance predicted by a computational fluid dynamic (CFD) model, which are 3D models that utilize parametric analysis, realizable k-epsilon turbulence models and experimental measurement for a jet. Jet flows are ejected from three different slot nozzles: round-shaped nozzle, rectangular-shaped nozzle and 2D-contoured nozzle. In this numerical study, velocities of free jets have been predicted for different axial distances from the nozzle exit in the range of 0.2 ≤ z / B ≤ 12 when center velocity at the nozzle exit. CFD simulation results are compared to experimental results from literature. These results are consistent with the existing experiments.


INTRODUCTION
Nozzles are widely used in connection with many different engineering applications, mainly to generate jets and sprays. The nozzle exit flow serves as the initial condition for the downstream flow. Experiments have been conducted with variations of nozzle exit Reynolds number by Yang et al. [1]. They measured developing structures of free jets by hot-wire anemometer to understand the characteristics of heat transfer in conjunction with measured jet flows. In that study, different flow characteristics have been observed depending on different nozzle shapes as in the experimental study implemented.
In most instances, flow non-uniformity and turbulence originate within the nozzle, but the nozzle contraction is generally designed to attenuate and minimize these effects [2].
The jet type flows occur in a variety of applications, especially in the industrial sector. For over a century, the theory of turbulent jets and their practical applications have attracted the specialist's attention in many research fields [3,4].
The capability for Navier-Stokes analysis of exhaust nozzle flow fields has progressed to the point that, for simple nozzle geometries, computational fluid dynamic (CFD) accuracy for performance quantities is comparable to experimental accuracy. The CFD simulation has the advantage that a discrete point approximation to the entire flow field is available [5][6][7][8]. This makes it possible to consider using the CFD solution to investigate a number of important nozzle performance effects that would be extremely difficult to investigate experimentally.
There are relatively few experimental data sets on nozzle thrust performance that are documented in the open literature in sufficient detail to be suitable for purposes of CFD verification. In this paper, the results of an investigation into utilization of scarfed, truncated perfect nozzle for thrust vector adjustment in tactical strap-on boosters are presented.
There is less published literature involving the numerical simulation of flow in nozzles. Yu et al. [2] have performed Reynoldsaveraged Navier-Stokes simulations to investigate the effect of nozzle geometry on the turbulence characteristics of incompressible fluid flow through nozzles at Reynolds number of approximately 50 000. Four nozzles have been considered: a baseline nozzle and three modified nozzles (extended, grooved and ringed). The flow in these nozzles has been simulated using different turbulence closure models, including Spalart-Allmaras, variants of k-ε and k-ω and the Reynolds stress model. Payri et al. [9] and Macian et al. [10] numerically investigated the effect of diesel nozzle geometry on the inception and development of cavitation. Sushma et al. [11] presented the results of an investigation into utilization of scarfed, truncated perfect nozzle for thrust vector adjustment in tactical strap-on boosters. The purpose of Qiang et al.'s [12] study is the development and validation of an internal three-phase flow model of the abrasive water jet with the capability to predict the acceleration of solid particles and the wear of nozzle wall.
Giannadakis et al. [13] developed a CFD cavitation model for diesel injector nozzles based on the Eulerian-Lagrangian approach. They demonstrated that their model can identify many of the cavitation structures present in internal nozzle flows and showed that these structures are dependent on nozzle design and flow conditions.
Nozzles are widely used in many different applications of engineering, especially to generate jets. While designing the nozzles, it was aimed to achieve a low turbulence density at the nozzle outlet. Therefore, this situation has been emphasized in experimental and numerical studies especially on jets. The nozzle exit flow serves as the initial condition for the downstream flow. In most instances, flow non-uniformity and turbulence originate within the nozzle, but the nozzle contraction is generally designed to attenuate and minimize these effects. The objective of this numerical study is to explain jet flow structure ejected from different shaped slot nozzles and to validate with experimental results.
In this sudsy, it is used of model-free simulations to broaden our understanding of some of underlying mechanisms involved in the near field of jet flows originating from different nozzles. Our primary objective is to assess the influence of the nozzle shape on the subsequent evolution of the jet flows and their mixing characteristics. This facilitated by analyzing the processes involved in entrainment. Three nozzles are considered: round-shaped nozzle, rectangular-shaped nozzle and 2D-contoured nozzle.

GEOMETRY AND GRID STRUCTURE
Three different geometries were created for rectangular-shaped nozzle, round-shaped nozzle and 2D-contoured nozzle. General structural for the computational geometries is shown as in Figure 1. Inlet zone was created at a distance of 200 mm before the end point of nozzle exit and dimensions of 60mm × 130mm. B is the jet width.
In the experimental study carried out by Yang et al. [1], measurements were taken up to 100 mm from the nozzle exit. Therefore, the data we received in the simulations had to be taken up to 100 mm accurately. In order to obtain these data, a volume of 100 × 30 × 130 mm, shown in the Figure 1, was applied to the body of influence. The body of influence influences the mesh density of the body that it is scoped to, but it is not be a part of the model geometry nor will it be meshed.
Meshes of the same characteristics were created for three different geometries. Figure 2 shows the specific locations of mesh zones. These locations are Inlet (A), outlet (B) and nozzle walls (C) and the body-of-influence volume (D). Table 1 shows qualities of the inflation zone and the body of influence zone. Inflation was applied to named selection that shown as C (nozzle wall) in Figure 2. Inflation qualities are maximum layers 6, growth rate: 1.1. For the body of influence, growth rate and element size are given as 1.1 and 1 mm, respectively.   Table 2 shows the mesh properties for each type of nozzles. Curvature and proximity qualities were applied for each mesh. In this study, grid independence tests were implemented to determine the optimal number of grids for each nozzle shape. Nozzles are divided into different grid numbers. 5 652 688, 6 102 688 and 5 595 724 elements were used for rectangular-shaped nozzle, round-shaped nozzle and 2D-contoured nozzle, respectively. For proximity qualities, numerical cells across gap were taken to be 6. Other mesh qualities are element size 5 mm, growth rate 1.1 and target skewness 0.8.
Grid structure is given in Figure 3 for different nozzles. When the mesh structure is examined, dense mesh was formed in the area created by body of influence. Inflation layers were formed along the nozzle walls.

Boundary conditions
Velocity inlet was defined by zone shown as A in Figure 2. The values of the velocity inlet were set as parameters. Table 3 shows input parameters and results. In order to compare the experimental results, the velocity-inlet parameter was changed and the results were approximated to the values used in the experimental results. The temperature value is given as 300 K.

COMPUTATIONAL METHODS
The commercial CFD software, Fluent 19.2 [14], is utilized to compute the unsteady 3D incompressible flow. In the general setting of the CFD simulation, solver type and time are selected as pressure based and steady, respectively. In addition, the gravitational acceleration in the Y direction was magnitude of9.81 ms −2 for simulation. In the model setting, firstly energy equations have been activated. Then the k-epsilon model has been selected from the viscous settings and, as a wall function, realizable and standard wall functions are used in k-epsilon models.
In solution methods setting, coupled scheme is applied for pressure-velocity coupling. Coupled algorithm solves the momentum and pressure-based continuity equations together; also this algorithm improves solution convergence rate. Spatial discretization settings, least-squares-cell based and second-order are implemented for gradient and pressure-interpolation-schemes, respectively. Second-order upwind schemes are selected for momentum, turbulent kinetic energy and turbulent dissipation rate. Hybrid initialization is applied and 1000 iterations are defined, solved and converged for each simulation. Each model is converged. The convergence criteria are 10 −6 and 10 −8 for the flow field and energy equations, respectively. Air is used as material and its properties are default. Even if the properties of the air define as ideal gas models or real gas models, the simulations results did not change greatly. For this reason, properties of material were used by default. Properties of air that used for simulation are the following: density, ρ=1.225 kgm −3 ; heat capacity, c p = 1006.43 Jkg −1 K −1 ; thermal conductivity, k = 0.0242 Wm −1 K −1 ; viscosity, μ = 1.7894 × 10 −5 kgm −1 s −1 .

Governing equations
In the current study, the CFD code was used for 3D numerical simulations of fluid flow. The developed model simultaneously solves the mass, momentum and energy conservation equations. Generally, for an incompressible flow, these equations are as follows [5,8]: Turbulent kinetic energy: Turbulent energy dissipation:

RESULTS AND DISCUSSION
CFD results are shown by the variables and values used in the experimental study by Yang et al. [1]. In the experimental study, U j is the exit velocity of the nozzle. B is the width of the nozzle and B = 5 mm. Figure 4 illustrates coordinates where CFD and experimental results are received. The term z/B defines the distance from the nozzle, while the term y/B defines the locations of the data line.  In Figure 5, the velocity distributions for round-shaped nozzle and rectangular-shaped nozzle at U j = 40 ms −1 are experimentally and numerically shown. As can be seen in Figure 5, it is clearly stated that experimental results presented by Yang et al. [1] and numerical results are similar. In the experimental study, the exit speed of the nozzle was taken as 40 ms −1 . In the CFD simulation, parametric analysis was performed for 40 ms −1 convergence of nozzle output speed. As a result of the parametric analysis, the appropriate inlet velocity was determined. The inlet velocity value for the rectangular-shaped nozzle shown in Table 3 Table 3 also shows the results of the 2D-contoured nozzle. Table 3 shows that the velocity-inlet value differs for each nozzle.
For the round-shaped nozzle, there are uniformly distributed velocities along the y/B (width), whereas for the rectangularshaped nozzle it does not seem to be distributed so uniformly. This is clearly seen in the CFD simulation. For the round-shaped nozzle, the speed reduction at y/B = 0 (center line) is less than for the rectangular-shaped nozzle.  In Figure 6, normalized velocity fluctuations, i.e. turbulence intensities, in the widthwise direction for round-shaped nozzle and rectangular-shaped nozzle at U j = 40 ms −1 are experimentally and numerically shown.
As shown in Figure 7, the numerical results are similar to the experimental results for all nozzle shapes, particularly at some values of z/B. The maximum turbulence intensity in the centerline for a rectangular shaped is observed experimentally and numerically at z/B = 12. Turbulence intensities at this point are about 9% and 10.5% experimentally and numerically, respectively. The maximum turbulence intensity in the centerline for a round shaped are 8% for numerically and 10% for experimentally.
The lowest turbulence intensity in the centerline for a rectangular shaped is observed at z/B = 0.2. Turbulence intensities obtained at this point experimentally and numerically are about 2% and 4%, respectively. Figure 7 shows the axial variations of jet flows along the centerline for three different nozzles with the increase of axial distance from nozzle exit in the range of at 0 < z/B < 20 at U j = 40 ms−1as experimentally and numerically.
For round-rectangular nozzle, the experimental and numerical results were very close for all z/B values. For round-shaped nozzle and 2D-contoured nozzle, the experimental and numerical results were very close to each other at 0 ≤ z/B ≤ 5 and 14 ≤ z/B ≤ 20. However, at other z/B ranges, deviations have occurred.

CONCLUSION
Despite some differences, experimental results and numerical results gave appropriate results. These differences can be explained as follows: In the experimental study, air passes through the blower, valve and settling chamber and the flow is made uniform and emerges from the nozzle. The equipment used in the experimental study was adjusted according to the nozzle types so that the nozzle output speed (U j ) could be 40 ms −1 . The flow rate of the uniform flow was varied for different nozzle types. In the CFD study, the flow is defined as uniform in the inlet region.
In addition, in the experimental study, measurements were made by taking time averages in a certain region of the experimental setup. In numerical analysis, the correct use of these measured values is not suitable for CFD algorithm. In any region, parametric analysis should be performed in accordance with the CFD algorithm to obtain the results measured by time averaging. The results found in the experimental study should be convergent in CFD.
Numerical investigations are carried out by comparing experimental results by Yang et al. [1] for three different nozzles. These simulations indicate that these studies can be performed easily with CFD. Numerical values are generally consistent with the experimental results. However, some deviations are observed. Also, as a result of these simulations, it has been seen that certain changes in nozzle geometry can result in major changes to the operating conditions of the nozzle, and this can have significant impact on flow characteristics.