Degree project in Materials Science and Engineering Second cycle, 30 credits
Numerical and experimental
investigation of multiple gas jet flow behaviour in the gas
atomization process
MAHSA DARVISHGHANBAR
Stockholm, Sweden 2022
i
Abstract
In several industrial applications, the interaction of supersonic gas jets is encountered such as gas atomization, jet engines and the basic oxygen furnace process. In the gas atomization process, high pressure gases are converted to high velocity gas jets through convergent- divergent nozzles. These high velocity gas jets break up the stream of the molten metal into fine droplets. Therefore, it is essential to develop a deep knowledge of interaction between the gas jets and the liquid metal and the dynamics of jets as a step towards optimizing the gas atomization process. This will enable higher process efficiency at lower cost and energy consumption.
In this study, the gas interaction behaviour of the two gas jets from two convergent-divergent nozzles with the same geometry have been modelled using Ansys Fluent software. The result of the computational fluid dynamics simulation has been also compared with an experimental study that has been done under similar conditions to the simulation.
The results of this study have shown that, by decreasing the nozzle interaction angle the maximum velocity along the symmetry axis will be increased. However, according to the velocity contour plots the maximum velocity when the gas interaction angle is 20°, 5° and 0°, the maximum velocity reached to 676 m s-1, 698 m s-1 and 696 m s-1 respectively.
In addition, it was found that the maximum value of the jet velocity along the symmetry axis decreases with an increase in distance between the nozzles. However, according to the velocity contour plots for the 18mm, 10mm and 5mm distance between the nozzles the maximum velocity reached to 696 m s-1, 685 m s-1 and 683 m s-1 respectively. In general, when the gas jets have higher velocity, they have higher kinetic energy to disintegrate the stream of the molten metal. Therefore, higher gas jet velocity leads to powder with smaller particle size.
The results of this study can be used to design better nozzles configuration in gas atomization process in order to achieve better process efficiency. Moreover, the finding of this study will help to build more complex simulations with more nozzles in the model.
ii
Sammanfattning
I flera industriella tillämpningar påträffas samspelet mellan överljudsgasstrålar, såsom gasförstoftning, jetmotorer och den grundläggande syrgasugnsprocessen. I gasatomiseringsprocessen omvandlas högtrycksgaser till höghastighetsgasstrålar genom konvergenta divergerande munstycken. Dessa gasstrålar med hög hastighet bryter upp strömmen av den smälta metallen till fina droppar. Därför är det viktigt att utveckla en djup kunskap om interaktionen mellan gasstrålarna och den flytande metallen och dynamiken hos strålarna som ett steg mot att optimera gasatomiseringsprocessen. Detta kommer att möjliggöra högre processeffektivitet till lägre kostnad och energiförbrukning. I denna studie har gasinteraktionsbeteendet för de två gasstrålarna från två konvergent-divergerande munstycken med samma geometri modellerats med hjälp av Ansys Fluent-programvara. Resultatet av simuleringen av beräkningsvätskedynamik har också jämförts med en experimentell studie som har gjorts under liknande förhållanden som simuleringen. Resultaten av denna studie har visat att genom att minska munstyckets interaktionsvinkel kommer den maximala hastigheten längs symmetriaxeln att ökas. Enligt hastighetskonturen plottas emellertid den maximala hastigheten när gasinteraktionsvinkeln är 20°, 5° och 0°, den maximala hastigheten nådde 676 ms - 1 , 698 ms -1 respektive 696 ms -1. Dessutom fann man att det maximala värdet för strålhastigheten längs symmetriaxeln minskar med en ökning av avståndet mellan munstyckena. Enligt hastighetskonturdiagrammen för 18 mm, 10 mm och 5 mm avståndet mellan munstyckena nådde den maximala hastigheten till 696 ms - 1 , 685 ms -1 respektive 683 ms -1. I allmänhet, när gasstrålarna har högre hastighet, har de högre kinetisk energi för att sönderdela strömmen av den smälta metallen. Därför leder högre gasstrålehastighet till pulver med mindre partikelstorlek. Resultaten av denna studie kan användas för att utforma bättre munstyckeskonfiguration i gasatomiseringsprocessen för att uppnå bättre processeffektivitet.
Dessutom kommer resultatet av denna studie att bidra till att bygga mer komplexa simuleringar med fler munstycken i modellen.
iii
Contents
Introduction ... 1
1.1 Aims and objective ... 2
1.2 Scope ... 2
1.3 Delimitation ... 3
1.4 Environmental and ethical consideration ... 3
Theoretical background ... 4
2.1 Powder production techniques ... 4
2.2 Water atomization ... 4
2.3 Gas atomization ... 5
2.3.1 Free-fall gas atomization process ... 5
2.3.2 Close-coupled gas atomization process ... 6
2.4 Gas nozzle in gas atomization process ... 6
2.5 Computational fluid dynamics ... 7
2.5.1 Pre-processing ... 7
2.5.2 Solver ... 8
2.5.3 Post-processing ... 8
2.6 Governing equation ... 8
2.6.1 Mass equation ... 9
2.6.2 Momentum equation ... 9
2.6.3 Energy equation ... 10
2.6.4 Equation of state ... 10
2.7 Types of the fluid flow ... 11
2.7.1 Turbulent flow ... 11
2.7.2 Turbulence models ... 12
2.8 Shadowgraph and Schlieren imaging ... 12
Methodology... 15
3.1 Numerical modelling procedure ... 15
3.2 Geometry ... 16
3.3 Meshing process of the computational domain ... 17
3.4 Numerical setup ... 17
3.4.1 viscous model ... 18
iv
3.4.2 Fluid properties ... 18
3.4.3 Boundary conditions ... 19
3.4.5 Solution methods and controls ... 22
3.5 Monitoring convergence progress ... 23
3.6 Steady state analysis ... 23
3.7 Transient analysis ... 24
3.8 Parametric study ... 24
3.9 Experimental study ... 25
3.9.1 Assembly and alignment ... 25
3.9.2 Experimental procedure ... 26
3.9.3 Schlieren image post-processing ... 28
3.9.4 Safety consideration and rules ... 28
Results ... 29
4.1 CFD simulation for experimental validation ... 29
4.2 Results of the experimental study ... 30
4.3 Effect of jet interaction angle ... 31
4.3.2 Effect of distance between the nozzles ... 39
Discussion ... 44
5.1 CFD simulation and experimental validation ... 44
5.1.2 Discretization error ... 44
5.1.3 Geometry modelling error ... 45
5.1.4 Boundary condition error ... 45
5.2 Parametric study ... 46
5.2.1 Effect of gas interaction angle ... 46
Conclusions ... 49
Future work ... 50
Acknowledgment ... 51
References ... 52
1
Chapter 1
Introduction
Several powder metallurgy-based technologies such as Additive Manufacturing (AM) and Metal Injection Molding (MIM) rely on powder with spherical shape and high purity level.
Another important characteristic of metal powder is Particle Size Distribution (PSD) since several processes require powder in a certain size range. Therefore, achieving the narrow particle size distribution leads to higher process efficiency of the processes that require powder in a certain size range [1,2].
Among the various powder production techniques, gas atomization, as shown in figure 1.1, is an effective way to produce metal powders and alloys with a high level of purity. There are two main methods for the gas atomization process which are known as free-fall and close coupled gas atomization.
Figure 1.1 Schematic view of vertical gas atomizer [3]
Currently, most metal powders are produced by the close coupled gas atomization process.
Despite this, due to the complexity of the process as well as the inadequate knowledge of gas and melt interaction, many challenges have not been resolved yet. Therefore, in order to increase process efficiency, many scholars have focused on these challenges [4].
2
Simulating the gas atomization process is widely done by using Computational Fluid Dynamics (CFD). However, due to the complexity modelling of the gas and melt interaction most of the studies are focused only on single-phase simulations. Several studies have been dedicated to the numerical and experimental investigation of gas flow behaviour in the absence of molten metal. However, there are still many aspects of the gas flow behaviour that needs to be studied in more detail. A better understanding of gas flow behaviour can be gained by studying multiple gas jets, rather than focusing only on one gas jet flow behaviour [5].
In the present study, as a step towards improving the process efficiency of the gas atomization process, the behaviour of the multiple gas jets under different conditions have been modelled using Ansys Fluent. In addition, the experimental study has been done to validate the result of the numerical study.
1.1 Aims and objective
The purpose of this project is to model the interaction of the two gas jets released from two similar convergent-divergent nozzles to achieve a better understanding of the gas jets interaction in the gas atomization process. This will be done by modelling the gas jets interaction in Ansys Fluent. Then, the experimental study will be performed to validate the simulation.
At the final stages of this study, a set of parametric studies will be done to investigate the influential parameters which could affect the gas jets interaction. The result of this study would lead to a better understanding of the gas jets interaction behaviour in gas atomization process and get more knowledge about the influential parameters on gas jets interaction. The study is planned to be done in 22 weeks.
1.2 Scope
As the transient simulation has been performed in this study and each simulation took longer than the initial prediction at the beginning, the project time limit was extended.
At the first stage of the thesis work, the literature study has been done to obtain a better understanding of the gas flow behaviour through the convergent-divergent nozzle and to be familiar with what has been done before in this topic.
Moreover, since the project should be validated using the experiment, an extensive amount of time was spent for improving the current shadowgraph and schlieren image setup at the KTH water-model lab.
3
1.3 Delimitation
The numerical simulation has been carried out as a time-dependent simulation. In order to avoid any convergence problems for the solution, a very small time-step has to be selected in this study, which leads to much higher computational time. The gas jets kept evolving over time.
Hence, due to the limited time, the simulation is stopped at a specific time.
The researcher also was limited to using only air as the atomizing gas in order to avoid any asphyxiation in the lab. Therefore, all the simulations have been done with air.
1.4 Environmental and ethical consideration
Since in the experimental study, the pressurized gas is used, all the experimental trials when the pressurized gas was released have been performed under the supervision of the thesis supervisor. Moreover, only air was used for the experimental study and other types of gases like nitrogen which is widely used in the gas atomization process were not used to prevent asphyxiation. The researcher sticks to the safety concern all the time in the lab to avoid any potential hazards.
In addition, the aim of this study a line well with some of the United Nations Sustainable Development Goals numbered 9, 12 and 13 that it is shown in figure 1.2. In this study, it is attempted to achieve better understanding of gas jets interaction in gas atomization process by investigating the effect of the nozzles’ interaction angle and distance between the nozzles on the gas jet flow behaviour. This investigation can be considered as an initial step to enhance and optimize the gas atomization process and in consequence, higher process efficiency. In addition, enhancing the gas atomization process would lead to narrow particle size distribution and powder with higher sphericity which are the key factors for enhancing the additive manufacturing process. Additive manufacturing process compared to the other common conventional production methods is a more sustainable production method.
Figure 1.2 United Nation Sustainable Development Goals [6]
4
Chapter 2
Theoretical background
This chapter provides readers with an introduction to powder production techniques, focusing on the gas atomization process. The topic is followed by a description of a CFD simulation.
Nevertheless, this chapter does not cover all the details. Therefore, readers are advised to refer to the reference list at the end of this document for more details.
2.1 Powder production techniques
There are three main categories of metal powder production techniques: mechanical, chemical, and physical. Each production method transfers energy from the source of the energy, which can vary depending on the fabrication technique, to the material to create surface area [7,8].
Today, one of the most common techniques for powder production is atomization. The atomization of the metallic materials is based on the molten metal break down into fine droplets.
Afterwards, these fine droplets will be solidified and produce solid particles.
There are two well-known atomization processes such as water atomization and gas atomization. Each of these processes will be discussed in more detail below [8].
2.2 Water atomization
The water atomization process is one of the cost-effective methods for powder production.
However, this method is not suitable for producing powder with a high degree of purity and sphericity [9].
In this process the molten metal stream is broken down into fine droplets by high-pressure water jets. The powder becomes irregular and rough as a result of the faster rate of solidification than the gas atomization process. This process requires superheating the molten material far above its melting point to produce powders with greater sphericity.
Water atomization is controlled by a combination of several parameters, but most importantly by pressure. Which means that by increasing the water pressure, the velocity of the water increases, and results in a smaller particle [8].
5
2.3 Gas atomization
One of the most common methods for producing fine spherical metal powder is gas atomization.
In gas atomization, high-velocity gas jets (usually air, nitrogen, helium, and argon) disintegrate melt flow into droplets. The powders produced in the gas atomization process are solidified under high solidification rates. Due to this, they have unique material properties which are not achievable by conventional methods such as ingot casting. For instance, in gas atomization, the high solidification rate might result in a reduction of the elemental segregation in highly alloyed materials [10,11].
This method involves heating molten metal far above its liquidus temperature, then transferring the melt from the ladle into a container which is called tundish. Tundish controls the melt flow rate into the atomizing chamber. Then melt is poured from the tundish into the ceramic melt delivery nozzle. By transferring kinetic energy from the gas jets to the molten metal, the molten metal is disintegrated into ligaments. Then, under the secondary break up process the ligaments break into droplets. When the droplets reach down to the melting temperature, they turn into solid particles. Finally, particles will be collected down to the atomizing chamber as metal powder.
In powder production industries; the gas atomization process is divided into two main categories that depend on the gas-melt interaction location which are Free-Fall Gas Atomization (FFGA) and Close-Coupled Gas Atomization (CCGA). Figure 2.1 is a schematic illustration of these two processes [5,7,12].
Figure 2.1 Schematic illustration of a) free-fall gas atomization b) close-coupled gas atomization [7]
2.3.1 Free-fall gas atomization process
In free-fall gas atomization, the molten metal flows down to the atomizing chamber due to the gravity before gas jets impinges upon the flow. The gas nozzles are located at a short distance
6
from the melt delivery tube. They can be located anywhere between 10 cm and 30 cm from each other. Afterwards, the gas jets hit the flow and lead to flow disintegration [7].
An advantage of this process compared with close-coupled gas atomization is that in FFGA it is much easier to control the gas-melt interaction. However, the productivity of this process, is significantly lower than that of close-coupled atomization. In addition, it is hard to control particle size distribution this process. Therefore, for large scale powder production, industries prefer using CCGA instead of FFGA [7].
2.3.2 Close-coupled gas atomization process
Close-coupled gas atomization process is a process in which the gas nozzles are placed immediately next melt nozzle. Since in CCGA, the gap between gas and melt nozzle is shorter than FFGA, the dissipation of energy will be lower. Due to this, melt flow will be disintegrated more easily and results in powder with finer particles and narrower particle size distribution.
Today, High-Pressure Gas Atomization (HPGA) can produce fine and spherical powder with a median diameter ranging from 1 to 250 µm. For CCGA this range varies between 10 to 100 µm [9,5,13].
However, each of these processes has its advantages and disadvantage. For instance, with close-coupled gas atomization, powder with smaller size can be produced compared to free-fall gas atomization. While in close-coupled gas atomization, it is difficult to control the gas and melt interaction. Moreover, backflow and freeze-off are usually occurred in close-coupled gas atomization while in free-fall gas atomization it rarely occurs [7].
Despite, many significant signs of progress in the close-coupled gas atomization process during recent years, this process is still not fully understood. Furthermore, one of the major problems in this process is wide particle size distribution which leads to lower efficiency. As a result, many researchers have been working on this area to obtain powder with narrower particle sizes and enhance the gas atomization process efficiency [9].
2.4 Gas nozzle in gas atomization process
Nozzles used in the gas atomization process, have two main roles; controlling the fluid flow direction and accelerating low velocity and high-pressure gas to supersonic speeds. Two common nozzles are used in the gas atomization process; cylindrical and Convergent-Divergent (CD) nozzles which are also called De Laval nozzles. A schematic view of the CD nozzle is shown in figure 2.2 [14].
7
Figure 2.2 Schematic sketch of Convergent-Divergent (CD) gas jet [4]
CD nozzles have three main sections; converging, throat and diverging. In the converging section, the flow has high pressure with low velocity and the Mach number is less than 1. Flow in this section is called subsonic. By going forward to the throat, the flow is becoming sonic and the Mach number in this section is equal to 1. At the final section which is called diverging section, fluid flow becomes supersonic and the Mach number in this area is larger than 1 [15].
𝑀𝑎ℎ𝑐 𝑛𝑢𝑚𝑏𝑒𝑟 = 𝑢
𝑐 (2.1) Mach number is defined in equation 2.1 Where u is the fluid velocity and c are the speed of the sound. Flow with Mach number less than 0.3 is considered as incompressible flow and flow with Mach number greater than 0.3 is considered as compressible flow.
2.5 Computational fluid dynamics
Computational Fluid dynamics, also known as CFD, is a computer-based simulation that is widely used in order to model and analyse systems containing fluid flow, heat transfer and other related phenomena [14].
CFD simulations consist of three sequential stages; pre-processor, solver, and post-processor.
Each of the will be described briefly below:
2.5.1 Pre-processing
The first step in CFD simulation is to specify a flow problem. This requires the creation of a computational domain using available software. Following that, the defined domain should be subdivided into discrete elements called meshes. In the next step, the fluid characteristics need to be determined. Finally, pre-processing should be completed by selecting appropriate boundary conditions.
8
At this stage, the quality of the mesh is one of the most important factors that must be considered. Due to the fact that CFD simulation accuracy is heavily dependent on mesh quality.
Depending on the area of the domain, it is usually recommended to use different sizes and numbers of meshes when performing CFD simulations. For instance, meshes near the walls usually are finer compared to other areas in the domain, due to the large fluctuations of fluid properties near the walls and to make software to be able to capture these changes in the fluid properties. In contrast, meshes in areas with slight changes in fluid properties can be larger to reduce computational cost. Today CFD software can do the process of making meshes finer in areas where there are large fluctuations automatically [14].
2.5.2 Solver
In the first stage, the discretization scheme should be selected in order to solve the governing equations. In addition, at this stage, the convergence criteria and solution method should be defined [1].
2.5.3 Post-processing
The last stage of each CFD simulation is visualizing and analysing the results. A wide range of data visualization tools is available such as in the software such as contour plots, XY plots, vector plots, particle tracking, etc. Moreover, for the time-dependent simulations, there is a possibility to record the flow behaviour as an animation [14].
2.6 Governing equation
Cloaude-Louis Navier at 1823, by assuming laminar behaviour for fluid flow and also considering a linear relationship between the shear rate in a fluid with shear stress, derived a set of equations to describe the motion of a viscous fluid. George Stokes in 1845 derived the equations of fluid movement but in a different way. These equations are currently known as Navier-Stokes equations and are used to model the fluid motions mathematically and describe the relationship between the parameters of the fluid flow with respect to time and position. As mentioned at the begging of this paragraph, these equations are derived for the laminar flow, however, they are widely used for the turbulent fluid by doing some modifications [4,16,17].
Navier-Stokes equations can be defined as nonlinear partial differential equations that are used for describing movements of the fluid flow. The Navier-Stokes equations are used to describe the conservation of mass, momentum and energy. For the sake of simplicity, the Navier-Stokes equation can be considered to be linear as well [4].
The fundamental laws of fluid flow modelling are listed below:
1. Mass is conserved 2. F= ma
9 3. Energy is conserved
As mentioned in the description of the CD nozzles, the flow through the CD nozzles is compressible. In addition, the model in this study is two dimensional. Hence, in all following expressions, parameters in z-direction should be ignored.
2.6.1 Mass equation
This equation is also called continuity equation. This equation indicates that mass is conserved.
In other words, mass can't be added or removed from a flow.
𝜕𝜌
𝜕𝑡+ 𝜕𝜌𝑢
𝜕𝑥 + 𝜕𝜌𝑣
𝜕𝑦 = 0 (2.2) In this equation, ρ represents density and u and v represent velocity in x and y directions respectively. However, it should be mentioned that the velocity changes in z-direction have been ignored in the above expression since the CFD model is two dimensional. Moreover, it should be noted that, for the incompressible fluid, mass variation over time is identically zero.
Hence the term of density gradient for incompressible flow must be ignored. In contrast, for the compressible flow, as the density is changing over time, the term of density changes over time should be retained in the expression [16,18].
2.6.2 Momentum equation
In order to model fluid flow motion, Newton's second law must be applied, which states that the element's mass multiplied by its acceleration will yield the total force of the element [19].
The momentum equations for the two-dimensional compressible flow are:
𝜕(𝜌𝑣)
𝜕𝑡 + 𝜕(𝜌𝑢𝑢)
𝜕𝑥 +𝜕𝑣𝑢
𝜕𝑦 = 𝜕
𝜕𝑥 [(µ + µ𝑇)𝜕𝑣
𝜕𝑥] + 𝜕
𝜕𝑦[(µ + µ𝑇)𝜕𝑣
𝜕𝑦] + 𝑆𝑢 (2.3)
𝜕(𝜌𝑣)
𝜕𝑡 +𝜕(𝜌𝑢𝑣)
𝜕𝑥 + 𝜕𝑣𝑣
𝜕𝑦 = 𝜕
𝜕𝑥 [(µ + µ𝑇)𝜕𝑣
𝜕𝑥] + 𝜕
𝜕𝑦[(µ + µ𝑇)𝜕𝑣
𝜕𝑦] + 𝑆𝑣 (2.4) The above equations derived from Newton’s second law express the momentum in the fluid flow is conserved. In both equations; the left-hand side of the equations represent the local acceleration and advection terms. The advection terms represent the velocity change which is due to the change in the position of fluid particles. On the right-hand side of the equations the diffusion coefficient is denoted as (µ+µT). Moreover, other influential sources like gravity are included in terms Su and 𝑆𝑣 [18].
10
2.6.3 Energy equation
The third and last statement is energy conservation, which is derived from the first law of thermodynamics.
𝜕(𝜌ℎ)
𝜕𝑡 + 𝜕(𝜌𝑢ℎ)
𝜕𝑥 + 𝜕(𝜌𝑣ℎ)
𝜕𝑦 = 𝜕
𝜕𝑥[𝜆𝜕𝑇
𝜕𝑥] + 𝜕
𝜕𝑦[𝜆𝜕𝑇
𝜕𝑦 ] + 𝜕
𝜕𝑥[µ𝑇
𝑃𝑟𝑇
𝜕ℎ
𝜕𝑥] + 𝜕
𝜕𝑦 [µ𝑇
𝑃𝑟𝑇
𝜕ℎ
𝜕𝑦] +𝜕𝑃
𝜕𝑡+ 𝛷 + 𝑆𝑇 (2.5)
Where:
𝜆: Thermal conductivity µ𝑇: Eddy viscosity 𝑃𝑟𝑇: Prandtl number Φ: Dissipation function 𝑆𝑇: Source term
2.6.4 Equation of state
According to the equations that have been mentioned in the previous sections, the motion of the fluid in two dimensional could be described using four partial differential equations; mass conservation, momentum conservation (in x and y directions), energy equation. In these equations, there are five flow-field unknown variables; ρ, p, u, v, e.
In many problems, especially engineering problems, it is common to assume the gas as an ideal gas which is also called perfect gas. In other words, the intermolecular forces are ignored in order to simplify calculations. All ideal gases follow the equation of state:
𝑝 = 𝜌𝑅𝑇 (2.6) Where:
𝑅 = 𝑅𝑢
𝜗𝑚 (2.7) Where, (p) is pressure, (ρ) is density, (T) is the temperature and (R) is the specific gas constant.
In equation 2.7 the Ru is the universal gas constant and ϑm is the molecular mass of the air. The equation of state is needed to calculate the five flow-field unknown variables that have been mentioned earlier. The equation of state adds another unknown variable which is the temperature (T). Hence, it is necessary to introduce some more equations to be able to calculate all the unknown variables [18, 19].
𝑒 = 𝐶𝑉𝑇 (2.8)
11 𝐶𝑉 = 𝑅
𝐾−1 (2.9) 𝑃 = (𝐾 − 1)𝜌𝑒 (2.10) In the above equations, e is referred to the internal energy, CV is the specific heat at constant volume and K is the heat capacity ratio.
2.7 Types of the fluid flow
Fluid flow properties can be described using several parameters, such as Taylor number, Grashof number, Richardson number, and Reynolds number. Among them, the dimensionless number, the Reynolds number, is widely used in order to describe the turbulent flow behaviour of the fluid. The Reynolds number can be calculated according to equation 2.11 which is the ratio of the inertial forces to the viscous forces.
𝑅𝑒 = 𝜌𝑉𝐿
µ (2.11) Where ρ and V are the fluid density and velocity respectively, L is the characteristic length and represents the inertial forces while µ is the fluid viscosity and represent the viscous forces. If the Reynolds number value is below than 2200, the flow is called laminar. While the flow with Reynolds number higher than 4000 is considered as turbulent flow. In the laminar flow, the fluid flows layer over layer with small or no mixing between the layers. In contrast, in turbulent flow, there is not any pattern for the fluid flow, which means that the fluid flow behaviour is chaotic with lots of fluctuations. Figure 2.3 shows the schematic of these flow behaviour [20, 21].
Figure 2.3 Schematic illustration of flow types [22]
2.7.1 Turbulent flow
It was mentioned in the previous section that fluid flows above a certain Reynolds number become turbulent, which implies that velocity, pressure and other fluid flow variables are changing continuously. The majority of the macroscopic flows in engineering problems and
12
nature, are turbulent and contain vortexes. Despite a good understanding of turbulent flow and its modelling, turbulent modelling remains one of the most challenging topics for researchers [14, 20, 23].
2.7.2 Turbulence models
The choice of the right turbulence model is essential when simulating turbulent flows in computational fluid dynamics. Due to the chaotic motion present in the turbulent flow, this type of modelling is complicated and CFD needs fine mesh to be able to model the small-scale vortices. Currently, there are several turbulence models such as Direct Numerical Simulation (DNS), Reynolds Averaged Navier Stokes equations (RANS) and Large Eddy Simulation (LES) [4,24].
In the DNS turbulence model, the Navier Stokes equations are being solved numerically without any additional turbulence model. The DNS simulation is used commonly for the low Reynolds number fluid flow and it is not applicable for fluids with a high Reynolds number since the element size must be fine enough. By reducing the element size the computational time will increase and makes the CFD simulations expensive from the computational time point of view.
Hence, for this reason, the DNS model must be used only for fluid flows with low Reynolds number [4,25].
The LES is another mathematical approach for modelling turbulent flows. The LES method compared to the DNS method is more computationally cost-effective.
The Reynolds Averaged Navier Stokes is widely used for modelling engineering problems in industries. Especially, for modelling the gas atomization process. This model could be used for both steady and transient (unsteady for URANS) problems. The RANS model needed an additional turbulence model to model the additional Reynolds stress terms which is available in RANS model. There are several RANS based models available in Fluent such as one equation model, two equations models; k-ε and k-ω, etc [4].
In this study, the SST k-ω turbulence model is taken to model the interaction of the two gas jets flow behaviour from the convergent-divergent nozzles.
2.8 Shadowgraph and Schlieren imaging
Among several visualization techniques for gas flow investigation in the gas atomization process, there are two well established optical methods; shadowgraph and schlieren imaging techniques.
According to the physics of light, light beams travel in a straight path without distortion when passing through homogeneous media. However, the environment around us is not homogenous
13
for several reasons, including thermal convection or turbulence. As a result, the refractive index and density of air can change. The Refractive index can be calculated as follows:
𝑛 = 𝐶
𝐶0 (2.12) Where C is referred to the speed of the light in the medium and C0 is referred to the speed of the light in the vacuum which is 3*108 m/s.
In addition, the refractive index and density of gas relate linearly in the following way:
𝑘𝜌 = 𝑛 − 1 (2.13) In Which k (Gladstone-Dale coefficient) is around 0.23 cm3/g for air at the standard condition and ρ is the gas density. Based on the equation 2.12, density gradient due to any distortion in the air would change the refractive index. The fundamental of the shadowgraph and schlieren imaging is based on the difference in the refractive index in a transparent medium which causes light beam refraction in the direction of the increasing refractive index [4,26].
Although the shadowgraph and schlieren techniques are similar to each other in many aspects.
But there are some differences between these two techniques which make them different from each other. For instance; in the schlieren technique a knife-edge is used for cutting off the refracted light beam whereas the shadowgraph technique does not need a knife-edge. Another distinction between these two techniques is the illuminance level in the schlieren technique respond to the first derivative of the refractive index, while in the shadowgraph technique the illuminance responds to the second derivative of the refractive index [26].
The schlieren imaging can be done either with mirrors or lenses. It should be noted that each of them has its advantages and disadvantage from image quality and economical point of view.
For instance, the mirror-based schlieren systems suffer from off-axis aberration, however, the lens-based system does not have this problem. However, in the lens-based setup, the quality of lenses should be high which leads to higher price and maintenance. In addition, by using the lens-based system, a smaller area can be studied. Since the size of the lenses cannot be as big as the mirror sizes. It should be mentioned that the mirror-based system requires a smaller area for the arrangement compared with the lens-based system. Therefore, using a mirror-based system could save more space in the laboratory as well [26].
As seen in figure 2.4, the Z type arrangement of Schlieren techniques is depicted, which contains two parabolic mirrors, a light source, a high-speed camera and the knife edge.
14
Figure 2.4 Schematic view of Z type schlieren technique [27]
For visualizing the supersonic gas jet from the CD nozzles, the shadowgraph and schlieren techniques have been taken in this study to visualize the density gradient caused due to the high-speed gas jets.
15
Chapter 3
Methodology
In this chapter, all the methodology and the procedure implemented in this study will be explained in detail.
3.1 Numerical modelling procedure
The first stage of each CFD simulation is geometry creation under the appropriate assumptions.
Less complication in the model leads to lesser computational time which is quite important in any industrial problem. Hence, it is important to avoid any unnecessary complications during the geometry creation stage, but it is also important to make sure physical situation is represented by the model.
The next step is meshing the computational domain. The accuracy of each numerical simulation is highly dependent on the mesh quality. Hence, it is important to mesh the computational domain to a high enough resolution. Conversely, finer meshing adds greatly to computational time, so it is important to find a good balance between detail and time. The quality of a mesh is measured according to mesh quality factors such as skewness, orthogonality. Skewness represents how far an element deviates from its ideal shape and orthogonality represents how close the face normal vector and the vector connecting two centroids of two adjacent cells are.
It is not recommended to have low orthogonality and high skewness values. In general, it is recommended to keep the orthogonality close to one and skewness close to zero. The mesh quality directly affects the accuracy, convergence and speed of the simulation. Therefore, it is crucial to ensure that the mesh quality meet the quality criteria.
In the next steps, the fluid properties and appropriate boundary conditions characterize the behaviour of the fluid flow through the computational model. Then the proper turbulence model should be selected. Simulation can be run both as a steady or unsteady simulation according to the physics of the flow. Finally, in the last step, the result of the computational simulation can be analysed using several data visualization tools that have been mentioned in the post- processor section.
Currently, several CFD codes such as Ansys Fluent, Comsol and OpenFOAM are available to perform the numerical study for a wide range of engineering problems. According to the previous studies that have been done in the gas atomization process, especially the gas flow
16
investigation, Ansys fluent is a powerful code for this purpose and has been used in many comparable studies in literature. Therefore, in this study, Ansys fluent 2020 R2 is taken to investigate the interaction of the gas jets with each other.
3.2 Geometry
The geometry can be created with Computer-Aided Design (CAD). Ansys software provides a specialized drawing program that was utilized to create the two-dimensional geometry in this study. The geometry has been created without the melt delivery nozzle to simplify the simulation and just investigate the gas flow behaviour. The model involves two convergent- divergent nozzles pointed towards each other which are attached to the atomizing chamber.
The first model has been created in which the gas jets interact with each other at 20º. Figure 3.1 shows the computational domain that has been used for this study in the first stage and figure 3.2 shows the nozzles’ shape and dimensions. To make comparisons between simulation and experiment more logical and easier, the dimensions of the convergent-divergent nozzles modelled numerically are considered the same as to the dimensions of the nozzles in the experiment.
Figure 3.1 Schematic view of the computational domain which is rotated 90°
17
Figure 3.2 Schematic view of the convergent divergent nozzle used in this study both in CFD and the experiment (dimensions are in mm)
3.3 Meshing process of the computational domain
After defining the computational domain, the domain must be divided into sufficiently fine cells which are also known as mesh. In the CFD simulation, it is quite important to choose the proper mesh size and perform a mesh independence study to ensure that the results do not depend on the mesh size. In order to perform the mesh independence study, element size must be coarse at the beginning, then the element size will be refined step by step until the CFD results do not change by decreasing the mesh size. Moreover, choosing the proper size for the mesh leads to saving computational time since by decreasing the element size the computational time would increase significantly.
In Ansys, there are several mesh types that should be chosen depending on the users’
applications. For two-dimensional geometries, meshes are triangular or quadrilateral. It should be noted that the combination of them is also possible. For the three-dimensional geometries, meshes are tetrahedral, hexahedral, pyramid, etc. For three dimensional geometries also, it is possible to use the combination of different mesh types. In this study, the quadrilateral mesh shape was used since the quad meshes give better results in higher order scheme and also maintain better numerical stability and accuracy compared to the meshes with triangular shape.
3.4 Numerical setup
As already mentioned in the previous sections, in this study commercial CFD code; Ansys Fluent is used to investigate the interaction behaviour of the two gas jets. Since, the CD nozzles produce high velocity gas jets at the nozzle outlet (higher than speed of the sound), the flow is considered to be compressible [28, 29]. Therefore, the compressibility effect of the gas jets should be involved in the model. To do so the density-based solver is used to take into account the compressibility effect of the flow and the density gradient properly. The flow is also assumed to be unsteady and turbulent. It should be noted that, for the sake of simplicity gravity is ignored.
18
Table 3.1: An overview of simulation scheme
Solver Density based
Geometry 2D planar
Turbulence model SST k- ω
Flow model Single phase
Time Unsteady
Time step 10-6
3.4.1 viscous model
Since the flow is in the turbulent regime, and in order to take the turbulence behaviour into account, the SST k-ω turbulence model is used. The k-ω turbulence was chosen since it can model the high-speed internal flows and shocks that might appear in this type of flows. In addition, the k-ω turbulence model is used since this model provides more accurate results in the near wall boundary regions, while the k-ε turbulence model predicts well far from the walls.
It should be noted that, when the fluid is considered to be compressible, the energy equation should be enabled [5,18].
3.4.2 Fluid properties
For this study, air was used as the fluid and modelled as a compressible ideal gas. Equation 3.1 employs the ideal gas law to calculate the density of the fluid within the simulation. In addition, fluid viscosity has been calculated according to Sutherland's viscosity law, shown in equation 3.2. Other characteristics of the fluid are available in the following tables [18].
𝜌 = 𝑝𝑜𝑝𝑅+𝑝 𝑀𝑤𝑇
(3.1)
µ = µ0(𝑇
𝑇0)
3 2 𝑇0+𝑆
𝑇+𝑆 (3.2) Where:
Pop = Operating pressure P= Static pressure R= Gas constant
Mw = Molecular weight T= Static temperature (K) µ = Viscosity (𝑘𝑔
𝑚𝑠)
19 µ0= Reference value (𝑘𝑔
𝑚𝑠) T0 = Reference temperature (K)
S = Effective temperature (K), (Sutherland’s constant)
Table 3.2 Air properties
Property Value
Specific heat capacity ( 𝐽
𝐾𝑔.𝐾) 1006.43
Thermal conductivity ( 𝑊
𝑚.𝐾) 0.0242
Reference viscosity (𝑘𝑔
𝑚𝑠) 1.72E-05
Reference temperature (K) 273.11
Effective temperature (K) 110.56
Molecular Weight 28.966
3.4.3 Boundary conditions
Ansys Fluent has a wide range of boundary conditions which gives the user the ability for implementing different boundaries based on their objective. In figure 3.3 the boundary conditions on the computational domain are shown.
20
Figure 3.3 Schematic view of the 2D planar geometry with boundary conditions (The dimension of the atomizing chamber is not same as the real model)
According to figure 3.3, the computational domain has three different boundary conditions, namely pressure inlet, pressure outlet, and stationary wall. The pressure inlet can differ depending on the atomization pressure; in this study, the inlet pressure is set at 20 bar.
Atmospheric pressure is considered to be the pressure at the pressure outlet. The nozzle and chamber walls of the domain are considered to be no-slip walls. Moreover, the inlet and outlet temperature are kept constant at 300K. The following table summarized the computational boundary conditions of the current study.
The gas pressure and temperature were set to be similar as experimental condition to make the comparison between the experimental and numerical results easier and perform the experimental validation.
21
Table 3.4 A summary of the boundary conditions
Boundary type Boundary condition Boundary condition (energy)
Inlet
Pressure inlet:
Gauge total pressure: 20 bar Supersonic/initial gauge
pressure: 18 bar
300K
Wall No slip wall No heat transfer (insulated)
Outlet
Pressure outlet Gauge pressure:
atmospheric pressure E.g.: 1.01 bar
300K
Turbulence in the inlet and outlet of the domain is one of the main factors that can impact the gas jet flow behaviour. Therefore, it is necessary to perform the proper calculations here and implement the correct inputs into the software. Table 3.4 summarizes turbulence boundary conditions [18,20]. The flow characteristics curve which is shown in figure 3.4 was used to calculate the turbulence boundary condition.
Table 3.5 A summary of turbulence boundary conditions
Boundary type Turbulence intensity Hydraulic diameter (m)
Inlet 4% 0.008
Outlet 4% 0.25286
Based on the following equation, the turbulence intensity presented in table 3.4 was calculated:
𝐼 = 0.16 (𝑅𝑒)−18 (3.3) Where:
Re is the Reynolds number and it was calculate using equation 2.11. The Reynolds number at the inlet was calculated to be 73387.
22
Figure 3.4 Flow characteristics curve of the gas regulator [30]
3.4.5 Solution methods and controls
The solution methods and the solution controls for the simulations in this study have been summarized in table 3.6 and 3.7 respectively. They have chosen according to knowledge gained through the literature studies and based on the previous work [18,20].
Table 3.6 An overview of solution methods
Formulation Implicit
Flux type Roe Flux-Difference splitting
Gradient Least squares cells based
Flow Second order upwind
Turbulent kinetic energy Second order upwind Turbulent dissipation rate Second order upwind
Table 3.7 An overview of solution controls
Courant number 1
Turbulent kinetic
energy 0.8
Turbulent
dissipation rate 0.8 Turbulent viscosity 1
23
3.5 Monitoring convergence progress
At this stage, the Ansys Fluent will perform an iterative calculation until the converged solution is achieved. For this study, the convergence criteria were set at 10-3 for the continuity, velocity in x and y directions, and at 10-6 for the k and ω equations. A number of parameters were monitored for assessment of solution convergence in addition to residual monitoring. The parameters for ensuring the convergence of the solution are listed below:
❖ Vertex maximum of static pressure at the nozzle exit
❖ Vertex maximum of velocity at the nozzle exit
❖ Vertex maximum of static temperature at the nozzle exit
❖ Mass flux
For a specified field variable, the vertex maximum represents the highest vertex value of its selected variable on a surface. These parameters have all been monitored at the exit of the nozzle until they did not change further when the calculation was carried out for further iterations.
3.6 Steady state analysis
For many industrial applications, the steady-state simulation results are acceptable. The main reason of using steady state simulation is that we aim for a steady state in practice with constant material input and output. Therefore, steady state CFD simulation is fairly representative of physical situation. Moreover, comparing the steady-state simulation to the transient simulation, the steady-state simulation takes much less time to compute than the transient simulation [31].
Consequently, a considerable amount of time and effort was devoted to achieving the steady- state simulation at the beginning of this thesis. Following are several methods that have been employed to obtain the converged steady-state simulation:
❖ Different turbulence models with various wall function
❖ Extending the chamber length and width to avoid getting high reverse flow
❖ Running the simulation when the reverse flow is enabled at the outlet
❖ Altering the number of elements on the computational domain
❖ Working on the 𝑦+ value
❖ Changing the Courant number and adjusting the under-relaxation factors
❖ Simulating with different flux types and discretization methods
Since the turbulence model plays a crucial role for prediction of the turbulent flow and due to the divergence of the model using SST k-ω turbulence model, according to the literature study other turbulence model such as k-ε and LES with various wall function have been tried in order to see if they made a difference or result in a converged solution or not.
Furthermore, during the simulation, it was observed that, there are a lot of flow going towards the nozzle at the outlet (revers flow), which was possibly due to the outlet being too close to
24
the nozzle, therefore, the chamber length was extended to avoid getting reverse flow and see if that made a difference. Moreover, for a set of simulation the reverse flow was enabled to see its effect on the simulation.
In addition, since the result of the accuracy of CFD simulation is highly dependent on the mesh, different mesh size has been tried to see how it can affect the result. By changing the element size, it was necessary to change the 𝑦+ and courant number accordingly. The courant number is a dimensionless value that indicates how long a particle stays in a cell of the mesh in the computational domain. It is important to select appropriate courant number for a simulation since if the courant number is large, the time step will be too large and it leads missing information in some cells which makes the results inaccurate. According to the Ansys Fluent documentation for the implicit density-based solver the courant number can be 100 or higher.
Therefore, different courant number have been tried to see its effect on the final result.
Finally, different flux types have been tried if it helps the convergence of the simulation. For the density-based software three different flux types are available. The first one is Reo-FDS which is the default and according to the Ansys Fluent documentation it is recommended in most cases. AUSM is another flux type that has been also tried. The other one is low diffusion Reo-FDS and it should be used when the LES viscous model is used.
None of the above changes led to the converged steady-state solution. Thus, it is important to mention that even though the steady-state simulation is more desirable than the transient simulation. However, sometimes it is impossible to achieve converged steady-state solutions due to physical or numerical unsteadiness. In this thesis work after 7000 iterations, the residual values increased significantly and attempt at a steady-state solution generally failed to converge. Thus, based on the study of Mullis [32] the steady-state simulation was abandoned, and the current study was done entirely as a transient simulation.
3.7 Transient analysis
According to what was mentioned in the previous section, the study was carried out as an unsteady analysis. To achieve reliable results and also avoid solution divergence, the time step was selected to be very small, 10-6. As a consequence of selecting a small time-step for the transient solution, the computational time would increase significantly. Hence, due to the small time-step and also limited power of the available computer resources, each simulation took around one week to be completed [33].
3.8 Parametric study
A set of simulations was conducted in order to investigate the effects of influential parameters on gas jet flow behaviour. As it is shown in figure 3.5 this was accomplished by modelling different gas jet interaction angles when it is varied between 20°, 5° and 0°. Moreover, the nozzle spacings is varied between 18mm, 10mm and 5mm.
25
Figure 3.5 Variables for the parametric study, (1) the wall to wall distance , (2)interaction angle
3.9 Experimental study
3.9.1 Assembly and alignment
According to the previous chapter, Schlieren and shadowgraph visualization techniques have been widely used for decades to visualize the gradient of the refractive index in different applications such as high-speed gas flow behaviour using convergent-divergent nozzles. The fundamental of the Schlieren and shadowgraph techniques have been mentioned in the previous chapter. Both Schlieren and shadowgraph techniques were employed in this study to visualize the turbulent flow interactions between the two gas jets. However, according to experimental results, it was found that the Schlieren method gave better results than the shadowgraph method.
The experiment investigation will therefore be conducted using Schlieren imaging [3].
The Schlieren and shadowgraph setups must be aligned correctly. Although, this may take some time, in order to obtain good results, it is important to align the setup properly [21]. The Schlieren setup needs to be sensitive enough to capture deflection of just a few arcseconds of angle. Since, large changes in a gas density corresponds to the small changes in a refractive index, it is crucial to ensure that the mirrors are well aligned to visualize these small deflections.
The schlieren setup utilized in this study can be seen in figure 3.6. Each component can be seen in the figure. Two off-axis parabolic mirrors are the main components of this technique. These mirrors have an off-axis angle of 30° and a focal point of 326.7 mm. Schlieren setup also includes a blue colourpoint light source, as well as a high-speed camera, two 670mm long plates and a knife-edge, which is normally a lazar bale. The knife edge is placed at the focal point of
2 1
26
the second mirror. The percentage of the light blocked due to the knife-edge is called the cut- off percentage and it could be vary depending on the experiment objective [20]. The sensitivity of the Schlieren setup can be defined as the percentage of the knife-edge on the light source.
For instance, 100% cutoff describes the situation, where the light source is being blocked completely by the knife-edge. In the Schlieren imaging, only a very slight shadowgraph effect can be seen for 10% or 20% cutoff. Conversely, the Schlieren setup with high cutoff produces over-ranged imaged. As a consequence of over-ranging image, local flow details will be lost.
Therefore, for the Schlieren imaging it is necessary to choose an optimal cutoff percentage in order to visualize the smallest turbulent structure and meanwhile avoid over-ranging image.
The optimal percentage would be, for instance in the 30-60% cutoff range [34].
Figure 3.6 A top view of schlieren setup showing all the components and their positions in the arrangement and the light paths
3.9.2 Experimental procedure
First, two convergent-divergent nozzles were machined. To make the comparison easier, the dimensions of the nozzles were kept similar to what has been modelled in the simulation. A special glue was then used to ensure the nozzles facing each other are stable at 20°. The nozzles were then connected to a set of connections that contained regulators and a 1-meter metal hose to connect them to the air gas of 200-bar pressure that was fixed in its position using a chain.
Figure 3.7 shows the shadowgraph imaging arrangement used in this study. In order to get
27
Schlieren images, a knife edge was added to the setup. In addition, figure 3.8 shows the nozzles with their connections.
1.5 m
Figure 3.7 Shadowgraph imaging setup and convergent-divergent nozzles connected to the pressurized gas cylinder
0.5 m
Figure 3.8 Zoomed view of nozzles and their connections
28
When all the connections in the setup are connected, the next step is to make sure the components are all located in the right places and no leaks are coming from the gas cylinder or any of the other connections. After that, the video started recording with the camera control software (MotionBLITZ). The gases were released simultaneously.
It should be noted that both shadowgraph and Schlieren imaging techniques were employed with different cut-off percentages and cut-off directions (vertical and horizontal) in this study.
However, the results of the experiments show that Schlieren imaging with horizontal cut-off gave a better result than the others. Finally, when all trials were completed, the gas cylinder was carefully sealed and the remaining gas in the system was vented.
3.9.3 Schlieren image post-processing
A group of images with the highest level of quality has been selected from each trial. In order to prepare these images for comparison with the results of the CFD simulation, these images were transferred to the ImageJ software to modify the brightness and contrast. Moreover, a series of schlieren images have been post processed using image processing in MATLAB in order to get more information from the experiment.
3.9.4 Safety consideration and rules
The experiment was conducted in the basement lab under the supervision of project supervisors.
Synthetic compressed air was used to prevent asphyxia in this study. Furthermore, compressed air was used just for taking pictures to prevent further asphyxiation. Due to the high Mach number of gas jets from CD nozzles, earplugs are used to protect against any potential sound hazards. Additionally, eye protection was necessary to prevent damage from the blue light source used in the experiment.
29
Chapter 4
Results
4.1 CFD simulation for experimental validation
A density gradient contour plot of the fluid flow to compare with the experimental results is shown is figure 4.1. The areas with higher density gradient which are visible in figure 4.1 are called shock diamonds or Mach disks. The number and the distance between the Mach disks in the density gradient contour plots have been compared with the images obtained from the experimental study.
Figure 4.1 Density gradient contour plot from the CFD simulation for experimental validation
30
4.2 Results of the experimental study
Figure 4.2, 4.3 and 4.4 show the results of the Schlieren imaging. The shadowgraph imaging results showed less detail in the jets, hence the comparison procedure proceeded with the Schlieren imaging. During the Schlieren imaging, both horizontal and vertical knife-edge were examined, and the horizontal knife-edge was found to be more effective than the vertical knife- edge.
60 mm
Figure 4.2 Raw schlieren image
60 mm
Figure 4.3 Edited versions of the figure 4.2
31
60mm
Figure 4.4 Image processed version of figure 4.2
4.3 Effect of jet interaction angle
The following figures show the results of the simulations performed to show the effect of interaction angle on the gas flow. The results show that by decreasing the nozzle interaction angle the maximum velocity along the symmetry axis will be increased.
32
Figure 4.5 Velocity contour plot of two gas jets with 20° interaction angle at 20 bar pressures
Figure 4.6 Velocity magnitude of two gas jets with 20° interaction angle along the symmetry axis
33
Figure 4.7 Velocity contour plot of two gas jets with 5° interaction angle at 20 bar pressures
Figure 4.8 Velocity magnitude of two gas jets with 5° interaction angle along the symmetry axis
34
Figure 4.9 Velocity contour plot of two gas jets with 0° interaction angle at 20 bar pressures
Figure 4.10 Velocity magnitude of two gas jets with 0° interaction angle along the symmetry axis
35
The velocity contours and the velocity XY plots of nozzles with different inclination angles have been illustrated 4.5, 4.6, 4.7, 4.8, 4.9 and 4.10. The gas pressure was kept at 20 bar pressures for all of the simulations and also the nozzles spacing were kept constant.
Figure 4.11 Density XY plot for 20° interaction angle
Figure 4.12 Density XY plot for 5° interaction angle
36
Figure 4.13 Density XY plot for 0° interaction angle
Figures 4.11, 4.12 and 4.13 have shown the density of the fluid along the centreline. The density XY plot for the 20 degrees interaction angle indicates that the fluid density varies between 1.2 and 2.6. When the interaction angle is 5 degrees, the density varies from 0.68 kg/m3 to 2.1 kg/m3. For zero degrees interaction, the density range is between 0.5 and 2 kg/m3.
Figures 4.14, 4.15, 4.16 and 4.17 compare the Mach number, turbulent kinetic energy, static pressure and velocity for different interaction angles and single nozzle case respectively. The distance between nozzles and all boundary conditions except the interaction angle were kept constant in all simulations with two nozzles. In addition, for the single nozzle simulation, the boundary conditions are set to be similar to the two nozzles simulation.
37
Figure 4.14 Comparison of Mach number along the symmetry axis for different interaction angle and single nozzle
Figure 4.15 Comparison of turbulent kinetic energy along the symmetry axis for different interaction angle and single nozzle
38
Figure 4.16 Comparison of static pressure along the symmetry axis for different interaction angle and single nozzle
Figure 4.17 Comparison of static pressure along the symmetry axis for different interaction angle and single nozzle
39
4.3.2 Effect of distance between the nozzles
Figure 4.18, 4.19 and 4.20 show the velocity contour plots of the simulations with different nozzle spacing. The density contour plots for different nozzle spacing is also shown in figure 4.21, 4.22 and 4.23. In addition, figure 4.24, 4.25 and 4.26 show the comparison of the static pressure, turbulent kinetic energy and velocity along the symmetry axis for different nozzle spacing. The result show that the maximum value of the jet velocity along the symmetry axis decreases with an increase in distance between the nozzles.
Figure 4.18 Velocity contour plot for 0 degree and 5mm distance
40
Figure 4.19 Velocity contour plot for 0 degree and 10mm distance
Figure 4.20 Velocity contour plot for 0 degree and 18mm distance
41
Figure 4.21 Density contour plot for 0 degree and 5mm distance
Figure 4.22 Density contour plot for 0 degree and 10mm distance
42
Figure 4.23 Density contour plot for 0 degree and 18mm distance
Figure 4.24 Comparison of static pressure for different nozzle spacing