A Computational Study of the Gas-Solid Suspension Flow through a Supersonic Nozzle ()
1. Introduction
High-velocity gas flows including very fine solid particles are often encountered in many diverse fields of engineering applications, such as solid rocket engines, pneumatic conveying systems, powdered drug delivery devices, thermal spray coating systems, etc. [1]. Such gas-solid suspension flows can be obtained in supersonic nozzles in which fine particles with several to several 10 μm in diameter are flowing suspended with the high velocity gas stream. The detailed flow physics in such two phase flows are extremely complex and difficult to understand [2]. The flow complexities mainly arise from particle-mean stream interactions, particle-flow turbulence interactions, inter-particle collisions, particle-wall interactions, particle-shock wave interactions, etc. [3].
A considerable deal of work has been made to get an insight into the gas-solid two phase flows and to specify the particle motion and its influence on the gas flow field. It has been comparatively well known that the suspendsion flow is governed by Reynolds number as well as Stokes number [4]. Many other parameters associated with the particle practically affect the two-phase flow characteristics. The flow of a gas-solid mixture can be categorized according to the significance of particle collisions on particle motion [5]. A flow in which particle motion is controlled by inter-particle collision is referred to as a “dense flow”. In this kind of flow, the particleparticle collision cannot be neglected. A flow in which particle motion is controlled by the aerodynamic forces on the particle is a “dilute flow” [6]. The researchers usually ignore the particle-particle collision when they study the dilute flow. In dilute flow, the phase interaction will be the one of the main characteristics. Since there is no fluid pressure appear in the dispersed particle phase, all the characteristics of particle are show by the fluid phase. The dispersed phase phenomena are related to turbulent fluctuations in the gas phase. Until now, the turbulent diffusion phenomena have not yet been satisfactorily explained [7].
Okuda and Choi [8] have done the analytical and experimental study gas-particle mixture flow in various types of convergent-divergent nozzle. They found the velocity of particle was influenced by particle size, particle density, nozzle geometry, and operating conditions, etc. Rumpf [9] used the formulation of particle velocity based on the experiment to predict the velocity of the particle. Kaushal [10] has used a CFD model to study the pipeline flow of fine particles at high concentration. However, very less people studied the micro-sized particle effect on supersonic two phase flow, mainly because of the extreme difficulty in experimentally measuring motion of micron-sized particle and the particle-turbulent interaction. The cost of the experiment also is very high. However, the numerical simulation can offer a convenient way to solve those problems, and it also can give the further details about the suspension internal flow.
The present study is the mainly to investigate the gassolid suspension flow through a convergent-divergent supersonic nozzle. According to the previous analytical work carried out by the authors, the two-phase flow is significantly different from the single-phase gas flow. The flow behavior depends on the particle loading as well as its diameter. Present study will investigate particle loading effect on supersonic suspension flow through a convergent-divergent nozzle. Four kinds of particle loading are used in simulation: 0.01, 0.03, 0.05, and 0.1, respectively. The discrete particle phase (DPM) from FLUNT was employed to calculate the particle motions, and the two way turbulence coupling method was used to monitor the particle-turbulent interactions.
2. Numerical Analysis
Computational Flow Model
For the CFD software, ANSYS Fluent 14.0 was chosen to simulate internal nozzle flows. Ideal gas was used as the primary fluid phase in all cases. A finite volume scheme and density-based solver with coupled scheme were applied in the computational process. Standard k-ω turbulent model, implicit formulations were used considering the accuracy and stability. Second-order upwind scheme was used for turbulent kinetic energy as well as spatial discretization.
The computational domain is shown in Figure 1. The nozzle part is highlighted using a red box. The axialsymmetric CFD model has been used for the present study. In order to get stable solution, the computational domain was extended up to the region of 5D (D is diameter of nozzle exit.) upstream of the nozzle inlet and up to the region of 20D downstream of nozzle exit. The diameter of nozzle throat, inlet, and outlet is 5.8 mm, 22 mm, 20 mm. respectively. The geometry was discretized into structured quadrilateral cells using commercial
Figure 1. Flow geometry and calculation domain.
software GAMBIT. Boundary layer effects were considered by making finer grid clustered towards the walls.
Four different grid systems were simulated using the same boundary conditions. The mesh independence study is shown in Figure 2, which shows the velocity distribution along the axis for four different mesh systems. The simulation with a grid system of 260,000 was chosen for all further studies as it shows lesser deviation in results when compared to it preceding cases with different meshes. For the present simulation, the inlet total pressure is 493,591 pa and back pressure is 101,325 pa, respectively. The inlet total temperature is 300 K.
Currently there are two approaches for the numerical calculation of multiphase flows: the Euler-Lagrange approach and the Euler-Euler approach. The Lagrangian discrete phase model in ANSYS FLUENT follows the Euler-Lagrange approach. The fluid phase is treated as a continuum by solving the N-S equations, while the dispersed phase is solved by tracking a large number of particles through the calculated flow field. The dispersed phase can exchange momentum, mass, and energy with the fluid phase. This approach is made considerably simpler when particle-particle interactions can be neglected, and this requires that the dispersed second phase occupies a low volume fraction, even though high mass loading is acceptable. The particle trajectory is computed individually at specified intervals during the fluid phase calculation.
Particle Force Balance equation is shown below:
(1)
FD is gas drag force which is calculated by:
(2)
Re is particle Reynolds number which is calculated by:
(3)
CD is drag coefficient which is fellows spherical drag law:
(4)
where: a1, a2, a3 are constants.
The trajectory equations, and any auxiliary equations describing heat or mass transfer to/from the particle, are solved by stepwise integration over discrete time steps. Integration of time in Equation (1) yields the velocity of the particle at each point along the trajectory, with the trajectory itself predicted by
(5)
For the particle velocity at the new location 
we get
(6)
The new location 
can be computed from a similar relationship:
(7)
At the beginning of the study, in order to test the accuracy of DPM method, 3 cases from Ref. [8] have been chosen to simulate in Fluent. The results were compared with experimental data. The Figure 3 shows the particle mean velocity along the axis. It can be seen that the numerical results are in good agreement with the experimental data.
Table 1 shows the different cases used for the present
Figure 3. Validation with experimental data (Solid lines are the present CFD results).
Table 1. Simulation conditions for different particle loading.
study. All the parameters are same except the particle loading.
3. Results and Discussion
Figure 4 shows the particle propagation through the C-D nozzle at different time intervals. At the initial stage the particle flow is uniform and is aligned perpendicular to the axis of the nozzle. When the flow reaches near to the convergent part which shown in Figure 4(d), the particle head trajectory will no longer obeys planar structure, but behaves in a parabolic structure. As the particle flow past the convergent section the particle inertia increases and some particles collides with the wall, but most of particles follow the gas flow trajectories. From the previous study, the flow chocking was observed at the throat section. The flow will change to supersonic speed after it passes the throat section. The shock cell formation in the divergent section leads to flow separation and a shear layer will be formed due to the high velocity gradient exiting between the core flow and the reverse flow in the boundary layer region. The shear layer formation after the oblique shock front causes the concentration of particles near to the shear layer, which can be observed from Figure 4(e). As the flow reaches the end plane of the nozzle, the particles becomes more evenly dispersed in the main gas flow.