Simulation of Supersonic Air-to-Air Ejector

Simulation of Supersonic Air-to-Air Ejector

Simulation of Supersonic Air-to-Air Ejector

In this study, the compressible turbulent flow through a supersonic ejector is modeled using the High Mach Number Flow interface in the CFD Module. Ejectors are simple mechanical components used for a wide range of applications, including industrial refrigeration, vacuum generation, gas recirculation, and thrust augmentation in aircraft propulsion systems. Ejectors induce a secondary flow by momentum and energy transfer from a high-velocity primary jet. The high-energy fluid (primary flow) passes through a convergent-divergent nozzle and reaches supersonic conditions. After exiting the nozzle, it interacts with the secondary flow and is accelerated through an entrainment-induced effect. The mixing between both flows takes place along a constant-area duct called the mixing chamber where complex interactions between the mixing layer and shocks can be observed. A diffuser is usually placed before the outlet to recover pressure and bring the flow back to stagnation.

Introduction

This application models compressible turbulent gas flow in a supersonic air ejector using the High Mach Number Flow interface in COMSOL Multiphysics. Ejectors are simple mechanical components used to induce a secondary flow by momentum and energy transfer from a high-velocity primary jet. The high-energy fluid (primary flow) passes through a convergent divergent nozzle and reaches supersonic conditions. After exiting the nozzle, it interacts with the secondary flow which is accelerated through an entrainment-induced effect. The mixing between both flows takes place along a constant area duct called the mixing chamber where complex interactions between the mixing layer and shocks can be observed. A diffuser is usually placed before the outlet to recover pressure and bring the flow back to stagnation.

Ejectors are used for a wide range of applications, including industrial refrigeration, vacuum generation, gas recirculation, and thrust augmentation in aircraft propulsion systems. Great efforts have been made to determine their optimum design and operating conditions, as well as how to describe the flow within them (Ref. 1). This application models an ejector working with air in both the primary and secondary streams. The geometry and boundary conditions are based on Ref. 2, and Ref. 3. The items of interest are the primary and secondary mass flows, the static pressure distribution along the centerline of the ejector, and the resolution of the flow in the mixing region.

Model Definition

Figure 1 shows the geometry of the ejector. Its dimensions can be found in Table 1. A two-dimensional axisymmetric geometry is used to approximate the 3D geometry of the device and to reduce the size of the problem. The flow velocity in the ejector is large enough to introduce significant variations in the density and temperature of the fluid, and the flow is governed by the fully compressible Navier-Stokes equations. Moreover, the Mach number is expected to be larger than one in the divergent section of the primary nozzle, as well as in the mixing chamber. Interaction between the boundary layers and mixing layers cause the deceleration from supersonic to subsonic flow to take place through a complex succession of shocks called shock train or pseudo-shock wave phenomenon (Ref. 4). Thus, the mesh has to be fine enough to accurately capture this phenomenon.

Figure 1. The geometry of the ejector.
Figure 1. The geometry of the ejector.
d1d2dtdnddmdd
161608122451
L1L2L3LmLdNXP
723902407015
Table 1: DIMENSIONS OF THE EJECTOR IN MM.

The problem is modeled using the Favre-averaged Navier-Stokes equations and the standard k-ε turbulence model. Both primary and secondary flows are air with a specific gas constant of 287 J/(kg.K) and a ratio of specific heats of 1.4. The dynamic viscosity and thermal conductivity of the air are computed from Sutherland’s law.

Boundary Conditions

– Inlet

The flow at the inlets is specified in terms of its total properties: T0 = 300 K and P0 = 5 atm for the primary flow, and T0 = 300 K and P0 = 0.55 atm for the secondary flow. The inlet conditions are applied using an Inlet feature, where the Flow condition is specified to be Characteristics based. This provides a numerically consistent boundary condition by evaluating the flow characteristics at the inlet.

The velocities at both inlets are unknown. However, they are expected to be very small compared to the velocities inside the nozzle and mixing chamber. The values that must be prescribed at the inlet are the total values of temperature and pressure, which define the energy of the flow. The Mach number can be set to 0 and will be determined by the characteristics based boundary condition at the inlet. This provides a good initial solution, but the total values of pressure and temperature may differ slightly. The solution can be improved if the problem is solved again setting the Mach number to the values computed by the characteristics based boundary condition at the inlets, which are 0.14 and 0.01 for the primary and secondary inlets, respectively.

The inlet values for the turbulent kinetic energy, k , and the turbulent dissipation rate, ε , are approximated from the turbulent intensity, IT , and turbulence length scale, LT. Turbulent intensity is set by default to 0.05 (5%). The length scale can be approximated as 7% of the pipe diameter or hydraulic diameter.

– Outlet

The flow reaches supersonic conditions inside the ejector. However, it is expanded and decelerated along the mixing chamber and the diffuser, reaching subsonic conditions before being discharged into the atmosphere. The outlet is then subsonic with atmospheric static pressure. This is modeled using an Outlet node with the Flow condition set to subsonic.

Results and Discussion

The mass flows obtained are depicted in Table 2. The distributions of Mach number and velocity inside the ejector are depicted in Figure 2 and Figure 3. The primary flow is accelerated in the convergent section of the nozzle, reaching sonic conditions at the throat, and is expanded further in the divergent section. At the outlet of the primary nozzle, the secondary flow acts as an artificial wall for the primary flow. This leads to the formation of virtual nozzle throats, and a succession of expansion and compression waves can be observed in the region upstream of the mixing zone. Then, the flow decelerates along the constant-area duct and is brought back to stagnation in the diffuser. The region where both flows mix can be visualized by plotting the turbulent kinetic energy, see Figure 4.

$ \displaystyle {{\dot{m}}_{1}}$$ \displaystyle {{\dot{m}}_{2}}$$ \displaystyle {{\dot{m}}_{{mixed}}}$
0.057 kg/s0.038 kg/s0.095 kg/s
Table 2: MASS FLOWS

Figure 5 plots the distribution of pressure along the centerline and walls of the mixing chamber. At the centerline of the duct, the flow successively changes from supersonic to subsonic flow via multiple shocks. However, this cannot be detected by wall pressure measurements because the surface pressures tend to be smeared out due to the dissipation in the boundary layer (see Ref. 4). The distribution of temperature is shown in Figure 6. Very low temperatures can be observed inside the device. This must be taken into account when designing an ejector, especially when working with two-phase flows. The results obtained correlate well with Ref. 2 and Ref. 3.

Figure 2. Mach number distribution
Figure 2. Mach number distribution
Figure 4. The distribution of turbulent kinetic energy. The mixing region is clearly identified
Figure 4. The distribution of turbulent kinetic energy. The mixing region is clearly identified
Figure 3. The distribution of velocity in the nozzle and the mixing chamber
Figure 3. The distribution of velocity in the nozzle and the mixing chamber
Figure 5. The distribution of pressure along the mixing chamber
Figure 5. The distribution of pressure along the mixing chamber
Figure 6. The distribution of temperature. Very low temperatures can be observed at the outlet of the nozzle. The temperature at the outlet of the ejector is lower than at both inlets.
Figure 6. The distribution of temperature. Very low temperatures can be observed at the outlet of the nozzle. The temperature at the outlet of the ejector is lower than at both inlets.

Notes about the COMSOL Implementation

The present application is highly nonlinear and sensitive to the solution procedure. The mesh needed to capture the interaction between the shocks and the mixing layer, and to resolve the solution near the walls, is extremely fine. However, convergence may be hard to achieve with such a fine mesh unless a very good initial solution is used. A way to overcome this is to first solve the problem on a coarse mesh and then refine it. The solution on the coarse mesh provides good initial values, but lacks accuracy in three important areas: wall resolution, capture of shocks, and resolution of the mixing layer. The adaptive mesh refinement feature can be used to overcome this. However, in order to fully resolve the mesh, a high element growth rate would be needed, potentially leading to convergence problems. An alternative option is to first refine manually both on the boundary layers and in the nozzle, and then to use the adaptive mesh refinement feature to resolve the mixing layer.



Source:
1. S. He, Y. Li, and R.Z. Wang, “Progress of Mathematical Modeling on Ejectors,” Renew. Sustain. Energy Rev., vol. 13, pp 1760–1780, 2009./ 2. Y. Bartosiewicz, Zine Aidoun, P. Desevaux, and Yves Mercadier, “Numerical and Experimental Investigations on Supersonic Ejectors,” Int. J. of Heat and Fluid Flow, vol. 26, pp 56–70, 2005./ 3. P. Desevaux,A. Bouhangel, and E. Gavignet, “Flow Visualization in Supersonic Ejectors Using Laser Tomography Techniques,” Int. J. of Refrigeration, vol. 34, pp 1633–1640, 2010./ 4. F. Gnani, H. Zare-Behtash, and K. Kontis, “Pseudo-shock Waves and their Interactions in High-speed Intakes,” Progress in Aerospace Sciences, vol. 82, pp 36–56, 2016. / 5. COMSOL Models, Blog, Cyclopedia.

CMS
CMS Website
Computational Modeling and Simulation is the simulation center of Acamech that models Mechanical Engineering Problems, especially Multiphysics Simulation; including Fluid Flow (CFD), Structural Mechanics, Acoustics, Heat Transfer as a unique Multiphysics problem. We use COMSOL Multiphysics, MATLAB, and Autodesk Inventor.

Leave a Reply

Your email address will not be published. Required fields are marked *