1. Introduction
Gas-fluidised bed reactors are frequently used in many important industrial processes, especially in the oil industry [
1,
2,
3], mineral processing [
4,
5] and electric power generation industries [
6] due to their excellent heat and mass transfer characteristics, on the one hand, and solid mobility, on the other hand. Despite its widespread application, the hydrodynamics of gas-fluidised beds, unfortunately, remains poorly understood. This lack of understanding poses a significant obstacle to the up-scale of industrially important reactors [
7,
8,
9]. Computational Fluid Dynamics (CFD) is a powerful tool for gaining a theoretical understanding of the complex multiphase flow and transfer processes in reactors [
10,
11,
12]. However, CFD has not matured enough to predict the flow behaviour of a gas–solid flow system containing solids of different sizes and densities.
Much progress has been made in recent years towards developing computer codes for describing the hydrodynamics of gas-fluidised beds. Most of the developed models are based on a two-phase description, one gas and one solid phase and all the particles are assumed to have one diameter, density and a coefficient of restitution [
13,
14,
15,
16]. However, in real particle systems, particles of different sizes and densities exist; furthermore, the operation of many industrial processes is strongly dependent on having different particle sizes in the reactors. For such systems, a multi-particle approach is required for modelling and describing this class of gas–solid flow systems. There are some studies available in the literature [
17,
18,
19,
20] where different sizes and densities of particles were considered as different phases. However, due to the limitations of their models [
3], none of them can be used to predict the behaviour of a multi-particle system. For example, Bell (2000) and Manger (1996) [
17,
18] extended the kinetic theory to binary mixtures of solids with unequal granular temperatures for the phases. In these models, fixed viscosities were used for each solid phase, and an interphase momentum transfer term was derived to account for the momentum transfer between solid phases due to collisions. However, arbitrary constants were used in determining the number of collisions. As the number of collisions can be obtained from kinetic theory, the kinetic theory approach would appear to be superior [
21,
22].
As highlighted earlier, many existing models have been tailored for single-particle flow scenarios [
23,
24,
25,
26,
27,
28,
29]. Consequently, the capacity to forecast the intricate flow dynamics of particles of varying sizes within a gas–solid flow framework remains a notable deficiency, leading to considerable inaccuracies in the advancement and upscaling of gas–solid flow systems such as fluidised beds. In light of this, the principal objective of this study is to pioneer a multi-particle Computational Fluid Dynamics (CFD) model designed for a Circulating Fluidised Bed (CFB) while scrutinising the intricate flow behaviours of diverse-sized particles. In order to address this gap, the current work leverages the kinetic theory of the model introduced by [
3] to simulate the behavior of a CFB riser. This kinetic theory model exhibits its versatility in accommodating multi-particle systems, where variations in particle mass, diameter, restitution coefficient, density and granular temperature are considered. Notably, the model takes into account the heterogeneity of particles and encompasses diverse flow characteristics within solid phases, including solid viscosity, solid pressure, collisional heat flux and bulk viscosity, stemming from intricate particle–particle interactions. For this investigation, the chosen CFB configuration aligns with a previous study conducted by Mathiesen in 1997 [
30], thereby establishing a solid foundation for the ensuing analysis.
As previously mentioned, most of the developed models are applicable to a single particle flow system [
23,
24,
25,
26,
27,
28,
29]. Thus, the ability to predict the flow behaviour of different-sized particles in a gas–solid flow system is still lacking, which causes significant errors in the development and scale-up of gas–solid flow systems such as fluidised beds. Therefore, the main objective of the present study is to develop a multi-particle CFD model for a Circulating Fluidised Bed (CFB) and analyse the flow behaviour of different-sized particles. The kinetic theory model developed by [
3] is used in the present work to simulate the CFB riser. This model is applicable to multi-particle systems, where the mass, diameter, restitution coefficient, density and granular temperature of the particles may be unequal. Different flow properties for solid phases (such as solid viscosity, solid pressure, collisional heat flux and bulk viscosity) resulting from particle–particle interactions are obtained from the multi-particle kinetic theory. The CFB that has been selected for investigation was previously tested by Mathiesen (1997) [
30].
2. Mathematical Model
Detailed development of the multi-particle kinetic theory, along with mathematical comparison with other available theories in the literature, has been presented in our previous publication [
3,
21,
31]. This theory has been implemented in the commercial CFD software CFX and used to simulate the riser section of a circulating fluidised bed having particles of different sizes. Two different particle species have been considered. Particles of each species are considered smooth, elastic and homogeneous spheres. Different flow properties for solid phases (such as solid viscosity, solid pressure, collisional heat flux and bulk viscosity) resulting from particle–particle interactions are obtained from the multi-particle kinetic theory. Interphase transfer terms (momentum transfer, fluctuating energy transfer) between the solid phases are also added to the code through the user subroutine. In the present model, we employed the standard k-epsilon turbulence model to simulate the experimental results. The choice of this turbulence model was motivated by its widespread use and applicability to a wide range of engineering scenarios. The k-ε model is well-suited for capturing turbulence characteristics and flow phenomena in various configurations, making it a suitable candidate for our investigation. A comparison of predicted results with experimental results validates the model [
32]. The CFB that has been selected for investigation was previously tested by [
30]. Details of the governing equations used in the simulations and the model formulation are summarised in
Table 1 [
3]:
Reynolds-Averaged Navier-Stokes equations (RANS) were used in the study (please refer to Table 5). RANS equations are only mentioned in Table 5 and not elaborately presented here in this paper, as the use of RANS Equations is standard practice in CFD. The standard k-ε model was used in this study (Table 5). In the Standard k-ε model, the eddy viscosity is computed from turbulent kinetic energy and turbulent dissipation. This eddy viscosity is used in RANS Equations. The electrostatic forces between the particles were ignored in the present study.
In the present model, the transport equations were discretised using the finite volume method (FVM). To discretise the convective term, we employ a second-order upwind scheme. This scheme is known for its ability to capture the directionality of flow and minimise numerical diffusion, especially in cases of high gradients. The diffusive term was discretised using a central differencing scheme, which provides second-order accuracy. This scheme is suitable for capturing diffusion effects accurately and maintaining stability. The source term was treated implicitly to ensure stability and accurate representation of the physics. We use the SIMPLE (Semi-Implicit Method for Pressure-Linked Equations) algorithm to handle the pressure-velocity coupling and ensure the pressure-velocity decoupling is carried out efficiently.
3. The CFB System
The CFB system experimentally investigated at Telemark Institute of Technology is shown in
Figure 1. The riser was cylindrical in shape with an internal diameter of 0.032 m and a height of 1.0 m. The primary gas inlet was located at the bottom of the riser. In order to provide a uniform gas velocity at the inlet, an air distributor was installed. The distributor was a Duran filter plate with a thickness and porosity of 0.004 m and 0.36, respectively. At the top of the riser, the suspended particles enter a glass cyclone where the solids are separated from the gas and recycled via a return loop. Supply of secondary air positioned at 0.05 m above the air distributor feeds the solids back to the riser.
Figure 1 shows a schematic sketch of the circulating fluidised bed system used in the experiment.
Two distinct particle groups were sieved out from a Gaussian particle size distribution with a Sauter mean diameter of 157 μm. The diameters of the sieved particles are between 100 and 130 μm and between 175 and 205 μm for the smallest and largest particles, respectively. The mean particle diameters of the two groups were approximately 120 and 185 μm. The two distinct groups were mixed together, and the initial volume concentration of each group was identical. The particle density was 2400 kg/m
3. The initial bed height was 0.04 m. Thus, the overall volume concentration of solids in the riser is 2.5%. The flow parameters used in this work have been shown in
Table 2.
4. Grid and Physical Domain
Only the riser part of the circulating fluidised bed shown in
Figure 1 has been modelled. In order to avoid convergence difficulties, the calculation domain is divided into five blocks. The grid characteristics and the grid information are listed in
Table 3 and
Table 4.
The grid independence test was performed for this study through the simulation of gas flow in the riser. Starting with a lower number of cells of 5600 in the riser, the number of cells in the riser was extended up to 33,600 in four steps. The calculated results for each step have been shown in Figure 3. It has been observed from Figure 3 that with the increase in cell number beyond 22,400, the velocity is independent of the number of cells. Therefore, for this study of the riser flow CFB, 22,400 cells have been used for further simulations. In this test, mass source residual (error in continuity) is used to control the convergence of the solution, and the tolerance limit was set to 10−6. In this simulation, the equation for continuity, momentum and transport equation for k and ε were solved for turbulence parameters.
5. Boundary and Initial Conditions
In this work, a wall boundary, inlet and outlet boundaries are used. The inlet boundaries are given by a specific inflow velocity and volume fraction. The inlet velocity and volume fraction used in this simulation are given in
Table 2. At the outlet, a pressure boundary condition with atmospheric pressure has been used. This essentially applies constant gradient conditions to the flow variables. Solids are also permitted to leave through the boundary. Buoyant flow has been enabled with gravity of 9.81 m/s
2.
For a gas, the no-slip wall condition is well accepted and used. However, for walls that are both non-slip [
17,
33] and free-slip [
34], solid velocity conditions have been used by different researchers. In general, it is not permissible to set the particle velocity equal to zero at a solid wall. Exceptions occur when the wall is sufficiently rough, minimising particle slip and when the bounding wall is sufficiently soft, creating highly inelastic particle–wall collisions. Tsuo and Gidaspow [
35] used a partial-slip boundary condition, which is between the two mentioned conditions. Insufficient numerical and experimental work has been undertaken to show any boundary condition as being superior with all capable of predicting clusters. In non-slip boundary conditions near the wall, some fluid (for example, a layer of fluid molecule/molecules) is assumed to attach to the solid wall, whereas in no slip boundary condition, fluid does not attach to the solid wall. Slip boundary conditions are used to model the behaviour of particles near solid surfaces, where the particles experience a slip velocity relative to the fluid due to a lack of adhesion. The choice of slip condition can indeed influence the results of simulations, and using different slip models, such as partial slip conditions or incorporating slip lengths, could provide valuable insights into the role of slip in the observed deviations. In our study, we chose a slip boundary condition based on the available literature and its relevance to the specific system we were simulating.
In this work, the riser is initially filled with a 0.04 m high bed where the total volume fraction of solids is approximately 0.63. The initial volume fractions for each individual phase have been show in
Figure 2. The two solid phases are perfectly mixed in the bed and are assumed to have an identical initial volume fraction. In order to avoid convergence difficulties, the initial volume fraction of the solids above the bed in the computational domain is set to 1.0 × 10
−10, and to ensure a small initial viscosity, the granular temperature has been set to 1.0 × 10
−10 in this work.
The proposed multi-particle kinetic theory of [
3,
21,
31] was implemented in the commercial CFD code CFX through user subroutines. A time step of 0.001 s is used for the calculations. The under-relaxation factor used for the velocities and volume fraction was 0.3, and for the granular temperature, it was 0.2. Typically, 32.5 h of computational time is required on an Intel Pentium 4 (Xeon) 2.0 GHz computer to simulate one second of real-time. A summary of the model formulation used in the present work is introduced in
Table 5.
7. Conclusions
In this work, a new kinetic theory (KT) model for particles of different densities and sizes has been implemented in the commercial CFD software CFX and used to simulate the riser section of a circulating fluidised bed having particles of different sizes. Different flow properties for solid phases, such as solid viscosity, solid pressure, collisional heat flux and bulk viscosity resulting from particle–particle interactions, are obtained from the present CFD model. Interphase transfer terms (i.e., momentum transfer and fluctuating energy transfer) between the solid phases are also implemented into the CFD model through user-defined functions (UDFs). The k-ε turbulence model is used in simulating the circulating fluidised bed model. For verification, simulation results obtained with the new KT model are compared with experimental data, and then the model is used for further analysis. Using the CFD model, results were obtained for a three-dimensional circulating fluidised bed model that are in fairly good agreement with experimental results. The model successfully predicts typical CFB behaviour, such as
Core–annular flow in the riser,
Particle carryover,
Cluster formation,
Downward particle flow near the riser wall,
Relative velocity between particles of different sizes,
Different granular temperatures for particles of different sizes,
A turbulent bed of large diameter particles in the base of the riser and transport of the smaller particles well in the top section of the riser,
A higher concentration of solids in the wall region compared to the centre.
The predicted results are in qualitative agreement with published experimental work. This indicates that the multi-particle multiphase gas–solid flow model works fairly well.