Analysis of the Internal Flow Field Characteristics of a Novel Cyclone Dust Removal Device

Abstract

This paper presents a novel cyclone dust removal device and conducts a preliminary investigation into its internal flow field characteristics. The device is equipped with an impeller with Archimedean spiral characteristics and a whip sheath structure arranged in a circle. Using the computational fluid dynamics (CFD) method, the velocity field, pressure field, vortex structure, and fluid trajectory characteristics are studied under the condition of a fixed rotational speed and different inlet velocities. The simulation results demonstrate that, under a fixed rotational speed of 24.5 rps and TSR = 2.0, the downstream vortex system of the impeller is more coherent and structured, developing into a stable configuration with alternating positive and negative vorticity. When the whip sheath structure is added, a larger radial velocity is generated. This study reveals the unique internal flow field evolution law of the device, which provides a theoretical basis for subsequent particle separation research.

1. Introduction

At present, industrial sources such as thermal power plants release a large amount of particulate matter into the atmosphere through their chimneys [1]. The risk of illness and death increases when people are exposed to fine particulate matter such as PM2.5 for a long time [2]. Meanwhile, particulate matter pollution has become one of the greatest environmental health risks worldwide. Therefore, how to effectively control industrial particulate matter emissions without inhibiting industrial economic development is a key issue to be solved in the field of environmental governance. At present, the treatment technology for gas particles mainly includes gravity sedimentation, centrifugal separation, dry dust removal, and wet washing, among which the cyclone separator based on the principle of centrifugal force is the most widely used. The device produces a centrifugal effect on the particulate matter to achieve separation [3,4]. Because the device has high separation efficiency, depends on its own wind energy to achieve separation, and has the advantages of a simple structure and low running cost, it is widely used in chimney discharge treatment units.

Experimental measurements are among the most effective ways to study the physical mechanisms of cyclone separators. By using a high-speed imaging system and a pressure measuring device in the experiment, the flow patterns of gas and particles and the pressure distribution pattern in the cyclone separator can be directly obtained to study the physical mechanism of centrifugal separation. Wang et al. experimentally studied a new oil–gas separator with a multi-layer central channel structure and found that the three-layer channel structure still maintained excellent separation performance at low inlet velocities [5]. Niraula et al. determined the cyclone separation efficiency from the Leith-Licht equation and studied the particle size separation efficiency by experimentally adjusting the motor to different speeds. The experimental results demonstrated an average efficiency of 85% in segregating particulates above 20 microns [6]. Wang et al. studied a new type of axial cyclone separator and set up an experimental setup to study how inlet conditions affect the separation characteristic parameters. Experimental studies show that the separation purity and extreme points of the air separation efficiency are independent of the inlet liquid flow rate. The separation pressure drop is quadratically related to the inlet airflow rate [7]. Peng et al. studied the properties of the vortex end of the cyclone separator by visualization using a stroboscope and high-time-resolution pressure measurements. Experimental studies show that the frequency with which the vortex core rotates varies in the same way as the frequency with which the gas rotates higher in the separator [8]. Elsayed et al. computationally studied the effect of four cyclone separators with different dust outlet geometries on the flow pattern and performance of cyclonic streamers. The study shows that the maximum tangential velocity of the four test cyclones is almost the same [9]. Sun et al. used 3D printing technology to manufacture an elliptical cyclone separator and revealed the strengthening mechanism of the circumferential acceleration/deceleration effect caused by the elliptical cross-section on particle separation through experiments and CFD. They found that the separation efficiency was increased by about 2% and the pressure drop was reduced by 43% compared with a circular cross-section [10].

It is very important to study the radial velocity, axial velocity, and vortex structure distribution in a cyclone separator, but they are difficult to measure experimentally. Compared with experiments, numerical simulations can effectively obtain the gas flow characteristics in the cyclone separator, which is helpful for further optimizing the design of a new cyclone separator. Wasilewski et al. used LES and DPM models to study the effect of a roof clean air inlet on the performance of a cyclone separator, and the new model improved the separation efficiency of clean gas at all inlet velocities [11]. Sajjad et al. enhanced the analysis of cyclone separators in terms of particulate collection efficiency, using fluid dynamics numerical simulations to analyze the impact of cyclone size on the flow field and particle collection efficiency [12]. Dziubak et al. numerically analyzed the effects of inlet velocity and geometric parameters on the separation efficiency and pressure drop of axial inlet cyclone separators, revealing the sensitivity ranking of key geometric parameters [13]. Nie et al. established a model through CFD to simulate and analyze the impact of different pitches on separation efficiency. The results show that the third pitch has the greatest impact on separation efficiency and pressure drop, while the first pitch has the least impact, with the separation efficiency of the cyclone structure exceeding 98% [14]. Calvopiña et al. used CFD simulations and modeled the SST turbulence model to simulate the effects of changes in the diameter of the vortex detector and inlet velocity on the separation efficiency and pressure drop of the Echeverría cyclone separator. The results indicate that increasing the diameter of the vortex detector can reduce tangential velocity and pressure drop. However, due to weakened centrifugal force and reduced particle residence time, the separation efficiency drops from 98.2% to 88.76% [15]. Guo et al. proposed an integrated optimization framework to analyze the relationship between different geometric size ratios and inlet gas velocity concerning performance metrics, deriving optimal design parameters using a non-dominated sorting genetic algorithm II. The results show that the optimized cyclone separator design improves separation efficiency by about 15.44%, reduces pressure drop by 15.6%, and decreases erosion rate by 9.18% [16]. Safikhani et al. used numerical simulations of the Euler–Lagrange two-phase method to study the tangential velocity profiles and velocity vectors of different profiles of a new type of cyclone separator [17]. Wang et al. analyzed the structural parameters of the insertion tube below the vortex detector using CFD and found that converging insertion tubes achieve better separation performance for small particles (<5 μm) [18]. Fu et al. systematically studied the correlation between the high-speed self-rotational motion and axial orbital motion of particles in cyclone separators under different structures and operating parameters using a CFD-DEM coupling method, pointing out that understanding the coupling mechanism between turbulence and particle spin can provide new theoretical support for improving separation performance [19].

Based on the above research, it is concluded that changes to various dimensions can improve the separation efficiency of the cyclone separator. However, the separation efficiency is also related to the physical geometry, which can easily lead to insufficient centrifugal force, resulting in inadequate removal capability for fine particles and small droplets. In this regard, Zhang et al. studied the addition of different-shaped baffles to increase the centrifugal force and found that the convex baffle structure can effectively increase the radial velocity near the wall, significantly enhancing the separation efficiency of 5 μm particles [20]. Therefore, according to the principle of the traditional cyclone dust collector, this paper designs a novel cyclone dust removal device to improve the flowability and finally achieve the purpose of dust removal. In this study, its structure and flow field characteristics are analyzed and optimized by numerical simulation.

2. Structural Design and Operating Principle

In this paper, a novel cyclone dust collector is designed. It is mainly composed of an Archimedean spiral impeller, the whip sheath structure, an outer shell, and an inner liner, as shown in Figure 1. The Archimedean spiral impeller is fixed at the bottom end of the transmission shaft and adopts three blades with a standard Archimedean spiral profile [21]. The three blade profiles are evenly distributed along the circumferential direction and arranged in a spiral upward manner. The whip sheath structure is arranged equidistantly along the axial direction of the transmission shaft and extends radially outward, with the ends of the whip sheath structure maintaining a slight clearance fit with the inner wall of the inner liner.

The parameters of the impeller and the whip sheath structure are shown in Figure 2. The key geometric parameters of the device are presented in

Table 1. Key geometric parameters of the main device.

Parameter Names	Specific Values
Number of blades	m = 3
Blade thickness	T = 2 mm
Impeller diameter	$D_1$= 260 mm
The opening angle of the first blade	${\alpha }_1={60}^{\circ }$
The opening angle of the second blade	${\alpha }_2={60}^{\circ }$
The opening angle of the third blade	${\alpha }_3={60}^{\circ }$
Blade pitch	S = 27 mm
Diameter of the rotation axis	d = 20 mm
Number of whip sheaths per strand	N = 10
Number of configurable whip sheath columns	n = 25
The thickness of the whip sheath	t = 5 mm
Whip sheath diameter	$D_2$ = 260 mm
Inner liner diameter	$D_3$ = 312 mm

. The whip sheath structure is made of a harder material. Under wind disturbance conditions, it can maintain its own shape. It also forms a coaxial arrangement with the impeller.

The expected operating principle of the proposed cyclone separator is shown in Figure 3. During operation, the gas enters the device through the gas inlet and is accelerated by the Archimedean spiral impeller. This process produces a high-speed rotating airflow at the rear of the impeller. The whip sheath structure rotates synchronously with the impeller to disperse the central airflow to the wall as much as possible. The device is expected to push impurities (dust particles) in the gas toward the wall. Under the force of gravity, they slide down the wall into the box. This time, only the airflow motion condition is considered, and the particle motion is not analyzed. While studying the internal flow field characteristics of the novel cyclone separator, the velocity, pressure, vortex structures, and streamlines at typical axial cross-sections were selected for analysis. The flow field shown later is a planar section extracted from 3D space, which is an instantaneous section fixed in a stationary reference frame.

3. Numerical Theory and Detailed Exposition

3.1. Numerical Model

For the internal flow field of the cyclone separator, the RSM model can fully capture Reynolds stress anisotropy, and its theoretical prediction accuracy is higher than that of the conventional two-equation model. However, it has drawbacks, including difficult convergence, strict mesh requirements, and a long simulation cycle. The LES model requires significantly finer mesh resolution, especially in the near-wall region, resulting in a substantial increase in computational cost [22]. The model is more accurate and reliable and applies to a wider range of fluid flow categories [23]. The model provides better prediction near the boundary layer with less computational cost. In addition, since the device involves mechanical rotation and the model is well-suited for simulating rotating flows, the SST k-ω model is adopted as the turbulence model.

Continuity equation:

$${\displaystyle \frac{\partial \rho }{\partial t}}+{\displaystyle \frac{\partial \left(\rho u_i\right)}{\partial x_i}}=0$$

(1)

where $\rho$ is the fluid density; $x_i$ is a Cartesian coordinate (i = 1, 2, 3); $u_i$ is the velocity component in the Cartesian coordinate system; and t is time.

Momentum conservation equation:

$${\displaystyle \frac{\partial \left(\rho u_i\right)}{\partial t}}+{\displaystyle \frac{\partial \left(\rho u_i{u}_j\right)}{\partial x_j}}=-{\displaystyle \frac{\partial P}{\partial x_i}}+{\displaystyle \frac{\partial {\tau }_{ij}}{\partial x_i}}+S$$

(2)

where P is the flow field pressure; S is a user-defined source term; $x_j$ is a Cartesian coordinate, j = 1, 2, 3; $u_j$ is the velocity component in the Cartesian coordinate system; ${\tau }_{ij}$ is the viscous shear stress and is expressed as follows.

$${\tau }_{ij}=\mu \left({\displaystyle \frac{\partial u_i}{\partial x_j}}+{\displaystyle \frac{\partial u_j}{\partial x_i}}-{\displaystyle \frac{2}{3}}{\delta }_{ij}{\displaystyle \frac{\partial u_k}{\partial x_k}}\right)$$

(3)

where $\mu$ is the dynamic viscosity; $x_k$ represents Cartesian coordinates, k = 1, 2, 3; ${\delta }_{ij}=\left\{\begin{array}{l}1\hspace{0.33em}\hspace{0.33em}\hspace{0.33em}i=j\\ 0\hspace{0.33em}\hspace{0.33em}\hspace{0.33em}i\ne j\end{array}\right.$ is the Kronecker symbol. Menter [24] proposed and combined the shear stress transfer SST k-ω turbulence model of FVM. The equations for the shear stress transfer turbulence model are given in Equations (4) and (5).

$${\displaystyle \frac{\partial \left(\rho k\right)}{\partial t}}+{\displaystyle \frac{\partial \left(\rho u_{j}k\right)}{\partial x_j}}={\tau }_{ij}{\displaystyle \frac{\partial u_i}{\partial x_j}}-{\beta }^{\ast }\rho k\omega +{\displaystyle \frac{\partial }{\partial x_j}}\left[\left(\mu +{\sigma }_k{\mu }_t\right){\displaystyle \frac{\partial k}{\partial x_j}}\right]$$

(4)

where $u_i$ and $u_j$ are velocity components in the x and y directions; k is the turbulent kinetic energy; $\omega$ is the specific dissipation rate; ${\sigma }_k=F_1{\sigma }_{k1}+\left(1-F_1\right){\sigma }_{k2}\omega$.

$${\displaystyle \frac{\partial \left(\rho \omega \right)}{\partial t}}+{\displaystyle \frac{\partial \left(\rho u_j\omega \right)}{\partial x_j}}={\displaystyle \frac{\gamma }{{\nu }_t}}{\tau }_{ij}{\displaystyle \frac{\partial u_i}{\partial x_j}}-\beta \rho {\omega }^2+{\displaystyle \frac{\partial }{\partial x_j}}\left[\left(\mu +{\sigma }_{\omega }{\mu }_t\right){\displaystyle \frac{\partial \omega }{\partial x_j}}\right]+2\rho \left(1-F_1\right){\sigma }_{\omega 2}{\displaystyle \frac{1}{\omega }}{\displaystyle \frac{\partial k}{\partial x_j}}{\displaystyle \frac{\partial \omega }{\partial x_j}}$$

(5)

where $v_t={\mu }_t/\rho$ is the turbulent eddy viscosity; ${\sigma }_{\omega }=F_1{\sigma }_{\omega 1}+(1-F_1){\sigma }_{\omega 2}$; $\gamma =F_1{\gamma }_1+(1-F_1){\gamma }_2$; ${\gamma }_1={\beta }_1/{\beta }^{\ast }-{\sigma }_{\omega 1}{k}^2\sqrt{{\beta }^{*}}$; ${\gamma }_2={\beta }_2/{\beta }^{\ast }-{\sigma }_{\omega 2}{k}^2\sqrt{{\beta }^{*}}$; $\beta =F_1{\beta }_1+\left(1-F_1\right){\beta }_2$; F₁ is the first mixing function. The constants in the SST k-ω turbulence model are shown in

Table 2. SST k-ω turbulence model constants.

Parameters	Value
α1	0.31
σk1	0.85
σk2	1.0
σω1	0.5
σω2	0.856
β1	0.075
β2	0.0828
k	0.41
β*	0.09

.

3.2. Computational Domain and Mesh Generation

To simulate the rotation state of the impeller, the model was simplified as follows: the rotating domain is employed to replicate the impeller’s rotational motion, while the stationary domain represents the internal space of the device. Both domains are configured as cylindrical flow regions coaxial with the Archimedes spiral impeller and defined as in Figure 4. The Cartesian coordinate system is used for the calculation. The diameter of the Archimedes spiral impeller is defined as D = 260 mm; the stationary domain features a circular cross-section with a length of 16D and a diameter of 1.5D. To ensure the impeller’s rotational motion is fully contained within the stationary domain, the rotating domain is designed as a cylindrical region with a length of 5.5D and a diameter of 1.2D. Furthermore, to improve the realism of the simulation and mitigate the impact of the impeller’s rotational motion on the incoming gas flow, the distance between the velocity inlet of the stationary domain and the rotating impeller domain is set to 2.5D. The inlet boundary condition is defined as a velocity inlet, the outlet boundary condition is set as a pressure outlet, and the wall boundary is used to calculate the side boundary of the domain as well as the spiral impeller blade, which is the gray boundary in Figure 4.

To facilitate the subsequent axial and radial correlation calculation, X is assumed to be axial. Then, $U_r$ stands for radial velocity, and $U_{\theta }$ stands for tangential velocity:

$$r={(y^2+z^2)}^{{\displaystyle \frac{1}{2}}}$$

(6)

$$U_r={\displaystyle \frac{(y{U}_y+z{U}_z)}{r}}$$

(7)

$$U_{\theta }={\displaystyle \frac{(-z{U}_y+y{U}_z)}{r}}$$

(8)

To obtain the internal flow field characteristics of the device, numerical calculations at different velocities are performed. The magnitude of the velocity is expressed in dimensionless form using the Tip–Speed Ratio (TSR), which is the ratio of the tip linear velocity to the wind velocity. The formula for calculating TSR is:

$$TSR={\displaystyle \frac{\omega R}{U_0}}={\displaystyle \frac{2\pi R\mathrm{n}}{U_0}}$$

(9)

where $\omega$ denotes the angular velocity of the rotor; R represents the rotor radius; and $U_0$ represents the incoming flow velocity. While the velocity of the incoming wind is constant, a larger tip–speed ratio (TSR) indicates a higher rotational speed of the rotor. The speed is fixed at n = 24.5 rps, and the incoming flow velocity is changed under different TSR values in this paper.

Table 3. Parameters at various operating conditions.

Rotational Speed (rps)	Inlet Velocity (m/s)	Operating Condition	Reynolds Number
24.5	20.0119	TSR = 1	344,578
24.5	13.3414	TSR = 1.5	229,719
24.5	10.0060	TSR = 2	172,288
24.5	8.0048	TSR = 2.5	137,830
24.5	6.6705	TSR = 3	114,856

shows the inlet velocity, TSR, and Reynolds number at a fixed speed. In the following, the study will be carried out at a fixed speed.

In this paper, the software Simcenter STAR-CCM+ version 2020.3 is used for simulation calculations. Rigid Body Motion (RBM) is used to simulate the real rotational motion of the impeller. In this paper, implicit unsteady algorithms are used for numerical calculations. The numerical scheme is designed as follows: the gradient uses a unit-based least-squares scheme, and the transient computation time is discretized implicitly at second order. The velocity–pressure coupling is solved using a segregated flow solver based on the SIMPLE algorithm, with the convection terms discretized using a second-order scheme. The near-wall treatment uses the full y+ adaptive wall treatment. The absolute residuals of all flow and turbulence equations converged to 10⁻⁵. The time step is 1.1337 × 10⁻⁴ s and corresponds to about 1° rotation of the impeller per step. The simulated physical time is 0.4081 s, corresponding to about 10 impeller rotation cycles, ensuring that the flow field is fully developed and has entered a statistically stable state. The torque coefficient is taken as the monitoring period quantity, and Figure 5 can be obtained using STAR-CCM+ software. The figure shows that the stable value is reached after 0.1 s. The inlet condition is turbulent. The turbulence intensity is 0.01, the turbulent viscosity ratio is 10, and the turbulent velocity ratio is 1 m/s. The rotation–fixed interface is defined as the sliding mesh interface, and the incompressible gas flow at room temperature is simulated. The air density is 1.184 kg/m³, and the dynamic viscosity is 1.855 × 10⁻⁵ Pa·s. The outlet pressure is atmospheric. The numerical method has been used to study a variety of similar cases. The current numerical method can reduce the computational cost and ensure the accuracy of the results. To achieve an accurate representation of the geometry, the mesh of the stationary domain and rotating domain were refined separately, as presented in Figure 6. To capture the fine flow field downstream of the impeller, local mesh refinement was implemented in regions with tip vortex structures and high velocity gradients, as illustrated in Figure 6b. The mesh generation process is described as follows: First, a surface remeshing generator was applied to the object surfaces, followed by the generation of a high-quality surface mesh with well-formed triangular tessellation. Subsequently, a volume mesh containing a prism layer mesh and trimmed mesh was generated based on this surface mesh. A boundary layer was configured on the object surfaces, consisting of 10 layers with a growth rate of 1.2 and a total thickness of 0.003 m, as shown in Figure 6c. To satisfy the algorithm requirements, the value of y+ is set below 30 to ensure the reliability and accuracy of the results that are produced in the numerical simulation, as shown in Figure 7.

3.3. Mesh Independence Analysis

The number and quality of the mesh significantly influence the computational efficiency and accuracy of the numerical results. To assess the mesh sensitivity, three mesh configurations (coarse, medium, and fine) are generated by adjusting the element size in refined regions and on the surfaces of objects. The element counts of these three meshes are approximately 699,399, 1,740,314, and 3,482,358, respectively. Numerical calculations were conducted for the operating condition of TSR = 2. The torque coefficient calculation formula is described as follows:

$$C_T={\displaystyle \frac{T}{0.5\rho S{U}_0^{2}R}}$$

(10)

where $\rho$ represents the fluid density, $T$ is the torque, $U_0$ represents the incoming flow velocity, and $S$ represents the area swept by the impeller.

Based on the above conditions and the formula, the torque coefficients of the impeller were obtained and are presented in

Table 4. Computational results of different mesh resolutions.

Case	Mesh Count	Torque Coefficient	Torque Error
Coarse	699,399	0.2882	2.205%
Medium	1,740,314	0.2945	0.068%
Fine	3,482,358	0.2947	-

.

When calculating torque error, ensure that the flow parameters are consistent. Meanwhile, the torque errors of the coarse and medium meshes are separately compared with the results obtained from the fine mesh. As shown in Table 4, the torque errors between the coarse and fine meshes and between the medium and fine meshes, are 2.205% and 0.068%, respectively, both of which are below 5%. Thus, mesh refinement contributes to reducing torque error and enhancing the stability of computational results.

Figure 8 presents a comparison of typical velocity contours for different meshes, revealing that the internal velocity distributions of the device are essentially consistent across all meshes, with the locations of maximum and minimum velocities remaining identical. In Figure 8, $U_x$ represents the axial velocity distribution value, and $U_0$ represents the incoming flow velocity. $U_x/U_0$ represents the dimensionless value of the axial velocity distribution. For further analysis, 100 monitoring points were selected along the line from coordinates [0.0, 0.0, 0.115] to [0.5, 0.0, 0.115] (as shown in Figure 8c), and the axial dimensionless velocities at these points were extracted, as illustrated in Figure 9. The results indicate that the velocity distributions are nearly identical among the three meshes, further demonstrating that the mesh has a minimal impact on the results. Figure 10 presents the comparison of pressures for different mesh resolutions. The denser the mesh, the smoother the pressure curve. The results also show that the pressures of different meshes are about the same, and the mesh has a minimal impact on the results. In this paper, the tangential velocity is also selected as the judgment index. The relationship between the tangential velocity and the mesh scheme is shown in Figure 11. By comparing the tangential velocities under different mesh schemes, it is found that the curves exhibit good agreement. This numerical method has been used to study many similar cases, and the results are stable after several calculations under the same operating conditions in this paper. Therefore, to achieve a balance between computational accuracy and simulation time, the medium mesh is adopted for all subsequent cases.

3.4. Sensitivity Analysis of Turbulence Models

To evaluate the influence of turbulence model selection on the calculation results, this paper supplements the sensitivity analysis with a turbulence model sensitivity analysis. The analysis follows the variable-unique logic: under the premise of keeping the computational mesh, boundary conditions, discrete scheme, convergence criterion, and wall treatment completely consistent, only the turbulence model is changed. By comparing the results of the Standard k-ε and SST k-ω models selected in this paper, this paper verifies whether model selection significantly affects the core conclusions.

Figure 12 illustrates the comparison of the flow fields. The left column is SST k-ω and the right column is Standard k-ε. The axial velocity distributions, pressure distributions, and vortex structures at the characteristic cross-sections exhibit excellent agreement. It can be concluded that no fundamental changes occur in the flow field structures and flow patterns. The torque coefficients predicted by the two turbulence models are shown in

Table 5. Torque comparison of turbulence models.

Turbulence Model	Torque Coefficient	Relative Deviation
Standard k-ε	0.2897	1.629%
SST k-ω	0.2945	-

. Taking the SST k-ω model as the benchmark, the relative deviation of the Standard k-ε model is within 5%, demonstrating satisfactory numerical consistency.

The foregoing results indicate that under the operating conditions of the present study, the flow field characteristics exhibit limited sensitivity to the selection of turbulence models, and the choice of turbulence model does not significantly alter the core conclusions of this work.

4. Results and Discussion

4.1. Analysis of Internal Flow Field Characteristics of the Device

4.1.1. Analysis of the Velocity Flow Field

Figure 13 presents the axial velocity contours at the mid-longitudinal cross-section under a fixed rotational speed and different TSR conditions. It is observed that after passing through the impeller, a distinct red region (high-speed zone) of axial velocity forms above the blade tip (near the surrounding wall surfaces). This phenomenon is primarily attributed to the pressure difference between the pressure and suction sides of the blades: fluid traverses the tip clearance, generating a high-speed tip jet. The jet interacts with the mainstream and wall surfaces, becoming compressed within the narrow near-wall region and thus accelerating. Low-speed regions are mainly distributed behind the suction side of the blades, near the hub, and in the core of the wake. This is because during the impeller’s rotational operation, the axial kinetic energy of the fluid is converted into mechanical energy, leading to a decrease in axial velocity as the fluid passes through the impeller disk. At a fixed rotational speed and low TSR, large areas of deep blue (low-speed zones) are observed in the contours, indicating severe stall and flow separation on the blade surfaces, with large-scale, disordered vortex shedding structures existing in the wake region. As TSR increases, the deep blue low-speed zones narrow and shorten significantly; the wake rapidly mixes with and dissipates into the mainstream downstream, resulting in a more uniform and stable flow field. Figure 14 shows the axial velocity distribution of the probe position under a fixed rotational speed and different TSR conditions. A total of 100 probe points are selected along the line from coordinates [0.0, 0.0, 0.115] to [0.5, 0.0, 0.115]. Overall, the axial velocity exhibits periodic variations with a gradually decreasing amplitude. At a fixed rotational speed and low TSR, the axial velocity fluctuation amplitude is significant, indicating strong unsteady disturbances in the flow field. As the TSR increases, the amplitude decreases monotonically, and the smoothest fluctuations are observed at TSR = 3; this reflects the process by which the flow field velocity distribution tends toward uniformity. Notably, the axial velocity curve for TSR = 2 exhibits the most pronounced periodicity, with the amplitude decreasing from large to small, suggesting that the fluid’s spiral motion is fully developed under this operating condition.

In this paper, the cross-sectional plane that is located 0.075 m downstream of the Archimedean spiral impeller is selected to carry out the numerical simulation, as shown in Figure 15. It is concluded that the high-speed and low-speed regions are alternately formed after passing through the impeller. This local gradient pattern is a typical hydrodynamic projection of tip leakage vortices (TLVs) on the cross-section. Under low-TSR conditions, the flow field is filled with extensive, alternately distributed high- and low-speed zones, indicating intense global radial mixing of the mainstream driven by strong centrifugal effects and large-scale vortex shedding. The radial velocity contours under different TSR conditions are depicted in Figure 16. Here, $U_r$ represents the radial velocity, and the rest is consistent with the representation in Figure 8. The red curve indicates fluid flowing outward (toward the tip) due to centrifugal force, the blue curve represents fluid moving inward (toward the hub) induced by vortices, and the green curve signifies near-zero radial velocity when the flow field is dominated by purely axial advection. As the value of TSR increases, the radial disturbances that occur in the mainstream are significantly suppressed, and the flow rapidly evolves into an ordered state dominated by axial advection. Combined with the dimensionless axial velocity distribution in the figure, it is seen that the swirling characteristics of the flow field at TSR = 2 are more significant.

4.1.2. Analysis of Pressure Flow Field

To analyze the flow field characteristics in the pressure field, the dimensionless pressure formula is used as follows:

$$C_p={\displaystyle \frac{p-p_0}{0.5\rho U_0^2}}$$

(11)

where $p$ represents the absolute total pressure, $p_0$ represents the static pressure, $\rho$ represents the density of the fluid, and $U_0$ represents the incoming flow velocity.

Figure 17 presents the pressure contours at the mid-span cross-section under fixed rotational speed and different TSR conditions. It is observed that upon impact with the blade leading edge, a distinct red high-pressure region forms on the blade pressure side. This phenomenon arises primarily from the rigid obstruction of the incoming flow by the pressure surface: the flow velocity decays sharply to near-zero over an extremely short distance, leading to extensive conversion of the fluid’s kinetic energy into static pressure energy. Low-pressure regions are concentrated in the wake vortex core and downstream of the blade trailing edge. During the impeller rotation, fluid acceleration along the blade, in accordance with Bernoulli’s principle, results in a significant reduction in static pressure as kinetic energy increases; additionally, high-speed rotation within the vortex core generates intense centrifugal effects, further contributing to low-pressure formation. As the TSR increases, the inflow velocity progressively declines, mitigating the impact on the impeller. Consequently, the red high-pressure zones exhibit noticeable contraction and reduced intensity, while deep blue low-pressure regions transition to light blue. Wake vortices undergo a reduction in size and an increase in the number of vortices, driving the flow field toward greater uniformity and stability. Figure 18 shows the probe pressure diagrams at a fixed location under fixed rotational speed and different TSR conditions. The probe position and velocity measurement parameters remain consistent across all cases. Overall, pressure curves under all operating conditions display distinct periodic fluctuation characteristics. As TSR increases from 1 to 3 at a fixed rotational speed, the pressure distribution undergoes a systematic evolution marked by decreasing amplitude and enhanced flow field uniformity.

4.1.3. Analysis of Flow Fields with Vortex Structures

In Figure 19, the formula represents the dimensionless vortex structure, where $\omega$ represents the vorticity, $D$ represents the impeller diameter, and $U_0$ represents the incoming flow velocity. In the mid-span longitudinal cross-section under a fixed rotational speed and different TSR conditions, the vorticity plots are depicted in Figure 18. The plots explicitly reveal that there is an interlaced distribution of red positive vortices (counterclockwise rotation) and blue negative vortices (clockwise rotation). This phenomenon arises from the formation of two oppositely oriented boundary layers on the blade pressure and suction sides: the flow velocity on the pressure side lags behind the mainstream and generates clockwise negative vortices, while the velocity on the suction side exceeds the mainstream, giving rise to counterclockwise positive vortices. Specifically, under the operating conditions of low TSR (TSR = 1 and 1.5), the wake region is fully occupied by large-scale, highly irregular block-shaped separated vortices, indicative of strong three-dimensional unsteady flow. As TSR increases to moderate values (TSR = 2 and 2.5), the wake exhibits distinct directional strip-like transitional vortex systems. At a high value of TSR (TSR = 3), a remarkably clear and continuous tip vortex is observed, which is accompanied by a hub vortex that extends steadily downstream along the central axis.

4.1.4. Analysis of Flow Fields Using Streamlines

The three-dimensional streamline visualization plots under fixed rotational speed and different TSR conditions are described in Figure 20. The plots demonstrate that the wake maintains distinct spiral swirling flow characteristics, with localized high-velocity regions forming near the blade tips. At a fixed rotational speed and low TSR, the fluid exhibits a highly chaotic and tangled morphology after passing through the impeller, with extensive low-velocity zones in the wake region. As the state changes to moderate TSR, the reverse flow is significantly reduced, and the wake still retains prominent spiral swirling features, while a relatively thick bundle of low-velocity streamlines persists in the central area. Furthermore, in the state of high TSR, the flow field becomes highly organized, the spiral swirling characteristics in the wake weaken, and the streamlines tend toward purely axial advection. Meanwhile, a thread-like helical trajectory (tip leakage path) is clearly captured around the blade tip periphery. The fluid streamlines show that the fluid is driven by the impeller to produce an obvious radial outward flow diffusion.

4.1.5. Analysis of Performance Quality

By comparing the fan’s instantaneous power efficiency, the advantages and disadvantages of its performance under different tip–speed ratio (TSR) conditions are analyzed. In this paper, the following formula is used for research:

$$P_{\mathrm{out}}=M\omega$$

(12)

where the $P_{\mathrm{out}}$ represents the total output power, $M$ represents the torque obtained by numerical simulation, and $\omega$ represents the angular velocity.

The formula for the total input power is:

$$P_{\mathrm{in}}={\displaystyle \frac{1}{2}}\rho U_0^{3}A$$

(13)

where $P_{\mathrm{in}}$ represents the total input power, $\rho$ represents the gas density, $U_0$ represents the inlet velocity, and $A$ represents the area swept, where $A=\pi R^2$.

When the total output power and the total input power are known, the instantaneous power efficiency of the fan can be obtained:

$$\eta ={\displaystyle \frac{P_{\mathrm{out}}}{P_{\mathrm{in}}}}$$

(14)

where $\eta$ represents the instantaneous power efficiency of the fan. Figure 21 illustrates the instantaneous power efficiency of the fan as a function of TSR. With the increase in TSR, the instantaneous power efficiency of the fan shows a trend of first increasing and then decreasing and reaches the peak when TSR = 2.

4.2. Analysis of Internal Flow Field Characteristics of the Device with the Whip Sheath

A comparison of the device’s geometric structure is shown in Figure 22. Here, 25 whip sheath structures are selected as the research objects. Based on the previous analysis of the internal flow characteristics, TSR = 2 was used for detailed flow field analysis of the selected operating conditions. By comparing with velocity, vortex structures, and streamline contours, the evolution of the internal flow field after adding the whip sheath structure is systematically analyzed, clarifying the mechanism by which the added whip sheath structure enhances the flow performance of the gas.

Figure 23 shows the comparison of the internal velocity field contours for devices with and without the whip sheath structure. Note that Figure 23a is identical to the verified mesh model in Figure 8b, which is reused here as the benchmark group to enable a clear control comparison. Overall, acting as a flow-disturbing element, the whip sheath structure disintegrates the low- and medium-velocity flow regions. The originally periodic low-velocity zones and concentrated medium-velocity regions uniformly evolve into fine small-scale streak structures, with the axial velocity increasing progressively from the inner to the outer side along the whip sheath structure. The high-velocity flow in the near-wall region transforms from a periodically distributed pattern into a continuous and smooth distribution. The recovery process of wake velocity is promoted. Consequently, with the introduction of the whip sheath structure, the central gas flow diffuses more effectively toward the periphery, and a continuous and uniform high-velocity zone is established along the wall surface.

The dimensionless axial velocity contour only observes the blocking effect of the whip sheath structure on the gas flow from the side. In contrast, the dimensionless radial velocity gives an intuitive view of the instantaneous flow of gas over the whip sheath structure. Therefore, the sections at 0.075 m, 0.278 m, and 0.482 m are selected to study the dimensionless radial velocity contour in this paper, as shown in Figure 24. The left column is the working condition without the whip sheath structure, and the right column is the working condition with multiple groups of the whip sheath structure. It is seen that under the working condition of the non-whip sheath structure, the velocity of each section presents a small number of alternating positive and negative distribution forms, and with the increase in the axial distance, the radial velocity intensity continues to decay along the path, and the radial flow tends to be smooth when the section is at 0.482 m. After adding multiple groups of the whip sheath structure, the radial flow strength of each section is significantly enhanced. The radial velocity region originally distributed on the wall is dispersed and evolves into a high-speed region with consistent diffusion from inside to outside. At the section of 0.482 m, it still maintains the high-speed alternating positive and negative morphology. In summary, the whip sheath structure effectively improves the radial velocity level of the whole flow field and converts the axial kinetic energy of the fluid into radial kinetic energy, so that the airflow effect persists over a longer axial distance.

The influence of the whip sheath structure on the distribution of the flow field was qualitatively analyzed through the radial velocity cloud map above. To further quantify the control effect of the whip sheath structure on the radial airflow, the area mean absolute radial velocity was selected as the characteristic index to compare the flow characteristics with and without 25 columns of the whip sheath structure. The above three cross-sections were selected as the research objects, and the area mean absolute radial velocity cloud map was obtained, as shown in Figure 25.

Table 6. Area-averaged absolute radial velocity.

Position of Cross-Sections	Without Whip Sheath	With Whip Sheath	Coefficient of Increase
0.075 m	1.8281	1.8788	2.877%
0.278 m	1.5162	1.5511	2.301%
0.482 m	0.9309	1.8480	9.852%

and

Table 7. Maximum radial velocity.

Position of Cross-Sections	Without Whip Sheath	With Whip Sheath	Coefficient of Increase
0.075 m	6.6513	9.9559	4.968%
0.278 m	4.1061	11.4243	178.228%
0.482 m	2.8055	7.8844	181.034%

present the maximum radial velocity and area-averaged absolute radial velocity. According to the tables, the maximum radial velocity and the area-averaged absolute radial velocity of the structure with the whip sheath are greater than those of the structure without the whip sheath. The average absolute radial velocity of the area increased by more than 2% and reached 9.852% at the distal end.

For further insight into flow characteristics, radial velocity values at 100 sampling points on the three cross-sections were extracted for comparative analysis, as shown in Figure 26. For the baseline case of the non-whip sheath structure, the amplitude of radial velocity exhibits a remarkable decay from the near-downstream cross-Section 1 to the far-downstream cross-Section 3. In contrast, the case equipped with the whip sheath structure exhibits a higher degree of dispersion among the sampling points, which is attributed to the perturbation of the original flow field by the whip sheath structure. Despite the obvious attenuation trend, the peak radial velocity in the case with the whip sheath structure is slightly higher than that in the baseline model. Compared with the working condition of the non-whip sheath structure, the sampling points on cross-section 2 show the opposite distribution. This phenomenon occurs because multiple groups of the whip sheath structure are installed, and the original spiral motion is rearranged.

To evaluate the aerodynamic energy consumption caused by the whip sheath structure, the dimensionless pressure loss coefficient $K_p$ is selected as the evaluation index:

$$\mathsf{\Delta }{p}_t=p_{t,\mathrm{in}}-p_{t,\mathrm{out}}$$

(15)

$$K_p={\displaystyle \frac{\mathsf{\Delta }{p}_t}{\frac{1}{2}\rho U_0^2}}$$

(16)

The inlet and outlet sections of the device were selected to carry out total pressure statistics, and the pressure loss difference between the working conditions with and without the whip sheath structure was compared. The schematic diagram of the inlet and outlet section selection and the comparison results of the pressure loss coefficient are shown in Figure 27 and Figure 28. The comparison results show that the pressure loss of the device increases after the addition of the whip sheath structure, which indicates that the radial airflow strengthening is accompanied by a certain aerodynamic loss.

Figure 29 shows the comparison of internal vortex structure fields in devices with and without the whip sheath structure. Here, the flow field of the original structure (Figure 29a) is the same case as shown in Figure 19c. It is reused in this section as the baseline to directly highlight the variations caused by structural modifications. In the baseline case without the whip sheath structure, a small number of intact discrete vortices are distributed downstream of the impeller, with positive and negative vorticity regions arranged periodically at intervals. After the installation of the whip sheath structure, the original vortex structures are broken up and evolve into dense, fine strip-shaped vortex structures. The positive and negative vorticity values are distributed alternately, and both the quantity and spatial density of vortex structures increase significantly. Such flow field characteristics are advantageous for radial transport. On the one hand, the fragmented vortex structures eliminate periodic entrainment and flow disturbance. On the other hand, the whip sheath structure forms a new shear boundary layer on the surface and fall off, thus generating additional vortex structures.

A comparative contour of the three-dimensional streamline fields that occur in devices with and without the whip sheath structure is shown in Figure 30. When the whip sheath structure rotates synchronously with the impeller, continuous shear, cutting, and disturbance effects are exerted on the fluid, and the originally continuous spiral trajectories are disrupted. This is due to the introduction of the whip sheath structure and the flow path, which break the original axis-dominated flow pattern, reconstruct it, and convert the fluid’s axial kinetic energy into stronger tangential and radial kinetic energy. Therefore, the streamlines mostly diffuse in the direction of the pipe wall.

The results of the velocity field, vortex structure, and streamlines reveal that the whip sheath structure significantly enhances the rotational and radial velocity improvement performance of the cyclone dust collector. By actively perturbing the flow field, the whip sheath structure effectively enhances the radial velocity of the fluid and yields a more concentrated flow field. It provides sufficient driving force for the gas to migrate toward the peripheral wall, effectively verifying the gas flow performance of the new cyclone separator. Through this design, the flow effect of the gas-phase medium attached to the cylinder wall is greatly strengthened, and the flow kinetic energy of the airflow itself is fully exerted. The structure effectively balances the two objectives of air distribution and flow field stability.

5. Conclusions

In this paper, numerical simulation methods are used to conduct a systematic study of the flow characteristics inside the device. Mesh sensitivity and limited turbulence model sensitivity were assessed. On this basis, the flow field evolution under a fixed rotational speed and different TSRs is comprehensively analyzed, and the mechanism by which the whip sheath structure optimizes the internal flow is elucidated. The main conclusions are summarized as follows:

(1)

The velocity and pressure distributions under different mesh resolutions are highly consistent, and the mesh has little influence on the results. The medium mesh achieves a good balance between accuracy and efficiency. In the sensitivity analysis of the turbulence model, the deviation between the calculated results of the standard k-ε model and the SST k-ω model is within 5%, and the model selection does not change the research results.

(2)

Under the fixed rotational speed condition, when TSR = 1–1.5, large-scale flow separation and turbulent vortex shedding occur in the wake region, producing unsteady disturbances in the flow field. When TSR = 2, the axial velocity exhibits clear periodicity, and the radial velocity gradient is moderate, causing the fluid to be ejected toward the wall in a regular spiral pattern. The instantaneous power efficiency of the fan is the highest. Therefore, this working condition was selected for detailed flow field analysis. When the value of the tip velocity ratio TSR is too high or too low, the flow will present a weak or disordered state. When TSR = 3, the flow field tends to be dominated by axial plug flow, weakening the spiral swirling characteristics.

(3)

The addition of the whip sheath structure significantly optimizes the motion characteristics of the internal flow field. Synchronously rotating with the impeller, the whip sheath structure breaks down large-scale vortices into numerous small-scale vortices and converts tangential fluid kinetic energy into radial kinetic energy, creating a continuous high-radial-velocity zone within the whip region. The average absolute radial velocity of the area increased by more than 2% and reached 9.852% at the distal end.

In this paper, the internal gas flow process of the new cyclone separator is verified, which provides a reference for its structural design and engineering optimization. However, further research is still needed, especially in the area of separation efficiency. Future research will focus on discrete phase modeling (DPM) and other calculations to analyze particle motion and interactions. At the same time, self-actuation at 6-DOF will be verified.