**Preface to "CFD Based Researches and Applications for Fluid Machinery and Fluid Device"**

The demand for computational fluid dynamics (CFD)-based numerical techniques is increasing rapidly with the development of the computing power system. These advanced CFD techniques are applicable to various issues in the industrial engineering fields and especially contribute to the design of fluid machinery and fluid devices, which have very complicated unsteady flow phenomena and physics. In other words, to aid the rapid development of CFD techniques, the performances of fluid machinery and fluid devices with complicated unsteady flows have been enhanced significantly. In addition, many persistently troublesome problems of fluid machinery and fluid devices such as flow instability, rotor–stator interaction, surging, cavitation, vibration, and noise are solved clearly using advanced CFD techniques.

This Special Issue on "CFD-Based Research and Applications for Fluid Machinery and Fluid Devices" aims to present recent novel research trends based on advanced CFD techniques for fluid machinery and fluid devices. The following topics, among others, are included in this issue:


**Jin-Hyuk Kim, Sung-Min Kim, Minsuk Choi, Lei Tan, Bin Huang, Ji Pei** *Editors*

### *Editorial* **Special Issue on "CFD Based Researches and Applications for Fluid Machinery and Fluid Device"**

**Jin-Hyuk Kim 1,2,\* , Sung-Min Kim <sup>3</sup> , Minsuk Choi <sup>4</sup> , Lei Tan <sup>5</sup> , Bin Huang <sup>6</sup> and Ji Pei <sup>7</sup>**

<sup>1</sup> Clean Energy R&D Department, Korea Institute of Industrial Technology, Cheonan 31056, Korea


The demand for computational fluid dynamics (CFD)-based numerical techniques is increasing rapidly with the development of the computing power system. These advanced CFD techniques are applicable to various issues in the industrial engineering fields and especially contributing considerably to the design of fluid machinery and fluid devices, which have very complicated unsteady flow phenomena and physics. In other words, with the rapid development of CFD techniques, the performances of fluid machinery and fluid devices with complicated unsteady flows have been enhanced significantly. In addition, many persistently troublesome problems of fluid machinery and fluid devices such as flow instability, rotor–stator interaction, surging, cavitation, vibration, and noise are solved clearly using advanced CFD techniques.

The Special Issue on "CFD-Based Researches and Applications for Fluid Machinery and Fluid Device" in Processes deals with topics related to CFD techniques and applications in various fluid machines and devices. Specifically, the 31 papers published in this Special Issue focus on the advancement in the detailed internal flow analyses and methodologies for designing various fluid machines and devices, as the following summaries indicate. The influence of a low-pressure environment on the aerodynamic and noise characteristics of a centrifugal fan was studied numerically and experimentally by Zhang et al. [1]. Luo et al. [2] analyzed systematically the dynamic characteristics of mechanical seals under different fault conditions. Yu et al. [3] numerically studied the influence of step casing on unsteady cavitating flows and instabilities in inducers with equal and varying pitches. A methodology to improve the aerodynamic design with low cost and high accuracy for a 1–1/2 axial compressor was presented by Xie et al. [4]. Wang et al. [5] conducted the multi-condition optimization to enhance the cavitation performance of a double-suction centrifugal pump based on an artificial neural network (ANN) and nondominated sorting genetic algorithm II (NSGA-II). Zhang et al. [6] proposed an improved aerodynamic optimization method for designing effectively a low Reynolds number cascade. The design optimization of a two-vane pump for wastewater treatment using machine-learning-based surrogate modeling was carried out by Ma et al. [7]. Wang et al. [8] analyzed numerically the axial vortex characteristics in a centrifugal pump as a turbine with an S-blade impeller. Li et al. [9] studied numerically and experimentally the transient characteristics of a centrifugal pump during the startup period with assisted valve. The thermal performance with the geometric parametrization of T-shaped obstacles in a solar air heater was performed by Ahn and Kim [10].

**Citation:** Kim, J.-H.; Kim, S.-M.; Choi, M.; Tan, L.; Huang, B.; Pei, J. Special Issue on "CFD Based Researches and Applications for Fluid Machinery and Fluid Device". *Processes* **2021**, *9*, 1137. https:// doi.org/10.3390/pr9071137

Received: 29 June 2021 Accepted: 29 June 2021 Published: 30 June 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

On the other hand, the effect of rotor spacing and duct diffusion angle on the aerodynamic performances of a counter-rotating ducted fan in a hover mode was analyzed numerically by Kim et al. [11]. Lei et al. [12] applied the CFD method to analyze the aerodynamic performance of an octorotor small unmanned aerial vehicle with different rotor spacing in hover. Shrestha and Choi [13] proposed a CFD-based shape design optimization process to improve the flow uniformity in the fixed flow passages of a Francis hydro turbine model. The influence analyses of the blade outlet angle on the flow and pressure pulsation characteristics in a centrifugal fan were carried out by Ding et al. [14]. Rui et al. [15] performed experimental and numerical studies to investigate the effect of the radius of a volute tongue on the aerodynamic and aeroacoustic characteristics of a Sirocco fan. The effect and mechanism of the triple hole on the film-cooling performance based on large eddy simulation (LES) were identified by Baek and Ahn [16]. Song et al. [17] verified the influence of tip clearance on the flow characteristics of an axial compressor through the CFD technique. Hur et al. [18] numerically investigated the effect of clearance and cavity geometries on the leakage performance of a stepped labyrinth seal. The effect of root clearance on the mechanical energy dissipation of an axial flow pump based on entropy production was analyzed by Li et al. [19]. Gao et al. [20] explored the hydraulic performance with different blade wrap angles of an impeller in an open-design vortex pump.

Moreover, the numerical and experimental studies on the waviness mechanical seal of a reactor coolant pump were conducted by Feng et al. [21]. Benišek et al. [22] suggested a new design of the reversible axial jet fan impeller with symmetrical and adjustable blades. Stelmach et al. [23] confirmed the influence of hydrodynamic changes in a system with a pitched blade turbine on mixing power using a particle image velocimetry (PIV) method. Wang et al. [24] optimized the shapes of the impeller and diffuser of a mixed-flow pump using the inverse design method and CFD analysis. Rakibuzzaman et al. [25] designed numerically a new prototype propeller-type tubular turbine utilizing discharge water from a fish farm, and its performance was verified experimentally. The characteristic implicit method based on the upwind differencing and implicit finite difference scheme to solve the mixed free-surface-pressurized flow in a hydropower station was suggested by Wang et al. [26]. Park et al. [27] carried out the multi-objective numerical optimization to simultaneously enhance the heat transfer efficiency and reduce the pressure loss of a wavy microchannel heat sink. Chen et al. [28] investigated numerically the dynamic stresses of the runner during start-up in the turbine mode of a pump turbine. Portal-Porras et al. [29] tested the accuracy of the cell-set model applied on vane-type sub-boundary layer vortex generators by using CFD techniques. Shamsuddeen et al. [30] suggested a new inducer-type guide vane to reduce the hydraulic losses at the inter-stage flow passage of a multistage centrifugal pump. The effect of micro-tab on the lift enhancement of airfoil S-809 with trailing edge flap in wind turbine blades was analyzed numerically by Ye et al. [31].

Finally, as the guest editors of this Special Issue, we would like to especially thank the Section Managing Editor, Ms. Shirley Wang, for organizing and helping the Special Issue of *Processes*. We are also thankful to all the reviewers for their valuable comments for improving the quality of papers published in this Special Issue. In addition, this valuable Special Issue is available at https://www.mdpi.com/journal/processes/special\_issues/ CFD\_Fluid\_Device.

**Author Contributions:** Writing—original draft preparation, J.-H.K.; writing—review and editing, J.-H.K.; S.-M.K.; M.C.; L.T.; B.H., and J.P. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research received no external funding.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**

<sup>1.</sup> Zhang, X.; Zhang, Y.; Lu, C. Flow and noise characteristics of centrifugal fan in low pressure environment. *Processes* **2020**, *8*, 985. [CrossRef]


### *Article* **Effects of Micro-Tab on the Lift Enhancement of Airfoil S-809 with Trailing-Edge Flap**

**Jianjun Ye 1,2, Shehab Salem <sup>1</sup> , Juan Wang 3,\*, Yiwen Wang <sup>1</sup> , Zonggang Du <sup>1</sup> and Wei Wang <sup>1</sup>**


**Abstract:** Recently, the Trailing-Edge Flap with Micro-Tab (TEF with Micro-Tab) has been exploited to enhance the performance of wind turbine blades. Moreover, it can also be used to generate more lift and delay the onset of stall. This study focused mostly on the use of TEF with Micro-Tab in wind turbine blades using NREL's S-809 as a model airfoil. In particular, the benefits generated by TEF with Micro-Tab may be of great interest in the design of wind turbine blades. In this paper, an attempt was made to evaluate the influence of TEF with Micro-Tab on the performance of NREL's S-809 airfoils. Firstly, a computational fluid dynamics (CFD) model for the airfoil NREL's S-809 was established, and validated by comparison with previous studies and wind tunnel experimental data. Secondly, the effects of the flap position (H) and deflection angle (αF) on the flow behaviors were investigated. As a result, the effect of TEF on air-flow behavior was demonstrated by augmenting the pressure coefficient at the lower surface of the airfoil at flap position 80% chord length (C) and α<sup>F</sup> = 7.5◦ . Thirdly, the influence of TEF with Micro-Tab on the flow behaviors of the airfoil NREL's S-809 was studied and discussed. Different Micro-Tab positions and constant TEF were examined. Finally, the effects of TEF with Micro-Tab on the aerodynamic characteristics of the S-809 with TEF were compared. The results showed that an increase in the maximum lift coefficient by 25% and a delay in the air-flow stall were accomplished due to opposite sign vortices, which was better than the standard airfoil and S-809 with TEF. Therefore, it was deduced that the benefits of TEF with Micro-Tab were apparent, especially at the lower surface of the airfoil. This particularly suggests that the developed model could be used as a new trend to modify the designs of wind turbine blades.

**Keywords:** computational fluid dynamics (CFD); trailing edge flap (TEF); trailing edge flap with Micro-Tab; deflection angle of the flap (αF); aerodynamic performance

#### **1. Introduction**

Wind energy plays a crucial role in tackling global climate issues and shaping tomorrow's energy systems. Recently, the wind turbine industry is becoming one of the best choices for energy production among all renewable energy choices [1]. The wind industry shows extensive financial progress and it is assumed to seriously compete with fossil fuel energy generation in the coming years. This progression attracts most scientists' attention to investigate feasible modifications that can enhance wind turbine performance and sustainability. This is supported by numerous recent studies, in which they claim that the efficiency of a wind turbine depends on many factors, including the rotational speed of the electrical generator [2] and the control of the airfoil aerodynamic shape and forces [3]. It is especially problematic for air-flow separation in the region near the hub. It was reported that the efficiency of wind turbines was diminished due to the drag penalty coming from air-flow separation at large angles of attack around the airfoil [4]. Due to

**Citation:** Ye, J.; Salem, S.; Wang, J.; Wang, Y.; Du, Z.; Wang, W. Effects of Micro-Tab on the Lift Enhancement of Airfoil S-809 with Trailing-Edge Flap. *Processes* **2021**, *9*, 547. https://doi.org/10.3390/ pr9030547

Academic Editor: Jin-Hyuk Kim

Received: 24 January 2021 Accepted: 1 March 2021 Published: 19 March 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

the increase in the angle of attack (α), the adverse stream-wise pressure counter-gradients increase correspondingly and lead to air-flow separation. α

Consequently, it is essential to study air-flow separation control methods to enhance wind turbines' aerodynamic performance. Thus, specialists could use modern methods, such as TEF, Micro-Tabs at the TEF with Tab, and vortex generators, to improve the wind turbine blades' performance. These methods can be applied at a low Reynolds number (Re) number to achieve high aerodynamics efficiency [5]. Hence, this work presents a convenient simulation to modify the airfoil design by using a flap and tabs at the airfoil's trailing edge. By employing a CFD simulation and using shear stress transport SST *k*-*ω* model, the standard airfoil shape is compared to different airfoil shapes with a TEF, and airfoil with TEF with Tab. The latter obtained the highest output power efficiency for the wind turbine blades [6,7]. -*ω*

Compared with the standard shape airfoil, TEF airfoils have been proven useful as wind turbine airfoils since they can be adopted in larger sectional areas, produce more aerodynamic forces (CL, C<sup>D</sup> and CP), and are insensible to leading-edge roughness [8,9]. Therefore, by using TEF airfoils, further improvement for both the structural strength and the aerodynamic performance of wind turbine blades could be achieved [10,11]. Different angles of installation can be applied in TEF with Micro-Tabs to increase the aerodynamic performance. It was suggested that Micro-Tabs should be maintained below 95% C to maximize the aerodynamic benefits [12]. After conducting a systematic experimental campaign on different shapes of the airfoil, there is compelling evidence that Micro-Tabs enhance the value of C<sup>L</sup> of airfoils and decrease the C<sup>D</sup> [13,14]. Figure 1 depicts the shape and flow of the streamlines with and without micro tabs

**Figure 1.** Aerodynamic performance for the streamline over the Micro-Tabs [15]. (**a**) Streamline over the standard airfoil; (**b**) streamline over the standard airfoil with a Micro-Tab.

Many researchers and studies later confirmed the presence of a characteristic separation bubble and rotating vortices as a result of installing a Micro-Tab [16,17]. Consequently, this part was fixed to the airfoil surface; it was responsible for an increasing suction on the airfoil upper surface and a pressure on the lower surface of the airfoil.

Interestingly, the aerodynamic impact of Micro-Tabs strongly depends on their design configuration parameters, such as Micro-Tab geometry and their mounting details, whereby the height and angle of installation of the Micro-Tab are indeed one of the most important design parameters. Furthermore, the C<sup>L</sup> parameter enhances the aerodynamic performance of any airfoil in different weather conditions. Likewise, for a certain threshold value of the C<sup>D</sup> parameter, it is confirmed that its size and angles could nullify the Micro-Tabs advantage. Therefore, many researchers are now looking for the best size and the best angle for an optimal installation of the Micro-Tabs [18,19]. Thus, this could provide the domain with the suite's highest efficiency and obtain a beneficial CL/CD.

Micro-Tabs have been confirmed to have interesting inferences in a wide range of flow fields. Wang et al. and Troolin [20,21] provided an extensive overview of Micro-Tab applications, which include different wind speeds [22], aircraft, and wind turbine blade design analysis [23]. In this paper, we focus on the latter application, and many literature instances suggested Micro-Tabs as a small but useful device for active air-flow control over the airfoil and wind turbine blade's aerodynamic performance increase [24]. α


Therefore, this study's main purpose is to scrutinize the influences of TEF with Micro-Tab on the performance of the airfoil S-809 with TEF using 2D CFD simulations by using shear stress transport SST *k*-*ω* model [25]. In particular, this study sets some important parameters that selectively tuned the aerodynamic performance by setting different TEF positions of the chord length (C), deflection angle, and angle of incidence TEF. Interestingly, it has been shown that this study is capable of predicting the qualitative effect of TEF with Micro-Tab at different positions on the airfoil surface of the airfoil with TEF, the highest aerodynamic performance, and improves the C<sup>P</sup> at a small α. In conclusion, when TEF was deflected, the flow was trapped on the airfoil's lower surface. In turn, a decrease in the flow velocities, an increase in pressure at the airfoil's lower surface, and an adverse pressure gradient may be achieved. α

#### **2. Geometric Description of the Trailing Edge Flap with Micro-Tab Airfoil**

This section discusses the TEF airfoil geometry parameters with a Micro-Tab at different position by using the airfoil S-809 with TEF. The position of TEF at H = 80% C and deflection angle α<sup>F</sup> of TEF 7.5◦ are shown in Figure 2a,b when TEF with Micro-Tab are mounted at the trailing edge of the TEF airfoil. Figure 2 and Table 1 show three patterns with different Micro-Tabs positions. The S-809 airfoil has been selected as the standard airfoil that has been identified as the most popular wind turbine on the market [26–29]. **α**

**Figure 2.** Geometrical parameters (**a**) of Trailing Edge Flap (TEF), (**b**) of Trailing-Edge Flap with Micro-Tab (TEF with Micro-Tab).


**Table 1.** The parameters of the airfoil with TEF with Micro-Tab.

The TEF was attached at the Trailing-Edge Standard airfoil S-809. For the length of the airfoil chord (C), a suitable length of 0.6 m was chosen. Moreover, the TEF's position and deflection angle were selected to generate the highest dynamic performance (according to the previous article [28]).

Therefore, the current study is based on TEF with a Micro-Tab at three different pattern positions according to the airfoil chord, and they are all further investigated using CFD simulation. Data and illustrations in Table 1 and Figure 3 show the design parameters and the tab position.

All TEF with Micro-Tabs have a height of 2% C with the position K = 95% C, and maximum width is 0.4% C, the lower position at k = 95% C, the upper position at K = 95% C, and upper/lower positions at K = 95% C, which are denoted as "Pattern 1", "Pattern 2", and "Pattern 3," respectively, as shown Figure 3a–c.

**Figure 3.** The geometry of TEF with Micro-Tab positions: (**a**) 3D front view, (**b**) Pattern 1 with lower Micro-Tab, (**c**) Pattern 2 with upper Micro-Tab, (**d**) Pattern 3 with upper and lower Micro-Tabs.

#### **3. Description of the Numerical Method**

*3.1. The Governing Equations*


Mass equation

$$\frac{\partial \rho}{\partial t} + \frac{\partial}{\partial \chi\_i} (\rho U\_i) = 0 \tag{1}$$

Momentum equation

$$\rho \left( \frac{\partial \mathcal{U}\_{\dot{l}}}{\partial t} + \mathcal{U}\_{\dot{k}} \frac{\partial \mathcal{U}\_{\dot{l}}}{\partial \mathbf{x}\_{k}} \right) = -\frac{\partial P}{\partial \mathbf{x}\_{\dot{l}}} + \frac{\partial}{\partial \mathbf{x}\_{\dot{l}}^{\dot{l}}} \left( \mu \frac{\partial \mathcal{U}\_{\dot{l}}}{\partial \mathbf{x}\_{\dot{l}}} \right) + \frac{\partial}{\partial \mathbf{x}\_{\dot{l}}} \mathbf{r}\_{\dot{l}\dot{l}} \tag{2}$$

μ and Here, *U<sup>i</sup>* is the free stream velocity component in the *x*-direction. *P* is the pressure, *t*, *µ* and *ρ* are the time, the dynamic viscosity, and air-flow density.

The SIMPLEC algorithm for the treatment of the pressure-velocity coupling was used. Second-order up-wind discretization was adopted for the convection terms and central difference schemes for the diffusion terms.

The SST *k*-*ω* (Shear Stress Transport) turbulence model (previously proposed by Menter [31]) was chosen in this work as it has shown good aerodynamic performance in wind turbines and turbo-machinery experiencing air-flow separation as expected for the blades during rotation [33].

This model's core idea was to utilize the robustness of the *k*-*ω* model to capture the flow within the viscous sub-layer. Moreover, one can use the k-ǫ model in the mainstream area to ban the disadvantage of the *k*-*ω* turbulence model. Overall, the SST *k*-*ω* model combines the advantages of the standard *k*-*ω* model and the standard k-ǫ model by mixing functions. Therefore, the SST *k*-*ω* model has higher accuracy and reliability in a wide range of flow fields. Yu et al. and Zhang et al. reported simulation results for the Spalart–Allmaras (S–A) turbulence model [34,35]. There was a good agreement between the simulation and the experimental data.

Additionally, Menter and Rogers et al. detected that for most high-lift problems [36], the S–A and SST *k*-*ω* model estimations were similar. However, it was proposed that the SST *k*-*ω* model is superior in accurately predicting pressure-induced separation. Therefore, the SST *k*-*ω* model was assumed to be more suitable in the present study than the S–A model [34,35] This will be shown in the results and discussions Section 4.1.2.

$$\frac{\partial \rho k}{\partial t} + \frac{\partial}{\partial \mathbf{x}\_{\dot{j}}} (\rho u\_{\dot{j}} k) = \frac{\partial}{\partial \mathbf{x}\_{\dot{j}}} \left[ (\mu + \sigma\_k \mu\_l) \frac{\partial k}{\partial \mathbf{x}\_{\dot{j}}} \right] + \tau\_{\dot{l}\dot{l}} \mathbb{S}\_{\dot{i}\dot{l}} - \beta^\* \rho \omega k \tag{3}$$

$$\frac{\partial \rho \omega}{\partial t} + \frac{\partial}{\partial \mathbf{x}\_{\dot{j}}} (\rho \mathbf{u}\_{\dot{j}} \omega) = \frac{\partial}{\partial \mathbf{x}\_{\dot{j}}} \left[ (\mu + \sigma\_{\omega} \mu\_{l}) \frac{\partial \omega}{\partial \mathbf{x}\_{\dot{j}}} \right] + \frac{\mathbb{C}\_{\omega} \rho}{\mu\_{l}} \tau\_{\dot{j}\dot{j}} \mathbb{S}\_{\dot{j}\dot{j}} - \beta \rho \omega^{2} + 2(1 - f\_{1}) \frac{\rho \sigma\_{\omega 2}}{\omega} \frac{\partial \mathbf{k}}{\partial \mathbf{x}\_{\dot{j}}} \frac{\partial \omega}{\partial \mathbf{x}\_{\dot{j}}} \tag{4}$$

where *U<sup>j</sup>* is the velocity component in the x-direction. *β*, *Cω*, *σ<sup>k</sup>* , and *σ<sup>ω</sup>* are coefficients of the SST turbulence model that can be obtained by blending the coefficients of the *k*-*ω* model.

#### *3.2. CFD Gird Model*

This research adopts the chord length C = 0.6 m and the free stream velocity V ≃ 51 m/s, and the Reynolds number Re = 2 <sup>×</sup> <sup>10</sup><sup>6</sup> . The C-type mesh provided by the elliptical method in ICEM CFD was used because of its high accuracy, as verified by Ma et al. [37]. The computational grid, shown in Figure 4, constituted 9 <sup>×</sup> <sup>10</sup><sup>5</sup> grid elements on the airfoil surface. The respective distance of the inlet and outlet boundaries away from the leading edge was 20 C and 30 C, respectively. The top and bottom boundaries were 15 C away from the chord. In particular, to capture the boundary layer, the grid should have a y+ value of less than one (y+ < 1). The y+ is a non-dimensional distance that indicates the degree of grid fineness in the near-wall region. In the current simulation, the first grid node above the surface was 1.5 <sup>×</sup> <sup>10</sup>−<sup>5</sup> times of chord length, in turn, y+ = 0.02. The mesh quality and the mesh at the edge of the airfoil for the TEF with Micro-Tab are depicted in Figure 4b. Figure 4b shows several details of the computational grid used for the airfoil's CFD simulations analysis, with a specific focus on the improvement zones used to properly discretize the airfoil LE and TE, such as the Pattern 3 configuration. The whole count of elements demonstrated that there is a very fine meshing in the sections inside the airfoil and a relatively rough meshing outside. However, the number of elements inside the airfoil was about 11 <sup>×</sup> <sup>10</sup><sup>5</sup> . To capture the boundary layer for Pattern 3, the grid should have a y+ value of y+ < 1. A mesh independency test was achieved to emphasize that the difference in the number of elements did not affect the solution, as shown in the results and discussions Section 4.1.1.

**Figure 4.** Detail of the grid structure of the airfoil: (**a**) boundary conditions and mesh domain on the airfoil S-809 with TEF; (**b**) mesh domain of TEF with Micro-Tab pattern 3.

(**b**)

#### **4. Results and Discussion**

#### *4.1. Validation of Accuracy S-809 and S-809 with TEF Airfoil*

4.1.1. Grid Independence Validation

To ensure grid independence in the CFD simulation predictions, calculations have been made for a typical TEF airfoil shape and air-flow configuration, using different grid accuracies. The verification of the predicted C<sup>L</sup> with the total number of the grid elements for the considered TEF airfoil and Pattern 3 is displayed in Figure 5a,b. The achievement of sufficient grid independence for grids with elements larger than 8 <sup>×</sup> <sup>10</sup><sup>5</sup> is observed in Figure 5a. Thereby, the grids created by the ICEM program and using the same grid strategy possessed an even finer resolution corresponding to the number of elements <sup>9</sup> <sup>×</sup> <sup>10</sup><sup>5</sup> and according to the grid independence curve.

**Figure 5.** Mesh verification: (**a**) mesh independence for TEF airfoil S-809; (**b**) mesh independence for TEF with Micro-Tab (pattern 3).

The illustrations in Figure 5b verify the grid independence around the airfoil for Pattern 3 (Micro-Tab position at the upper and lower on the TEF surface), where the flowfield model of grid elements ranged from 6 <sup>×</sup> <sup>10</sup><sup>5</sup> to 11 <sup>×</sup> <sup>10</sup><sup>5</sup> . From these findings, it was observed that the convergence was determined with high accuracy and the aerodynamic performance reached a stable value when the number of grid elements reached a value of more than 9 <sup>×</sup> <sup>10</sup><sup>5</sup> . Therefore, a model with a grid element number of 11 <sup>×</sup> <sup>10</sup><sup>5</sup> was further selected for the next modelling assessments.

#### 4.1.2. Comparison between CFD and Experimental Data for TEF Airfoil S-809

≃ − ω To validate the CFD simulation, the experimental data of the S-809 airfoil with TEF provided by the Ohio State University were compared with the numerical results [38,39] The Mach number (Ma <sup>≃</sup> 0.15) and the Re = 2 <sup>×</sup> <sup>10</sup><sup>6</sup> in the numerical simulation are the same as those of the wind tunnel test. The chord of the S-809 airfoil with TEF was C = 0.6 m. The simulation results are compared with the experimental data in Figure 6. The findings illustrate that the C<sup>L</sup> coincides with the measurement for the range of angles of attack from −2 ◦ to 13◦ , as shown in Figure 6a. After the flow separation took place, the C<sup>L</sup> was a little overestimated but within an acceptable range. Moreover, the variation trend was well observed. The C<sup>D</sup> was obviously overestimated, as shown in Figure 6b. The possible reason was that the S-809 with TEF was a laminar airfoil, and there probably existed a transition flow on the airfoil surface during the experiment. Table 2 shows a comparison of the CFD results and experimental data for the TEF airfoil. For example, for the angle = 4◦ , the CFD simulation lift coefficient is now equal to the experimental value. Table 2 presents the results obtained from the preliminary CFD analysis (SST-kω and S-A). The C<sup>L</sup> compared with the experimental data has a 2% error and the error in the calculated drag has been reduced to 9%. The errors in the coefficients at 0◦ and 1◦ have also been significantly reduced. These angles of attack were rerun using the same grid as for all cases. In summary, the numerical results concur with the experimental data. This indicated the accuracy of the numerical method in this study. Besides, Ramsay carried out a similar validation strategy to validate their numerical results [40]. Therefore, the present study's subsequent research used the full turbulence model to carry out the numerical simulations.

**Figure 6.** Comparisons between the computational fluid dynamics (CFD) calculated and experimentally determined pressure distributions for TEF airfoil with angles of attack of 0◦ : (**a**) C<sup>L</sup> distribution; (**b**) C<sup>D</sup> distribution; (**c**) C<sup>P</sup> distribution.

**Table 2.** Comparisons between CFD results and experimental data for the TEF airfoil.


Figure 6c shows the comparison between the CFD calculated and experimental surface pressure coefficient distributions for an angle of attack of 0◦ [40]. The C<sup>p</sup> comparisons for 0 ◦ are in a reasonably good agreement over the entire S-809 airfoil with TEF surface except in the regions of the laminar separation bubbles. The experimental pressure distributions show the laminar separation bubbles just near the chord on both the upper and lower surfaces. They are indicated in the experimental data that become more-or-less constant with respect to X/C, followed by an abrupt increase in pressure as the flow undergoes turbulent reattachment. Since the calculations assume a fully turbulent flow, no separation is indicated in the numerical results.

#### *4.2. Effect of the Trailing Edge Flap with Micro-Tab (TEF with Micro-Tab) on the Air-Flow Behaviour*

α This section presents the results of our investigation on the aerodynamic performance of TEF with Micro-Tab attachment. The aerodynamic performance results presented

include stall angles of attack α, CL, CD, and CL/C<sup>D</sup> distribution. In order to articulate the results, the 2D air-flow streamlines distribution and vortices in the wake area have been analyzed. Different TEF's aerodynamic performance with Micro-Tab at different positions have been analyzed to control the proposed TEF's control aerodynamic performance with Micro-Tab. The angles of attack ranging from 0◦ to 25◦ to simulate the S-809 airfoil by using TEF with Micro-Tab were chosen. The position of the TEF (H = 80% C) and deflection angle (α<sup>F</sup> = 7.5◦ ) was chosen based on airfoil S-809 with TEF results (the TEF result in Section 4.1.2); as it showed the highest aerodynamic performance. Subsequently, the TEF with Micro-Tab attachments was readjusted to S-809 with TEF (H = 80% and deflection angle α<sup>F</sup> = 7.5◦ ). α

Figure 7a shows a comparison of the different settings for the aerodynamic performance effect. As seen in the figure, the C<sup>L</sup> curves depict a gradual upward shift due to the TEF airfoil with Micro-Tab for the proposed α values and for the TEF. When α = 13◦ , C<sup>L</sup> was enhanced by 15% and 28.6% for Pattern 2 and Pattern 3, respectively. Figure 7b shows the variation of C<sup>D</sup> with varying α at different TEF airfoil with Micro-Tab configurations. Thus, when the TEF with Micro-Tab was positioned at both directions (up and lower flap surface), as seen in Pattern 3, the F<sup>L</sup> showed the highest values compared with the other configurations. α α α α

α **Figure 7.** The aerodynamic performance effect of TEF with Micro-Tab: (**a**) comparison of CL; (**b**) comparison of CD, (**c**) comparison of CL/CD; (**d**) comparison of C<sup>P</sup> distribution at α = 0◦ .

The analysis of the F<sup>L</sup> and F<sup>D</sup> curves described before is not comprehensive enough to design blades. Thus, a comprehensive understanding of blades' design needs the estimation of the CL/C<sup>D</sup> ratio for the design of the wind turbine blades. The CL/C<sup>D</sup>

ratio is important in determining the most appropriate angle and TEF with Micro-Tab configurations for the proposed blade design. The estimate of CL/C<sup>D</sup> based on parameters in Figure 7a,b is shown in Figure 7c. The results reaffirm that value of C<sup>L</sup> was increasing due to the TEF airfoil with Micro-Tab attachment. A possible explanation for the increase in the CL/C<sup>D</sup> ratio of an airfoil is due to TEF with Micro-Tab attachment. The C<sup>L</sup> ranged between 0.9 (Pattern 1) and 1.6 (Pattern 3) at α = 15◦ , and the value of C<sup>D</sup> decreased from 0.03536 to 0.03219 when the TEF airfoil with Micro-Tab was attached.

The α was readjusted between 5◦ to 15◦ to obtain the optimal effect on the CL/C<sup>D</sup> ratio, as seen in Pattern 3 in Figure 7c. Comparing the airfoil with TEF to the other patterns, no air-flow separation on the airfoil was observed at an angle less than 23◦ . Pattern 3 depicts the highest lifting force compared to other patterns.

A possible explanation for this might be the opposite sign vortices caused by fitting the TEF with upper/lower Micro-Tabs.

Upon closer inspection of Pattern 3, as seen in both C<sup>D</sup> (Figure 7b) and CL/C<sup>D</sup> (Figure 7c), one observes a higher aerodynamic performance (CL/C<sup>D</sup> > 35%) in comparison to the standard airfoil and other patterns. A higher aerodynamic performance results from the opposite sign vortices and, at the same time, the contribution of the low C<sup>D</sup> decreases. Another important finding is that Pattern 3 is an optimal choice when α is between 15◦ to 23◦ and for an airfoil with TEF with Micro-Tab. The high efficacy experienced for Pattern 3 is assumed to be due to the CL/C<sup>D</sup> ratio that increases by over 35% and due to the low C<sup>D</sup> contribution.

Figure 7d illustrates the C<sup>P</sup> distribution on the standard airfoil, airfoil with TEF, and TEF with Micro-Tab patterns. The C<sup>P</sup> factor of the Trailing-Edge changed when deploying TEF with Micro-Tab.

The C<sup>P</sup> factor of the Trailing-Edge changed from −1200 Pa at the TEF airfoil to 1000 Pa when TEF airfoil with Micro-Tab was attached. Correspondingly, an enhancement in the suction of the upper surface for the airfoil and an increase in the pressure at the lower surface was observed and the performance of the airfoil was increased. Finally, the configuration of Pattern 3 did not show the air-flow separation compared with the TEF airfoil. This was probably due to the separation bubble and opposite sign vortices. Therefore, the air flowed smoothly along the upper surface of the airfoil without separation.

The next section gives a detailed discussion of the pressure distribution at the small and large angles of attack for each pattern.

#### *4.3. Discussion of the Surface Pressure Distribution of the TEF Airfoil with/without Micro-Tab*

In order to investigate the effects of different Micro-Tab positions on the pressure distribution, contours of C<sup>P</sup> are used, as shown in Figure 8. Each subplot in Figure 8 represents the C<sup>P</sup> values as a function of airfoil chord location in the x-axis direction and the Micro-Tab positions.

The upper-pressure distribution represents the airfoil's suction side, whereas the lower C<sup>P</sup> distribution represents the pressure side of the airfoil. The Micro-Tab position at 98% C Pattern 1 at the lower surface for the TEF airfoil, for the Pattern 2 the Micro-Tab position 98% C and the upper surface for the TEF airfoil, for the Pattern 3 the MicroTab at 98% C at the lower and upper surface for the TEF airfoil, and the TEF airfoil when there is no Micro-Tab on the airfoil S-809.

To better explain the C<sup>P</sup> displayed in this analysis at α = 0◦–13◦ , the traditional C<sup>P</sup> polar for the TEF airfoil upper and lower sides is presented for the three patterns of the TEF airfoil with Micro-Tab that are specified by the solid and dashed lines on the color contour plots. Figure 8 displays an overview of the C<sup>P</sup> distribution corresponding to α = 0 to 13◦ with standard airfoil, TEF airfoil, Pattern 1, Pattern 2, and Pattern 3. These pressure distributions over the airfoil were then integrated to determine the lift (CL) and drag (CD) coefficients.

α − **Figure 8.** Pressure distribution and color contour plots at the α = 0◦–13◦ , (**a**) S−809 airfoil, (**b**) TEF airfoil, (**c**) Pattern 1, (**d**) Pattern 2, (**e**) Pattern 3.

Two C<sup>P</sup> distributions are presented for two different α, which represent low and high α, respectively. Unsurprisingly, for both angles, Pattern 1 increases the pressure on the pressure side of the airfoil, Pattern 2 decreases the suction on the suction side, and Pattern 3 increases the pressure on the pressure side and the suction side of the airfoil compared to TEF airfoil and standard airfoil. A case-study approach was used to evaluate TEF airfoil's effectiveness with Micro-Tab on pressure distributions and lift force. This effectiveness clearly comes from the increased adverse pressure gradient, opposite sign vortices, and separation bubbles generated in front of the Micro-Tab on the side on which it has been attached. On the other hand, it is important to indicate that the TEF airfoil with Micro-Tab has also changed the effective aerodynamic performance, angle of attack, and the effective airfoil camber, both of which can considerably impact the pressure distribution over both surface sides of the TEF airfoil. The Micro-Tab effect on the suction side of the airfoil is also noticeable; this appears in Pattern 1 and Pattern 3, as shown in Figure 8c,e.

Pattern 1 has improved the suction on the TEF airfoil's top surface, even though, at the lowest α, the effect is not high, and, as the angle of attack increases, this effect becomes enhanced. Pattern 2 also affects the pressure the side of the airfoil. As observed for lower angles of attack, Pattern 2 has significantly reduced the pressure on the bottom side of the TEF airfoil, and, for the highest angles, this effect is not high. As for Pattern 3, it combined each of the features of Pattern 1 and Pattern 2. This is because both of these enhance the lower pressure of the wing and increase the lift force, as shown in Figure 8e. It is also fairly apparent that, for average angles, Pattern 1, Pattern 2, and Pattern 3 show comparable effectiveness of the aerodynamic performance on both sides of the TEF airfoil. This investigation of the pressure measurements clearly shows that the Micro-Tab's effectiveness is not only Micro-Tab dependent but also depends considerably on the airfoil angle of attack and the TEF of the airfoil. The velocity profiles and the streamline distribution data from the CFD simulation can better clarify this dependency.

#### *4.4. Discussion of the Streamline Distribution and the Velocity Profiles of the TEF Airfoil with/without Micro-Tab*

This study identified the dependency of the angle of attack (α) of the TEF airfoil with Micro-Tab performance on the TEF airfoil. CFD results near the airfoil trailing edge are shown for different patterns in Figure 9. Each column in Figure 9 shows three different TEF configurations for the same angle of attack (α). The deflection of the airfoil trailingedge flow when the TEF with Micro-Tab is deployed is clear for each attack angle. When Pattern 1 is attached, the findings show that the down-wash flow is more apparent, as shown in Figure 9c. This would imply that the lift is greater in these cases. On the other side, Pattern 2 decreases the down-wash flow, which insinuates a smaller lift at the small angle of attack, as shown in Figure 9d. At α = 0◦ Pattern 2 has induced an up-wash that implies a negative lift in this configuration. These deflections in the airfoil down-wash imply that the effective camber and angle of attack have changed. These changes significantly affect the pressure distribution and, as a result, the lift and moment behavior of the airfoil change.

Following the previous discussion that suggested the dependency of the TEF airfoil with Micro-Tab effectiveness on the angle of attack, it can be clearly observed that, at lower angles, Pattern 2 is more exposed to the flow. Concurrently, Pattern 1 is more exposed to the flow at higher angles of attack. The CFD results clearly show this dependency and support the observations in the pressure distributions. Physically, it can be inferred that, for the Pattern 1 cases at lower angles of attack, the pressure gradient on the airfoil's pressure side is so high that the increment produced by the flap is no longer significant. As a result of configuringthe opposite sign vortices at the Micro-Tab, as shown in Figure 9c. For a higher angle of attack, when the Micro-Tab is exposed to the suction side of the airfoil, the pressure gradient on the suction side of the airfoil is so high that the Micro-Tab cannot affect the flow in a manner as significant as at smaller angles of attack; as a result, the pressure gradients are much weaker. Finally, Pattern 3 has an overall advantage because it combines Pattern 1 and Pattern 2 to the same TEF airfoil. Pattern 3 can work at both small and large angles of attack as a result of high aerodynamic performance.

**Figure 9.** Comparison of streamline distribution of the TEF airfoil with/without Micro-Tab at three different positions, (**a**) Standard airfoil, (**b**) TEF airfoil, (**c**) Pattern 1, (**d**) Pattern 2, (**e**) Pattern 3.

#### **5. Conclusions**

This paper describes a methodology for computing the effect of TEF with Micro-Tab on airfoil sections by using CFD. A grid generation method was developed to allow an easy way for repositioning the TEF in the chord-wise direction on the S-809 airfoil. This study was able to predict the qualitative effect of TEF with Micro-Tab, and it was possible to obtain the highest aerodynamic performance at a high C<sup>P</sup> value. The findings indicated that the best pattern with the highest aerodynamic performance was provided by three patterns of TEF with Micro-Tab. Based on the above, the following may be concluded:


**Author Contributions:** Conceptualization, J.Y. and S.S.; methodology, S.S.; software, S.S. and Y.W.; validation, J.Y., J.W. and S.S.; formal analysis, W.W.; investigation, S.S. and Z.D.; resources, J.Y.; data curation, Z.D.; writing "original draft preparation, S.S.; writing "review and editing, J.Y.; visualization, J.Y.; supervision, J.Y. and J.W.; project administration, J.Y.; funding acquisition, Y.W. All authors have read and agreed to the published version of the manuscript.

**Funding:** National Natural Science Foundation of China, Grant/Award Number: 51976067, the Open Foundation of the Key Laboratory of Low-grade Energy Utilization Technologies and Systems, Grant/Award Number: LLEUTS-201905, the Open Foundation of the State Key Laboratory of Fluid Power and Mechatronic Systems, Grant/Award Number: GZKF-201811.

**Data Availability Statement:** The data used to support the findings of this study are available from the corresponding author upon request.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Abbreviations**



#### **References**


### *Article* **Effect of an Inducer-Type Guide Vane on Hydraulic Losses at the Inter-Stage Flow Passage of a Multistage Centrifugal Pump**

**Mohamed Murshid Shamsuddeen 1,2 , Sang-Bum Ma <sup>2</sup> , Sung Kim <sup>2</sup> , Ji-Hoon Yoon <sup>3</sup> , Kwang-Hee Lee <sup>4</sup> , Changjun Jung <sup>4</sup> and Jin-Hyuk Kim 1,2,\***


**Abstract:** A multistage centrifugal pump was developed for high head and high flow rate applications. A double-suction impeller and a twin-volute were installed at the first stage followed by an impeller, diffuser and return vanes for the next four stages. An initial design feasibility study was conducted using three-dimensional computational fluid dynamics tools to study the performance and the hydraulic losses associated with the design. Substantial losses in head and efficiency were observed at the interface between the first stage volute and the second stage impeller. An inducer-type guide vane (ITGV) was installed at this location to mitigate the losses by reducing the circumferential velocity of the fluid exiting the volute. The ITGV regulated the pre-swirl of the fluid entering the second stage impeller. The pump with and without ITGV is compared at the design flow rate. The pump with ITGV increased the stage head by 63.28% and stage efficiency by 47.17% at the second stage. As a result, the overall performance of the pump increased by 5.78% and 3.94% in head and efficiency, respectively, at the design point. The ITGV has a significant impact on decreasing losses at both design and off-design conditions. An in-depth flow dynamic analysis at the inducer-impeller interface is also presented.

**Keywords:** multistage centrifugal pump; double-suction impeller; twin-volute; computational fluid dynamics; inducer-type guide vane

#### **1. Introduction**

According to statistics, electric motors consume 46 percent of the world's electricity and account for nearly 70% of the net consumption of industrial energy [1]. Power consumption by pump systems alone accounts for about 22% of the world's energy out of which centrifugal pumps consume 16% [2]. Centrifugal pumps have tremendous energy consumption and substantial potential for energy savings. Therefore, researching the possibilities of increasing the efficiency of pump units are need of the hour.

Multistage centrifugal pumps are capable of increasing liquid pressure and pump fluids to a large distance and are widely used in field irrigation, urban afforestation, groundwater supply, and chemical and petroleum industries. Among them, the doublesuction centrifugal pumps can achieve twice the flow rate of a single-suction pump with the same diameter and have better cavitation performance [3]. A double-suction multistage centrifugal pump requires a great deal of energy for the year-round operation and achieving an energy-efficient design can save cost and improve the overall pump performance.

A double-suction multistage centrifugal pump was designed for specific applications in the petrochemical processing plants. The design feasibility study of the pump showed effectiveness in handling multiple fluids without performance degradation [4]. In our

**Citation:** Shamsuddeen, M.M.; Ma, S.-B.; Kim, S.; Yoon, J.-H.; Lee, K.-H.; Jung, C.; Kim, J.-H. Effect of an Inducer-Type Guide Vane on Hydraulic Losses at the Inter-Stage Flow Passage of a Multistage Centrifugal Pump. *Processes* **2021**, *9*, 526. https://doi.org/10.3390/ pr9030526

Academic Editor: Krzysztof Rogowski

Received: 15 February 2021 Accepted: 12 March 2021 Published: 15 March 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

previous study [5], the hydraulic loss analysis of the pump revealed vast potentiality in stage-wise performance recovery specifically at the second stage. The losses were mostly associated with large radial forces in the fluid passing from Stage 1 to 2 through a twin volute. The high circumferential velocity of the fluid at the interface between Stages 1 and 2 caused excessive pre-swirl at the second stage impeller inlet. The fluid pre-swirl induced losses at the second stage impeller thereby decreasing the pump efficiency. Certain design recommendations were provided to control the pre-swirl and enhance the pump characteristics. The recommendation to use a guide vane between the first and second stages is presented in this paper.

Inlet guide vane installation is a common technique to control the fluid circulation and pressure ratio at the inlet of a turbomachine. This method was initially carried out in compressors and fans and was recently applied to centrifugal pumps to regulate fluid pre-swirl at the inlet [6]. Tan et al. [7] studied the effect of an adjustable inlet guide vane for the pre-swirl regulation of a single-stage centrifugal pump and obtained a higher efficiency and head at the design point at an angle of 24◦ . Yuchuan et al. [8] studied the same IGV for angles ±36◦ and ±60◦ to find the influence of guide vanes on unsteady flow. Qu et al. [9] studied the clocking effect of the same IGV and found little influence on pump performance. Liu et al. [10] compared the performance between a 2D IGV and a 3D IGV with a similar design and obtained a higher efficiency with a minimum impact velocity moment for the 3D IGV model. Further investigation by Liu et al. [11] succeeded in suppressing the losses associated with high pressure near the impeller inlet and facilitated a uniform distribution of pressure in the impeller channels at the rotational frequency. Liu et al. [12] studied the influence of the IGV angle and axial distance range between IGV and impeller. The IGV angle had a significant impact in reducing the pressure fluctuation at the blade leading edge while the axial distance had only a slight impact on the pump performance. Lin et al. [13] used an adjustable two plate inlet guide vane at the suction pipe of a single-stage centrifugal pump to reduce the negative pressure at the impeller leading edge. The pump performance was improved at a vane angle of 25◦ , weakening the vortex flow at the pump inlet. Hou et al. [14] studied the effect of the number of IGV vanes on the hydraulic characteristics and suggested a six-vane design for a higher head and better efficiency. It is evident from the literature that an IGV is capable of regulating the pre-swirl at the impeller inlet. However, all these IGV configurations were applied to regulate the pre-swirl in single-stage pumps with an option to control the IGV angle. This is not the case with multistage centrifugal pumps. The usage of pre-swirl regulation of IGV is extremely rare for multistage pumps simply due to the physical constraint to control the IGV angle using gears or levers during operation. Typically, radial diffusers and return guide vanes of fixed angles are used in multistage pumps to transfer fluid from one stage to another. However, a radial diffuser-return vane combination cannot be used to regulate the axial flow exiting the twin volute of the proposed pump. An axial diffuser or a guide vane with a fixed angle is the technically feasible unit that can be installed to regulate this flow.

In order to govern the pre-swirl of the flow between the volute and the second stage impeller, the stationary guide vane design must be meticulously configured since the vane angle is not adjustable. An inducer type, a screw-type, or a helico-axial design is selected for this purpose since the twisted vane design can convert the rotational inertia of the fluid to axial momentum without the need to adjust the angle. Several inducer type pump designs can be found in the literature. Li et al. [15] studied the flow through a three-blade inducer on an axial flow pump and found that the maximum pressure is generated when the inducer angle is aligned with the impeller such that the wake from the inducer impinges the impeller blade minimizing hydraulic losses. Campos-Amezcua et al. [16] studied a two-blade inducer design in a turbo-pump with and without clearance and observed that a uniform axial velocity profile is obtained for an inducer without clearance. Yang et al. [17] studied the clocking effect between the inducer and impeller in a high-speed centrifugal pump and obtained the best performance when the relative

angle between the inducer trailing edge and impeller leading edge was 0◦ . Several pump designers used inducers at the upstream of the impeller to reduce pump cavitation [18–22]. Although inducers were used in centrifugal pumps for decades, they are not commonly found in multistage centrifugal pumps. Sedlár et al. [23] installed a three-bladed inducer in a two-stage centrifugal pump between the inlet guide vane and the first stage impeller. The pump with an inducer showed better cavitation reduction than the pump without an inducer. From these works of literature, it can be said that the application of inducers in centrifugal pumps showed great potential in improving the performance and decreasing the cavitation phenomena. However, all the inducers mentioned are rotating devices with the same speed as the impeller. Since a stationary guide vane is the requirement of the proposed pump, the number of vanes and other design configurations of the inducer shape is influenced by the literature to create an inducer-type guide vane. The ITGV design specifications are provided in the next section.

A multistage centrifugal pump design with an ITGV device to minimize the hydraulic losses occurring at the inter-stage flow passage between the twin volute and second-stage impeller is presented in this paper. The effect of the ITGV design on the overall performance of the pump and the dynamics of the fluid passing through the ITGV is explained in detail.

#### **2. Design Configurations**

The centrifugal pump is designed to pump fluids used in petrochemical refineries satisfying high-head and high-flow rate requirements. The number of stages, the impeller dimensions and other design parameters are determined by API BB5 centrifugal pump standards [24]. The initial pump model is obtained from a dynamically similar scaleddown pump model used for low flow rate operations. The multistage centrifugal pump consists of an inlet passage, a double-suction impeller and a twin-volute in the first stage. Stages 2–4 have a single-suction impeller, a stationary diffuser and return guide vanes. The fifth stage consists of the impeller, diffuser, and outlet volute. Figure 1 shows the exploded view of the pump components.

**Figure 1.** Exploded view of the multistage centrifugal pump and its components.

The theoretical performance curve of the pump is obtained from the pump affinity laws as shown below:

$$\frac{Q\_1}{Q\_2} = \left(\frac{n\_1}{n\_2}\right); \frac{H\_1}{H\_2} = \left(\frac{n\_1}{n\_2}\right)^2; \frac{P\_1}{P\_2} = \left(\frac{n\_1}{n\_2}\right)^3\tag{1}$$

where *Q*, *H*, *P*, and n represents the flow rate, head, input power and rotational velocity, respectively. The subscripts 1 and 2 correspond to the model and the prototype.

Water is chosen as the working fluid for the simulations as the pump affinity laws apply only for water or pure liquids with kinematic viscosity less than 10 cS [25]. The five-stage centrifugal pump has a flow coefficient of ∅ = 0.01 and head coefficient *ψ* = 0.67. The impellers at stages 2–5 have a diameter 20% larger than the first stage impeller. The fifth stage diffuser is 16% larger in diameter than the diffusers in stages 2–4. The twin-volute is staggered at 180◦ to each other to balance out the radial forces. The impellers contain seven blades while the diffuser and return vane consist of eight vanes.

The flow coefficient, the head coefficient and efficiency are calculated using the following equations:

$$
\psi = \frac{gH}{n^2 D^2} \tag{2}
$$

$$
\varphi = \frac{Q}{nD^3} \tag{3}
$$

$$\eta = \frac{\rho Q \text{g}H}{P} \tag{4}$$

where *D*, *g*, *η*, and *ρ* corresponds to the diameter of the impeller, acceleration due to gravity, the efficiency and the density of the fluid, respectively.

A stationary inducer-type guide vane is installed between the first and the second stage with a length of 0.27D. The ITGV consists of three blades shrouded to the casing without clearance. The preliminary design is inspired by a helico-axial impeller designed and optimized in our laboratory [26–28]. The design thus obtained is modified to suit the pump dimensions. The ITGV inlet is designed symmetrically with the fluid which exits the volute being with perfect hydraulic symmetry at all flow conditions. The exit blade angle is matched with the second stage impeller inlet blade angle. The shroud diameter of the ITGV is chosen to be the same as the second stage impeller diameter while the hub diameter is equal to the diameter of the pump shaft. The thickness is maintained equally throughout the blade length. Figure 2 shows the 3D ITGV CAD model and the overall pump design with ITGV.

**Figure 2.** (**a**) The ITGV CAD model and, (**b**) the entire pump with ITGV.

ε

® (

ω

ω

® (

® (

® (

#### **3. Numerical Model**

Three-dimensional mass and momentum equations are solved in a commercial CFD solver to study the flow behavior inside the pump. The fluid transportation equations are based on the steady incompressible Reynolds-averaged Navier–Stokes (RANS) equations solved using an iterative approach in ANSYS CFX 19.1®software (ANSYS, Inc., Pennsylvania, PA, USA). These equations are very well documented in numerous literature [29–31]. The turbulence model, k–ω based shear stress transport (SST) is used to predict the turbulence occurring inside the pump. The SST model uses an integrated feature to shift from a high Reynold's number form of the k–ε model away from the boundary layer and the k–ω model near the wall region [32]. A blending function is used to ensure a smooth transition between the models. Similar studies by the authors using the SST model are well proved to predict the turbulent behavior in a three-stage centrifugal pump [33,34].

The 3D design of the impeller blades, ITGV blades, diffuser and return channel vanes are generated using ANSYS Bladegen®tools (ANSYS, Inc. Pennsylvania, PA, USA) while the inlet passage, the twin-volute and the outlet volute are designed using CAD software. The fluid domains are extracted using ANSYS SpaceClaim®module (ANSYS, Inc. Pennsylvania, PA, USA)while ANSYS meshing tool is used for the grid generation. The impeller domain grids are created using ANSYS TurboGrid®software (ANSYS, Inc. Pennsylvania, PA, USA)which provides an exceptional level of mesh quality with preferred boundary layer resolution. The CFD model including the boundary conditions for the numerical analysis was prepared using CFX-Pre. The governing equations were solved in CFX-Solver and the post-processing was done in CFX-Post. Figure 3a shows the CFD domain used for the pump without the ITGV component. Due to the periodic nature of the geometry; the impellers, diffuser, and return channel domains are chosen as a single passage to save computational resources without compromising on the accuracy of the results. The impeller domains are rotating along the rotational axis while all other domains remain stationary. The outlet pipe is extended to avoid any unlikely backflow occurring at the outlet. The working fluid is water. Atmospheric pressure condition and mass flow rate is defined at the inlet and outlet, respectively. Since the pitch ratio is high at the interface between the stationary domains and rotating domains, the mixing-plane (stage) interface model is applied for the steady-state simulations. General Grid Interface (GGI) mesh connection is provided at all the interfaces to connect the non-conformal elements between the domains. The GGI determines the connectivity between the grids on either side of the interface using an intersection algorithm [35]. The convergence criterion for the RMS residual target was set at 1 <sup>×</sup> <sup>10</sup><sup>6</sup> . Due to the complexity of the multistage pump geometry, the convergence was ensured by monitoring important variables such as the flow rate at the pump outlet, the torque at the impeller blades and the head generated by the pressure gradient at all timesteps. A reasonable convergence was obtained for all the simulations.

**Figure 3.** (**a**) Computational domain of entire pump. (**b**) Generated grids.

#### *Overview of Grid Generation*

The simulation-based study requires a grid independency test to ensure that the results obtained do not vary with grid size. Due to the complexity of the multistage centrifugal pump, the grid study was carried out separately for stages 1 and 2. The optimum grids thus obtained would satisfy the entire pump model since the other stages are a replication of the second stage. The grid number for the outlet volute in the fifth stage is generated analogously to the first stage inlet passage. Since the simulations for the grid independency tests are carried out in two stages, the boundary domains of the individual stages are extended to avoid possible backflow in the simulations. The generated grids are shown in Figure 3b. To resolve the boundary layers, multiple layers of hexahedral meshes are stationed along the blade suction and pressure side surfaces for the impeller, diffuser, and return vanes. The y+ values at these boundaries are kept below 30 while they are maintained below 100 at other locations.

The grid convergence index (*GCI*), derived based on the Richardson extrapolation method, is the most reliable method for a grid convergence study [36]. An approximate relative error (*ea*) and fine grid convergence index (*GCIfine*) is calculated for a key variable obtained from three different sets of grids with significant resolutions. The efficiency of the centrifugal pump is taken as the key variables in this study. The grid convergence index can be calculated from:

$$\text{GCI}\_{fine} = \frac{1.25 \text{ e}\_d}{r - 1} \tag{5}$$

where *r* is the grid refinement factor.

The *GCIfine* for stage 1 and stage 2 were obtained as 0.6% and 0.91%, respectively. Since the efficiency obtained for the fine grid has *GCI* value of less than 1%, it can be said that the generated grids are optimum and further grid refinement is not necessary. The number of nodes for the optimum grid was 1.75 and 1.35 million for stages 1 and 2,

respectively. The total number of nodes generated to create the entire pump domain was 6.25 million. Based on the optimum grid, the grid for the ITGV domain was generated with almost the same number of nodes as the impeller blades. Therefore, further grid study with the ITGV pump is unnecessary.

=

1.25 െ1

#### **4. Pump Performance**

The performance of the pump design obtained from the affinity laws are firstly calculated theoretically and then numerically using CFD tools. The overall pump performance curve obtained by the theoretical calculation is compared with the CFD results in Figure 4. The head coefficient, flow coefficient and efficiency are normalized by their corresponding design point values. The predicted trend of the head and efficiency curves along the change of flow has concurred with the theoretical prediction. The curves obtained from the CFD simulations are in reasonable agreement with the theoretical calculations with an error percentage of less than 8%. The calculation accuracy has a certain influence because of the limitations of the steady-state simulation, the simplified geometrical model and overlooking of losses in the CFD simulation. Since this is a preliminary design feasibility study prior to experimental analysis without considering the unaccounted mechanical losses, the obtained CFD results are acceptable for further analysis.

**Figure 4.** Pump performance comparison of theoretical calculation and numerical simulations.

The overall performance of the pump with and without ITGV is compared in Figure 5. The efficiency of the pump remains unaffected in the low flow rate condition while the head increases slightly due to a minor increase in pressure gradient at the ITGV. At the best efficiency point (BEP), the efficiency has increased by 3.94% while the head increased by 5.78%. The overall performance of the pump has increased by a great margin with the installation of ITGV. The improvement in the pump performance, however, comes at a cost of increased power consumption. The power consumption increased by 1.78% at the BEP and by 8.85% at the maximum flow rate condition with the installation of ITGV. The increase in power consumption is not high at the BEP point at which the pump would be operated normally, and it is high at the maximum flow rate, which is seldom operated. Even with the rise in power consumption at the maximum flow rate condition, the increase in efficiency and head is large enough to offset the difference.

**Figure 5.** Performance comparison of the pump with and without ITGV.

The performance study of the individual stages is as important as the overall performance in a multistage centrifugal pump. The stage-wise efficiency and head coefficient curves of the two pumps are presented in Figure 6. The efficiency at the low flow rate is almost the same at all stages for the pump with and without ITGV. As the flow rate increases, the hydraulic efficiency improves for all stages except for stage 2. The efficiency at stage 2 descends at high rates beyond BEP for the reference pump. Similarly, the head coefficient drops near 0.1 at the maximum flow rate. The large drop in efficiency and head of the reference pump indicates a very large loss at the second stage. The pump with ITGV has improved the efficiency by 47.17% and head by 63.28% at the design point of stage 2. A similar increase is also observed at the maximum flow rate condition of stage 2. The small improvement in the parameters can be found in other stages as well. Installing the IGTV has thus not only improved the performance of stage 2 by a great margin but also improved the performance at all stages. This increase in efficiency and head at all stages reflects the overall improvement in the pump performance as found in Figure 5.

**Figure 6.** Stage performance comparison: (**a**) Efficiency; (**b**) head coefficient.

A detailed analysis of the losses observed at stage 2 and the influence of the ITGV in mitigating these losses must be studied in-depth to understand the flow physics at the ITGV-Impeller interface. The pump is operated at the design point more often than others and as a reason; the pump operating at the design point is chosen for the in-depth analysis. The second stage consists of the impeller, diffuser and return vanes. The losses are mostly observed at the inlet of the impeller and, thus, the loss analysis is focused on the flow through the ITGV and second stage impeller only. Henceforth, the term 'impeller' refers to the second stage impeller unless stated otherwise.

The blade loading at the mid-span of the impeller along the streamwise direction of the pump with and without ITGV is shown in Figure 7. The pressure is normalized by its maximum value. A large drop in pressure at the leading edge is observed in the reference pump indicating the location of the maximum loss. Such sharp pressure drops may cause the formation of cavitation bubbles and can easily lead to pump failure. The installation of the ITGV device at the upstream of the impeller has decreased the pressure drop by 66.13% at the leading edge of the impeller. The overall blade loading has improved significantly by a weighted average of 35.6% with the installation of the ITGV. The weighted average is calculated to accurately represent the average of the percentage change in quantity. The ITGV not only has an impact on the stage 2 impeller but also on the downstream impellers. The blade loading of impellers at stages 3, 4, and 5 (not shown here) was also improved by a weighted average of 17.96%, 10.32%, and 7.09%, respectively.

**Figure 7.** Blade loading comparison of the second stage impeller at mid-span.

The significance of improvement in the blade loading is explained by its effect on individual stages. The head and efficiency trend graph along the mid-span of the impellers for stages 2–5 at the design point is plotted in Figure 8. The parameters are normalized by the corresponding maximum values of the reference pump. Since the ITGV does not affect the upstream flow, the trend line is not plotted for stage 1. A head drop is observed at the second stage of the reference pump at about 20% of the streamwise direction. This corresponds to the pressure drop observed in Figure 7 at 0.2 streamwise. The head rises again towards the trailing edge of the impeller. The head increases at each stage and finally achieves the maximum head at the end of the 5th stage. The ITGV has prevented the drop in pressure gradient at the 2nd stage, which resulted in an increase of head at this stage and an overall increase in the consecutive stages. The overall head trend graph increased by a weighted average of 17.87% with ITGV compared to the reference pump.

**Figure 8.** Head (**a**), and efficiency (**b**) trend graphs plotted at the mid-span of the impellers at the design point.

The efficiency trend graph shows the rise in efficiency at each stage. At the beginning of each stage, the dive in the efficiency curve is due to the abrupt change in the pressure gradient as the fluid travels from one stage to another. While the efficiency dives at each impeller's leading-edge, it immediately climbs back up and rises sharply at the trailing edge. However, the efficiency remains the lowest at the second stage of the reference pump due to the losses mentioned earlier. The introduction of ITGV has aided in reducing the losses and improving the efficiency at the second stage as well as an overall increase in the consecutive stages. The weighted average increase in the overall efficiency trend graph is 14.48% compared to the pump without ITGV. The potential of the ITGV is remarkable in improving the pump characteristics. However, how the ITGV design affects the fluid flow behavior and the reason for losses and the effects of ITGV are studied qualitatively in the next section.

#### **5. Flow Field Analysis**

The fluid flowing through the volute, ITGV and the second stage impeller is analyzed in detail to determine the causes for the losses and the correction by the ITGV at the design point. From the first stage impeller, the fluid entering the volute splits into the two arms of the 180◦ staggered twin-volute, flows along the surfaces of the volute and joins back towards the exit of the volute. The fluid is found to have a greater radial force than the axial force at the volute exit and, as a result, produces a pre-swirl at the inlet of the second stage impeller. This high-intensity swirl flow causes deviation between the fluid incidence angle and blade angle at the impeller leading edge. The flow through the volute and the impeller is shown in Figure 9a. The 3D velocity streamlines show a shift in the flow direction due to the fluid moving from a stationary domain to a rotating domain. However, the flow direction entering the impeller flows away from the blade incidence angle due to the high swirl intensity. The absolute velocity increases at the impeller inlet due to the large circumferential velocity at the volute exit. This causes flow separation at the leading edge and gives rise to recirculation regions at the inlet and the pressure side of the impeller, leading to the formation of vortices in the flow. The vortex core region formed at the impeller is shown in Figure 9b. The vortices thus formed cause blockage to the incoming flow thereby decreasing the pressure at this region. The pressure drop directly affects the stage performance and result in losses at the second stage impeller.

− **Figure 9.** (**a**) Three-dimensional velocity streamlines of the fluid flowing through the volute and impeller, (**b**) Vortex core region inside the second stage impeller (velocity swirling strength = 1500 s−<sup>1</sup> ).

The installation of the ITGV does not prevent the formation of the high-intensity swirl flow observed at the exit of the twin-volute; it rather continues the flow along the ITGV blades without changing its direction. The magnitude of the velocity decreases as the fluid flows through the stationary blades of the ITGV as shown in Figure 10a. The average velocity of the fluid decreased from 33.86 m/s at the volute exit to 22.65 m/s at the ITGV exit. The decrease in circumferential velocity at the exit of the ITGV allows the fluid to flow towards the incidence angle of the blade leading edge. This is because the ITGV exit blade angle is configured to match the impeller inlet blade angle. As a result, the flow separation at the impeller leading edge is moderated and thereby decrease the intensity of the vortices formed at the impeller. Figure 10b shows the decrease in vortex core in the second stage impeller. The blockage in the flow is removed with the installation of ITGV and hence the pressure losses are diminished.

The flow angles are explained in detail by plotting the velocity diagram at the leading edge of the impeller in Figure 11. The vectors U and C<sup>U</sup> represent the blade velocity and the tangential velocity, respectively. In Figure 11a, the relative flow angle is *β* = 128.5◦ while the absolute flow angle is *α* = 11.86◦ at the inlet of the impeller for pump without ITGV. The large relative flow angle force the fluid to flow virtually perpendicular to the blade. The relative flow angle decreases sharply to *β* = 56.4◦ and the absolute flow angle rises to *α* = 17.6◦ for the pump with ITGV as shown in Figure 11b. The magnitude of the relative velocity (W) remains essentially the same while the direction changes towards the blade angle similar to the observation in Figure 10a. The magnitude of the absolute velocity (C) decreases by 22.46%. The velocity triangles of the rest of the stages are approximately the same for both pumps.

− **Figure 10.** (**a**) Three-dimensional velocity streamlines of the fluid flowing through the volute, ITGV, and impeller. (**b**) Vortex core region inside the second stage impeller (velocity swirling strength = 1500 s−<sup>1</sup> ).

**Figure 11.** Velocity triangles at the leading edge of the impeller (**a**) pump without ITGV, and (**b**) pump with ITGV.

The relative flow angle correction achieved by the ITGV has a significant impact on the fluid inside the impeller. The velocity streamlines at the mid-span of the impeller is compared in Figure 12a,b. There is an adverse pressure gradient between the blades leading to the formation of the vortex and a non-uniform flow is observed at the reference pump. The flow through the impellers appears to be smooth and uniform with the disappearance of vortices in the pump with ITGV. The total pressure in stationary frame contour is shown in Figure 12c,d. The low-pressure region at the pressure-side of the blades is eliminated to obtain a smooth transition of fluid pressure from the inlet to the outlet of the ITGV pump impeller. The increasing pressure increases the head developed at this stage as observed earlier.

**Figure 12.** Velocity streamlines at the mid-plane of the impeller for (**a**) a pump without ITGV, (**b**) a pump with ITGV, and the total pressure contour in a stationary frame at the mid-plane of the impeller for (**c**) a pump without ITGV and (**d**) a pump with ITGV.

#### **6. Performance Analysis at Off-Design Conditions**

The centrifugal pump is generally operated at its design point (Qd) at which the efficiency curve reaches its maximum. However, the pump may be operated at off-design points at times by force of circumstances to deliver fluid either below or above the capacity at BEP. An adverse pressure gradient, flow separation, and flow recirculation at the inlet and exit always occurs under off-design points. The flow phenomenon is more complex than the design point, especially at the high flow rate conditions. Therefore, it is necessary to study the pump performance at these conditions too. Two off-design conditions are tested at 25% below and excess flow capacity of the design point. The head trend line is compared for low flow rate and high flow rate for both the pumps in Figure 13a,b. There is a minor increase in the head trend line of the pump with ITGV at 0.75Q<sup>d</sup> and a significant increase at the 1.25Q<sup>d</sup> flow condition. The head increases by a weighted average of 3.58% at the low flow rate and gains a weighted average of 20.48% at the high flow rate condition for the ITGV pump. A similar increase of weighted average head by 17.87% was observed previously at the design point, too. The losses inside the pump escalate as the flow rate rises but the ITGV is capable of executing head loss correction at all flow rates.

**Figure 13.** Head and efficiency trend graphs (**a**–**d**) and second stage blade loading chart (**e**,**f**) comparison at the mid-span of the impellers at off-design conditions for the pump with and without ITGV.

The efficiency trend graph measured at the mid-span of the impellers at both flow rates is compared for the two pumps in Figure 13c,d. A notable improvement in efficiency is found at the second stage of 0.75Q<sup>d</sup> for the ITGV pump while there is only a slight improvement at other stages. Meanwhile, there is no significant improvement in efficiency at the leading edge of the second stage impeller at 1.25Q<sup>d</sup> for the pump with ITGV, but it rises near the trailing edge. The rise in efficiency continues for stages 3–5. The ITGV installation improved the overall efficiency of the stages by a weighted average of 13.7% and 18.45% at 0.75Q<sup>d</sup> and 1.25 Qd, respectively. This also proves that correcting the losses at the second stage improves the performance at other downstream stages too. This can be analyzed by plotting the blade loading curve at the mid-span of the second stage impeller along the streamwise direction as shown in Figure 13e,f. The blade loading distribution was improved by a weighted average of 24.9% and 37.6% at 0.75Q<sup>d</sup> and 1.25Qd, respectively, for the pump with ITGV. Even though the pressure-drop at the leading edge of the impeller decreased by 41% at the high flow rate of the ITGV pump, the pressure is still low enough to cause cavitation damage in the long run. A detailed cavitation analysis may be necessary to find the cavitation zones in the off-design points.

The vortex core region formed near the second stage impeller has practically disappeared with the installation of ITGV at the 0.75Q<sup>d</sup> flow condition as shown in Figure 14a,b. Several large and small vortices are observed at the high flow rate condition near the impeller inlet (Figure 14c). The large vortices are formed due to huge flow separation at the leading edge which increases with the flow rate. The ITGV pump has diminished the large vortices formed at the blade suction side and decreased the intensity of the vortices formed at the pressure side of the impeller (Figure 14d). Further suppression of the vortices may be achieved after a design optimization strategy applied to optimize the ITGV and impeller shapes with an objective function to minimize leakage vortices and improve the pump performance at this particular flow condition.

<sup>−</sup> **Figure 14.** Vortex core region inside the second stage impeller (velocity swirling strength = 1500 s−<sup>1</sup> ) calculated at (**a**) 0.75Q<sup>d</sup> without ITGV (**b**) 0.75Q<sup>d</sup> with ITGV (**c**) 1.25Q<sup>d</sup> without ITGV, and (**d**) 1.25Q<sup>d</sup> with ITGV

The installation of ITGV has aided in improving the pump efficiency and head at various flow rates. The losses associated with the twin-volute and the second stage blades have been successfully diminished by placing the ITGV between them. However, the ITGV installation comes with certain restrictions. Firstly, the ITGV installation expanded the pump size by 0.27D. This may come as a drawback at locations with size restrictions for a multistage centrifugal pump. Secondly, manufacturing the ITGV unit requires precision machining tools and skilled operators which may induce additional cost to the pump manufacturer. This is determined in the economic analysis and feasibility study of the pump in the manufacturing stage.

#### **7. Conclusions**

Installation of an inducer-type guide vane at the inter-stage flow passage of a multistage centrifugal pump is studied for its loss mitigating capability and performance enhancement. The CFD model consisted of an inlet passage that contains a double-suction impeller and a twin volute in the first stage. Series of impeller, diffuser, and return vanes were installed for the rest of the stages with an outlet volute at the end of the fifth stage. The grids generated are tested for grid independency and they satisfy the GCI criteria. The pump performance was analyzed analytically and compared with the CFD results for initial validation. The design was tested for loss analysis at individual stages. Very large losses were observed at the inlet of the second stage impeller due to the large circumferential velocity of the fluid exiting the twin volute. A stationary ITGV was installed between the twin volute and the second stage impeller to regulate the pre-swirl and correct the incoming flow angle at the blade inlet. The beta angle at the ITGV trailing edge was designed to match the beta angle at the leading edge of the impeller such that the relative flow angle is tangential to the blade incidence angle. The effects of the ITGV compared to the initial pump model are:


The ITGV was successful not only in decreasing the circumferential velocity of the fluid but also improved the overall performance of the pump by diminishing the losses occurring at the second stage. The ITGV pump would be tested experimentally to validate the CFD results and is ongoing research. The effect of ITGV on pump cavitation and the optimization of the ITGV blade design is the future work of this study. The optimized design would be tested again in the laboratory before commercialization.

**Author Contributions:** Conceptualization: J.-H.K., S.-B.M. and M.M.S.; methodology: S.-B.M. and M.M.S.; software: M.M.S.; validation: J.-H.Y. and M.M.S.; formal analysis: M.M.S.; investigation: S.K., S.-B.M. and M.M.S.; resources: J.-H.Y., K.-H.L. and C.J.; data curation: M.M.S. and S.-B.M.; writing original draft preparation: M.M.S.; writing—review and editing: S.-B.M. and M.M.S.; visualization: M.M.S.; supervision: J.-H.K.; project administration: K.-H.L.; funding acquisition: J.-H.K. and K.-H.L. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was supported by grants (no. EE200001) and (no. JB210001) of the Korea Institute of Industrial Technology (KITECH).

**Institutional Review Board Statement:** Not Applicable.

**Informed Consent Statement:** Not Applicable.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


### *Article* **Testing the Accuracy of the Cell-Set Model Applied on Vane-Type Sub-Boundary Layer Vortex Generators**

**Koldo Portal-Porras <sup>1</sup> , Unai Fernandez-Gamiz 1,\* , Iñigo Aramendia <sup>1</sup> , Daniel Teso-Fz-Betoño <sup>2</sup> and Ekaitz Zulueta <sup>2</sup>**


Vitoria-Gasteiz, 01006 Araba, Spain; daniel.teso@ehu.eus (D.T.-F.-B.); ekaitz.zulueta@ehu.eus (E.Z.)

**\*** Correspondence: unai.fernandez@ehu.eus; Tel.: +34-945-014-066

**Abstract:** Vortex Generators (VGs) are applied before the expected region of separation of the boundary layer in order to delay or remove the flow separation. Although their height is usually similar to that of the boundary layer, in some applications, lower VGs are used, Sub-Boundary Layer Vortex Generators (SBVGs), since this reduces the drag coefficient. Numerical simulations of sub-boundary layer vane-type vortex generators on a flat plate in a negligible pressure gradient flow were conducted using the fully resolved mesh model and the cell-set model, with the aim on assessing the accuracy of the cell-set model with Reynolds-Averaged Navier-Stokes (RANS) and Large Eddy Simulation (LES) turbulence modelling techniques. The implementation of the cell-set model has supposed savings of the 40% in terms of computational time. The vortexes generated on the wake behind the VG; vortical structure of the primary vortex; and its path, size, strength, and produced wall shear stress have been studied. The results show good agreements between meshing models in the higher VGs, but slight discrepancies on the lower ones. These disparities are more pronounced with LES. Further study of the cell-set model is proposed, since its implementation entails great computational time and resources savings.

**Keywords:** vortex generator (VG); computational fluid dynamics (CFD); cell-set model; RANS; LES

#### **1. Introduction**

Vortex Generators (VGs) are passive flow control devices, whose objective is to delay or remove the flow separation, transferring the energy generated from the outer region to the boundary layer region. They are small vanes placed before the expected region of separation of the boundary layer. They are usually mounted in pairs, with an incident angle with the oncoming flow. Regarding their shape, VGs can be of various geometries, but they are mainly triangular or rectangular. Their height is typically similar to the boundary layer thickness where the VG is applied, in order to ensure a good interaction between the boundary layer and the vortex generated in the VG. However, since tall VGs lead to high drag forces, VGs with smaller heights than the local boundary thickness, i.e., Sub-Boundary-Layer Vortex Generators (SBVGs), are used in many applications, see Ashill et al. [1,2]. Aramendia et al. [3,4] comprehensively reviewed the available flow control devices, including VGs, and Lin [5] conducted an in-depth review of the control of flow separation in the boundary layer using SBVGs.

Since their introduction by Taylor [6] in the late 1940s, VGs have been used in a wide range of industries for numerous applications. Among these industries, aerodynamics and thermodynamics are the most remarkable. Øye [7] and Miller [8] implemented VGs on 1 MW and 2.5 MW wind turbines, respectively. Heyes and Smith [9] added VGs of numerous shapes on the wing tip of an aircraft, and Tai [10] studied the effect of Micro-

**Citation:** Portal-Porras, K.; Fernandez-Gamiz, U.; Aramendia, I.; Teso-Fz-Betoño, D.; Zulueta, E. Testing the Accuracy of the Cell-Set Model Applied on Vane-Type Sub-Boundary Layer Vortex Generators. *Processes* **2021**, *9*, 503. https://doi.org/10.3390/pr9030503

Academic Editor: Jin-Hyuk Kim

Received: 15 February 2021 Accepted: 9 March 2021 Published: 11 March 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

Vortex Generators (MVGs) on V-22 aircraft. All of them showed a significant aerodynamic performance improvement when implementing VGs.

Another sector in which VGs are widely used is thermodynamics. Currently, major efforts are being made in the thermodynamics field to increase heat and mass transfer, see Agnew et al. [11]. For this reason, numerous authors have implemented in different thermodynamic systems. For example, Joardar and Jacobi [12] studied the heat transfer and pressure drop of a heat exchanger before and after the addition of VGs, showing an increase of the heat transfer coefficient between 16.5% and 44% with a single VG pair and between 30% and 68.8% with 3 VG pairs.

Although many studies use experimental techniques, the use of Computational Fluid Dynamics (CFD) tools for performing numerical studies is becoming a very popular choice for studying VGs. CFD studies of VGs are currently focused on two main goals. The first goal is to optimize the position and distribution of VGs, see the studies of Subbiah et al. [13] and Yu et al. [14]. The second goal is to analyze the swirling vortexes generated on the wake behind the VG, see the studies of Carapau and Janela [15] and Sheng et al. [16] about this phenomenon.

Many authors have studied SBVGs using CFD. Ibarra-Udaeta et al. [17] and Martinez-Filgueira et al. [18] analyzed the vortices generated by rectangular vane-type SBVGs on a flat plate under negligible pressure gradient flow conditions. They analyzed VGs with heights equal to 0.2, 0.4, 0.6, 0.8, 1, and 1.2 δ and incident angles equal to 10◦ , 15◦ , 18◦ , and 20◦ . Fernandez-Gamiz et al. [19] studied three different SBVGs with heights of 0.21, 0.25, and 0.31 δ and an incident angle equal to 18◦ . Gutierrez-Amo et al. [20] analyzed a rectangular, a triangular, and a symmetrical NACA0012 SBVG. Fully resolved mesh modelling technique was used in all the mentioned studies, and all of them showed good agreements with experimental data.

The main disadvantage of the fully resolved mesh model is the fine mesh that requires to accurately capture the physical phenomena, especially in the near-VG region and in the wake behind the VG. For that reason, numerous authors [21–23] have implemented alternative models. The majority of these models are based on the BAY model developed by Bender et al. [24], which models the force produced by a VG. Errasti et al. [25] implemented the jBAY source-term model developed by Jirasek [26] in vane-type SBVGs under adverse pressure flow conditions and showed accurate results in terms of vortex path, vortex decay, and vortex size.

The cell-set model is another alternative model, which consists of leveraging the previously generated mesh to build the desired geometry. Besides the advantages that the cell-set model provides over the fully resolved mesh model, there are not many studies in which this model has been applied. Ballesteros-Coll et al. [21,27] used the cell-set model to generate Gurney flaps and microtabs on DU91W250 airfoils, and Ibarra-Udaeta et al. [28] modelled conventional vane-type VGs with this model.

The goal of the present paper is to evaluate the accuracy of the cell-set model applied on SBVGs with heights of 0.2, 0.4, 0.6, 0.8, and 1 δ. For that purpose, CFD simulations of SBVGs on a flat plate in a negligible streamwise pressure gradient flow conditions are conducted using the fully resolved mesh model and the cell-set model, and the results obtained with the fully resolved mesh model are taken as benchmark. With the purpose of testing the cell-set model with RANS and LES, both models are used to conduct the simulations.

The remainder of the manuscript is structured as follows: Section 2 provides a general description of the used numerical domain and meshing models. Section 3 explains the results obtained in the present work. Finally, Section 4 summarizes the main conclusions reached from the results and future directions.

#### **2. Numerical Setup**

CFD simulations of sub-boundary layer vane-type VGs on a flat plate in a negligible streamwise pressure gradient flow were conducted with the intention of investigating the accuracy cell-set model. Star CCM+v14.02.012 [29] CFD commercial code was used to conduct all the simulations.

#### *2.1. Computational Domain and Physic Models*

The computational domain consists of a block with a rectangular VG situated on its lower surface. The flow goes from the upstream part of the block to its downstream part; hence, they are set as inlet and outlet, respectively. The bottom surface of the block and the faces of the VG are set as no-slip walls, and symmetry plane conditions are assigned to the rest of the surfaces, ensuring that the flow is not affected by their presence. The computational domain has been designed to ensure that the boundary layer thickness (δ) at the location of the VG is equal to 0.25 m.

Regarding the fluid, an incompressible turbulent flow is considered, in a steady-state with RANS and in an unsteady-state with LES. According to expression (1), the Reynolds number (Re) of this flow is around 27,000.

$$Re = \frac{\mathcal{U}\_{\infty} \cdot \delta}{v} \,\tag{1}$$

where *v* refers to the kinematic viscosity and *U*∞ to the free stream velocity of the flow, which is set at 20 m/s for this study.

As the objective of this paper is to analyze the cell-set model on SBVGs, 10 different SBVGs are considered. Five different VG heights (H), 0.2, 0.4, 0.6, 0.8, and 1 δ, and two different incident (α) angles, 18◦ and 25◦ , are considered. The length (L) of the VG is equal to 2 δ for every case. More information about the VGs and the computational domain is shown in Table 1 and Figure 1.



For the simulations in which α is equal to 18◦ , Menter's k-ω SST (Shear Stress Transport) [30]. RANS-based turbulence model is selected. This model has been selected since, as demonstrated by Allan et al. [31], SST models provide more accurate vortex trajectory and streamwise peak vorticity predictions than other RANS models. In contrast, Urkiola et al. [32] showed that when working with high incident angles, RANS-based models are not able to capture flow characteristics as accurately as when working with low incident angles. Hence, for the simulations in which the incident angle is equal to 25◦ , LES Smagorinsky SGS (sub-grid-scale) [33] model is selected. Furthermore, this selection of turbulence models allows the cell-set model to be analyzed using both RANS and LES.

For data extraction, 12 spanwise planes normal to the streamwise direction located on the wake behind the VG are considered. These planes are located from 3 to 25 δ from the LE (Leading Edge), separated 2 δ between each other.

#### *2.2. Fully Resolved Mesh Model*

Five different structured meshes of around 11.5 million hexahedral cells were generated, one for each VG height. In all the cases, the normalized height of the closest cell to the wall (∆z/δ) was set at 1.5×10−<sup>6</sup> . For the generation of these meshes, the procedure described by Urkiola et al. [32] was followed. In order to obtain more accurate results in the near-VG region, these meshes are refined in this zone. The meshes were rotated to obtain the desired incident angles (α = 18◦ and α = 25◦ ). Figure 2 shows the mesh refinement around the VG for the case H = 1 δ.

**Figure 1.** (**a**) Numerical domain (not to scale). (**b**) Vortex Generator (VG) parameters.

**Figure 2.** Refined mesh around the VG for H = 1 δ. (**a**) Top view and (**b**) side view.

The skewness angle, volume change, and face validity cell quality parameters have been selected to assess the quality of the tested meshes. The skewness angle is the angle between a face normal vector of a cell and the vector connecting the centroids of this cell and the neighbor cells. The volume change is the ratio of the volume of a cell to that of its largest neighbor. The face validity is a measure of the correctness of the face normal relative to its attached cell centroid.

According to [29], the skewness angle should be as low as possible, and cells with a skewness angle greater that 85◦ could result in solver convergence issues, so they are considered low-quality cells. These problems appear since the diffusion term for transported scalar variables contains in its denominator the dot product between the face normal vector and the vector connecting the centroids, and therefore, skewness angles close to 90◦ imply very high values of this term. The volume change ratio should be close to 1, since large jump in volume from one cell to its neighbor can cause inaccuracies and instability in the solvers. Therefore, cells with volume changes below 0.01 are considered inadequate. The face validity must be equal to 1, since different values mean that the face normals do not point away from the cell centroid correctly, and values below 0.5 signify a negative volume cell. As Table 2 shows, all the meshes fulfill these criteria.

**Table 2.** Cell quality parameters of the used meshes with the fully resolved mesh model.


To verify sufficient mesh resolution, two different procedures were followed, one for each turbulence model. Both mesh resolution studies were applied for the case H = 1 δ. For RANS, the General Richardson Extrapolation method [34] was performed, applied to lift and drag forces of the VG. This method consists of estimating the value of the analyzed parameter when the cell quantity tends to infinite from a minimum of three meshes. For this study, a coarse mesh (0.2 million cells), a medium mesh (1.4 million cells), and a fine mesh (the previously explained mesh, 11.5 million cells) were considered. As summarized in Table 3, the convergence condition, which should be between 0 and 1 to ensure a monotonic convergence, is fulfilled, and the estimated values (RE) of the evaluated parameters are close to the ones obtained with the fine mesh. Therefore, the mesh is suitable for RANS simulations.

**Table 3.** Mesh verification for Reynolds-Averaged Navier-Stokes (RANS).


In LES, Taylor length-scale (λ) was examined to verify sufficient mesh resolution. According to Kuczaj et al. [35], the mesh resolution (∆ = <sup>√</sup><sup>3</sup> *<sup>V</sup>cell*) should at least be in order of λ to completely solve the Taylor length-scale. As explained in [35], Taylor length-scale calculation procedure consists of obtaining the autocorrelation function from the Taylor expansion coefficient, then, calculating the Taylor time-scale, and finally, estimating λ from the Taylor hypothesis [36]. This method has been applied on the wake behind the VG, at y/δ = 1, since this area is expected to be the area where the effects of the turbulence are most noticeable, and therefore, the area where the best resolution is required. As Figure 3

shows that the criteria proposed by Kuczaj et al. [35] is fulfilled along the whole wake behind the VG, which means that the mesh is suitable for LES simulations.

**Figure 3.** Mesh resolution and Taylor length scale on the wake behind the VG at y/δ = 1 for the case H = 1 δ with the fully resolved mesh model.

#### *2.3. Cell-Set Model*

In the present work, the accuracy of the cell-set model applied on sub-boundary layer VGs is evaluated. This model consists of generating the desired geometry in a mesh that initially does not contain such geometry. To apply the cell-set model, the place where the geometry should be located in the mesh is indicated, as displayed in Figure 4a. Later, the cells that correspond to this geometry are selected by means of their cell ID. Finally, with the selected cells a new cell-set region is created, as shown in Figure 4b, and wall conditions are assigned to this new region.

**Figure 4.** Sketch of the selected cells when using the cell-set model. (**a**) Geometry of the VG and (**b**) cell-set representation.

With the cell-set model, meshes of around 7.2 million cells have been generated. Thus, the meshes are coarser with this model than with the fully resolved mesh model. In addition, the mesh design and generation processes are faster with the cell-set model. As in the fully resolved mesh, <sup>∆</sup>z/<sup>δ</sup> is equal to 1.5×10−<sup>6</sup> . Figure 5 shows the top and side views of the VG generated with the cell-set model for H = 1 δ and α = 18◦ .

**Figure 5.** Cell-set construction of the VG with the cell-set model for α = 18◦ and H = 1 δ. (**a**) Top view and (**b**) side view.

As with the fully resolved mesh model, the quality of the meshes generated with the cell-set model has been evaluated with skewness angle, volume change and face validity parameters. As shown in Table 4, and according to the previously explained criteria, the cell quality of the meshes generated with the cell-set model is adequate.


**Table 4.** Cell quality parameters of the used meshes with the cell-set model.

To verify sufficient mesh resolution, as with the fully resolved mesh model, two different procedures have been followed, one for each turbulence model. In both cases, the mesh verification has been performed with the H = 1 δ case. For RANS, the General Richardson Extrapolation method has been applied. However, in this case, the three meshes are made of 7.2 million cells (fine mesh), 3.6 million cells (medium mesh), and 1.8 million cells (coarse mesh). As Table 5 shows, the results fulfill the convergence condition. Thus, the mesh generated using the cell-set model is adequate for RANS simulations.

For LES simulations, Taylor length-scale (λ) is examined to verify sufficient mesh resolution. As shown in Figure 6, the mesh satisfies the criteria proposed by Kuczaj et al. [35] on the whole wake behind the VG, and therefore, it is suitable for LES simulations.


**Table 5.** Mesh verification for RANS.

**Figure 6.** Mesh resolution and Taylor length scale on the wake behind the VG at y/δ = 1 for the case H = 1 δ with the cell-set model.

#### **3. Results and Discussion**

In this study, the vortices generated in the wake behind the VGs have been analyzed. Moreover, an exhaustive analysis of the primary vortex has been performed, studying its path, size, and strength and the wall shear stress behind it.

For the interpretation of RANS results, the last obtained values have been considered, whereas for the results of LES simulations, the average values of 2 s of simulation have been considered, after the flow is completely developed.

Parallel computing with 56 Intel Xeon 5420 cores and 45 GB of RAM were used to carry out all the simulations. Simulations performed with fully resolved mesh modelling were run for about 47 h using the RANS turbulence model and for around 184 h using the LES model. In contrast, simulations in which cell-set modelling was applied were run for approximately 28 h for RANS and 111 h for LES.

#### *3.1. Vortex Structure Regimes in the Wake*

As measured by Velte [37], two basic vortex mechanism appear in the wake behind the VG. The main vortex system is composed of a primary vortex (P), which is formed on the wing tip, and a horseshoe vortex, which is generated from the rollup vortex around the LE of the VG. This horseshoe vortex is divided in two sides, the pressure side (Hp) and the suction side (Hs). As the primary vortex is stronger than these sides, the primary vortex pulls the suction side. As the primary vortex and the pressure side have the same sign, the pressure side remains undisturbed.

The secondary vortex structure is created by the local separation of the boundary layer in the lateral direction between the primary vortex and the wall. Due to the dragging of the suction side by the primary vortex, the primary vortex becomes stronger, the boundary layer region grows, and finally detaches, forming a discrete vortex (D). Figure 7 shows a representation of the primary and secondary vortexes.

**Figure 7.** Vortex mechanisms in the wake behind a VG.

Nevertheless, Velte [37] showed that these structures can vary, depending on the incident angle and the height of the VG. Figure 8 displays a comparison of the vortical structures predicted by the numerical simulations with both studied models at a distance of 5 δ from the VG Trailing Edge (TE), and the vortical structures measured by Velte [37].

Regarding the main vortex structure, the results show that both RANS and LES are able to accurately predict the primary vortex with the fully resolved mesh model and the cell-set model. In LES simulations, the horseshoe vortex, which is expected to appear in VGs with heights above 0.4 δ, is predicted for all the heights, including 0.2 δ. In contrast, RANS is not able to capture the pressure side of this horseshoe vortex for heights below 0.8 δ.

The largest discrepancies between the simulations and the experimental results appear in the secondary vortex structure. This vortex structure is expected to appear in VGs whose heights are below 0.4 δ. In LES, this vortex is only visible for H = 0.2 δ with the fully resolved mesh model. This vortex is not predicted in RANS for neither height.

Despite showing different values, the fully resolved mesh model and the cell-set model predict very similar vortexes in terms of vortex shape and direction.

#### *3.2. Vortical Structure of the Primary Vortex*

The Q-criterion [38] method has been used to compare qualitatively the primary vortex generated by each VG in terms of shape and size. This method visualizes structures of the flow, and its value is defined by *Q* = <sup>1</sup> 2 kΩk <sup>2</sup> − k*S*<sup>k</sup> 2 , where Ω is the spin tensor and S the strain-rate tensor. As the value of Q is set at Q = 2500 s−<sup>2</sup> , the vortical structures are displayed. Figure 9 shows the representation of the primary vortex at 5 δ from the VG TE by means of the Q-criterion.

The results show that for α = 18◦ , the taller the VG, the larger the vortex. However, for α = 25◦ , although this also occurs, the differences between heights are smaller, with the size of the vortices being more similar than when α = 18◦ .

**Figure 8.** Vortical structures predicted on the wake behind the VG. (**a**) Reynolds-Averaged Navier-Stokes (RANS) (α = 18◦ ) and (**b**) Large Eddy Simulation (LES) (α = 25◦ ).

**Figure 9.** Primary vortex represented by the Q-criterion with a value of Q = 2500 s−<sup>2</sup> . The black squares are the projections of the VG Trailing Edges: (**a**) RANS Fully Resolved Mesh model (α = 18◦ ), (**b**) RANS cell-set model (α = 18◦ ), (**c**) LES fully resolved mesh model (α = 25◦ ), and (**d**) LES cell-set model (α = 25◦ ).

With RANS, even if they have the same circular shape, the vortexes predicted by the cell-set model are larger than the ones predicted by the fully resolved mesh model. With LES, generally, the vortexes predicted by the cell-set model are smaller than those predicted by the fully resolved mesh model. In this case, slight disparities between models are visible in terms of vortex shape, which are attributed to the unsteadiness of the flow.

#### *3.3. Vortex Path*

In order to analyze the vortex path of the primary vortex, the location of the center of this vortex is studied. According to Yao et al. [39], the vortex center is the point in where the peak vorticity appears. Figure 10 shows the vertical and lateral path of the primary vortex normalized with the height of each VG. The lateral path obtained in the present study for α = 18◦ is compared to the one obtained experimentally by Bray [40].

The lateral path shows that in all the cases, the vortex tends to follow the flow direction, showing a linear trend. With both turbulence models, the lower the height of the VG, the greater the horizontal displacement. Good agreements are obtained with the experimental data reported by Bray [40]. Near the VG, the lateral displacements are nearly equal, except with H = 0.2 δ and α = 18◦ , but as the flow distances from the VG, the differences between cases increase, most notably with α = 25◦ .

Corresponding the vertical path, the results show that the vortexes tend to collapse near y/H = 1, except for the case H = 0.2 δ, in which the vortex continues its upward climb as it distances from the VG, this is more noticeable with α = 18◦ than with α = 25◦ .

**Figure 10.** Non-dimensional path of the primary vortex obtained with the fully resolved mesh model (FM), the cell-set model (CS), and experimentally (EXP). (**a**) Non-dimensional lateral path with RANS, (**b**) non-dimensional lateral path with LES, (**c**) non-dimensional vertical path with RANS, and (**d**) non-dimensional vertical path with LES.

The comparison between the fully resolved mesh model and the cell-set model shows that in both cases, the same trend is followed with both models. With RANS, larger lateral displacements are obtained with the cell-set model, while with LES, the larger lateral displacements are obtained with the fully resolved mesh model. The cell-set model predicts larger vertical displacements with RANS and LES. For the highest VGs, the results are very similar with both models, but as the VG height decreases, the differences between models increase, especially with LES.

#### *3.4. Vortex Size*

The vortex size is analyzed by the Half-Life Radius (R05) parameter developed by Bray [40]. This parameter determines the distance between the vortex center and the point where the local vorticity is equal to *<sup>ω</sup>peak* 2 . As shown in Figure 9, the vortex shape is not always circular, therefore, R<sup>05</sup> has been estimated by averaging the values in vertical and lateral directions. Figure 11 shows the R<sup>05</sup> values normalized with δ on the wake behind the VG for the tested cases.

**Figure 11.** R<sup>05</sup> normalized with δ. (**a**) RANS and (**b**) LES.

The results show that the greatest vortexes appear in the taller VGs. In RANS, the R<sup>05</sup> increases linearly from the near-VG region, but in LES, R<sup>05</sup> remains almost constant near the VG, and it starts increasing at 10 δ from the VG LE.

Despite showing the same trend, in all the cases, the cell-set model predicts smaller vortexes than the fully resolved mesh model, these differences are more notable with LES. The largest discrepancies between models are visible in the lower VGs, most notably with LES.

#### *3.5. Vortex Strength*

To quantify the vortex strength, vortex circulation (Γ) is considered. This parameter determines the capacity of the vortex to mix the outer flow with the boundary layer [2]. According to Yao et al. [39], the vortex circulation can be estimated by expression (2). Figure 12 shows the vortex circulation normalized with the VG height and the flow streamwise velocity.

2

**Figure 12.** Vortex circulation normalized with the VG height and the flow streamwise velocity. (**a**) RANS and (**b**) LES.

As expected, the vortex losses its strength as it distances from the VG. Close to the VG, the stronger vortices appear in the lower VGs. With RANS, as the distance between the VG and the flow increases, the results tend to collide with both models. In contrast, with LES, this trend is only visible with fully resolved mesh modelling, since with the cell-set model, despite following a falling tendency, the collision of the results is not achieved. With this turbulence model, the normalized circulations are considerably higher with the cell-set model than with the fully resolved mesh model for the lower VGs, but for the higher ones, the differences decrease.

Although, as mentioned before, the R<sup>05</sup> values predicted with the fully resolved mesh model are higher, vortex circulation values are very similar with the RANS model. This is attributed to the consideration of the vorticity in the expression of the circulation. With LES, despite showing less differences in Γ than in R05, differences are significant for low VG cases.

#### *3.6. Wall Shear Stress*

Wall shear stress is a major parameter to quantify the capacity of the VG to delay the flow separation. Figure 13 shows the values of the wall shear stress on the wake behind the VG for all the tested cases.

In the tested cases, the wall shear stress goes from a low value to a maximum value, which appears between x/δ = 3 and x/δ = 6, depending on the case. The lower the VG, the closer to the VG the maximum appears. Then, as expected, wall shear stress slightly decreases as it distances from the VG.

According to Godard and Stanislas [41], the optimum angle for the maximum wall shear stress is around 18◦ , and the wall shear stress is not very sensitive to the aspect ratio. The obtained results are in accordance to these statements, since the values obtained with α = 18◦ are greater than the ones obtained with α = 25◦ , and in the majority of the cases, very similar values are obtained, specially far away from the VG.

**Figure 13.** Wall shear stress on the wake behind the Trailing Edge (TE) of the VG. (**a**) RANS and (**b**) LES.

With RANS, nearly equal locations of the maximums are obtained with both models. Considering the values, very similar values are obtained with both models, but the biggest deviations between models appear when H = 0.2 δ and H = 0.4 δ. With LES, larger discrepancies between models are visible regarding the locations of the maximums, since the cell-set predicts the maximum closer to the VG. The values of the maximums show that the cell-set underpredicts these values for the taller VGs (H = 0.8 δ and H = 1 δ) and overpredicts the values for the lower VGs (H = 0.2 δ and H = 0.4 δ). Far away from the VG, the cell-set model underpredicts the wall shear stress value for all the cases, except for H = 0.2 δ.

The differences visible on the lower VGs for the LES case are attributed to the fact that these VGs are located on the buffer layer region, where the viscous effects are dominant and the flow is strongly turbulent. In this region, the cell-set seems not to be able to provide accurate predictions of both the viscous and turbulent shear stresses.

#### **4. Conclusions**

Numerical simulations of 10 different SBVGs on a flat plate in a negligible streamwise pressure gradient flow conditions were conducted using the fully resolved mesh model and the cell-set model with RANS and LES turbulence models, with the objective of analyzing the accuracy of the cell-set model.

The meshes generated with the fully mesh model are made of around 11.5 million cells, while the meshes generated with the cell-set model are composed of around 7.2 million cells. This fact has resulted in savings of around the 40% in terms of computational time.

This study is mainly focused on analyzing the vortexes generated on the wake behind the VG. Therefore, the vortex structure regimes on the wake behind the VG; the path, size, and strength of the primary vortex; and the wall shear stress behind it have been studied. The results demonstrate that the cell-set model is able to predict the vortexes generated on the wake behind the VG. Regarding the primary vortex, nearly equal values of its path and fairly accurate predictions of its size have been obtained. The vortex size and strength show that the cell-set models overpredict the vorticity of the core of the primary vortex, but underpredicts its size, especially with LES. This is reflected in the large differences that appear in the R05, but close values obtained in Γ and wall shear stress.

The major agreements between models appear in the higher VGs, and the biggest disparities appear in the lower ones. This is attributed to the location of the VGs on the boundary layer, since the lower VGs (H = 0.2 δ) are located on the buffer layer and the higher ones (H = 0.8 δ and H = 1 δ) on the outer region. These discrepancies are more notable in LES.

In conclusion, it has been demonstrated that the cell-set model is suitable for RANS turbulence modelling with all the tested SBVGs. With LES, it is adequate for VGs whose height is around the boundary layer, but for lower VGs, the differences with the fully resolved mesh model are significant. Hence, the cell-set model presented in the current work seems to be not very accurate for vane heights within the buffer layer.

Since the cell-set model represents a great advantage in terms of computational and meshing time savings, additional research is proposed, applying the studied meshing model on VGs with different conditions and geometries, or using it for generating other devices. Furthermore, more investigations should be done in order to improve the accuracy of the cell-set modelled geometries with heights within the buffer layer.

**Author Contributions:** K.P.-P., U.F.-G. and I.A. wrote the paper. K.P.-P. and U.F.-G. prepared the numerical simulations and D.T.-F.-B. validated them. E.Z. provided effectual guidelines to prepare the manuscript. All authors have read and agreed to the published version of the manuscript.

**Funding:** The authors are thankful to the government of the Basque Country and the University of the Basque Country UPV/EHU for the ELKARTEK20/78 and EHU12/26 research programs, respectively.

**Institutional Review Board Statement:** Not applicable.

**Informed Consent Statement:** Informed consent was obtained from all subjects involved in the study.

**Data Availability Statement:** The data presented in this study are available on request from the corresponding author.

**Acknowledgments:** The authors thank for technical and human support provided by SGIker (UPV/EHU/ERDF, EU). This research has been developed under the framework of the Joint Research Laboratory on Offshore Renewable Energy (JRL-ORE).

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Nomenclature**

#### **Definition**




#### **References**


### *Article* **Investigation on Dynamic Stresses of Pump-Turbine Runner during Start Up in Turbine Mode**

**Funan Chen, Huili Bi, Soo-Hwang Ahn , Zhongyu Mao, Yongyao Luo and Zhengwei Wang \***

State Key Laboratory of Hydroscience and Engineering & Department of Energy and Power Engineering, Tsinghua University, Beijing 100084, China; cfn18@mails.tsinghua.edu.cn (F.C.); bihuili2014@mail.tsinghua.edu.cn (H.B.); shahn@mail.tsinghua.edu.cn (S.-H.A.); maozy14@mails.tsinghua.edu.cn (Z.M.); luoyy@tsinghua.edu.cn (Y.L.)

**\*** Correspondence: wzw@mail.tsinghua.edu.cn

**Abstract:** The startup process occurs frequently for pumped storage units. During this process, the rotating rate that changes rapidly and unsteady flow in runner cause the complex dynamic response of runner, sometimes even resonance. The sharp rise of stress and the large-amplitude dynamic stresses of runner will greatly shorten the fatigue life. Thus, the study of start-up process in turbine mode is critical to the safety operation. This paper introduced a method of coupling one dimensional (1D) pipeline calculation and three-dimensional computational dynamics (3D CFD) simulation to analyze transient unsteady flow in units and to obtain more accurate and reliable dynamic stresses results during start up process. According to the results, stress of the ring near fixed support increased quickly as rotating rate rose and became larger than at fillets of leading edge and band in the later stages of start-up. In addition, it was found that dynamic response can be caused by rotor stator interaction (RSI), but also could even be generated by the severe pressure fluctuation in clearance, which can also be a leading factor of dynamic stresses. This study will facilitate further estimation of dynamic stresses in complex flow and changing rotating rate cases, as well as fatigue analysis of runner during transient operation.

**Keywords:** pump-turbine; dynamic stress; start-up process; pressure fluctuation; clearance

#### **1. Introduction**

Pumped storage units have great significance to the power grid. Recent years have witnessed the development of new renewable energy sources such as wind and solar. However, both wind and solar are not stable and continuous, causing large oscillation for the load of electrical power grid. Therefore, pumped storage units are required to absorb extra electric energy generated by wind or sun, maintaining the safety and stability of power grid. In addition, pumped storage units can also help solving the problem of frequency modulation, phase modulation as well as peak regulation for their effective storage and flexible switch between turbine mode and pump mode [1]. As the critical component of pumped storage unit, the pump turbine runner may suffer from dynamic stresses, and sometimes cracks at the location of stress concentration. Damages have been reported by many researchers [2–4] and may cause a great loss to power station.

The complex and unstable internal flow is one of the main causes of dynamic stresses. Rotor-stator interaction (RSI) is one of the most common phenomena in hydraulic units and has been studied for many years [1,5,6]. For a runner with low specific speed, it is the main reason of dynamic stresses at full load conditions [7]. When working at part load, the vortex rope in draft tube also affects the dynamic stresses of runner. The rate of damage caused by dynamic stresses becomes larger as the load decreases, and at part load it can be 100 times higher than at best efficiency point (BEP) [8]. At some working conditions, the Von-Karman vortex shedding induces the vibration of blades [9]. The S-shaped region of pump turbine has been studied widely and deep understanding is still needed because

**Citation:** Chen, F.; Bi, H.; Ahn, S.-H.; Mao, Z.; Luo, Y.; Wang, Z. Investigation on Dynamic Stresses of Pump-Turbine Runner during Start Up in Turbine Mode. *Processes* **2021**, *9*, 499. https://doi.org/10.3390/ pr9030499

Academic Editors: Krzysztof Rogowski and Jin-Hyuk Kim

Received: 14 January 2021 Accepted: 8 March 2021 Published: 10 March 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

the flow structure is very complicated. When runner is working in the S-shaped region, the greater static stress and dynamic stress amplitudes can result in earlier occurrence of cracks and fatigue failures. Moreover, the stochastic hydraulic loads tend appear in the S-shaped region, especially at no-load condition [10]. C Mende et al. [11] and JF Morissette et al. [12] suggested that Large Eddy Simulation (LES) turbulence model is a better choice to predict the stochastic pressure fluctuations, and low-frequency events can be captured by one-way fluid structure interaction (FSI) simulation method.

Dynamic stresses in transient processes can lead to more damage to runner than normal working conditions because the hydraulic loads and performance characteristics change rapidly. Many researches focused on the operating mechanism of pump turbine and studied the unstable behavior during transient processes. Rotating stall has been studied both in turbine mode [13,14] and in pump mode [15]. Rotating stall was observed in a reduced scale model at runaway and became more obvious when discharge decreased [16]. The flow separations in several neighboring runner channels caused a stall cell, and backflow and vortices were induced. Several studies [17–21] indicated the vortex appearing in runner and vaneless space is the main reason of dynamic instability in transient process. The vortex varies with time, enhances the pressure fluctuations, and causes some low-frequency components in pressure fluctuations. In addition, Li et al. [22] observed a ring-shaped flow enlaced the vaneless space and blocked the flow during start up in turbine mode. Zuo et al. [23] summarized the stability criteria of the overall system which can evaluate the unstable characteristics of pump-turbine. These unstable behaviors affect the dynamic stresses of runner. The measurements on runner [24] suggested that the static stress and the amplitude of dynamic stress during start-stop are both greater than at normal operating conditions and can cause severe damage to runner.

As described above, the research on dynamic stresses and its influencing factors mainly focused on the normal working conditions. Various studies have discussed the hydraulic excitation and its unsteady and complex characteristics in transient process. However, only a few papers have dealt with its influence on dynamic stresses of runner, especially in the transient process. Furthermore, other factors such as rotating rate and flow in clearance were rarely mentioned.

In this paper, the dynamic stresses of a pump-turbine runner during start up are analyzed using FSI method. The hydraulic loads during start up are obtained from computational fluid dynamics (CFD) simulation, with one dimensional (1D) pipeline calculation providing the boundary conditions. The paper initially discusses the effects of rotating rate, torque of runner, and the axial force. Then, the dynamic stresses are analyzed not only from viewpoint of the RSI but also under angle of the severe pressure fluctuation in clearance. This study can provide a better understanding to the dynamic response of runner under complex external excitation.

#### **2. Numerical Method**

#### *2.1. Sturctural Governing Equations*

The dynamic response of structure can be solved using finite element method (FEM). The matrix formulation of the governing equations can be expressed as

$$\left[\mathbf{M}\right]\left\{\ddot{\boldsymbol{u}}\right\} + \left[\mathbf{C}\right]\left\{\dot{\boldsymbol{u}}\right\} + \left[\mathbf{K}\right]\left\{\mathbf{u}\right\} = \left\{F\_{\mathbf{s}}\right\} \tag{1}$$

where [M], [C], and [K] represent for structure mass matrix, damping matrix and stiffness matrix, respectively, {*Fs*} is the load vector and {u} is the displacement vector.

Normally, the Von-Mises equivalent stress *σequ* is used to evaluate the stress characteristics of runner. It can be expressed as

$$
\sigma\_{equ} = \sqrt{\frac{1}{2} [(\sigma\_1 - \sigma\_2)^2 + (\sigma\_2 - \sigma\_3)^2 + (\sigma\_3 - \sigma\_1)^2]} \tag{2}
$$

where *σ*1, *σ*2, and *σ*<sup>3</sup> represent for first, second and third principal stress, respectively.

#### *2.2. 1D Pipeline Governing Equations*

The flow in pipeline can be simplified into one dimensional flow and solved by method of characteristics (MOC). The continuity equation and momentum equation are

$$V\frac{\partial \mathbf{H}}{\partial \mathbf{x}} + \frac{\partial \mathbf{H}}{\partial t} - V\sin\alpha + \frac{a^2}{g}\frac{\partial \mathbf{V}}{\partial \mathbf{x}} = \mathbf{0} \tag{3}$$

$$
\delta g \frac{\partial \mathbf{H}}{\partial \mathbf{x}} + V \frac{\partial \mathbf{V}}{\partial \mathbf{x}} + \frac{\partial \mathbf{V}}{\partial t} + \frac{fV|V|}{2D} = \mathbf{0} \tag{4}
$$

where V is the average velocity at cross section, H is piezometric head, *α* is the angle between center line of pipe and horizontal line. *a* is wave speed, *g* is gravity acceleration, *f* is Darcy–Weisbach friction factor, *D* is the pipe diameter.

Other components in hydraulic system such as surge tank and pipe with branches can also be simplified and solved.

#### *2.3. CFD Governing Equations and Turbulence Model*

The flow in the unit is assumed as three-dimensional incompressible unsteady flow. According to the Reynolds averaged theory, the governing equations are described as follows:

$$\frac{\partial \overline{u\_i}}{\partial x\_i} = 0 \tag{5}$$

$$\frac{\partial \overline{u\_i}}{\partial t} + \overline{u\_j} \frac{\partial \overline{u\_i}}{\partial \mathbf{x}\_j} = F\_i - \frac{1}{\rho} \frac{\partial \overline{p}}{\partial \mathbf{x}\_i} + \nu \frac{\partial^2 \overline{u\_i}}{\partial \mathbf{x}\_i \partial \mathbf{x}\_j} - \frac{\partial}{\partial \mathbf{x}\_j} \left( \overline{u\_i'} \overline{u\_j'} \right) \tag{6}$$

where u is velocity, p is pressure, F is body force, *ρ* is density, and *ν* is kinematic viscosity. Turbulence model is needed to close the equations above. In this paper, the Shear-Stress Transport (SST) k-ω model is used to calculate the turbulence in pump-turbine.

#### **3. Calculation Model and Boundary Conditions**

*3.1. The Pump-Turbine Runner*

#### 3.1.1. The Finite Element Model

The runner has 5 main blades and 5 splitter blades with the inlet diameter of 4.3 m and outlet diameter of 2.125 m. The runner is made of stainless steel. The Young's modulus is 2.1 <sup>×</sup> <sup>10</sup><sup>11</sup> Pa, Poisson's ratio is 0.3 and density is 7850 kg/m<sup>3</sup> .

The finite element model of runner is shown in Figure 1. Most of the meshes are hexahedral and in regions of low stress gradients, some wedges are used. Refinements are made at the stress contribution regions, as shown in Figure 1.

**Figure 1.** Finite element model of runner (R1 is the node at the ring near fixed support; R2 is the node at the fillet of leading edge and crown; R3 is the node at the fillet of leading edge and band).

#### 3.1.2. Mesh Independency Check

The calculation grids were checked with gravity and centrifugal force acting on the runner. The results shown in Figure 2 indicate that the grid with 305,505 nodes is enough for this calculation. This mesh was used in the following analysis.

**Figure 2.** Mesh independency analysis.

It is worth noting that besides the fillets of leading edge, a ring near fixed support is also the stress concentration area and suffers from higher stress than other parts. On one hand, the centrifugal force of whole runner results in a bending moment acting on the ring. On the other hand, the geometry changes suddenly at the corner of ring without any fillets for transition and, thus, concentrates the stress sharply. Stress singularity appears at the nodes closest to the corner. Fillets with 5–20 mm radius can help reduce the stress singularity but cannot eliminate it. Thus, the results of nodes closest to the corner were ignored. Node with the convergence stress (node R1 in Figure 1) was chosen in mesh independency check and in the following analysis. ‐

‐

#### 3.1.3. Boundary Conditions

Fixed support is defined at area where bolts connect the shaft and runner. The loads of runner include gravity acceleration, centrifugal force and hydraulic loads. The rotating rate is changed over time during start-up process. Therefore, the centrifugal force is different at different time. The hydraulic loads on both inner surface and outer surface can be obtained from CFD simulation, as shown in Figure 3. In traditional FSI simulation, only loads on inner surface are considered. However, the loads on outer surface also have a great influence on the stress-state of runner [25] and were considered in this paper. ‐ ‐ ‐ ‐ ‐ ‐

**Figure 3.** The fluid structure interaction (FSI) interface.

#### *3.2. The Hydraulic System of Pump Storage Station*

‐ ‐ The considered hydraulic system consists of reservoirs, surge tanks, tunnels, pipelines, pump turbine units, and valves. The diagram of the hydraulic system is shown in Figure 4. The layout of three units with one diversion tunnel is adopted. The total length of the pipeline is more than 3.6 km. Surge tanks are placed at the upstream and downstream to reduce the rapid change of pressure caused by water hammer. ‐ ‐

**Figure 4.** The diagram of the hydraulic system.

In this paper, the start-up process of 1# unit is the major concern. The other 2 units operate at normal condition and suffer small fluctuations induced by the start-up of 1# unit. The water level is 762.1 m at upstream reservoir and 98.0 m at downstream reservoir and assumed to remain constant during start up process. The guide vane opens with the rate of

0.48 degrees per second until the rotating rate reaches rated value, then speed controller begins to work and controls the guide vane opening angle.

‐

‐

‐

‐

‐

#### *3.3. Pump-Turbine Unit ‐*

The internal flow of casing, stay vane, guide vane, runner, and draft tube can be simulated as three-dimensional (3D) turbulent flow. The unit is shown in Figure 5. In order to provide complete hydraulic loads of runner, the labyrinth seals and clearances around runner are also considered. The rated head of the unit is 653 m. There are 16 guide vanes and the maximum opening degree is 24◦ . ‐

‐ ‐ **Figure 5.** The pump-turbine unit (**a**) pump-turbine unit; (**b**) runner (blue) and clearances (green).

‐ The flow domain was discretized by tetrahedral mesh and hexahedral mesh. The total number of nodes is 4,643,402 and the number of elements is 9,737,666. The domain of runner has 1,171,402 nodes and the clearance has 1,771,714 nodes. In the region of high stress gradient, the size of mesh cells in CFD analysis is similar to that in FEM analysis. The mesh is shown in Figure 6.

 െ The internal flow of the pump-turbine unit at typical time points was calculated, as shown in Table 1. Figure 7 shows the boundary conditions of CFD method. In this paper, the relative pressure coefficient *C<sup>p</sup>* is defined as

$$\mathcal{C}\_p = \frac{p - P\_{ref}}{\rho gH} \tag{7}$$

‐ ‐ ‐ ‐ where *p* is pressure, *Pre f* is the pressure at the end of downstream pipeline, *H* is the rated head. In Figure 7, Pin is total pressure coefficient at casing inlet, and Pout is static pressure coefficient at draft tube. These are calculated though 1D MOC and used as inlet and outlet boundary conditions of 3D CFD. All walls are set as no-slip walls. The domain of runner and clearances are rotating domains. The model of interface between rotating domain and stationary domain is set as transient rotor-stator to simulate the RSI phenomenon. The unsteady calculation is conducted with steady simulation result as initial guess. The number of timesteps is 300 in each revolution. In addition, the pressure-based solver is used in this study. Second-order accuracy is used for the pressure equation and second-order upwind discretization for other convection-diffusion equations.

‐ ‐

‐

**Figure 6.** Mesh of the flow domain (**a**) the whole flow domain; (**b**) runner; (**c**) clearance between runner and head cover; (**d**) clearance between runner and bottom ring.

**Table 1.** Time points.


**Figure 7.** The inlet and outlet boundary conditions.

#### *3.4. The Structure-Fluid Coupling Model*

In this study, the influence of 3D flow on the dynamic response of runner is analyzed by one-way FSI simulation method, which is calculated using a coupling of Fluent and ANSYS Mechanical. The coupling process is as follows.

First, the Fluent simulation is conducted. The hydraulic loads at each step are obtained. Second, the data transfer is performed manually. Pressure from the cell zones of Fluent simulation can be mapped onto locations associated with the ANSYS Mechanical mesh by using an interpolation method provided by ANSYS (ANSYS, Inc., Pittsburgh, PA, USA). Many FSI simulations require strict match at the interface of CFD grid and structural grid, which increases the complexity of meshing, and may cause a too fine mesh in modeling the dynamic stresses of runner. The interpolation method effectively avoids this problem.

Third, the ANSYS Mechanical simulation is performed, and the timestep is the same with CFD calculation.

#### **4. Results and Discussion**

#### *4.1. The Variation of Performance Characteristics*

The energy characteristics such as discharge and power change rapidly during start-up process. Meanwhile, the pressure wave as a result of the operating condition change of unit travels through pipeline, and this travel in turn affects the operating condition change of unit. Through 1D MOC, this complex process can be simulated. However, in this paper, the pressure wave is not the key point and is not discussed here.

3D simulation was conducted based on the result of 1D MOC at typical time points. Total pressure and static pressure are set as inlet and outlet boundary condition respectively, so head is a given quantity. Discharge and torque on blades of 1# unit are calculated by 3D simulation and the verification is shown in Figure 8. The guide vane opening is also plotted here. The discharge, torque and guide vane opening are expressed as relative values: Q/*Qn*, T/*T<sup>n</sup>* and A/*Amax*, where *Q<sup>n</sup>* and *T<sup>n</sup>* are rated discharge and torque, *Amax* is the maximum guide vane opening. The calculation of 1D MOC are based on model test, therefore the consistency of 3D CFD results and 1D MOC results in Figure 8 indicates that the accuracy of 3D CFD is enough for this study.

‐ **Figure 8.** The variation of torque and discharge during start-up process.

The relative rotating rate is plotted in Figure 9, where N is the rated rotating rate. The start-up process in turbine mode can be divided into three stages. In the first stage, guide vane opens at preset speed. As a consequence of increasing water flow, torque on the blades increases. The increasing torque accelerates the rotation of runner, raising the 64

‐

‐

‐

rotating rate is maintained at rated value. At 25 s, the torque almost drops to zero. In third stage, the unit reaches speed-no-load condition and stabilizes in this condition. ‐

**Figure 9.** The variation of rotating rate (n/N).

‐ ‐ ‐ In steady state CFD calculation, the flow in runner is modelled with Moving Reference Frame (MRF), and the phenomenon of RSI cannot be considered. Therefore, the static stress calculation at each point is not enough to reflect the true stress of runner. In this paper, unsteady simulation was conducted to model the flow in a whole rotation cycle. The dynamic stresses of runner were calculated using FSI method, which encounter for their temporal changes as the relative position of runner and guide vanes changing. Then the mean value is defined to describe the stress at each time point. It can be called as mean stress and expressed as

$$\overline{\sigma}\_{eq\mu} = \frac{1}{T} \int\_{t=0}^{T} \sigma\_{eq\mu} dt \tag{8}$$

where *T* is the time for a whole rotation cycle of each time point.

#### *4.2. Mean Stresses of Runner*

The stress characteristics of pump-turbine runner were obtained by FEM simulation. Two different types of stress distribution can be observed, as shown in Figure 10. In the first stage of start-up process, the fillets of leading edge and band suffered the maximum stress, as shown Figure 10a. There was no stress concentration appearing in other parts of runner. Among time points 1–6, the maximum stress at the concentration region was 245.7 MPa at TP3, the stress of other parts was less than 78 MPa. In the last two stages of start-up process, the ring near fixed support was the region of maximum stress, as shown in Figure 10b. The fillets of leading edge and band suffered low stress less than 55 MPa.

Further observation indicates that in the last two stages of start-up process, stress concentration also appeared at the fillets of leading edge and crown. For further explanation of the stress characteristics during start-up process, five nodes were selected in the high stress regions and marked as S1–S5, as shown in Figure 11. S2 and S3 locate at splitter blade while S4 and S5 locate at the main blade.

‐ **Figure 10.** Stress distribution at start-up process (**a**) TP3; (**b**) TP9.

‐

‐

‐

The mean stress of S1–S5 during start-up process is plotted in Figure 12. In order to make the influence of hydraulic loads explicit, the FEM analysis considering only hydraulic loads was performed and the mean stress is also shown in Figure 12. The stress at rated working condition was calculated, and marked as grey dotted lines.

‐ **Figure 12.** The change of mean stresses in start-up process (**a**) S1; (**b**) S2 and S4; (**c**) S3 and S5.

‐ As indicated in Figure 12, for S1, S2, and S4, the high stress in the last two stages of start-up process was mainly caused by centrifugal force. The stress is slightly higher than the value under rated working condition. Meanwhile, the hydraulic loads lead to the high stress of S3 and S5 in the first stage. The maximum stress of S5 at TP3 can be 3.56 times of rated working condition.

‐

‐

‐ ‐ ‐ During start-up process, the rotating rate rises quickly in the first stage, and later the growth rate is under control, the value is near the rated value. Thus, centrifugal force contributes to a rapid rise of stress in first stage and the stable high stress in the last two stages. In addition to large centrifugal force, high rotating rate also leads to flow instabilities [26,27], which is another factor causing the high stress. There is circumferential velocity gradient between upper wall and lower wall of clearance, as shown in Figure 13. As rotating rate rises, velocity gradient increases; thus, the shear stress becomes larger, leading to the high stress of runner.

**Figure 13.** The velocity gradient in clearance.

Due to the shape of the runner, the regions with sudden change of geometry such as S1–S5 can be easily influenced by centrifugal force. In addition, the fillets of trailing edge and crown\band are also high stress regions though these regions are not discussed in

௪ ௗ

௪ ௗ

௪ 

ௗ 

௪ ௗ

௪ <sup>∗</sup> ൌ

ௗ <sup>∗</sup> ൌ ௪

ௗ

௪ ௗ

detail in this paper. Other parts of runner, for instance, the middle parts of blades, suffer low stress in the whole process and are hardly affected by centrifugal force.

From Figure 12b, more information can be found that the mean stress of S2 was larger than S4. Considering the fact that the size of elements near S2 is similar to that near S4, a reasonable explanation is the geometry difference of main blade and splitter blade caused the difference of mean stress. The leading edges of the two blades are almost the same. However, the splitter blade is more curved than main blade, as shown in Figure 14. The centrifugal force of blade causes the bending moment on the fillet of blade and crown, which is one of the reasons for the stress of S2 and S4. The more curved blade leads to the lager moment and larger mean stress.

**Figure 14.** The comparison of geometry between main blade and splitter blade.

௪ ௗ For all the five nodes, the mean stress caused by hydraulic loads followed a similar law: increase and reach the maximal value in the first stage and then decrease. In this paper, the hydraulic loads on runner can be simplified as two axial forces (*Fcrown* and *Fband*) and a torque on blades (*T*). It is the superposition of axial hydraulic forces and hydraulic torque on the blade that leads to this law.

௪ ௗ Figure 15 provides the relative value of *Fcrown* and *Fband*, which are defined as

$$F\_{crown}^{\*} = \frac{F\_{crown}}{m\_r g} \tag{9}$$

$$F\_{band}^{\*} = \frac{F\_{band}}{m\_r g} \tag{10}$$

‐ ‐

‐

‐

‐

௪ ௗ ௪ ௗ ௪ ௗ where *m<sup>r</sup>* is the mass of all the rotating components. According to the regulations, the downward axial force is defined as positive. At TP1–6, *Fcrown* and *Fband* drag crown and band away from each other. At TP7, *Fcrown* and *Fband* both drop to near zero. AT TP8 and TP9, *Fcrown* and *Fband* change direction and begin to push crown and band to each other. The stress of runner decreases to the minimum value at TP7 and then increases under the influence of axial forces.

**Figure 15.** Axial forces of runner.

‐

The variation of *T* can be found in Figure 8 as relative value *T*/*Tn*. At TP3–6, the value of T is higher than other time points, making the stress of runner higher. At TP7–9, T is close to 0, and the stress of runner also decreases.

‐

‐ ‐

The axial force and the torque both have great influence on the mean stress of runner. They are loaded together on the runner, causing the higher stress at TP3–4 and the lower stress at TP7–9.

However, compared to centrifugal force, the hydraulic loads effected only S3 and S5, as shown in Figure 12. The maximum stress caused by hydraulic loads of S1, S2, and S4 was less than 35 MPa, while that of S3 and S5 was as high as 236 MPa. First, the discharge is quite small in start-up process, so the flow direction is different from blade angle. When the water flows into runner, it impacts on the pressure side of blade, causing a high-pressure region at the impact point, as shown in Figure 16. The pressure distribution shows the pressure difference mainly affects the inlet area of blade. Therefore, S3 and S5 are easier to suffer large stress. Second, the angle between leading edge and axis is 32.9 degree for main blade and 32.6 degree for splitter blade. Compared with other pump-turbine runner shown in Figure 17, the runner in this paper has a more leaning leading edge. As shown in the sketch map, this leaning leading edge contributes to the gentle transition to crown and the steep transition to band. When hydraulic loads act on the runner, S3 concentrates stress more quickly than S2, as do S5 and S4. ‐ ‐ ‐ ‐ ‐ ‐

**Figure 16.** Pressure distribution and streamlines in the middle section of runner (Cp).

**Figure 17.** The leaning leading edge of runner studied in this paper.

‐

At most time points, there was little difference between the pressure distributions in each passage of runner. Therefore, the mean stresses of S3 and S5 were almost the same. At TP3, the pressure distributions of two neighboring passages were different from each other, which can be seen in Figure 16. That is the reason why the mean stress of S5 was larger than of S3 at TP3.

#### *4.3. The Amplitudes and Frequency Components of Dynamic Stresses*

At each time point, the stress of runner will change as the relative position of runner and guide vanes changes, also known as RSI. The pressure fluctuations induced by RSI are the main reason of dynamic stresses of runner. In this section, the variation of amplitudes and frequencies of dynamic stresses during start-up process will be discussed. ‐ ‐

Figure 18 is the frequency domain diagram of dynamic stresses at TP6. The variable of horizontal axis is the ratio of frequency and rotating frequency *fn*. As can be seen from Figure 18, the amplitudes of S3 and S5 were far lager that of S1, S2, and S4. This is consistent with the previous analysis that stress of S3 and S5 were mainly affected by hydraulic loads while S1, S2, and S4 were by centrifugal force. ‐ ‐

**Figure 18.** Frequency domain diagram of dynamic stresses at TP6.

Two points in flow domain were selected to reflect the pressure fluctuation. The point in runner was named P1 and the point in clearance was P2, as shown in Figure 19. Figure 20 is the frequency domain diagram of relative pressure coefficient at TP6. The main frequency was 16 *fn*, usually called as vane passing frequency (VPF). The pressure fluctuations also included low frequency components (1–4 *fn*), which were induced by the irregular flow in runner with small discharge. Under the effect of pressure fluctuation, the main frequency of dynamic stresses was also VPF. The low frequency components also existed in dynamic stresses, as shown in Figure 18.

The dynamic stresses at other time points were also investigated. The peak-to-peak value during start-up process is shown in Figure 21. In first stage, though the discharge and rotating rate were increasing, the peak-to-peak value did not show a significant growth trend and stabilized about 20 MPa. At TP7, the value increased and reached 50 MPa. Later on, it dropped back to about 20 MPa. Compared with the normal condition, peak-to-peak value in start-up process was far larger and may cause fatigue crack after a few times.

**Figure 19.** The pressure fluctuation measure points (P1 is the pressure fluctuation recording point in runner; P2 is the pressure fluctuation recording point in clearance).

‐

‐

‐

‐

‐

‐

‐ ‐

‐

‐

‐ ‐

**Figure 20.** Frequency domain diagram of pressure coefficient at TP6. (**a**) P1; (**b**) P2.

‐ ‐ **Figure 21.** The peak-to-peak value of dynamic stress.

‐ ‐

‐ ‐ Figure 22 shows the amplitudes of 1/4 VPF and VPF in start-up process. At TP1, the pressure fluctuation in runner was mainly caused by RSI, thus VPF was the main

‐ ‐

frequency of dynamic stress while the amplitude of 1/4 VPF was almost zero. Later as the discharge and torque of runner increased, the amplitude of VPF rose slightly. The irregular flow in runner also became violent and led to an amplitude growth of 1/4 VPF. In second and third stage, the torque and discharge began to drop, but the influence of RSI continued, so the amplitude of VPF did not decrease. Moreover, there was a sudden rise of 1/4 VPF at TP7, and the amplitude fell rapidly at TP8. That was the reason for the maximum peak-to-peak value at TP7 in Figure 21. ‐ ‐ ‐ ‐

‐

‐

‐

‐

‐

**Figure 22.** The dynamic stress amplitude of 1/4 VPF and VPF. (**a**) S3; (**b**) S5.

The modal analysis was performed to tell whether the sudden rise of 1/4 VPF was caused by resonance. The natural frequency of first mode is 95.95 Hz and the mode shape is shown in Figure 23. There is a nodal diameter in this mode shape, so it is usually marked as 1ND [28]. This is a common mode shape for most runners and other structure similar with the disc [29,30]. The rotating rate at TP7 is 489.24 rpm, and the value of 1/4 VPF is 32.62 Hz, far from 95.95 Hz. Therefore, the steeply increase of dynamic stress at TP7 is not the contribution of resonance.

**Figure 23.** The mode shape of runner. (**a**) front view; (**b**) top view.

‐ ‐ Then the effect of pressure fluctuation is taken into consideration. The amplitudes of two specific frequencies, 1/4 VPF and VPF at all time points were obtained and shown in Figure 24. For P1, VPF was the main frequency at most time points, as shown in Figure 24a. The pressure fluctuation induced by RSI and the vortex flow were violent in guide vane and runner. When it spread to clearances, the amplitude decreased. Thus, in most cases, the amplitude of P2 was far smaller than P1, as shown in Figure 24b. However, at TP7, the amplitude of 1/4 VPF was much greater than other time points. Considering the high-speed rotating flow in clearances and the approximately axial symmetry of clearances,

the amplitude of pressure fluctuation is similar in the circumferential direction. When the strength of pressure fluctuation in clearances is enough, it can have a great influence on the dynamic stress of runner. At other time points, the strength of pressure fluctuation in clearance is low, the dynamic stress is mainly affected by the pressure fluctuation in runner. ‐ ‐

‐ ‐

**Figure 24.** The pressure fluctuation amplitude at 1/4 VPF and VPF. (**a**) P1; (**b**) P2.

‐ The low frequency component such as 1/4 VPF in clearance may come from the vortex generation and shedding process or the stochastic events as mentioned in Ref. [12]. The reasons of the sudden increase of 1/4 VPF pressure fluctuation will be discussed in further work.

#### **5. Conclusions**

The dynamic stresses of pump-turbine runner during start-up process in turbine mode were calculated in this paper. The coupling of 1D pipeline and 3D pump-turbine unit was conducted to obtain the performance characteristics and internal flow characteristics of the unit during the transient process. The dynamic stresses of runner were simulated using one-way FSI method. The influence of both inner surface and outer surface was taken into consideration in the interaction of fluid and structure. The conclusions are as follows:

(1) The start-up process was divided into three stages in this paper. In the first stage the discharge and hydraulic torque rise up, the runner is accelerated. In the second stage, rotating rate reaches the rated value, the guide vane begins to close, and the hydraulic torque of blades decreases gradually to zero. Finally, in the third stage, the unit stabilizes in speed-no-load condition.

(2) In the first stage of start-up, the maximum stress could be generated at the fillets of leading edge and band, and can reach 3.56 times of rated working condition. It was mainly induced by the increasing torque on blades and the large axial forces of crown and band. Moreover, as rotating rate rise, the centrifugal force and fluid shear stress in clearance increases. As a result, stress of the ring near fixed support quickly increased in first stage and was finally maximized in contrast with other parts of runner in the second and third stage.

(3) The amplitude of dynamic stresses could be maximized at the fillets of leading edge and band. In most of time during start-up, the dynamic stress was mainly characterized by VPF due to the RSI, which was the determining factor causing pressure fluctuation. However, the severe pressure fluctuation in clearance was found in the second stage with the main frequency of 1/4 VPF. It can also be a leading factor of dynamic stresses in a short

time. Therefore, the pressure fluctuation in clearance should be taken into consideration in the stage of runner design.

In this paper, the added mass and transient integral effect were not taken into consideration. Their influence on the dynamic stresses in start-up process will be studied in further work.

**Author Contributions:** Methodology, Z.W.; investigation, F.C.; validation, H.B. writing—original draft preparation, F.C.; writing—review and editing, S.-H.A., Z.M., and Y.L.; funding acquisition, Z.W. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by National Key R&D Program of China, grant number 2016YFC0401905 and National Natural Science Foundation of China, grant number 51909131.

**Institutional Review Board Statement:** Not applicable.

**Informed Consent Statement:** Not applicable.

**Data Availability Statement:** Not applicable.

**Acknowledgments:** Special thanks are due to the Construction and Management Branch of CSG Power Generation Co. Ltd.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


### *Article* **Optimization of a Wavy Microchannel Heat Sink with Grooves**

**Min-Cheol Park, Sang-Bum Ma and Kwang-Yong Kim \***

Department of Mechanical Engineering, Inha University, Incheon 22212, Korea; pjch0825@naver.com (M.-C.P.); sbma@kitech.re.kr (S.-B.M.)

**\*** Correspondence: kykim@inha.ac.kr; Tel.: +82-32-860-7317

**Abstract:** In this study, a wavy microchannel heat sink with grooves using water as the working fluid is proposed for application to cooling microprocessors. The geometry of the heat sink was optimized to improve heat transfer and pressure loss simultaneously. To achieve optimization goals, the average friction factor and thermal resistance were used as the objective functions. Three dimensionless parameters were selected as design variables: the distance between staggered grooves, groove width, and groove depth. A modified Latin hypercube sampling (LHS) method that combines the advantages of conventional LHS and a three-level full factorial method is also proposed. Response surface approximation was used to construct surrogate models, and Pareto-optimal solutions were obtained with a multi-objective genetic algorithm. The modified LHS was proven to have better performance than the conventional LHS and full factorial methods in the present optimization problem. A representative optimal design showed that both the thermal resistance and friction factor improved by 1.55% and 3.00%, compared to a reference design, respectively.

**Keywords:** microchannel heat sink; wavy microchannel; groove; heat transfer performance; laminar flow; multi-objective optimization; LHS; full factorial methods

**Citation:** Park, M.-C.; Ma, S.-B.; Kim, K.-Y. Optimization of a Wavy Microchannel Heat Sink with Grooves. *Processes* **2021**, *9*, 373. https://doi.org/10.3390/pr9020373

Academic Editor: Fabrizio Scala

Received: 16 January 2021 Accepted: 15 February 2021 Published: 18 February 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

#### **1. Introduction**

Microprocessors generate high heat flux and thermally interact with their surroundings. Because they are composed of many integrated components, their efficiency and performance are significantly influenced by temperature. The temperature must be kept between 363 K and 383 K to maintain the best performance [1]. Therefore, it is essential to develop an effective cooling system to maintain a proper temperature even with high heat generation.

Cooling systems are being made less noisy and smaller, and it is estimated that heat sinks capable of cooling at more than 1000 W/cm<sup>2</sup> will be required in the near future [2]. Both air and water can be used for cooling systems, but as the heat generation increases with the development of microprocessors, air cooling systems have a limitation in maintaining effective cooling performance [1]. In addition, to increase air-cooling performance, the fan speed must be increased, which increases noise.

Water-cooling microchannel heat sinks have been widely used to reduce noise and meet increased requirements for cooling. Numerical and experimental studies on these heat sinks have been actively conducted. Tuckerman and Pease [3] experimented with a microchannel heat sink consisting of straight channels with heat flux of 790 W/cm<sup>2</sup> using water as a coolant. They confirmed that the water had great heat transfer characteristics. Wang et al. [4] carried out experiments and numerical analyses on a microchannel heat sink consisting of straight channels with ribs and grooves. They found that secondary flows occurring behind the ribs and grooves prevented the formation of the thermal boundary layer and promoted fluid mixing and heat transfer.

Ansari et al. [5] and Farhanieh et al. [6] investigated the cooling performance of straight microchannels with grooves. They found that the interfacial area of heat transfer is increased by the grooves, thereby increasing the cooling performance. Ansari et al. [5] suggested that high local Nusselt numbers are obtained near the upstream and downstream regions of the groove structures. Farhanieh et al. [6] confirmed that although the heat transfer performance was low due to recirculating flow in the grooved area, the groove structure prevented the formation of the thermal boundary layer, enhancing the overall heat transfer performance.

Greiner et al. [7] evaluated the friction coefficient and cooling performance of flow paths with triangular grooves through experimental and numerical analyses. In the case of laminar flow, the friction coefficient decreased as the hydraulic diameter was increased by the grooves. As the Reynolds number increased, the flow over the triangular grooves became more complex. Consequently the heat transfer performance improved. Xie et al. [8] confirmed that in the case of grooved channels, the heat transfer performance improved in the area, where the fluid velocity increased due to the narrowed channel.

Recently, some studies were performed on curved microchannel heat sinks [9,10]. Gong et al. [9] proposed wavy microchannels for a heat sink and studied its cooling performance. They found that the wavy microchannel heat sink caused a vortex at the trough and crest sections in each cycle, resulting in a significant improvement in cooling performance compared to a straight-microchannel heat sink. The pressure losses did not increase significantly. Sui et al. [10] investigated a wavy microchannel heat sink for various flow conditions and amplitudes. They compared three-dimensional numerical analyses and experiments in all cases. The numerical results of the cooling performance and friction coefficient were reliable, and vortices were developed at the trough and crest sections in each cycle.

With the rapid development of computing power, optimization designs that can handle a huge amount of data have become practical [11–13]. In particular, optimization based on a surrogate model has been widely used to reduce the computing time [14–16]. A surrogate model is constructed using sample data at several selected points in the design space. Design of experiments (DOE) is used to extract the sample data. The prediction accuracy of surrogate models is affected by the sample data, so DOE should be carried out carefully [17]. DOE can typically be classified into two categories according to the extraction method: factorial design [18] based on orthogonal extraction and Latin hypercube sampling (LHS) [19], which uses random extraction.

Factorial designs are experiments that combine all levels of each factor with all levels of all other factors in an experiment [18]. This method is very intuitive, and the number of sample data is determined by the number of design variables. Therefore, it is easy to use because it can be applied without considering the distribution and number of sample data. However, the features within the design space are considered less because the sample data are focused on the boundaries of the design space.

LHS uses a random extraction method for sample points within the design space. This method is widely used because the space-filling quality of the sampling points is good. In addition, it can create any allotted number of sampling points [19]. However, since LHS extracts sample data inside the design space, the boundary values of each design variable are not considered. Therefore, a surrogate model based on LHS often makes predictions that are too high at the bounds of design variables.

In the present work, a modified LHS that uses the advantages of orthogonal and random extraction methods is proposed. The modified LHS extracts sample data by applying LHS inside the design space and prevents excessive prediction of the surrogate model by applying the three-level full factorial method to the boundaries of the design space. A wavy microchannel heat sink improves the heat transfer efficiency compared with straight microchannels. In this study, a wavy microchannel heat sink with grooves attached to the channel walls is proposed. A numerical analysis of the laminar flow and heat transfer in the microchannels was performed using three-dimensional Navier-Stokes equations.

Multi-objective optimization of the wavy microchannels was also performed to simultaneously enhance the heat transfer efficiency and reduce the pressure loss. The proposed modified LHS was compared with conventional DOE methods to determine the effectiveness of the proposed sampling method in constructing surrogate models. For the optimization, response surface approximation (RSA) [20] and a genetic algorithm [21] were used as a surrogate model and searching algorithm, respectively.

μm μm

μm

#### **2. Numerical Analysis**

The computational domain and design variables are shown in Figure 1. The heat sink consists of 62 wavy microchannels, and the computational domain includes one of them, which is composed of 10 cycles. Two grooves are attached to each channel wall in one cycle of the channel, as shown in Figure 1. The amplitude of the wavy channel is 138 µm, and the total length (20*P*) is 25,000 µm. The thickness of the side wall (2*t*) is 193 µm, the channel width (*W*) is 207 µm, and the height of the flow path (*h*) is 406 µm. μm μm μ

**Figure 1.** Geometry of the wavy microchannel with grooves and computational domain comprising 10 cycles of wavy channel.

**r μ** The information for the reference channel is shown in Table 1. In the reference channel, the horizontal locations of grooves on both the walls are the same (*D* = 0). Grooves are attached to crests and troughs when *D* = 0. As *D* increases, grooves on the left wall (located at *z* = 400 µm in Figure 1) move in the −*x* direction, and grooves on the right wall (located at *z* = 0 in Figure 1) move in the +*x* direction from a crest (or a trough).

**Table 1.** Dimensions of the reference wavy channel with grooves.


Conjugate heat transfer analysis was carried out on the flow channel and solid domain for laminar flow in steady state using three-dimensional Navier-Stokes equations. The commercial computational fluid dynamics code ANSYS CFX 15.0® (Version 15.0, ANSYS Inc., Canonsburg, PA, USA, 2013) [22] was used for the analysis. The boundary conditions are shown in Figure 2. The boundary conditions were used in the same way as in a previous study [10]. The working fluid was water at 300 K, and the material of the solid wall was copper.

**Figure 2.** Boundary conditions.

 = /μ The inlet Reynolds number (*Re* = *ρUDh*/µ) was 700, and the corresponding flow rate was assigned at the inlet. The average velocity of water at the inlet is 1.992 m/s. The static pressure was used as an exit boundary condition. Periodic conditions for temperature were applied to both side boundaries (i.e., wavy surfaces) considering the neighboring microchannels. Uniform heat flux conditions (50 W/cm<sup>2</sup> ) were applied to the bottom boundary (substrate), and the upper boundary was assumed to be adiabatic.

The fluid and solid computational domains consist of hexahedral and unstructured tetrahedral meshes, respectively. Since the flow velocity changes near the groove, dense meshes are placed there. Near the solid wall, dense meshes were also placed in anticipation of large temperature and velocity gradients due to the boundary layer. Figure 3 shows an example of the grid system. Convergence conditions were set so that the root-meansquared residual values of all parameters fell to 1.00 <sup>×</sup> <sup>10</sup>−<sup>6</sup> . Each computation took about 5–6 h on a computer with an Intel Core i7–4790K 4GHz CPU.

**Figure 3.** Example of a computational grid system on one cycle of wavy channel.

≤ ≤ ∈

#### **3. Optimization Procedure**

The multi-objective optimization problem was formulated as follows:

Minimize: **F**(**x**) = [F1(**x**), F2(**x**)]

Design variable bound: **LB** ≤ **x** ≤ **UB**, **x**∈**R**, ≤ ≤ ∈

where **F**(**x**) is the vector of real-valued objective functions, **x** is a vector of the design variables, and **LB** and **UB** indicate the vectors of the lower and upper bounds, respectively [23]. Figure 4 shows a flowchart for the multi-objective genetic algorithm (MOGA) optimization process using a surrogate model. Firstly, the objective functions and constraints are defined according to the design goals. Secondly, the design variables and their ranges are selected.

**Figure 4.** Multi-objective optimization procedure.

The full factorial method, LHS, and modified LHS were used in DOE to select design points (i.e., sample designs). Values of the objective functions were evaluated by numerical analysis at these design points. Next, to approximate the objective functions, surrogate models were constructed using these objective function values. A genetic algorithm (GA) was used to find the global optima. Finally, Pareto-optimal solutions (a collection of nondominated solutions) were derived using MATLAB (Release 14, the Math Work Inc., Natick, MA, USA, 2004) [24].

#### *3.1. Design Variables and Objective Functions*

For optimization, three geometric parameters were selected as the design variables through a preliminary parametric study: the ratio of the groove depth to half of the side wall thickness (*d*/*t*), the ratio of the groove width to half of the cycle length (*w*/*P*), and the distance between staggered grooves on the opposite walls to half of the cycle length (*D*/*P*). The depth and width of the grooves were expected to affect the vortices occurring around the grooves and thus have sensitive effects on the heat transfer. The distance between staggered grooves affects the disturbance of the main flow.

The average Nusselt number *Nu* is defined as follows [10]:

$$\overline{Nu} = \frac{\overline{h}D\_h}{k\_w} \tag{1}$$

where *D<sup>h</sup>* is the hydraulic diameter of the microchannel, and *k<sup>w</sup>* is the thermal conductivity of water. *h* is the average convective heat transfer coefficient, which is defined as follows:

$$\overline{h} = \frac{q}{(A\_b + 2A\_s)(T\_w - T\_m)}\tag{2}$$

where *q* is the heat flux, *A<sup>b</sup>* and *A<sup>c</sup>* are the bottom area and the side area of the flow channel, and *T<sup>w</sup>* and *T<sup>m</sup>* are the average temperature at the solid wall and the average of the inlet and outlet temperatures, respectively.

The friction factor *f* is defined as follows [10]:

$$f = \frac{(dp/dx)D\_h}{0.5\rho Ul^2} \tag{3}$$

where *dp*, *ρ*, and *U* are the pressure difference between the inlet and outlet, the density of water, and the average velocity at the inlet, respectively. The thermal resistance *Rth* is defined as follows [5]:

$$R\_{th} = \frac{T\_{s,max} - T\_{f,inlet}}{qA} \tag{4}$$

where *Ts,max* and *Tf,inlet* are the highest temperature at the bottom substrate and the average temperature of the cooling fluid at the inlet, respectively, and *A* is the area of the microchannel substrate. The local Nusselt number (*Nux*) is defined as follows:

$$N\mu\_X = \frac{q\_l D\_h}{\left(T\_{w,l} - T\_{f,inlet}\right)k\_w} \tag{5}$$

where *q<sup>l</sup>* and *Tw,l* are the local heat flux and local temperature at the surface of the solid wall, respectively.

*Rth* and *f* were selected as objective functions for the multi-objective optimization: *FRth* = *Rth* and *F<sup>f</sup>* = *f*. The thermal resistance *Rth* is related to the highest local temperature, which affects the performance of micro devices. The friction factor *f* was used to reduce the pressure drop through the microchannel. A parametric study was carried out for the performance functions using three design variables: *D*/*P*, *w*/*P*, and *d*/*t*. Based on the parametric study, the ranges of the three design variables were selected, as shown in Table 2.

**Table 2.** Ranges of design variables.


#### *3.2. Modified LHS*

Factorial design [18,25] is a classical DOE method that explores the design space. 2–level and 3–level full factorial designs are widely used to estimate interactions between design variables. Figure 5 shows examples of 2– and 3–level full factorial designs for two design variables. In the 2–level full factorial design, the sample points are located at the ends of each boundary, as shown in Figure 5a. In the 3–level full factorial design, the sample points are located at the ends and middle of each boundary, as shown in Figure 5b. In these full factorial designs, the distribution and number of the sample points are determined according to the number of design variables when the level is determined.

**Figure 5.** Examples of the full factorial designs.

LHS [19] is one of the most popular DOE methods for random sample distributions. To allocate *p* samples using LHS, the range of each parameter is separated into *p* bins, which yields a total number of *p <sup>n</sup>* bins for n design variables in the design space. The samples are randomly chosen in the design space, each sample is randomly arranged inside a bin, and for all one-dimensional projections of the *p* samples and bins, there is exactly one sample in each bin, as shown in Figure 6. Therefore, LHS is relatively incapable of handling samples at the boundaries of the design space compared to the full factorial designs.

**Figure 6.** Example of conventional LHS.

y() =

ே

ୀଵ

y() = +

ே

ୀଵ

() +

Since the surrogate model is built using the data at the sample points, the distribution of the sample points has a very significant influence on the prediction accuracy of the surrogate model. Therefore, when using LHS with sample points concentrated inside the design space, it is possible to predict the interaction well inside the design space, but predictions that are too high may occur at the boundaries where there are no data. On the other hand, in the full factorial design, the sample points are focused on the boundaries of the design space, so it is possible to make a relatively accurate prediction at the boundaries, but there is a problem in the prediction inside the design space.

To solve this problem, a modified LHS is proposed. In the modified LHS, sample points are extracted using the 2–level full factorial method at the boundaries of the design space, and the LHS method is used to select sample points inside the design space. An example of the modified LHS for two design variables is shown in Figure 7. In this method, the surrogate model does not show high predictions at the boundaries of the design space. Furthermore, by selecting the sample points inside the design space, the shortcomings of

, E(ε) = 0, () = <sup>ଶ</sup>

ε

+ ே

ழ

+

ே

ୀଵ

ଶ

*β*

the full factorial design can be overcome. MATLAB [24] was used to extract the sample points. Three–level full factorial design, LHS, and the modified LHS were tested for the same optimization problem. Twenty-seven sample points were extracted for all these DOE methods.

**Figure 7.** Example of the modified LHS.

ୀଵ

#### *3.3. Surrogate Model and Searching Algorithm*

ୀଵ

ୀଵ

The surrogate model was configured based on the sample points obtained using DOE methods. Response surface approximation (RSA) [20] was used as the surrogate model. MOGA coupled with the RSA model was used to obtain Pareto-optimal solutions [24].

The RSA model is multivariate polynomial model, and a continuous response *y*(*x*) is usually modeled as follows [20]:

$$\text{y} \qquad \text{y} \qquad \text{y} \\ \text{(x)} = \sum\_{j=1}^{N} \beta\_{j} f\_{j}(\text{x}) + \varepsilon, \text{ E}(\varepsilon) = 0, \text{ } V(\varepsilon) = \sigma^{2} \tag{6}$$

*β* ε where *x* is a vector of design variables, *f*<sup>j</sup> (*x*) (*j* = 1, . . . , *N*) are the terms of the model, *β<sup>j</sup>* (*j* = 1, . . . , *N*) are the coefficients, and the error *ε* is assumed to be uncorrelated and distributed with a mean of 0 and constant variance [20]. A second-order polynomial is used for the RSA model, and the model can be expressed as follows:

$$y(\mathbf{x}) = \beta\_0 + \sum\_{i=1}^{N} \beta\_i \mathbf{x}\_i + \sum\_{i=1}^{N} \beta\_{ii} \mathbf{x}\_i^2 + \sum\_{i$$

The model involves an intercept, linear terms, quadratic interaction terms, and squared terms (from left to right). *R <sup>2</sup>* and *Radj <sup>2</sup>* are used to decide the goodness of the fit and should be close to 1 for a good fit [20].

ழ

GA is a random global search technique that solves problems based on natural evolution. An initial population of individuals is defined to represent a part of the solution to a problem [21]. Before starting the search, a set of chromosomes is randomly selected from the design space to obtain the initial population. Through subsequent computations, the individuals adapt in a competitive way. The initially selected set of chromosomes is called the parental generation, and the subsequent selected set of chromosomes is called the child generation. In this process, genetic search operators (selection, mutation, and crossover) are used to obtain chromosomes that are superior to the previous generation [21]. MATLAB [24] was used to invoke the GA for multi-objective optimization.

#### **4. Results and Discussion**

#### *4.1. Grid Dependency Test and Validation of Numerical Results*

A grid dependency test was carried out for the reference shape based on Richardson's extrapolation method and grid convergence index (GCI), which represents numerical uncertainty by estimating the discretization error according to the procedure presented by Roache [26] and Celik and Karatekin [27].

Table 3 shows the results of calculating the discretization error for *Nu*. The number of grid nodes was adjusted by setting the grid segmentation index to 1.3, and three different grid systems were analyzed. When *N<sup>2</sup>* was used, the extrapolation error (*e* 21 *ext*) was about 0.3%, and *GC I*<sup>21</sup> *f ine*was about 0.4%, which indicate small numerical uncertainty. Therefore, *N<sup>2</sup>* was selected as the optimal grid system.


**Table 3.** Analysis of grid convergence index.

To verify the numerical results, they were compared with experimental data obtained by Sui et al. [10] for the Nusselt number and friction factor in a wavy microchannel under the same boundary conditions, as shown in Figure 8. As shown in Figure 8, the numerical results for the friction factor show good agreement with the experimental data, except at the lowest Reynolds number. The numerical results for the Nusselt number deviate slightly from the experimental data over the whole *Re* range but show the same qualitative tendency. At *Re* = 300, the errors are relatively large because the pressure drop and the flow rate are relatively small, as discussed by Sui et al. [10].

**Figure 8.** Validation of numerical results compared with experimental data [10].

തതതത

1.61 × 10–ଵ 1.59 × 10–ଵ

തതതതത

#### *4.2. Heat Transfer Performance Enhancement by Grooves*

Table 4 shows the comparison of the performance parameters between the smooth and reference wavy microchannels. In the wavy channel with grooves, *Nu* increased by about 8.34%, and *Rth* decreased by about 2%, but the friction factor *f* also increased by about 1.25% in comparison with the smooth wavy channel. This means that the grooves largely enhance the heat transfer but with less increase in the friction. This improvement in the heat sink performance with grooves is expected to be further increased by optimization.

**Table 4.** Performance comparison between reference and smooth wavy microchannels.


The temperature distributions on the wavy wall on the right side of the reference and smooth microchannels are shown in Figure 9. In the case of the reference design, it can be seen that the temperature increase in the flow direction is smaller than that of the smooth microchannel, resulting in lower maximum temperature. This shows improved heat transfer performance on the sidewalls and confirms the results shown in Table 4.

**Figure 9.** Temperature distributions on a right side wall: (**a**) smooth microchannel and (**b**) reference design.

The local Nusselt number (*Nux*) distributions on the wavy side walls are shown in Figure 10. High *Nu<sup>x</sup>* regions are found between the crest and the trough (e.g., *x*/2*P* = 5.75–6.25) on the left wall, but they are found between a trough and crest (e.g., *x*/2*P* = 6.25–6.75) on the right wall. In addition, most of the high *Nu<sup>x</sup>* regions are distributed near the top and bottom of the flow path. In the case of the smooth microchannel, a low *Nu<sup>x</sup>* region is found near the middle height of the flow path immediately after each crest (e.g., *x*/2*P* = 5.75). In the reference design, the high *Nu<sup>x</sup>* regions are found just downstream of the grooves, and the total area of the high *Nu<sup>x</sup>* regions is larger than that of the smooth channel. This results in high *Nu* in the grooved microchannel, as shown in Table 4.

**Figure 10.** Local Nusselt number distributions on wavy walls: (**a**) smooth microchannel and (**b**) reference design.

Figure 11 shows the flow fields of the reference design and the smooth wavy microchannel. Figure 11a shows that the velocity gradients near the left wall are larger than those near the right wall between a crest and trough (*x*/2*P* = 5.75–6.25), but vice versa between the trough and crest (*x*/2*P* = 6.25–6.75). This phenomenon occurs due to the fluid inertia. The regions with high velocity gradients and those with high *Nu<sup>x</sup>* shown in Figure 10 are nearly the same. Thus, it can be inferred that the high velocity gradient near the wall promotes the heat transfer and enhances *Nux*.

**Figure 11.** Velocity vectors on *x*–*z* plane and *y*–*z* plane (**a**) velocity vectors on the *x*–*z* plane (*y*/*H* = 0.6) (**b**) velocity vectors on the *y*–*z* plane.

Figure 11b shows the velocity vectors in the *y*–*z* plane. Vortices are found near the top and bottom of the flow channel in the crest. In the case of the reference design with grooves, a complicated flow structure is found near the left wavy wall at the edge of a groove (*x*/2*P* = 5.875) due to the upward flow escaping from the groove, which promotes mixing of the fluid (and thereby heat transfer) in these regions. This is due to sudden contraction of the flow area just downstream of a groove and provides a reason for the high *Nu<sup>x</sup>* regions downstream of the grooves shown in Figure 10b. Even though the grooves are at the same locations on both the wavy walls, the flow fields shown in Figure 11b are not symmetric in the *z* direction because the main flow upstream of the groove proceeds in the +*z* direction.

Figure 12 shows the temperature distributions in the *y*–*z* plane at the inflection point of the wavy channel (*x*/2*P* = 6). The temperature gradient is relatively small near the upper and lower sides of the flow path in common. This is thought to be due to the strong vortices shown in Figure 11b. These low temperature gradients also contribute to the distribution of high *Nu<sup>x</sup>* in these regions (Figure 10). Figure 12 shows that the temperature on the left side in the reference design is still low, even at the medium height, unlike in the smooth wavy microchannel. This is due to the fluid mixing caused by the strong secondary flow downstream of the grooves.

**Figure 12.** Temperature distributions at inflection point (*x*/2*P* = 6) in the *y*–*z* plane.

തതതതത

87

തതതതത

#### *4.3. Parametric Study*

Figure 13 shows the results of the parametric study for *Nu*, *Rth*, and *f*. When one parameter was changed, the other parameters were fixed at the reference values shown in Table 2. With the change of parameters, the friction factor *f* shows small variations of less than 2.5%. At *d*/*t* = 0.5, the maximum *Nu* and *f* and minimum *Rth* are found, which indicates that there is an optimum groove depth for heat transfer enhancement. തതതതത തതതതത

**Figure 13.** Results of the parametric study.

*Rth* and *Nu* are inversely correlated with the variation of *d/t*. *Nu* and *f* have maximum values at *w*/*P* = 0.15, but *Rth* has a minimum value at *w*/*P* = 0.25. *Rth* decreases as *w*/*P* increases in the tested range. This means that wide grooves are effective in reducing thermal resistance. In the case of *D*/*P*, *Nu* and *f* increase as *D*/*P* increases, but *Rth* shows a maximum at *D*/*P* = 0 (non-staggered grooves). This indicates that if the absolute value of *D* is fixed, the relative locations of grooves between the two wavy walls do not affect *Rth* unlike *Nu* and *f*.

At *D/P* = 0.5, *Nu* shows the maximum value of 20.2. This is the value improved by 23.2% from the value (*Nu* = 16.4) of the wavy microchannel heat sink without grooves predicted by Sui et al. [10] under the same geometric and Reynolds number conditions.

#### *4.4. Optimization Results with Different DOEs*

Figure 14 shows the distribution of sample points of three different DOEs. In Figure 14a, the 3-level full factorial design shows that the sample points are located on only the boundaries of the design space. In the case of the conventional LHS, the sample points are distributed in only the design space, as shown in Figure 14b. However, in the modified LHS, the sample points are located on the boundaries and inside of the design space, as shown in Figure 14c. The RSA models for the objective functions, *F<sup>f</sup>* and *FRth*, were formulated in terms of the design variables normalized between 0 and 1 for three different DOEs as follows:

*<sup>F</sup><sup>f</sup>* \_ *f ull f actorial* <sup>=</sup> 0.1591 <sup>+</sup> 0.0092 d *Sw* <sup>−</sup> 0.0120 *D P* <sup>−</sup> 0.0018 *w P* <sup>−</sup> 0.0025 d *Sw <sup>D</sup> P* +0.0084 d *Sw w P* <sup>−</sup> 0.0008 *D P w P* <sup>−</sup> 0.0049 d *Sw* 2 <sup>+</sup> 0.0139 *D P* 2 −0.0031 *w P* 2 (8) *<sup>F</sup>Rth*\_ *f ull f actorial* <sup>=</sup> 4.6438 <sup>−</sup> 0.0086 d *Sw* <sup>+</sup> 0.2094 *D P* + 0.1187 *w P* +0.0703 d *Sw <sup>D</sup> P* <sup>−</sup> 0.2730 d *Sw w P* <sup>−</sup> 0.0409 *D P w P* −0.0403 d *Sw* 2 <sup>−</sup> 0.3249 *D P* 2 <sup>−</sup> 0.0534 *w P* 2 (9) *<sup>F</sup><sup>f</sup>* \_*conventionalLHS* <sup>=</sup> 0.1589 <sup>+</sup> 0.0099 d *Sw* <sup>−</sup> 0.0095 *D P* <sup>−</sup> 0.0050 *w P* −0.0110 d *Sw <sup>D</sup> P* <sup>+</sup> 0.0092 d *Sw w P* <sup>+</sup> 0.0041 *D P w P* −0.0060 d *Sw* 2 <sup>+</sup> 0.0150 *D P* 2 + 0.0005 *w P* 2 (10) *<sup>F</sup>Rth*\_*conventionalLHS* <sup>=</sup> 4.9136 <sup>−</sup> 1.0222 d *Sw* <sup>−</sup> 0.2633 *D P* <sup>−</sup> 0.4524 *w P* +0.9502 d *Sw <sup>D</sup> P* <sup>−</sup> 0.4268 d *Sw w P* <sup>−</sup> 0.2243 *D P w P* +0.7657 d *Sw* 2 <sup>−</sup> 0.0067 *D P* 2 + 0.4980 *w P* 2 (11) *<sup>F</sup><sup>f</sup>* \_*modi f iedLHS* <sup>=</sup> 0.1588 <sup>−</sup> 0.0082 d *Sw* <sup>−</sup> 0.0038 *D P* + 0.0074 *w P* −0.0025 d *Sw <sup>D</sup> P* <sup>+</sup> 0.0085 d *Sw w P* <sup>−</sup> 0.0002 *D P w P* +0.0137 d *Sw* 2 <sup>+</sup> 0.0048 *D P* 2 <sup>−</sup> 0.0118 *w P* 2 (12) *<sup>F</sup>Rth*\_*modi f iedLHS* <sup>=</sup> 4.6170 <sup>−</sup> 0.2504 d *Sw* <sup>+</sup> 0.5430 *D P* <sup>−</sup> 0.2220 *w P* −0.0329 d *Sw <sup>D</sup> P* <sup>−</sup> 0.2677 d *Sw w P* <sup>−</sup> 0.0816 *D P w P* +0.2165 d *Sw* 2 <sup>−</sup> 0.5965 *D P* 2 + 0.3226 *w P* 2 (13)

Figure 15 shows the Pareto-optimal solutions using three different DOEs. The Paretooptimal solutions are the best solutions that can be achieved for one objective without disadvantaging another objective and are sensitive to the constructed surrogate model [28]. Pareto-optimal fronts obtained using the conventional and modified LHS methods have similar smooth curves, as shown in Figure 15. However, the full factorial design shows a curve that has two inflection points, unlike the other curves. The Pareto-optimal front from modified LHS predicts the lowest optimum values of the two objective functions among the tested DOEs in most of the range. The Pareto-optimal fronts of the two LHS methods cover wider ranges than that of the full factorial design.

To compare the optimization results, three Pareto-optimal designs (PODs) were extracted from each Pareto-optimal front using K-means clustering [29], as presented in Figure 15. The predicted objective function values at the PODs and numerical calculations at the same PODs are compared in Table 5. In case of the full factorial design, the PODs are close to the boundaries of one or two design variables. However, the PODs of conventional LHS are found inside the design space. In this case, a POD close to a boundary (*D*/*P* = −0.8802 in POD A) yields a larger relative error between the predicted and calculated objective function values than the other PODs. As mentioned earlier, the surrogate model obtained using conventional LHS over-predicts the values at the boundary of the design space, and the error increases near the boundary.

−

−

− −

തതതതത തതതതത

തതതതത

തതതതത

തതതതത

തതതതത = 16.4

**Figure 14.** Distributions of sample points for three different DOEs. − − −

**Figure 15.** Pareto-optimal solutions for three different DOEs.

. In the case of the modified LHS, even the POD located close to the boundary shows good prediction with maximum relative error less than 1.5%. Thus, the modified LHS shows the best prediction accuracy among the tested DOEs. The full factorial design and conventional LHS generally over-predict the objective function values with positive relative errors at the three PODs, but the modified LHS generally under-predicts the values. Therefore, there is not much difference in the calculated objective function values at the PODs among the tested DOEs.


**Table 5.** Results of optimizations with three different DOEs. (a) Full factorial design; (b) Conventional LHS; (c) Modified LHS.

The *R <sup>2</sup>* and adjusted *R <sup>2</sup>* values of the RSA models constructed using three different DOEs are listed in Table 6. As mentioned earlier, values closer to 1 indicate a better surrogate model. In this respect, the modified LHS shows the best results in Table 6. This is consistent with the results shown in Table 5. In addition, the RSA model with the full factorial design has the worst performance. Applying a DOE method that properly locates the sample points on the boundaries and inside of the design space makes it possible to construct a more accurate surrogate model and obtain superior optimization results.

**Table 6.** Statistical analysis of the RSA models. (a) Full factorial design; (b) Conventional LHS; (c) Modified LHS.


```
(a)
```
#### *4.5. Analysis of the Optimized Design*

POD 2 obtained with the modified LHS was selected for further analysis because the values of both the objective functions were improved compared to the reference design. In POD 2, *Rth* and *f* are reduced by 1.55% and 3.00%, respectively, compared with those of the reference design. The *Nu<sup>x</sup>* distributions on the wavy walls are shown in Figure 16, which compares the heat transfer performance between POD 2 and the reference design. In the case of the reference design, there are high *Nu<sup>x</sup>* regions on the left wall between the grooves in the crest and the trough (*x*/2*P* = 5.75–6.25). In the case of POD 2, high *Nu<sup>x</sup>* regions are shown on the left side wall between the inflection point where the groove is located and the trough (*x*/2*P* = 5.50–6.25). The right wall between *x*/2*P* = 7.00 and 7.50 shows the same *Nu<sup>x</sup>* distribution as the left wall between *x*/2*P* = 5.50 and 6.25. Unlike the reference design, the high *Nu<sup>x</sup>* distribution for POD 2 from the inflection point to the crest (*x*/2*P* = 5.50–5.75) seems to be one of the important factors in reducing *Rth* compared to the reference design.

**Figure 16.** Local Nusselt number distributions on wavy walls: (**a**) reference design, and (**b**) optimal design (POD2).

Figure 17 shows the streamlines and velocity vectors. Figure 17a shows that the recirculating flow develops in the grooves in the reference design. These recirculating flow regions correspond to the low *Nu<sup>x</sup>* regions in the grooves in Figure 16. This occurs because the flow recirculation hinders the heat transfer on the wall. Figure 17b shows the velocity vectors at the cross sections perpendicular to the flow direction. As mentioned earlier, in the reference design, a strong interaction between the vortical flow in the channel and upward flow from the groove is found near the left wall at the edge of the groove (*x*/2*P* = 5.875). In the case of POD 2, this phenomenon is also found near the left wavy wall at the edge of the groove (*x*/2*P* = 5.593) but is weaker than in the reference design. This seems to be affected by the location of the groove (which is the crest in the reference design but an inflection point in POD 2) and the fact that the two grooves on both the walls are attached at the same location in the reference design.

However, in POD 2, the vortices in the channel become stronger at a location downstream (*x*/2*P* = 5.875). This is consistent with the *Nu<sup>x</sup>* distributions shown in Figure 16. In the reference design, the high *Nu<sup>x</sup>* region persists from the groove edge (*x*/2*P* = 5.875) to a location far downstream but disappears before the next groove. However, in POD 2, the high *Nu<sup>x</sup>* region is relatively narrow at the edge of the groove (*x*/2*P* = 5.593) but grows downstream and becomes widest at the upstream edge of the next groove. Thus, the total area of the high *Nu<sup>x</sup>* regions is larger in POD 2 than that in the reference design.

**Figure 17.** Streamlines and velocity vectors: (**a**) streamline distributions on the *x*–*z* plane (*y*/*H* = 0.6) (**b**) velocity vector in cross-section perpendicular to flow direction.

#### **5. Conclusions**

A wavy microchannel heat sink with grooves was optimized using RANS analysis of the flow and conjugate heat transfer. In the reference wavy channel with grooves, *Nu* increased by about 8.34%, and *Rth* decreased by about 2%, but the friction factor *f* also increased by about 1.25% compared to the smooth wavy channel. Thus, using grooves, the enhancement of the heat transfer surpasses the increase in the friction.

For optimization, the distance between staggered grooves on opposite wavy walls, the groove depth, and the groove width were selected as design variables. The thermal resistance (*Rth*) and friction factor (*f*) were used as objective functions. A modified LHS that uses the advantages of conventional LHS and the three–level full factorial method was also proposed. The optimization performance of three DOE methods was estimated. Surrogate models of the objective functions were constructed by RSA with each DOE method. The corresponding Pareto optimal solutions were derived, and three representative optimal solutions were selected to compare the predictions of the DOE methods.

The results showed that the optimal solutions using modified LHS methods have the best predictions with less than 1.5% error compared to the numerical calculations. They also had the largest *R <sup>2</sup>* and adjusted *R <sup>2</sup>* values, which indicate the best statistical accuracy of the RSA models. For one of the representative optimal solutions, POD2, *Rth* and *f* decreased by 1.55% and 3.00%, respectively, compared to the reference design, indicating that both the objective functions were improved. Therefore, the multi–objective optimization with modified LHS could effectively improve the performance of the wavy microchannel heat sink with grooves.

**Author Contributions:** M.-C.P. presented the main idea of the wavy microchannel heat sink with groove; M.-C.P. and S.-B.M. contributed to the overall composition and writing of the manuscript; M.-C.P. analyzed the proposed wavy microchannel with grooves and performed the numerical analysis; S.-B.M. analyzed the data; K.-Y.K. revised and finalized the manuscript. All authors have read and agreed to the published version of the manuscript.

**Funding:** This work was supported by the National Research Foundation of Korea (NRF) grant funded by the Korean government (MSIT) (No. 2019R1A2C1007657).

**Institutional Review Board Statement:** Not applicable.

**Informed Consent Statement:** Not applicable.

**Data Availability Statement:** Data is contained within the article.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Abbreviations**


#### **References**


**Xinlong Wang <sup>1</sup> , Honggang Fan 1,\* and Bing Liu 2,\***


**Abstract:** The mixed free-surface-pressurized flow in the tailrace tunnel of a hydropower station has a great impact on the pressure, velocity, and operation stability of the power station. In the present work, a characteristic implicit method based on the upwind differencing and implicit finite difference scheme is used to solve the mixed free-surface-pressurized flow. The results of the characteristic implicit method agree well with the experimental results, which validates the accuracy of the method. Four factors that influence the amplitude of pressure fluctuation are analyzed and optimized, and the results show that the relative roughness can influence the maximum pressure in the tailrace tunnel. Additionally, the maximum pressure decreases with the increase of the tunnel's relative roughness. When the surface relative roughness increases from 0.010 to 0.018, the maximum pressure can decrease by 4.33%. The maximum pressure in the tailrace tunnel can be effectively restrained by setting vent holes in the flat-topped tunnel section (tunnel (4)) and a vent hole at 81.25%L (L is the length of tunnel (4)), which can reduce the maximum pressure by 56.72%. Increasing the vent hole number can also reduce the maximum pressure of the mixed free-surface-pressurized flow in the tailrace tunnel. An optimal set of two ventilation holes 10 m in diameter at 93.75%L and 56.25%L is proposed, which can reduce the maximum pressure by 15.30% in comparison with the single vent case.

**Keywords:** the mixed free-surface-pressurized flow; characteristic implicit method; relative roughness; vent holes; optimization control

#### **1. Introduction**

Energy is one of the most important basic elements of economic and social development, and the utilization of energy can greatly improve the living quality of humans. After hundreds of years of exploitation and utilization, traditional fossil energy is decreasing day by day. As a consequence, the development of renewable energy has become an important development direction for global energy. Every country takes the development of renewable energy, such as hydropower, wind energy, and solar energy, as an important means to meet the challenges of energy security and climate change [1–4]. Among them, hydropower, with its low power generation cost and high power generation efficiency, has become a great alternative in recent years [5–10].

With the development of the national economy and hydropower, many large-scale water conservancy and hydropower projects have been built in China, such as the Three Gorges power station, Baise Underground power station, Xiangjiaba power station, and Xiluodu power station. To ensure the safe operation of hydropower stations, sufficient hydraulic analysis and hydraulic calculation must be carried out for the hydraulic transition process. The purpose of the transition process calculation is to reveal the dynamic

**Citation:** Wang, X.; Fan, H.; Liu, B. Optimization Control on the Mixed Free-Surface-Pressurized Flow in a Hydropower Station. *Processes* **2021**, *9*, 320. https://doi.org/10.3390/ pr9020320

Academic Editors: Hussein A. Mohammed and Jin-Hyuk Kim Received: 15 December 2020 Accepted: 2 February 2021 Published: 9 February 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

hydro-mechanical characteristics of the water transmission and power generation system of a hydropower station in various transitional processes. To improve the reliability, stability, flexibility, and overall economy of hydropower station operation, reasonable control methods and technical measures are necessary. The hydraulic transition process of the hydropower station is complex and involves many theoretical and computational problems. In the tailrace tunnel of the hydropower station, the free surface flow and the pressurized flow may appear alternately in the transition process, which is called the mixed free-surface-pressurized flow. When the mixed free-surface-pressurized flow occurs, the wave velocity and pressure at the interface will change rapidly.

This complicated flow phenomenon will have an important impact on the stability of the whole system's operation and will cause great pressure fluctuation in the transition process, especially for the tailwater systems of hydropower stations. Therefore, it is necessary to establish a reasonable, feasible, and identical model for calculation. At present, the main calculation methods are the virtual slit method [11–13], the shock wave fitting method [14,15], and the rigid water body method [16]. The virtual slit method was proposed by Preissmann [17], which assumes that there is a very narrow gap at the top of the closed tunnel and the gap does not increase the cross-section of the pressure water pipe and the hydraulic radius. When the pipeline is full of water, it can be regarded as an open channel with a very small water surface, and then the unified St. Venant equation can be used to solve free surface flow and pressurized flow. This model has been successfully used by Chaudhry and Kao [18] to analyze the mixed free-surface-pressurized flow in the tailwater system of the Shrum hydropower station in Canada. Ji [13] also used this model to calculate the mixed free-surface-pressurized flow in a rainwater drainage pipe. Trajkovic et al. [19] used the Maccormack scheme to simulate the mixed free-surface-pressurized flow in a circular cross-section pipeline, and the numerical results were in good agreement with the experimental results. Ferreri et al. [20] analyzed the steady pressurized flow in a sewer by using the virtual slit method. Maranzoni et al. [21] applied the virtual slit method to the two-dimensional transient mixed flow.

However, the setting of the virtual slit method is not consistent with actual situations under some conditions. Firstly, the criterion to determine the open channel flow and the pressurized flow is that the water pressure is lower or higher than the pipe's top. If there is a large bubble, even if the pressure is higher than the pipe's top, the open channel flow will not become the pressurized flow. Secondly, the equation of unsteady flow in an open channel is only applicable to the gradual change flow. Guo and Song [22] found that when the sudden change flow was formed and the surge wavefront was steep, the calculation of the virtual slit method would be unstable or not convergent when they studied the mixed free-surface-pressurized flow in the joint underground drainage system in Chicago.

When bubbles and negative pressure appear in the mixed free-surface-pressurized flow, the shock wave fitting method is proposed, which regards the free surface flow and pressurized flow as two flow states and calculates the velocity and position of the moving interface. Wiggert [23] introduced a moving interface between the free surface flow and pressurized flow to modify the Pressimann slit method, and the free surface flow was solved by the characteristic line method. Miyashiro and Yoda [15] used the characteristic line method to solve the Venant equation for free surface flow in a study of the mixed free-surface-pressurized flow in the underground drainage system. Song [24] used a shock wave moving equation and interface characteristic line equation to calculate the free surface flow and pressurized flow for the transition process of the pipeline.

However, some calculation results showed that the shock wave fitting method was not stable enough. When the surge wavefront is steep, it will lead to numerical divergence. Because the wave velocities of the free surface flow and the pressurized flow are quite different, special mesh generation technology should be adopted to meet the requirements of calculation accuracy and stability. When the moving interface passes through boundary conditions such as bifurcation pipes and surge chambers, it will become very difficult to deal with the shock wave. In particular, the shock wave fitting method considers

that the interface of the mixed free-surface-pressurized flow and positive surge wave is consistent, which is not suitable for some cases, such as a positive surge wave in a tailrace tunnel with a variable top height. Hamam and McCorquodale [25,26] proposed the rigid water body method to solve the mixed free-surface-pressurized flow, which assumes that water is incompressible and the flow velocity is uniform. Rigid water body theory is adopted for the liquid phase, and compressible flow theory is adopted for the gas phase. Li and Alex [16] developed the rigid water body method to calculate the bubble motion. However, the algorithm of the rigid water body method is complex, and there are many discrepancies with physical reality. Therefore, this method is rarely used to simulate the mixed free-surface-pressurized flow.

The existing work outlined above shows that the three calculation methods to solve the mixed free-surface-pressurized flow have their limits. Therefore, it is vital to propose a stable calculation format for the mixed free-surface-pressurized flow which can smoothly calculate and obtain results consistent with the actual situation, even when the water surface fluctuates greatly and the pressure fluctuates violently.

The basic structure of the present work is as follows. Firstly, the characteristic implicit scheme method [27] is used to solve the mixed free-surface-pressurized flow, and the experimental validation is carried out. Then, the influence of the relative roughness of the tailrace tunnel on the maximum pressure in the tunnel is analyzed. The restraining effect of setting single vent holes at different positions in the flat-topped tunnel section on the maximum pressure in the tunnel is discussed. The influence of ventilation holes with different diameters on the maximum pressure in the tunnel is calculated. The influence of setting multiple vent holes in the flat-topped tunnel section on suppressing the pressure fluctuation in the tunnel is also studied.

#### **2. Research Object and Mathematical Model**

#### *2.1. Research Object*

Figure 1 shows the layout of the water conveyance system of a hydropower station. The downstream is a tailwater tunnel that starts at the altitude of 548.70 m and ends at the altitude of 577.00 m. As shown in Tables 1 and 2, the total length of tunnels (1), (2), (3), and (4) is 1541.10 m, where the mixed free-surface-pressurized flow may occur. The shape of tunnel (4) is rectangular with an arch crown; its width is 18 m, and its height is 20 m. The operating conditions are 825 m at the upstream and 597 m at the downstream, respectively, which means that the downstream water level is equal to the top of tunnel (4).

**Figure 1.** The layout of the water conveyance system of a hydropower station.


#### **Table 1.** Tunnel parameters.

**Table 2.** Description of the tunnel shape.


#### *2.2. Mathematical Model*

In recent work, the virtual slit method was mainly used to calculate the alternating full flow. According to the Preissmann model [17], a virtual slot on the top of the pipe or tunnel is assumed, and the slot will slightly influence the tunnel cross-section area *A*. The wave velocity of the free surface flow *c* is determined by *c* = p *gA*/*B*, where *B* is the surface width and *g* is gravity. Then, the wave velocity of the pressurized flow *a* can be chosen as *a* = *c*. This is a way to simulate the pressurized flow by modifying the free surface wave velocity. Then, the free surface flow and the pressurized flow can be described by the same partial equations [28] as follows:

$$
\log\frac{\partial h}{\partial \mathbf{x}} + v\frac{\partial v}{\partial \mathbf{x}} + \frac{\partial v}{\partial t} = \mathbf{g}(i - I\_f) \tag{1}
$$

$$v\frac{\partial h}{\partial \mathbf{x}} + \frac{\partial h}{\partial t} + \frac{a^2}{g}\frac{\partial v}{\partial \mathbf{x}} = 0\tag{2}$$

where *h* is the flow depth, *v* is the flow velocity, *i* is the tunnel slope, and *J<sup>f</sup>* is the slope of the energy grade line.

#### *2.3. Characteristic Implicit Method*

With the rapid increase of the wave velocity *c*, the numerical calculation would be difficult to converge when the interface of the free surface flow and the pressurized flow passes the computational nodes. In the present work, the characteristic implicit method provides a differencing scheme with good stability and high accuracy to solve the mixed free-surface-pressurized flow. Since the system made up of the continuity and momentum equations is a hyperbolic system, upwind differencing can avoid nonphysical oscillations, and the implicit scheme is used for stability and accuracy.

To transform Equations (1) and (2) into the norm forms of the hyperbolic system and to replace *v* with *Q*/*A*, where *Q* is the volume flow, Equations (3) and (4) are derived as follows:

$$\mathcal{B}\mathfrak{c}^{-}\left(\frac{\partial \mathfrak{h}}{\partial t} + \mathfrak{c}^{+}\frac{\partial \mathfrak{h}}{\partial \mathfrak{x}}\right) - \left(\frac{\partial \mathcal{Q}}{\partial t} + \mathfrak{c}^{+}\frac{\partial \mathcal{Q}}{\partial \mathfrak{x}}\right) = f \tag{3}$$

$$\mathcal{B}c^{+} \left(\frac{\partial \hbar}{\partial t} + c^{-} \frac{\partial \hbar}{\partial \mathbf{x}}\right) - \left(\frac{\partial \mathcal{Q}}{\partial t} + c^{-} \frac{\partial \mathcal{Q}}{\partial \mathbf{x}}\right) = f \tag{4}$$

where *c* ± = *Q A* ± p *gA*/*B*, *f* = −*gA*(*i* − *J<sup>f</sup>* ), *J<sup>f</sup>* = *n* <sup>2</sup>*Q*<sup>2</sup> *<sup>A</sup>*2*R*4/3 , and *R* is the hydraulic diameter. Equations (3) and (4) are differenced at the point of (m, n) by using the differencing scheme as follows. The forward differencing in time is found by

$$\begin{aligned} \frac{\partial \mathcal{Q}}{\partial t} &= \frac{\mathcal{Q}\_m^{n+1} - \mathcal{Q}\_m^n}{\Delta t} \\ \frac{\partial h}{\partial t} &= \frac{h\_m^{n+1} - h\_m^n}{\Delta t} \end{aligned} \tag{5}$$

For the upwind differencing in space, Equation (3) is differenced along the *c* <sup>+</sup> line:

$$\frac{\partial \mathcal{Q}}{\partial \mathbf{x}} = \frac{\mathcal{Q}\_{m}^{n+1} - \mathcal{Q}\_{m-1}^{n+1}}{\Delta \mathbf{x}} \qquad \frac{\partial h}{\partial \mathbf{x}} = \frac{h\_{m}^{n+1} - h\_{m-1}^{n+1}}{\Delta \mathbf{x}} \tag{6}$$

Equation (4) is differenced along the *c* − line:

$$\frac{\partial \mathcal{Q}}{\partial \mathbf{x}} = \frac{\mathcal{Q}\_{m+1}^{n+1} - \mathcal{Q}\_{m}^{n+1}}{\Delta \mathbf{x}} \qquad \frac{\partial h}{\partial \mathbf{x}} = \frac{h\_{m+1}^{n+1} - h\_{m}^{n+1}}{\Delta \mathbf{x}} \tag{7}$$

The substitution of Equations (5) and (6) into Equation (3), as well as the substitution of Equations (5) and (7) into Equation (4), lead to the system in Equation (8):

$$\begin{cases} a\_1 h\_{m-1}^{n+1} + b\_1 Q\_{m-1}^{n+1} + c\_1 h\_m^{n+1} + d\_1 Q\_m^{n+1} = e\_1 \\\ a\_2 h\_m^{n+1} + b\_2 Q\_m^{n+1} + c\_2 h\_{m+1}^{n+1} + d\_2 Q\_{m+1}^{n+1} = e\_2 \end{cases} \tag{8}$$

where *a*<sup>1</sup> = − *B n mc* −*c* <sup>+</sup>∆*t* ∆*x* , *b*<sup>1</sup> = *<sup>c</sup>* <sup>+</sup>∆*t* ∆*x* , *c*<sup>1</sup> = *B n mc* <sup>−</sup> − *a*1, and *d*<sup>1</sup> = −(1 + *b*1). Additionally,

$$\begin{aligned} c\_1 &= B\_m^n c^- h\_m^n - Q\_m^n + \Delta t f\_\prime & a\_2 &= B\_m^n c^+ + a\_1 \\ b\_2 &= -(1 - \frac{c^- \Delta t}{\Delta x})\_\prime & c\_2 &= -a\_1 \\ d\_2 &= -(1 + b\_2)\_\prime & e\_2 &= B\_m^n c^+ h\_m^n - Q\_m^n + \Delta t f\_\prime \\ &\quad \cdot c^\pm = \frac{Q\_m^n}{A\_m^n} \pm \sqrt{\frac{g A\_m^n}{B\_m^n}}, \\ f &= -g A\_m^{n+1} (i\_m^{n+1} - \frac{n^2 Q |Q|}{A^2 R^{4/3}} \Big|\_{m}^{n+1}) \end{aligned}$$

Equation (8) is constituted by a set of two nonlinear algebraic equations with six independent unknowns, two of which are the same in any two neighboring nodes, and a similar pair of equations are written for each of the M-2 internal points in the tunnel. Thus, there are two M-2 equations in 2 M unknowns. Equation (8) can provide one equation for each boundary point. The boundary condition at the end of the tunnel can provide two additional equations, so a unique solution can be obtained. In this paper, the new method is named the characteristic implicit method with first-order accuracy. By using the friction term and gravity term of the *n* + 1 time step, the computation precision and stability can be improved.

#### *2.4. Experimental Validation*

The purpose of this experiment was to verify the correctness of the characteristic implicit method for solving the mixed free-surface-pressurized flow. In this experimental model, the diversion system and tailwater system adopted the diversion mode that one tunnel distributed one machine. The tailrace adopted the four-in-one arrangement scheme, in which four branch tunnels converged to one main tunnel. Figure 2 shows the diagram and experimental rig of the tailrace tunnel.

**Figure 2.** The diagram (**a**) and experimental rig (**b**) of the tailrace tunnel.

*λ* The experimental tunnel was a model with a proportion scale *λ<sup>L</sup>* = 30, according to the gravity similarity principle [29]. The prototype of the tailrace runner was the concrete surface, and its relative roughness was 0.014. According to the scale of relative roughness, the relative roughness of the model material was 0.0079, while the relative roughness of the plexiglass pipe was also 0.0079, so the tailrace channel model was made of plexiglass could meet the requirement.

The model structure and schematic diagram of the monitoring points on the main tailrace tunnel are shown in Figure 2a, in which the tailrace of the power station was connected with a large tailwater pond. The reason for this was that the tailrace of the prototype power station flowed into the natural river channel, and the tailrace water level of the power station was determined by the discharge flow of the discharge structure and the discharge flow of the power station. The discharge flow of the power station was relatively low, and the tailrace water level of the power station was relatively stable in the transient process. In the present experiment, the discharge flow was only from the power station, so it was necessary to manually adjust the actual tailrace level. In the unsteady experiment, a relatively stable boundary condition of downstream tailrace could be obtained by connecting a large pool with the model tailrace and adopting a wide weir at the pool end.

In the present experiment, the flow rate was measured by the rectangular, thin-walled weir, and the zero reading of the thin-walled weir was calibrated before the experiment. The water depth at each point of the main tunnel was measured by the pulsating pressure sensor. The pulsating pressure sensor was connected with the computer through a DJ800 multifunctional monitor to form a data acquisition and processing system. The system was used to measure the fluctuation of the water depth at various points in the tailrace system. To observe the obvious mixed free-surface-pressurized flow in the main tailrace tunnel, the downstream water level was set to 0.807 m. Under this condition, the first half of the tailrace was the pressurized flow, and the second half of the tailrace was the free surface flow. The discharge was calculated to be 0.066279 m3/s, according to the Rehbock weir formula [30]. When the butterfly valves at the inlets of four branch tunnels were suddenly closed, the phenomenon of mixed free-surface-pressurized flow in the main tailrace tunnel could be observed.

The flow rate condition was given at the upstream, and the flow rate of the four adits was assumed to be the same at 0.016570 m3/s. When the butterfly valve quickly closed, the flow rate became zero in a short time, and the variation of the flow rate was recorded. Although the downstream was a large pool, there were still small fluctuations in the water level, which were recorded and input into the calculation. Figure 3a–h shows the comparison curves of the water depth in the experiment and calculations. The results show that the water levels of the time domain agreed well between the experiment and calculations. The frequency results of the experiment and calculations also coincided well, and the dominant frequencies were both 0.1 Hz. It can be seen that the calculation results and the experimental results were consistent, and the change period of the water depth

was nearly the same. The water level at point 1 exceeded the tunnel's top, so the flow in the transient process was pressurized. The water level at point 4 was below the tunnel top, so the flow in the transient process was a free surface flow. In the transient process, the water level at the second and third points would be below or exceed the tunnel's top, so the mixed free-surface-pressurized flow would occur. This is consistent with the experimental results that the separation interface between pressurized flow and free surface flow appeared near point 3 under the initial water level of 0.807 m.

Figure 3e shows that when the water surface reached the tunnel's top at point 3, the free surface flow became the pressurized flow. The curve of the experimental results shows a large pressure fluctuation at this time, which agrees well with the calculated results. Due to the pressure fluctuation at measuring point 3, the pressure fluctuation also appeared at points 1 and 2. Therefore, the calculation model could accurately predict the interface of the free surface flow and the pressurized flow.

**Figure 3.** *Cont.*

**Figure 3.** The curve of the stage (pressure) in the tailrace tunnel, shown for (**a**) the time domain of point 1, (**b**) frequency domain of point 1, (**c**) time domain of point 2, (**d**) frequency domain of point 2, (**e**) time domain of point 3, (**f**) frequency domain of point 3, (**g**) time domain of point 4, and (**h**) frequency domain of point 4.

#### **3. Analysis of Influencing Factors for the Mixed Free-Surface-Pressurized Flow**

Many factors can affect the occurrence and development of mixed free-surfacepressurized flow, which are important for the construction design of hydraulic engineering and the operation of hydraulic machinery.

#### *3.1. Influence of the Tunnel Relative Roughness*

When the mixed free-surface-pressurized flow occurs in the tailrace tunnel, the wave velocity at the interface between the free surface flow and the pressurized flow will change suddenly and cause great pressure fluctuation. According to Equations (3) and (4), the surface relative roughness of the tunnel wall will affect the amplitude of the pressure fluctuation.

Tunnels with the relative roughness of 0.010/0.012/0.014/0.016/0.018 were selected to calculate the influence of the tunnel surface relative roughness on the mixed free-surfacepressurized flow. The maximum pressure in the tunnel with different relative roughnesses was calculated and shown in Table 3, and the results show that the maximum pressure

in the tunnel decreased with the increase of the tunnel's relative roughness. This means that increasing the relative roughness of the tunnel surface could suppress the maximum pressure in the tunnel. The reason for this is that the increasing relative roughness will increase the hydraulic loss, which makes the maximum pressure lower. When the surface relative roughness increased from 0.010 to 0.018, the maximum pressure of the tunnel could decrease by 4.33%. However, increasing the relative roughness of the tunnel surface would reduce the power generation efficiency of the hydropower station. Therefore, a relative roughness of 0.014 is recommended upon consideration of the balance of economy and construction.


**Table 3.** Maximum pressure in the tailrace tunnel with different relative roughnesses.

#### *3.2. Influence of Vent Position*

The vent can greatly discharge pressure when the mixed free-surface-pressurized flow appears. To study the effect of vent holes at different positions on the maximum pressure in the tunnel, the water level of the tailrace tunnel under the mixed free-surface-pressurized flow was calculated, as is shown in Figure 4. The diameter of the vent hole was set as *D* = 10 m in the calculation. In Figure 4, the red line represents the water level in the tunnel when the mixed free-surface-pressurized flow occurred, the blue line represents the tunnel's top, and the black line represents the tunnel's bottom.

**Figure 4.** *Cont.*

**Figure 4.** *Cont.*

**Figure 4.** Water level with a vent at different positions: (**a**) 6.25%L, (**b**) 18.75%L, (**c**) 31.25%L, (**d**) 43.75%L, (**e**) 56.25%L, (**f**) 68.75%L, (**g**) 81.25%L, (**h**) 93.75%L, and (**i**) no vent.

For the no vent scenario, the maximum value of the pressure in the tunnel was 152.785 mH2O. For the different vent positions of 6.25%L, 18.75%L, 31.25%L, 43.75%L, 56.25%L, 68.75%L, 81.25%L, and 93.75%L, the maximum values of the pressure in tunnel were 151.493 mH2O, 144.734 mH2O, 134.734 mH2O, 120.974 mH2O, 104.851 mH2O, 86.844 mH2O, 66.124 mH2O, and 77.665 mH2O, respectively. It can be seen that the vent at 81.25%L had the best suppression effect on the maximum pressure in the tunnel, and the corresponding maximum pressure was 66.124 mH2O with a decrease of 56.72%. When the free surface flow turned into the pressurized flow, the wave velocity increased instantaneously, which caused a rapid increase of the pressure fluctuation in the tunnel. On the one hand, according to the design manual of the hydropower station, the wave velocity of the tailwater tunnel of the prototype power station was 1160 m/s under the pressurized flow. On the other hand, the vents in the tunnel could be thought of as small open channels, and the wave velocity in the vent could be calculated to be about 19 m/s by the wave velocity formula. Therefore, the maximum values of the pressure in tunnel 4 could be greatly reduced by setting proper vent positions. This method can be an alternative with the surge shafts to guarantee the stable operation of the hydropower station.

#### *3.3. Influence of the Vent Diameter*

According to the formula of the wave velocity for the open channel, the wave velocity decreased with the increase of the vent diameter. It can be inferred that the diameter of the ventilation holes affected the maximum pressure inside the tunnel. Vent holes with different diameters were set at 81.25%L, and the maximum pressure when the mixed free-surface-pressurized flow occurred in the tunnel was calculated, as is shown in Figure 5.

Three vent diameters of 5 m, 10 m, and 15 m were set to investigate the influence of the vent diameter on the suppression effect on the maximum pressure in the tunnel. The results show that the maximum pressure in the tunnel decreased with the increase of the vent diameter. When the diameter of the vent hole increased from 5 m to 10 m and 15 m, the maximum values of the pressure in the tunnel were 68.541 mH2O, 66.124 mH2O, and 66.026 mH2O, with a decrease of 3.53% and 3.67%, respectively. Therefore, further increasing the diameter had a slight effect on the maximum pressure suppression.

**Figure 5.** Water level with different vent diameters: (**a**) vent diameter of 5 m, (**b**) vent diameter of 10 m, and (**c**) vent diameter of 15 m.

#### *3.4. Influence of the Vent Number*

A vent can effectively reduce the maximum pressure in the tunnel, so the influence of the vent number should be further investigated. Because the vent position at 93.75%L could effectively suppress the maximum pressure at the upstream of the tunnel, the first vent position was set at 93.75%L. Then, the second or third vent was set at different positions, and five cases with different vent numbers and corresponding positions were determined, as is shown in Table 4.

**Table 4.** Maximum pressure in the tailrace tunnel with different numbers of vents.


Figure 6 shows the maximum pressure of the mixed free-surface-pressurized flow in the tunnel with vents. The results show that the maximum pressure in the tunnel was

56.006 mH2O for vent positions at 93.75%L and 56.25%L, which was reduced by 15.30% in comparison with the single-vent case. For the three vent positions at 93.75%L, 68.75%L, and 43.75%L, the maximum pressure in the tunnel was 55.398 mH2O, which was reduced by 16.22% in comparison with the single-vent case. It can be concluded that increasing the vent number can strengthen the suppression effect on the maximum pressure; however, more vents may influence the safety of the tunnel structure.

**Figure 6.** Water level with different numbers of vents: (**a**) 93.75%L/43.75%L, (**b**) 93.75%L/56.25%L, (**c**) 93.75%L/68.75%L, (**d**) 93.75%L/81.25%L, and (**e**) 93.75%L/68.75%L/43.75%L.

#### **4. Conclusions**

In the present work, the characteristic implicit method was used to investigate the mixed free-surface-pressurized flow in the tailrace tunnels of a hydropower station, and the main conclusions are as follows:


**Author Contributions:** Conceptualization, H.F., B.L.; methodology, H.F., B.L.; software, X.W.; validation, H.F. and X.W.; formal analysis, H.F. and X.W.; investigation, B.L.; resources, B.L.; data curation, X.W.; writing—original draft preparation, X.W.; writing—review and editing, H.F. and B.L.; visualization, B.L.; supervision, H.F.; project administration, H.F.; funding acquisition, H.F. All authors have read and agreed to the published version of the manuscript.

**Funding:** This work has been funded by the National Key R&D Program of China, grant number [2016YFC0401905], the National Natural Science Foundation of China, grant number [51879140], the Tsinghua-Foshan Innovation Special Fund, grant number (TFISF)[2020THFS0107], and the Creative Seed Fund of the Shanxi Research Institute for Clean Energy.

**Acknowledgments:** This work has been supported by the National Key R&D Program of China [2016YFC0401905], the National Natural Science Foundation of China [51879140], the Tsinghua-Foshan Innovation Special Fund (TFISF) [2020THFS0107], and the Creative Seed Fund of the Shanxi Research Institute for Clean Energy.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


### *Article* **Development of a Hydropower Turbine Using Seawater from a Fish Farm**

**Md Rakibuzzaman <sup>1</sup> , Sang-Ho Suh 2,\*, Hyoung-Ho Kim 3,\* , Youngtae Ryu <sup>4</sup> and Kyung Yup Kim <sup>5</sup>**


**Abstract:** Discharge water from fish farms is a clean, renewable, and abundant energy source that has been used to obtain renewable energy via small hydropower plants. Small hydropower plants may be installed at offshore fish farms where suitable water is obtained throughout the year. It is necessary to meet the challenges of developing small hydropower systems, including sustainability and turbine efficiency. The main objective of this study was to investigate the possibility of constructing a small hydropower plant and develop 100 kW class propeller-type turbines in a fish farm with a permanent magnet synchronous generator (PMSG). The turbine was optimized using a computer simulation, and an experiment was conducted to obtain performance data. Simulation results were then validated with experimental results. Results revealed that streamlining the designed shape of the guide vane reduced the flow separation and improved the efficiency of the turbine. Optimizing the shape of the runner vane decreased the flow rate, reducing the water power and increasing the efficiency by about 5.57%. Also, results revealed that tubular or cross-flow turbines could be suitable for use in fish farm power plants, and the generator used should be waterproofed to avoid exposure to seawater.


**Citation:** Rakibuzzaman, M.; Suh, S.-H.; Kim, H.-H.; Ryu, Y.; Kim, K.Y. Development of a Hydropower Turbine Using Seawater from a Fish Farm. *Processes* **2021**, *9*, 266. https://doi.org/10.3390/pr9020266

Academic Editor: Jin-Hyuk Kim Received: 31 December 2020 Accepted: 26 January 2021 Published: 30 January 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

**Keywords:** small hydropower; tubular turbine; fish farm; computational fluid dynamics; performance test; design factors; optimum model

#### **1. Introduction**

Hydropower is expected to remain the world's largest source of renewable electricity and to play a critical role in decarbonizing the power system and improving system flexibility. In 2016, world hydropower installed capacity was 1064 GW, and annual power generation was 3940 TWh [1]. Hydropower generation has been declining in Southeast Asia and the Americas due to continued drought caused by climate change. However, demand for hydroelectric power generation is increasing to cope with the increasing proportion of renewable energy and to adapt to increasing power demands from industrialization and the climate change crisis [2]. The hydropower industry is improving its efficiency, output, and system resilience through modernization, improving old facilities and renovating and expanding existing facilities [3,4]. Small scale hydropower development is being studied worldwide to improve technology to make it more reliable and economically efficient, which is necessary due to climate change, high oil prices, and environmental problems [2]. In addition, domestic small hydroelectric power generation technologies are being localized due to new and renewable energy certificates (RECs) and the sale of electric power in domestic institutions and corporations; a continuous decrease in the development unit price has also been affected by small and medium enterprises [3,5,6]. Therefore, particular attention should be paid to small scale hydropower plants operating in low head conditions [7,8], the significant possibility of which is still not fully identified.

Small hydropower (SHP) has been used to produce renewable, clean, and abundant energy [9]. In a study of SHP, Ma et al. conducted a study on runners to develop general purpose 2.5 kW micro-water vehicles [10]. Borkowski et al. validated computational fluid dynamics (CFD) on SHP with electrical generator integrated with experiments, and the main results were the mechanical power losses in the hydro-set gap and selection of suitable turbulence model [11]. Huidong et al. conducted a study on the possibility of replacing composite runner blades and mechanical stainless steel runner blades as a way to increase the economics of SHP in stream sites [12]. Wen-Quan et al. investigated the development of water turbines available in rivers through computational fluid dynamics [13]. Punys et al. [14], reviewed small scale hydropower resource assessment for the development of small hydropower plants using sophisticated software tools.

However, it represents only around 1.5% of the world's total installed electricity capacity, 4.5% of its total renewable energy capacity, and 7.5% (<10 MW) of its total hydropower capacity [15,16]. Currently, there are few possibilities to develop and construct small hydropower plants [17].

In Korea, fish farms operate approximately 600 units from the southern area, which is at 350 units, and Jeju Island, which is at 250 units. Fish farms are environmentally friendly, pollution-free, low cost, and guarantee the income of fishing villages. A small hydropower plant that produces from 20–500 kW can utilize surplus recirculated water from fish farms [18–20]. Propeller-type tubular turbines could be suitable for use in fish farm hydropower plants [21]. Propeller turbines have a simple structure and a fixed blade, the cost is relatively lower than that of the Kaplan turbine, and they have a high likelihood of successful use in small hydropower plants [22–25]. Li et al. [26], analyzed hydraulic performance according to the operating conditions of turbines through numerical analysis and studied the effects of the opening angle of the guide vanes.

CFD has been applied to the design of hydro turbines and can be used in numerical simulation to obtain hydraulic performance. Vu et al. [27] studied a Pico propeller hydro turbine using the old runner model and improved the performance of the turbine using CFD. Park et al. [28] studied the flow analysis of 30 kW gate turbines using a permanent magnetic generator as well as the dynamic behavior of the flow stability of operating conditions. Nasir, B. A. [29] was focused on the selection of suitable micro-scale hydropower plant components. In [30], the authors focused on preliminary studies of economic feasibility, the design of civil works, and the selection of electro mechanical components, and developed a 15 kW micro-scale hydropower plant for rural electrification. In [31], the authors investigated four different propeller turbine models with head ranges of 4–9 m and generated an efficiency of 68%. The efficiency of small hydropower plants is generally in the range of 60–80% [27]. In [32], the authors studied the fish passage experience and passage facilities, especially how fish friendly they were, at a small scale hydropower plant. However, the study did not show design and performance improvements in a micro-scale hydropower plant using seawater from a fish farm.

Therefore, this study has especially focused on the applicability of a 100 kW class small propeller-type turbine (with an annular permanent magnetic generator). It is intended to serve as a reference for researchers who want to approach this field in the future by conducting prior research on the development of SHP available in Korea's marine characteristics, such as fish farms, through computational fluid dynamics and certificated field tests. In addition, we intend to provide basic data on the possibility of hydrodynamic characteristic changes due to simple feature changes in draft tubes, guide vanes, and runner vanes, which are important components of SHP.

#### **2. Hydropower Turbine Design**

#### *2.1. Fish Farm Facilities*

In fish farm facilities, seawater is supplied through the water supply system by a pipeline 20–30 m above sea level. The water is recirculated for use in the fish farm and finally discharged through the discharge channel into the sea. Fish farm facilities are shown in Figure 1. The plan was to install the hydropower plant on a shared water surface along the coast. Therefore, data regarding sea level and tide observations was important for the development of the fish farm. Figure 2 illustrates the monthly average tide levels in the southern sea off the coast of Korea [33].

**Figure 1.** Fish farm facilities: (**a**) water supply system; (**b**) discharge water system; (**c**) fish farm.

**Figure 2.** Monthly average tidal status, Southern sea, Korea.

#### *2.2. Hydroturbine Design*

A horizontal propeller type tubular turbine was designed with nine fixed guide vanes, which were attached via a guide vane casing. Runner blades were directly attached to the end of the permanent magnet synchronous generator (PMSG) [34], and an s-shaped draft tube, which was chosen to ensure maximum recovery with minimum loss. The generator was designed to be installed on a shared seawater surface. The fish farm hydropower plant layout was chosen for its low head and flow rate, compact and simple mechanism, low maintenance needs, and environmental friendliness. Table 1 shows the major design parameters of the tubular turbine. When the one dimensional (1–D) design of the turbine was considered, specific speed (*NS*) was a meaningful parameter for identical geometric proportions if the sizes and speeds were different. The specific speed was expressed as follows:

$$N\_{\rm S} = N \frac{\sqrt{P}}{H^{5/4}} \tag{1}$$

where *N* is the turbine rotational speed in rpm, *H* is the net head in m, and *P* is the turbine power in kW. The choice of the blade rotational speed depends on the generator and the type of the drive used [35–37].

**Table 1.** Design specifications of the tubular turbine.


We considered two rotational speeds in this study, 600 rpm and 900 rpm. The turbine selection was referenced from the H–N<sup>S</sup> chart [37]. The chart shows that at 600 and 900 rpm, the specific speeds were 230 and 345 respectively. The diameter of the turbine is calculated as follows:

$$D = \frac{60k\_{\mu}\sqrt{2gH}}{\pi N} \tag{2}$$

where, *k<sup>u</sup>* is the non-dimensional blade velocity, and the value is 1.5~2 [35]. The main specifications of the turbine runner blade are shown in Table 2. The hub ratio was 0.5. The block diagram of the design process for the new propeller turbine model has been shown in Figure 3. The turbine design process used a trial and error-based algorithm with several times numerical analyses for optimum geometry [35].

**Table 2.** Main design parameters of the turbine blade.


**Figure 3.** Block diagram of the design process for the hydraulic turbine.

#### **3. Methodology**

The installation location of the small hydropower plant was the southern area of Korea. This fish farm was equipped with a water pump supply system. Seawater is recirculated into the fish farm and discharged through the discharge water channel. The installation facilities were designed to be installed in a shared water surface without a building, that is, they were environmentally friendly. A schematic installation diagram of the marine small hydropower plant has been shown in Figure 4.

**Figure 4.** Schematic installation diagram of an offshore small hydropower plant.

#### *3.1. Numerical Method*

3.1.1. Geometrical Model and Meshing

The three dimensional (3D) geometry of the horizontal prototype propeller type tubular turbine was selected to analyze the flow characteristics as shown in Figure 5. The 3D turbine model was meshed by ANSYS ICEM-CFX (16.2) software (16.2, ANSYS Inc.,

Canonsburg, PA, USA, 2016) The flexibility of the complex design of the hydraulic turbine allowed the unstructured prism tetrahedral grid system to be employed to make the grid. Overall, meshing grids comprised 1,192,047 nodes and 4,302,575 elements. Unstructured tetra-prim meshing grids have been shown in Figure 6. To precisely simulate the flow in a whole turbine channel, further grid refinement is required. However, the grid cannot be too large, which is needed for a comparatively fine grid, as numerical simulations lead to a considerable amount of computational data. To reduce the influence of grid number on computational results, a grid dependency study at the rated head (15 m) operating condition (GV 60◦ and RV 24◦ ) was conducted. This showed that the efficiency deviation was less than 1% [38,39], as shown in Figure 7. The grid independency test was carried out based on the grid convergence index (GCI) method [40–42]. With this, the approximate and extrapolated relative errors can be written as:

$$
\varepsilon\_d = \left| \frac{\varepsilon\_{new} - \varepsilon\_{old}}{\varepsilon\_{new}} \right| \times 100\% \tag{3}
$$

The grid convergence index can be calculated as

$$\text{GCI} = \frac{1.25 \times \varepsilon\_a}{r^2 - 1} \tag{4}$$

where *ε<sup>a</sup>* is the relative error and r is the mesh ratio.

**Figure 5.** Three dimensional (3D) geometry of a propeller type turbine: (**a**) turbine; (**b**) generator, runner, and guide vane; (**c**) dimension of runner.

**Figure 6.** Unstructured prism grids: (**a**) inlet pipe and generator; (**b**) guide vane; (**c**) runner; (**d**) draft tube.

**Figure 7.** Grid independency test of the tubular turbine (vertical dotted line represents the used grid).

The cells' finite volume approaches near the wall boundary are irregular, potentially requiring a special procedure. First, prisms create a layer near the wall of regular prisms and then mesh the remaining volume with tetrahedrons [39,43]. This grid approach improves the near walls and provides better solutions and convergence of computational methods [43].

The mesh quality of the tubular turbine is shown in Table 3. The estimated numerical uncertainties in the hydraulic turbine are shown in the Table 4. From the table, the 1,192,047 grid density showed higher efficiency with lower uncertainties compared to the other grid density. Therefore, 1,192,047 grid densities were selected as the final grid scheme for numerical computation. The Y+ contour of the runner and hub has been shown in Figure 8.


**Table 3.** Grid quality of the tubular turbine.

**Figure 8.** Y+ contour of the runner.


**Table 4.** Grid convergence uncertainties in the numerical solutions.

#### 3.1.2. Governing Equations

Numerical analysis of the fluid flow was based on continuity and momentum equations [44,45], which are expressed as:

$$\frac{\partial \mu\_i}{\partial x\_l} = 0 \tag{5}$$

$$\rho \left( \frac{\partial u\_i}{\partial t} + u\_j \frac{\partial u\_i}{\partial x\_j} \right) = -\frac{\partial p}{\partial x\_i} + \frac{\partial}{\partial x\_j} \left( \mu \frac{\partial u\_i}{\partial x\_j} - \rho \overline{u\_i' u\_j'} \right) \tag{6}$$

where *ρ* and *µ* are density and dynamic viscosity respectively, *p* is the pressure scalar, and −*ρu* ′ *i u* ′ *j* is the apparent turbulent stress tensor.

For numerical simulation, the tubular turbine domain was considered a steady-state, incompressible flow. The flow through the tubular turbine was simulated with the commercial code ANSYS-CFX (16.2) based on finite volume methods (FVM) [44]. The runner domain was rotating on the *z*-axis at a given rotating speed of 850 rpm, and the inlet pipe, generator, guide vane, and draft tube were a stationary domain.

Figure 9 shows the tubular turbine domain for the computer simulation. All boundary conditions were assumed as smooth walls with no-slip, and automatic wall functions were considered in the near wall region. Moreover, regular smooth wall functions were used, so that at a non-dimensional distance from the walls Y+ the first grids were placed. Near a no-slip wall, there are negative gradients in dependent variables, according to conventional theory. Also, the viscous effects on transport processes are relatively high; these measurements are spread across the wall-adjacent viscosity-affected sublayer. Computer performances and ability demands are greater than those of the wall function, and a certain strong computational resolution in the near-wall area can be taken care of to understand the rapid difference in variables [44]. An automated wall treatment mechanism has been developed by ANSYS-CFX to minimize the resolution requirements, allowing a gradual switch between wall functions and low-Reynolds number grids, without loss of precision [44]. The well-accepted way to account for wall effects is through wall functions. In CFX, an automatic near-wall treatment feature was reported in the near-wall region for *k-ω*–based models (including the SST model) [44,45].

**Figure 9.** Prototype turbine domain for computational analysis.

The static pressure boundary conditions were imposed on the inlet and outlet of 1.47 bar and −0.0245 bar. A frozen rotor was applied to couple the rotation and stationary domain. Menter's shear stress transport (SST) *k-ω* turbulence model [46,47] was used to solve the turbulence phenomena of the fluid. Also, the SST model accounts give highly accurate predictions of the onset and the amount of flow separation under adverse pressure gradients [46]. Advection term dealt with high-resolution discretization scheme, and the first-order upwind difference was used to solve the turbulence numeric. The residual value was 1 <sup>×</sup> <sup>10</sup>−<sup>5</sup> controlled by convergence criteria.

#### *3.2. Experimental Method*

The performance of the manufactured water turbine was measured in the field. Experimental measurements and calibrations were taken using the IEC-60193 procedure and guidelines [48]. The inlet pipe diameter was 925 mm. A pressure gauge at a range of 0~1 MPa was installed and located at the turbine upstream. Flow rates were measured by the differential pressure sensors located near the generator. The flow rate was measured based on the pressure differential chart provided by Korea Testing Certification (KTC). The experiment was carried out three times at 30 min intervals. The combined standard uncertainty in the hydraulic turbine is the effect of the standard uncertainty of the independent variable on the uncertainty of the flow rate. Unfortunately, only three measurement data for the degree of freedom (DoF) could not illustrate the 95% confidence limit and error propagation from the result (Table 5) [39]. Figure 10 illustrates the experimental layout and devices of the small hydropower plant at the fish farm.

**Table 5.** Comparison of experimental and simulation test results of the tubular turbine.


**Figure 10.** Experimental layout and devices: (**a**) pressure and temperature sensor; (**b**) offshore small hydro power plant.

#### **4. Results and Discussion**

#### *4.1. Validation of Numerical Results*

Numerical simulations were validated with experimental data. Table 5 illustrates CFD performance and experimental results for the tubular turbine. As shown in Table 6, the average deviation of the head was 0.231%, and the flow rate deviation was only 2.105% at a rotational speed of 496 rpm [39,49]. The power output and efficiency of the turbine were different due to the different runner vane openings in the experiment and simulation. The power and efficiency of the measuring procedure were different due to the different runner vane angles in the experiment and simulation. Also, in simulation, we did not take into account the bearing and generator loss. In a hydraulic system, the three kinds of losses are hydraulic loss, shaft loss, and generator or bearing loss. However, in the simulation, we only considered the hydraulic part, as shown in Figure 11, that included hydraulic and shaft losses. Also, different runner vane openings were used in the simulation because when it created the exact opening angle, the runner blades were crossed the interface between the guide vane outlet and runner vane inlet. If it could happen in the computer-aided design (CAD) model, the simulation would not run by the ANSYS-CFX solver. Therefore, we solved this issue as much by opening the runner vane angle which was closed to the experimental vane opening. When the runner vane opening angle was 24◦ , and the guide vane opening angle was 60◦ , the power output was 97.13 kW. As the opening angle of the runner vane decreased, efficiency increased, but flow rate and power decreased. When the opening angle of the guide vane angle was 40◦ , and the opening angle of the runner vane was 19◦ ; maximum power output (128.78 kW) was possible under a flow condition of 1.13 m3/s. Further review of this part is needed. With an efficiency of 79.90% in close proximity, the runner vane angle was between 26◦ and 28◦ . However, power and flow decreased. A field performance test was conducted under the environmental conditions of 1024 kg/m<sup>3</sup> , a working dry temperature of 26 ◦C, a relative humidity of 74%, and an atmospheric pressure of 101 kPa. Turbine output obtained from the field performance test was 98.7 kW, and the overall efficiency of the hydraulic turbine was 79.90%, which was 3.9% higher than the guaranteed efficiency of 76%. The turbine efficiency curve is shown in Figure 12 as a comparison between the expected efficiency of the computer simulation and the efficiency obtained from the field performance test.

**Table 6.** Performance according to guide vane shape (H = 14.84 m).


**Figure 11.** Different losses in the hydraulic turbine (P<sup>w</sup> = hydraulic power, P<sup>s</sup> = shaft power, and P<sup>G</sup> = generator power).

**Figure 12.** Comparison of turbine efficiency across various runner vane opening angles.

#### *4.2. Performance Characteristics*

Computer simulations were conducted at different flow rates by changing the guide vane and runner vane opening angles of the tubular turbine. Guide vane opening angles varied from 40◦~60◦ , and runner vane opening angles varied from 14◦~24◦ . Figures 13 and 14 show the efficiency, flow rate, and power performance characteristics of the tubular turbine with different runner vane and guide vane opening angles. In the graph, maximum efficiency was 81.67%, and power output was 101.54 kW at a flow rate of 0.854 m3/s. In this case, the runner vane opening angle was 14◦ , and the guide vane opening angle was 50◦ . As the runner vane angle increased, the flow rate increased linearly, and the power increased sharply as shown in Figure 14. Also, when runner vane and guide vane angles varied to maximum (fully open, Figures 13 and 14), efficiency was low (67.13%), and power was 97.13 kW at a flow rate of 0.994 m3/s.

**Figure 13.** Efficiency changes according to runner vane and guide vane opening angles.

**Figure 14.** Flow rates, power versus runner vane, and guide vane opening angles.

The rated flow rate was found when the runner vane opening angle was 19◦ , and the guide vane opening angle was 40◦ . In this case, efficiency was found to be 78.44%, and power output was 128.78 kW at a flow rate of 1.13 m3/s. Figure 15 shows the blade-toblade pressure and velocity (magnitude) distributions at a 0.5 span (non-dimensional blade height = 0.5). In this figure, the dotted circle represents the leading edge and trailing edge of the runner blade. The pressure was maximum, and the velocity was minimum at the leading edge of the pressure side. Velocity was not distributed uniformly from the leading edge to the trailing edge of the runner vane. Velocity decreased at the trailing edge of the runner vane, and a small vortex formed in this region.

**Figure 15.** Blade-to-blade pressure and velocity contours (span = 0.5).

Figure 16 shows the velocity vector and streamlines of the blade-to-blade guide and runner vane. The figure shows that the guide vane makes the flow pattern non-uniform through the runner vane, and this phenomenon could not reach the desired value. A vortex was also formed near the front of the guide vane and a recirculating flow occurred. Large recirculation flow occurred near the hub of the runner outlet [49].

**Figure 16.** Blade-to-blade velocity vector and velocity streamlines (span = 0.5).

#### *4.3. Design Modification for Performance Improvement of Turbine* 4.3.1. Shape of Guide Vanes

The performance of guide vanes with short and long chords was compared. Figure 17 shows the cross-section before and after the shape of the guide vane was changed. The vane-to-vane streamlines distribution of guide vanes and runner vanes are shown in Figure 18. In Figure 18, a vortex occurred at the leading edge of the guide vane in both the short and long blade chords. When the blade chord was long, the pressure difference between the leading edge and the trailing edge of the guide vane was large, but the size of the recirculation area was slightly reduced. Additionally, velocity decreased slightly in the leading edge of the guide vane.

**Figure 17.** Shapes of short and long guide vanes.

Table 6 shows performance characteristics according to guide vane shape. As the size of the blade chord of the guide vane increased, flow rate decreased, as a result of reducing the water power and shaft power and increasing the efficiency by 0.56%. Compared to guide vanes with short chords, guide vanes with long blade chords had lower flow rates due to the change in pressure distribution, even though the recirculation area was slightly reduced. Figure 19 shows the turbine loss analysis. From a loss analysis point of view, efficiency changed generally around 1–2% according to changes in the length of the guide vane. Additionally, it was more important to change the shape of the runner vane than the shape of the guide vane.

**Figure 18.** Vane-to-vane velocity streamline distribution of guide vanes and runner vanes: (**a**) at short chord; (**b**) at long chord.

**Figure 19.** Turbine loss analysis.

The optimum total efficiency depends on the design and operating conditions of turbine, it is especially important to reduce the main losses which are divided the losses into frictional and kinetic parts. Loss analysis states that loss due to runner is a mainly large part of the number of losses and determines hydraulic overall efficiency [37,50]. Therefore, it is necessary to first look at the efficiency changes caused by the change in runner shape and analyze the effects of the closely related guide vane shape changes. From a loss analysis point of view, efficiency changed generally around 1–2% according to changes in the length of the guide vane. The flow rate into the runner is controlled by the shape of the guide vanes. As a result, the velocity triangles in the runner will vary from section to section. Thus, it was more important to change the shape of the runner vane than the shape of the guide vane.

#### 4.3.2. Guide Vanes Attached to the Generator Side

Figure 20 shows that the guide vane is attached to the generator side when the chord is short. Figure 21 shows the vane-to-vane pressure and streamline distribution of the guide vane and runner vane. Table 7 shows performance characteristics of the guide vane attached to the generator side. Results showed that efficiency increased by 1.33% when guide vanes were attached to the generator side. However, a vortex flow occurred at the front of the guide vane, and a large pressure drop appeared.

**Figure 20.** Guide vane attached to the generator side (short chord).

**Figure 21.** Vane-to-vane pressure and streamline distribution of guide vanes and runner vanes: (**a**) pressure contours; (**b**) streamline contours.

**Table 7.** Performance of guide vane attached to the generator side (short chord, H = 14.84 m).


4.3.3. Streamlining the Shape of the Guide Vane

(1) In the case of a short cord

In this investigation, the shape of the guide vane was changed to a streamlined shape. Figure 22 illustrates a cross-sectional view of the guide vane's streamlined shape. Figure 23 shows the vane-to-vane streamline distributions of guide vanes and runner vanes. Changing the streamline shape of the guide vane improved its pressure distribution. As shown in the streamline diagram (Figure 23), flow separation was also reduced due to the streamlined shape around the front of the guide vane, improving the efficiency of the

turbine. Table 8 shows performance characteristics of guide vanes with a streamlined shape when the wing string was short. After guide vanes were streamlined, efficiency decreased, and the rated flow rate was not reached. Changing the opening degrees of guide vanes and runner vanes to bring out the rated flow increased efficiency by 0.21%. It was believed that efficiency did not increase much, because the shape of the leading edge of the runner vane was designed incorrectly.

**Figure 22.** Changing the shape of guide vanes with short chords to make them streamlined.

**Figure 23.** Vane-to-vane streamline distribution of guide vanes and runner vanes: (**a**) streamline distribution before shape change; (**b**) streamline distribution after shape change.

**Table 8.** Performance characteristics according to guide vane shape (short chord, H = 14.84 m).


(2) In the case of long chords

In this investigation, the long chord shape of the guide vane was chosen. Figure 24 shows the vane-to-vane pressure and streamlines distributions of guide vanes and runner vanes. The flow separation was disappeared from the guide vane. Table 9 illustrates the performance characteristics of streamlined guide vanes when the wing string was long. In Table 9, efficiency changes were insignificant in the case of short and long chords.

**Figure 24.** Vane-to-vane pressure and streamline distribution of guide vanes and runner vanes when chords were long: (**a**) pressure distribution; (**b**) streamline distribution.



#### 4.3.4. Runner Vane Shape

The shape of the runner vane was changed as shown in Figure 25. Table 10 shows the performance characteristics of different runner vane shapes. Flow rate decreased according runner vane shape, reducing the water power and increasing the efficiency by about 5.57%.



**Figure 25.** Changing the shape of the runner vane.

When the opening angle of the guide vane and runner vane was changed to reach the rated flow rate (1.131 m3/s), efficiency increased by 4.47%. Figure 26 shows the vaneto-vane pressure and streamline distribution of guide vanes and runner vanes. In the figure, flow separation disappeared after changing the shape of the runner vane. Also, performance characteristics of turbines with different shapes were compared. Figure 27 shows the efficiency and flow performance characteristics of guide vanes with different opening degrees (GV-38◦ and GV-40◦ ). Results showed that efficiency was lower in short guide vanes than in long guide vanes.

**Figure 26.** Pressure and streamline distribution between guide vanes and runner vanes: (**a**) pressure contour after shape change; (**b**) streamline contour after shape change.

**Figure 27.** Comparison of efficiency and flow rate according to guide vane opening (RV-19~24◦ ).

#### 4.3.5. Rotational Speed

The performance characteristics of generators with different rotational speeds were investigated. When the generator ran at 850 rpm, the tubular turbine would not operate functionally, and an increase in vibration could stop the hydroelectric power plant. Therefore, a reduced rotational speed was considered to stabilize the turbine operation. Table 11 shows the performance of runner vanes with different rotation speeds. In the table, efficiency gradually decreased as rotational speed decreased. The flow rate and output also decreased sharply. There was no major change in efficiency (only 0.86% difference) when the rotation speed was 650 rpm.


**Table 11.** Performance characteristics according to runner vane rotation speed (H = 14.84 m, GV-40◦ ).

The effect of tidal level on the turbine was investigated. Figure 28 shows changes in performance characteristics according to the rotational speed and tidal level (high and low tide). At higher tides, the efficiency and flow rate of the turbine was slightly higher than at low tides for different rotational speeds. There was a remarkable power output difference between high and low tides (Figure 28c).

**Figure 28.** Performance changes according to rotational speed and tidal level: (**a**) rotational speed versus flow rate; (**b**) rotational speed versus efficiency; (**c**) rotational speed versus power.

#### 4.3.6. Optimum Model

After changing the shape of the turbine draft tube, performance characteristics were reviewed. Efficiency after the shape modification of the draft tube was 77.67%, which was 0.98% less than efficiency before modification. The influence of the shape of the draft tube on efficiency was insignificant. Performance changes when the guide vane was changed to short and long blade strings were examined. Vortex flow occurred at the leading edge of the guide vane for both short and long blade strings. As flow rate decreased, the difference in efficiency in the case of power was within the error range. Efficiency increased by 1.33% when guide vanes were attached to the generator side. Streamlining the shape of the guide vane improved the pressure distribution around it. Streamlining the shape around the front side of the guide vane reduced flow separation and improved efficiency. Changing the shape of the guide vane made the recirculation zone and flow separation disappear when blade chords were both long and short. However, it was more important to change the shape of the runner vane than the shape of the guide vane. Changing the runner vane shape increased efficiency by 4.47%, and the rated flow rate emerged at a runner vane opening angle of 24◦ . When comparing the performance characteristics of runner vanes with long and short chorded guide vanes, the efficiency of short guide vanes was lower than that of long guide vanes.

The optimized runner vane and guide vane angles were RV-24◦ and GV-40◦ , respectively. Design specifications were considered for the manufacture and development of the fish farm power plant. At a rotational speed of 850 rpm, the flow rate was 1.101 m3/s, output was 133.43 kW, and efficiency was 83.41%. At a rotation speed of 650 rpm, stable performance was obtained. In this case, the flow rate was 0.994 m3/s, output was 114.03 kW, and efficiency reached 78.75%.

#### **5. Conclusions**

This study investigated the applicability of using fish farm recirculating discharge water. A new prototype propeller type tubular turbine was designed, and a CFD analysis was carried out to analyze its performance. Numerical simulations were validated with experiments using the IEC-60193 procedure. Various design parameters were investigated to determine the rated flow rate at the best efficiency. When runner vane and guide vane angles varied to the maximum (fully open), efficiency was low (67.13%), and power was 97.13 kW at a flow rate of 0.994 m3/s. With smaller runner vane opening angles, efficiency increased, but flow rate and output decreased. The maximum output (133.43 kW) was reached at a flow rate of 1.13 m3/s when the opening angle of the guide vane angle was 40◦ , and the runner vane opening angle was 19◦ . In this case, turbine efficiency was 78.44%. Recirculation formed near the front of the guide vane and rear of the hub. Velocity streamline distributions of the turbine were distributed non-uniformly. The tubular turbine was optimized using computer simulation to modify the shapes of runner and guide vanes, opening angles, and so on. From a loss analysis point of view, the runner component was the main part of the loss, more than the guide vane component. Thus, total efficiency sharply increased when the shape of the runner vane changed. Optimized runner vane and guide vane angles were RV-24◦ and GV-40◦ , respectively. The guide vane should be fixed, and the runner vane should be adjustable, so the vane angle can be adjusted according to the installation location. Turbine performance was optimized satisfactorily. Tubular or cross-flow type turbines are suitable for use in fish farm power plants, and generators should be waterproofed to prevent exposure to seawater. Using renewable energy from the circulated water of fish farms could meet the challenges faced during the development of hydroelectric power plants.

**Author Contributions:** M.R. conceived and designed the study, analyzed the results, wrote the paper, and edited the draft; S.-H.S. contributed to project administration, conceptualization and supervised the work; H.-H.K. managed resources and edited the draft; Y.R. contributed to fund acquisitions and resources the work; and K.Y.K. managed resources, fund acquisition, and advised on project work. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by the Korea Technology and Information Promotion Agency for SMEs (TIPA), grant number S8025391, and the article processing charge (APC) was funded by grant number S8025391.

**Data Availability Statement:** The data that support the findings of this study are available from the corresponding author, upon reasonable request.

**Acknowledgments:** This research was supported by TIPA. The grant number was S8025391 for the promotion of science. Authors also extend their gratitude to Hyung-Woon Roh for his assistance during the project work.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Abbreviations**



#### **References**


**Mengcheng Wang , Yanjun Li \*, Jianping Yuan and Fareed Konadu Osman**

National Research Center of Pumps, Jiangsu University, Zhenjiang 212013, China; jdwmc2018@163.com (M.W.); yh@ujs.edu.cn (J.Y.); 5102190340@stmail.ujs.edu.cn (F.K.O.)

**\*** Correspondence: lyj782900@ujs.edu.cn; Tel.: +86-150-0610-9630

**Abstract:** When considering the interaction between the impeller and diffuser, it is necessary to provide logical and systematic guidance for their matching optimization. In this study, the goal was to develop a comprehensive matching optimization strategy to optimize the impeller and diffuser of a mixed flow pump. Some useful tools and methods, such as the inverse design method, computational fluid dynamics (CFD), design of experiment, surrogate model, and optimization algorithm, were used. The matching optimization process was divided into two steps. In the first step, only the impeller was optimized. Thereafter, CFD analysis was performed on the optimized impeller to get the circulation and flow field distribution at the outlet of the impeller. In the second step of optimization, the flow field and circulation distribution at the inlet of the diffuser were set to be the same as the optimized impeller outlet. The results show that the matching optimization strategy proposed in this study is effective and can overcome the shortcomings of single-component optimization, thereby further improving the overall optimization effect. Compared with the baseline model, the pump efficiency of the optimized model at 1.2*Q*des, 1.0*Q*des, and 0.8*Q*des is increased by 6.47%, 3.68%, and 0.82%, respectively.

**Keywords:** inverse design method; matching optimization; diffuser; impeller; flow field

**Citation:** Wang, M.; Li, Y.; Yuan, J.; Osman, F.K. Matching Optimization of a Mixed Flow Pump Impeller and Diffuser Based on the Inverse Design Method. *Processes* **2021**, *9*, 260. https://doi.org/10.3390/pr9020260

Academic Editor: Jin-Hyuk Kim Received: 27 December 2020 Accepted: 26 January 2021 Published: 29 January 2021

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

#### **1. Introduction**

As one of the most important machines in modern civilization, the performance of rotating machinery will have a great influence on the development of wider society. Published data in the Annual Work Report of the Chinese Government in 2019 revealed that more than 98% of the country's electric power conversion is done by rotating machinery. Consequently, a marginal increase in the efficiency of rotating machinery will produce unimaginable economic benefits. For instance, in China, for every 1% increase in rotating machinery efficiency, about 70 billion kilowatts of electricity can be saved annually. As a kind of rotating machinery, mixed flow pumps play an important role in industrial production, agricultural irrigation, and urban drainage due to their moderate head, wide high efficiency range, and good anti-cavitation performance. Thus, it is of great significance to study the optimization design of mixed flow pumps.

In the field of rotating machinery optimization, computational fluid dynamics (CFD) prediction is a better method than experimental investigation, because the former is more convenient and cheaper [1]. More importantly, CFD prediction can provide flow details inside the rotating machinery, which can help designers better understand the reasons for performance changes and make targeted optimization [2]. However, CFD prediction cannot directly provide the optimal solution for the optimization of rotating machinery. Like most complex optimization problems, the optimization of rotating machinery usually entails multiple indicators, and each target affects the other. Therefore, considering the multi-objectivity of the rotating machinery optimization is inevitable [3]. Several attempts have been made to solve the above problem. Eventually, the method of combined optimization strategy consisting of CFD, design of experiment (DOE), surrogate models, and

optimization algorithms came to the fore and achieved satisfactory results. Meng et al. [4] combined CFD, Latin hypercube sampling (LHS), a two-layer artificial neural network (ANN), and a non-dominated sorting genetic algorithm (NSGA) to successfully improve the reverse operation performance of the axial flow pump without reducing the forward flow performance. Shi et al. [5] applied LHS, the response surface method (RSM), and an adaptive mutation probability genetic algorithm (AMGA) to the multi-disciplinary optimization of the axial flow pump. This effectively reduced the weight of the blade and enhanced its hydraulic efficiency on the premise of meeting the requirements of blade strength. Pei et al. [6] and Wang et al. [7] used LHS, ANN and modified particle swarm optimization (MPSO) to optimize the impeller and diffuser of a centrifugal pump, and widen the high efficiency area. Shim et al. [8] optimized the efficiency, cavitation, and stability of a centrifugal pump by combined usage of LHS, kriging model, and NSGA. Kim et al. [9] studied the influence of hub ratio on the performance of the mixed flow pump at the same specific speed through the combined optimization strategy. Suh et al. [10] combined central composite design (CCD), RSM, and sequence quadratic program (SQP) to improve the efficiency and cavitation performance of mixed flow pumps at the design point.

In the above optimization, the parameterization of the impeller is completed by geometric parameters. With the development of computational fluid dynamics, the use of hydrodynamic parameters to parameterize the impeller has shown great potential. This technique is also known as the inverse design method (IDM). In IDM, the blade shape is controlled by blade loading, circulation, and stacking condition. Compared with the former, the latter requires fewer design parameters and has a closer relationship between design parameters and hydraulic performance [11]. Goto et al. [12] and Zangeneh et al. [13] ascertained the efficacy of IDM in mixed flow pump design by simulation and experiment. Huang et al. [14] improved the head and efficiency of the mixed flow pump at design point by using IDM, LHS, radial basis neural network (RBNN), and NSGA. Yiu et al. [15] increased the mixed flow pump efficiency and suction performance by combined usage of IDM and a genetic algorithm (GA). Zhu et al. [16] optimized the pressure distribution of the compressor through IDM, GA, and adjoint method, thus expanding its high efficiency area. The efficiency, stability, and cavitation performance of pump as turbine were improved by combining the use of IDM, DOE, RSM/RBNN, and NSGA [17–20].

There is a common point in the above studies, which is only the impeller or diffuser was optimized in each study, and the interaction between the two was ignored. Only a few kinds of research have studied the matching optimization of impeller and diffuser. Bonaiuti et al. [21] studied the simultaneous optimization of compressor impeller and diffuser through five loading parameters. Subsequently, in another work [22], by optimizing the diffuser first and then the impeller, the matching optimization of a waterjet pump diffuser and impeller was studied by the trial-and-error method. Yang et al. [23] investigated the influence of blade loading on the impeller and diffuser of the submersible axial-flow pump. However, due to the particularity of IDM, there are still some defects in these matching optimization studies. In IDM, the flow field and circulation distribution at the diffuser inlet are two important input parameters. To reduce the hydraulic losses, the flow field and circulation distribution at the diffuser inlet should be set to be the same as the impeller outlet [24]. Therefore, in the matching optimization of impeller and diffuser, the impeller should be optimized before the diffuser was optimized.

This study aims to provide systematic guidance for the matching optimization of a mixed flow pump impeller and diffuser based on IDM. Firstly, the mixed flow pump design specification and matching optimization strategy were introduced, and the accuracy of the CFD analysis was verified. Then, the strategy was applied to the matching optimization of the impeller and diffuser, and the key points of matching optimization were introduced. Finally, the optimization mechanism was clarified by a comparative analysis of the internal flow field of the two models.

#### **2. Mixed Flow Pump Model**

The mixed flow pump as shown in Figure 1 was selected as the baseline model, which consists of an outlet elbow, a seven-blade diffuser, a four-blade impeller and a straight inlet pipe. The design flow rate *Q*des is 0.4207 m3/s, the design head *Hdes* is 12.66 m, the rotational speed *N* of the impeller is 1450 r/min, and the specific speed *n<sup>s</sup>* can be calculated by Equation (1): ܪௗ௦ ܰ ݊<sup>௦</sup> des s 0.75 3.65 ܪௗ௦ ܰ ݊<sup>௦</sup> des 3.65

**2021**, , x FOR PEER REVIEW 3 of 16

**2021**, , x FOR PEER REVIEW 3 of 16

$$m\_{\rm s} = \frac{3.65 N \sqrt{Q\_{\rm des}}}{H^{0.75}} \tag{1}$$

The performance of the baseline model was tested by Tianjin experimental bench, China. On the test bench, an intelligent differential pressure transmitter and intelligent torque speed sensor are used to measure head and torque, respectively. These devices yielded measurement errors of <±0.1%. Also, an intelligent electromagnetic flowmeter is used to measure flow rate, and the measurement errors is <±0.2%. The random uncertainty and overall uncertainty of this test bench are less than 0.1% and 0.3%, respectively. The test results shown in Figure 2 show that the efficiency of the baseline model at the design point is 86.3%. In this figure, *Q*<sup>∗</sup> = *Q*/*Q*des is the normalized flow rate, and *H*<sup>∗</sup> = *H*/*H*des is the normalized head. (The same dimensionless method was used in other parts of this paper.) . ܳ ܪ ୱୢୣ ܳ⁄ ܳ<sup>∗</sup> = <sup>∗</sup> = ୱୢୣ ⁄ܪ ܪ . ܳ ܪ ୱୢୣ ܳ⁄ ܳ<sup>∗</sup> = <sup>∗</sup> = ୱୢୣ ⁄ܪ ܪ

**Figure 1.** Baseline model.

**Figure 2.** Performance curves for the baseline model.

#### **3. Optimization Strategy**

As shown in Figure 3, the optimization system was built by combining the IDM, CFD, optimal Latin hypercube sampling (OLHS), RSM, Multi-island genetic algorithm (MIGA) and NSGA-II. The entire optimization process was divided into two steps. In the first step

of optimization, only the impeller was optimized, and the objective function was set as the impeller weighted efficiency at 1.2*Q*des, 1.0*Q*des and 0.8*Q*des. Thereafter, CFD analysis was performed on the optimized impeller to get the circulation and flow field distribution at the outlet of the optimized impeller. In the second step of optimization, the diffuser was optimized, and the objective functions were the levels of pump efficiency at 1.2*Q*des, 1.0*Q*des and 0.8*Q*des. To improve the optimization effect of this step, the flow field and circulation distribution at the inlet of the diffuser were set to be the same as the optimized impeller outlet. Ⅱ.

**2021**, , x FOR PEER REVIEW 4 of 16

**Figure 3.** Flowchart of optimization strategy.

#### *3.1. 3D Inverse Design Method*

<sup>ఏ</sup>ܸݎ)∂ തതത) ∂݉ ⁄

<sup>ఏ</sup>ܸݎߨ2 <sup>ఏ</sup>ܸݎ The parameterization of the impeller is done by the inverse design software TURBOdesign 6.4 developed by Advanced Design Technology. In this procedure, we assume that the fluid is steady, inviscid and uniform, so that the only vorticity is the bound vorticity on the blades, and its strength was determined by a specified distribution of circumferentially averaged swirl velocity *rV<sup>θ</sup>* (directly related to the bound circulation 2*πrV<sup>θ</sup>* ) [11,25]:

$$r\overline{V\_{\theta}} = \frac{B}{2\pi} \int\_{0}^{\frac{2\pi}{B}} rV\_{\theta} \mathbf{d}\theta \tag{2}$$

ݎ ܤ <sup>ఏ</sup>ܸݎ Here, *rV<sup>θ</sup>* , *B*, and *r* are the circumferentially averaged velocity, blade numbers, and radius, respectively.

0

<sup>ఏ</sup>ܸݎ When the meridional shape and the distribution of *rV<sup>θ</sup>* are given, the pressure field in the blade passage can be calculated by the meridional derivation of circulation *∂ rV<sup>θ</sup>* /*∂m*:

$$p^{+} - p^{-} = \frac{2\pi}{B} \rho \overline{\mathcal{W}\_{\text{m}}} \frac{\partial r \overline{V\_{\theta}}}{\partial m} \tag{3}$$

θ m <sup>୫</sup>ܹ ݉ ߩ ି − ା Here, *p* <sup>+</sup> <sup>−</sup> *<sup>p</sup>* −, *ρ*, *m*, and *W*<sup>m</sup> are pressure difference across the blade, fluid density, normalized streamline on the meridional shape, and pitch-wise averaged relative velocity, respectively.

The blade shape can be calculated by the following equation:

$$(\overline{V\_z} + v\_{zbl})\frac{\partial f}{\partial z} + (\overline{V\_r} + v\_{rbl})\frac{\partial f}{\partial r} = \frac{r\overline{V\_\theta}}{r^2} + \frac{v\_{\theta bl}}{r} - \omega \tag{4}$$

Here, *v* and *V* are the periodic velocity and circumferential average velocity, respectively, and subscripts *r* and *z* represent the radial and axial components of velocity, respectively. *f* is the blade wrap angle that is *θ* value at the blade between the leading edge and trailing edge.

#### *3.2. CFD Analyses and Validation*

In this study, CFD analyses have the following three functions: one is to calculate the objective functions, the other is to analyze the flow field distribution of the optimized impeller and provide inlet flow field information for diffuser optimization, and the third is to verify the final optimization results. Therefore, the accuracy of CFD analyses is critical to the reliability of this work.

Thus, 3D steady incompressible Reynolds-Averaged Navier–Stokes (RANS) equation was used in the full-passage simulation of the mixed flow pump. The RANS equation was solved by the shear stress transport *k* − *ω* turbulence model, because this model has the advantage of accurately calculating the internal flow pattern of the mixed flow pump [26]. A high-resolution scheme was selected to discretize the convective-diffusion terms [27]. The mass flow rate was set at the inlet, and the static pressure was set at the outlet. The frozen rotor frame of reference was adopted at the interface between the stationary and rotating domains. The convergence criteria were set to 5 <sup>×</sup> <sup>10</sup>−<sup>5</sup> .

The discretization of the computational domain is the basis of CFD analysis. In this study, the discretization of the computational domain is completed by structured grids, which have the advantages of controllable quality and quantity compared to unstructured grids. Mesh refinement was performed to all walls to ensure a small Y+ near the wall, O-type grids were used near the blade surface, and H/C-type grids were used near the blade edge. The meshing of the entire computational domain was completed by hexahedral grids as shown in Figure 4. Table 1 shows the results of the mesh independence analysis by using the same boundary conditions and governing equations. When the total number of grids is greater than 4.71 million, the head and efficiency reveal a small difference with the increase in grid numbers. Meanwhile, the maximum Y+ on the blades is no more than 65.

To verify the accuracy of the CFD analysis, the baseline model was numerically calculated using the above grid division and calculation setting, and the results are shown in Figure 2. The maximum head difference does not exceed 4% and the maximum efficiency difference does not exceed 2.5%. Therefore, the numerical simulation method adopted in this study is reliable.



**Figure 4.** Mesh of computational domains.

#### *3.3. Optimization Process*

The optimization process can be accelerated by constructing the approximate model between optimization objectives and design parameters. In this study, the second-order RSM was used to construct the approximate model:

$$y = a\_0 + \sum\_{i=1}^{N} a\_i \mathbf{x}\_i + \sum\_{i=1}^{N} a\_{ii} \mathbf{x}\_i^2 + \sum\_{i \neq j}^{N} a\_{ij} \mathbf{x}\_i \mathbf{x}\_j \tag{5}$$

ߙ ߙ ߙ ߙ Here, *α*0, *α<sup>i</sup>* , *αii* and *αij* are the undetermined coefficients and can be obtained by the least square method from the optimization objectives and design parameters.

In DOE, the optimal Latin hypercube sampling (OLHS) method was employed to generate the random, equiprobable, and orthogonally distributed sample points [28]. The structure of the sample space is consistent with the design space, which helps to reduce the number of calculation times.

A genetic algorithm (GA) was used for global optimization in the entire design space. In GA, crossover and mutation were adopted to ensure that the final result is the global optimal solution. Generally, the two main strategies for solving multi-objective optimization problems are the aggregation approach [29] and Pareto front [30]. Compared with the Pareto front, the aggregation approach has lower complexity because it converts the multi-objective optimization problem into a single-objective optimization problem through the weighted average method. However, in Pareto front, the nature of the tradeoffs between optimization objectives can be more intuitively reflected.

The optimization process starts from the selection of the optimization objectives and design parameters. After determining the range of the design parameters, OLHS was used to generate different combinations of design parameters. Thereafter, IDM was used to perform 3D modeling for each parameter combination, and CFD analysis was used to calculate the model optimization objectives. Then, RSM was used to construct the approximate model between optimization objectives and design parameters. Finally, GA was used to determine the global optimal solution.

#### **4. Redesign Setting**

#### *4.1. Design Parameters*

In this study, no changes have been made to the meridional shape of the mixed flow pump; thus, the mixed flow pump can be parameterized by the parameterization of the blade. As described in Section 3.1, circulation, blade loading, and stacking have the

greatest effect on blade shape in IDM. As a result, these parameters were selected as design parameters.

**2021**, , x FOR PEER REVIEW 7 of 16

Generally, we assume that the circumferential distribution of the circulation is uniform. Therefore, the three-dimensional distribution of the circulation can be simplified to a twodimensional distribution along the spanwise. Wang et al. [31,32] and Chang et al. [33] pointed out that the non-linear circulation distribution has more advantages than the linear circulation distribution in the mixed flow pump optimization design. Therefore, the curve shown in Figure 5 was used to control the circulation distribution with controlled parameters of *rV*<sup>h</sup> and *rV*s. In this figure, *rV*f*<sup>θ</sup>* <sup>=</sup> *rVθ*/*ω*<sup>2</sup> *r*shroud is the normalized circulation, and <sup>e</sup>*<sup>r</sup>* <sup>=</sup> (*<sup>r</sup>* <sup>−</sup> *<sup>r</sup>*hub)/(*r*shroud <sup>−</sup> *<sup>r</sup>*hub) is the normalized spanwise distance. <sup>ఏ</sup>ܸݎ = <sup>ఏ</sup>෪ܸݎ <sup>ୱ</sup>ܸݎ <sup>୦</sup>ܸݎ തതത/߱<sup>ଶ</sup> ୢ୳ୱ୦୰୭ݎ (ୠ୳୦ݎ − ୢ୳ୱ୦୰୭ ⁄ ݎ) (ୠ୳୦ݎ − ݎ) =̃ݎ <sup>ఏ</sup>ܸݎ = <sup>ఏ</sup>෪ܸݎ <sup>ୱ</sup>ܸݎ <sup>୦</sup>ܸݎ തതത/߱<sup>ଶ</sup> ୢ୳ୱ୦୰୭ݎ (ୠ୳୦ݎ − ୢ୳ୱ୦୰୭ ⁄ ݎ) (ୠ୳୦ݎ − ݎ) =̃ݎ

**Figure 5.** Circulation distribution at the impeller outlet and diffuser inlet.

݉=݉ ݉⁄ ୲୭୲ୟ୪ ܴܸܶܦ ܭ ܦܰ ܥܰ The blade loading distribution is usually controlled by two parabolas and a connecting straight line as shown in Figure 6, where *<sup>m</sup>*<sup>e</sup> <sup>=</sup> *<sup>m</sup>*/*m*total is the normalized meridional distance. The control parameters are the loading *DRVT* at the leading edge, the locations *NC* and *ND* of the connection point, and the slope *K* of the middle straight line. ݉=݉ ݉⁄ ୲୭୲ୟ୪ ܴܸܶܦ ܭ ܦܰ ܥܰ

**Figure 6.** Blade loading distribution along the streamline.

ߙ ߙ The stacking condition *α* shown in Figure 7 is usually imposed linearly along the blade trailing edge. Zangeneh [13] pointed out that it plays an important role in suppressing the flow separation in mixed flow pump. Zhu [34] also reported that it has a greater influence on the pressure pulsation in the impeller.

**Figure 7.** Stacking condition.

#### *4.2. Optimization Setting*

ܵ<sup>୫୧୬</sup> = (ܰ + 1) × (ܰ + 2) 2⁄ 2ܵ<sup>୫୧୬</sup> To determine the undetermined coefficients in Equation (5), the minimum number of sample points required is *S*min = (*N* + 1) × (*N* + 2)/2, where *N* is the number of design parameters. However, to improve the accuracy of the approximate model, the number of sample points used in this study is 2*S*min. As shown in Figure 3, the impeller and diffuser of the mixed flow pump were optimized by the two-step optimization method. In Table 2, the design parameters (subscripts h for hub and s for shroud), constraints, and optimization objectives during the two-step optimization process were given.



ܴܸ<sup>୦</sup> ܦܴܸܶ<sup>୦</sup> − ܴܸ<sup>ୱ</sup> ܰܥ<sup>୦</sup> <sup>୦</sup>ܦܰ − <sup>୦</sup>ܴܸܶܦ − <sup>୦</sup>ܭ <sup>୦</sup>ܥܰ − <sup>ୱ</sup>ܴܸܶܦ <sup>୦</sup>ܦܰ In the first step of optimization, only the impeller was optimized. The design parameters are the two circulation distribution control parameters, eight blade loading distribution control parameters and stacking condition. The range of these eleven parameters is shown in Table 2. To achieve the two purposes of maximizing overall efficiency and reducing the complexity of multi-objective optimization at the same time, the aggregation approach was used in this step. The weighted efficiency of the impeller at 1.2*Q*des, 1.0*Q*des and 0.8*Q*des was set as the optimization objective, with weights of 0.25, 0.5, and 0.25, respectively. To make the head difference between the optimized impeller and the baseline impeller fall within an acceptable range, the impeller head change at the design point of less than

<sup>ୱ</sup>ܥܰ − <sup>୦</sup>ܭ

3% was taken as the constraint condition. The impeller head (*H*) and efficiency (*η*) are calculated by Equations (6) and (7), respectively.

$$H = \frac{p\_{\rm out} - p\_{\rm in}}{\rho \mathfrak{g}} \tag{6}$$

$$
\eta = \frac{(p\_{\rm out} - p\_{\rm in})Q}{T\omega} \tag{7}
$$

where *p*out, *p*in, *ρ*, *g*, *ω*, and *T* are the impeller outlet total pressure, impeller inlet total pressure, fluid density, acceleration due to gravity, rotational angular velocity of the impeller, and the torque of the impeller, respectively.

After the first step of optimization, the impeller with the best performance was selected. CFD analysis was performed on the optimized impeller to extract the axial and circumferential velocity distribution at the outlet. Due to the non-uniformity of velocity distribution at the impeller outlet, directly using it as the inlet condition of the diffuser will result in the divergence of the IDM calculation, and thus the shape of the diffuser cannot be obtained. Therefore, the optimized impeller outlet velocity distribution needs to be smoothed, and the smoothed velocity will be taken as the initial condition for the second step of optimization.

In the second step of optimization, the diffuser was optimized. To reduce the hydraulic loss at the inlet of the diffuser, the circulation and flow field distribution at the diffuser inlet was set to be consistent with the optimized impeller outlet. Therefore, only the blade loading and stacking were selected as design parameters in this step. To comprehend the nature of the trade-offs made in choosing the final solution, Pareto front was used in this step, and the pump efficiencies at 1.2*Q*des, 1.0*Q*des, and 0.8*Q*des were selected as the optimization objectives. To reduce the head change of the optimized mixed flow pump at the design point, the pump head change at the design point was restricted to less than 3%.

Therefore, in this study, to improve the accuracy of the RSM in the optimization process, the number of sample points used in the first and second steps is 156 and 110, respectively. The parameter settings for MIGA and NSGA-II are shown in Table 3, and the number of impellers and diffusers with different configurations generated in the first and second steps are both 12,000.


**Table 3.** Parameters setting for MIGA and NSGA-II.

#### *4.3. Optimization Result*

The iteration history of the first step optimization is shown in Figure 8, and the best impeller A is obtained after 12,000 steps of calculation. The performance predicted by RSM and CFD of optimized impeller A is shown in Table 4, which indicates a good consistency between the two. The weighted efficiency of the optimized impeller A is 94.29%, which is 1.63% higher than the baseline impeller. In detail, the maximum improvement of the impeller efficiency occurred at 1.2*Q*des, which is 5.5%. At 1.0*Q*des, the efficiency of the optimized impeller is improved by 0.79%. However, at 0.8*Q*des, the efficiency of the optimized impeller is reduced by 0.56%. Moreover, the best efficiency point in the optimized impeller A is consistent with the design point, while in the baseline impeller, the best efficiency point appears at small flow conditions.

94 95

.଼ߟ .ଵߟ ߟଵ.ଶ <sup>୵</sup>ߟ ܪ

.଼ߟ .ଵߟ ߟଵ.ଶ <sup>୵</sup>ߟ ܪ

**Figure 8.** Optimization results of the first step. History points

̃ݎ ̃ݎ **Table 4.** Performance comparison between computational fluid dynamics (CFD) calculation and response surface method (RSM) prediction. 92 93 Selected point A


̃ݎ

Unavailable points

ߟଵ.ଶ

ߟଵ. ߟଵ.ଶ

0 0.2 0.4 4 6 8 10 12 Figure 9 shows the axial and circumferential velocity distribution at the outlet of the impeller A, these values were extracted at 0.15e*r*~0.85e*<sup>r</sup>* after considering the influence of the wall on the flow field. As described in Section 4.2, the velocity distribution needs to be smoothed. In this study, the widely used linear distribution assumption was used, and the results of the smoothing treatment are shown in Figure 9. ̃ݎ ̃ݎ

A

Velocity (m/s)

**Figure 9.** Velocity distribution at the impeller outlet and diffuser inlet.

.଼ߟ ଶ.ଵߟ .ଵߟ .଼ߟ ߟଵ.ଶ ߟଵ. ߟଵ.ଶ ଶ.ଵߟ .ଵߟ .଼ߟ The optimization result of the second step is shown in Figure 10. In this step, the Pareto front seems separated, which means there is a trade-off relationship between the pump efficiency at 0.8*Q*des (*η*0.8), 1.0*Q*des (*η*1.0) and 1.2*Q*des (*η*1.2). Figure 10a shows that *η*0.8 and *η*1.2 have a strong competitive relationship, while Figure 10b shows an interesting fact that *η*1.0 and *η*1.2 are positively correlated to some extent. After carefully considering the relationship between *η*0.8, *η*1.0 and *η*1.2, the optimized diffuser B was selected for further study. The performance predicted by RSM and CFD of the optimized mixed flow pump is shown in Table 4. It is observed that the RSM prediction results corroborate with the CFD

.଼ߟ ଶ.ଵߟ .ଵߟ .଼ߟ

ଶ.ଵߟ .ଵߟ .଼ߟ

calculation results with the maximum error not exceeding 1%. The pump efficiency of the optimized mixed flow pump at 1.2*Q*des, 1.0*Q*des is 0.8*Q*des is 80.31%, 88.89% and 81.30%, respectively, which is 6.47%, 3.68% and 0.82% higher than the baseline model.

**Figure 10.** Optimization results of second step. (**a**) *η*ߟ0.8 .଼ vs. ߟ*η*ଵ.ଶ1.2; (**b**) ߟ*η*1.0 ଵ. vs.ߟ*η*ଵ.ଶ1.2. ߟ.଼ ߟଵ.ଶ ߟଵ. ߟଵ.ଶ

Figure 11 shows the blade loading and circulation distribution of the optimized impeller and diffuser. It can be seen that the blade loading distribution at the hub and shroud of the optimized impeller A is fore-loaded and mid-loaded, respectively, while the blade loading distribution at the hub and shroud of the optimized diffuser B is fore-loaded and aft-loaded, respectively. The circulation distribution at the optimized impeller A outlet and the optimized diffuser B inlet is a second-order parabola, and the value of the circulation at the mid-span is the smallest.

**Figure 11.** Blade loading distribution and circulation distribution of optimized impeller and diffuser.

#### **5. Performance Comparison and Analysis**

Figure 12 shows the performance comparison of the optimized mixed flow pump with the baseline model. When the flow rate is greater than 0.75*Q*des, the pump efficiency of the optimized model is higher than the baseline model, and the location of the best efficiency point does not change. The head of the optimized model presented an interesting change compared to the baseline model. Under the design condition, the pump head of the optimized model is almost the same as the baseline model, which means that the matching optimization results meet the constraints. However, under small flow conditions, the pump head of the optimized model is lower than the baseline model, and the lower the flow rate, the greater the head difference. The decreased head and increased efficiency under small flow conditions represented the reduction of shaft power and energy-saving when the pump is operating in this area.

**2021**, , x FOR PEER REVIEW 12 of 16

**Figure 12.** Performance comparison between optimized model and baseline model.

Table 5 shows the comparison of hydraulic losses of each flow passage component between the optimized model and baseline model under different flow rates. Compared with the baseline model, the hydraulic loss of the optimized impeller under large flow conditions is effectively suppressed, and the hydraulic loss of the optimized diffuser under the design condition is significantly reduced. Moreover, the hydraulic loss of the inlet pipe is positively related to the flow rate and independent of the impeller. However, the hydraulic loss of the outlet pipe is related to both the diffuser and flow rate. Compared with the baseline model, the hydraulic loss of the optimized model outlet pipe is reduced under all flow conditions.


**Table 5.** Analysis of hydraulic loss.

To clarify the reasons for the change of hydraulic loss in detail, the internal flow field of the optimized model and the baseline model were analyzed and compared. The streamline contours and total pressure on the mid-span of the baseline model and optimized model are shown in Figure 13. At 0.8*Q*des and 1.0*Q*des, a large-scale flow separation occurs at the diffuser outlet of the baseline model, which not only increased the hydraulic losses at the diffuser but also at the outlet pipe. At 1.2*Q*des, an obvious low-pressure region appeared on the working surface near the impeller inlet of the baseline model. Zhang [35] pointed out that this region has a great influence on the blade vibrations and pressure fluctuation. After the matching optimization, the flow separation in the optimized diffuser was effectively suppressed, especially at 1.0*Q*des, and the low-pressure region at the impeller inlet at 1.2*Q*des was also weakened. As Zangeneh [12,13,36] mentioned, in the optimization design of mixed flow pump, the flow separation can be effectively suppressed by fore-loading at the hub and aft-loading at the shroud. This paper verifies this point of view again.

**Figure 13.** Comparison of the internal flow field between the optimized model and baseline model.

ܵሚ ܵሚ = 0 ܵሚ = 2 ܵሚ ܵሚ ܵሚ ܵሚ ܵሚ ܵሚ The comparison of the total pressure distribution along the streamline between the baseline model and the optimized model is shown in Figure 14. The horizontal axis is the standardized streamline distance *S*e, *S*e = 0 means at the impeller inlet and *S*e = 2 means at the diffuser outlet. It can be seen that the total pressure rises rapidly between 0.2*S*e~0.8*S*edue to the work done by the impeller to the fluid. However, the total pressure drops rapidly between 0.8*S*e~1.2*S*e, because the fluid in this interval has just left the blade zone of the impeller and has not yet entered the blade zone of the diffuser. Compared with the baseline model, the hydraulic loss of the optimized model in this interval was significantly reduced, which may be related to the setting of the diffuser inlet conditions during the matching optimization. The total pressure decreases slowly between 1.2*S*e~2*S*e due to the rectification effect of the diffuser. ܵሚ ܵሚ = 0 ܵሚ = 2 ܵሚ ܵሚ ܵሚ ܵሚ ܵሚ ܵሚ

**Figure 14.** Total pressure distribution along the streamline.

#### **6. Conclusions**

To further improve the optimization effect of the mixed flow pump, a matching optimization strategy of impeller and diffuser was proposed in this study. The matching optimization process was divided into two steps. In the first step of optimization, only the impeller was optimized. In the second step of optimization, the diffuser was optimized. Some important conclusions are as follows:


In summary, the matching optimization strategy proposed in this study is effective and can overcome the shortcomings of single-component optimization and thereby further improve the overall hydraulic performance of the mixed flow pump. The results of this study can also provide guidance for the optimization of other rotating machinery.

**Author Contributions:** Conceptualization, Methodology, Software, Writing—original draft and Writing—review and editing, M.W.; Data curation, Project administration and Validation, Y.L. and J.Y.; Writing—review and editing and Validation F.K.O. All authors have read and agreed to the published version of the manuscript.

**Funding:** This study supported by Science and Technology Plan of Wuhan (Grant No.2018060403011350), National Key Research and Development Plan (Grant No. 2018YFB0606103).

**Institutional Review Board Statement:** Not applicable.

**Informed Consent Statement:** Not applicable.

**Data Availability Statement:** All the data is already in the article.

**Acknowledgments:** The author sincerely thanks the ADT for its support, and reviewers for their constructive comments, and editors for their enthusiastic work.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Nomenclature**


#### **Superscripts**


#### **References**


### *Article* **The Influence of Hydrodynamic Changes in a System with a Pitched Blade Turbine on Mixing Power**

**Jacek Stelmach <sup>1</sup> , Czesław Kuncewicz <sup>1</sup> , Szymon Szufa 1,\* , Tomas Jirout <sup>2</sup> and Frantisek Rieger <sup>2</sup>**


**Abstract:** This paper presents an analysis of hydrodynamics in a tank with a 45◦ and 60◦ pitched blade turbine impeller operating while emptying the mixer and with an axial agitator working during axial pumping-down of water at different water levels above the impeller. Measurements made with the PIV method confirmed the change in direction of pumping liquid after the level dropped below the critical value, with an almost unchanged liquid stream flowing through the mixer. It was found that an increase in the value of the tangential velocity in the area of the impeller took place and the quantity of this increase depended on the angle of the blade pitch and the rotational frequency of the impeller. Change in this velocity component increased the mixing power.

**Keywords:** mixing; power consumption; pitched blade turbine; impeller

**Citation:** Stelmach, J.; Kuncewicz, C.; Szufa, S.; Jirout, T.; Rieger, F. The Influence of Hydrodynamic Changes in a System with a Pitched Blade Turbine on Mixing Power. *Processes* **2021**, *9*, 68. https://doi.org/ pr9010068

Received: 14 December 2020 Accepted: 28 December 2020 Published: 30 December 2020

**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

**Copyright:** © 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/).

#### **1. Introduction**

Batch production of suspensions in mechanically stirred tanks is often used in industrial practice [1,2]. The impeller is left running inside to prevent the solids from falling when emptying the tank. During tests on the suspension production process in a tank with a capacity of 300 m<sup>3</sup> , an increase in the need for mixing power was observed when emptying the tank shortly before the emergence of the impeller from the mixed liquid [3]. The observed increase in power is significant and can lead to engine overload and even damage. This phenomenon has not been described so far in classic monographs on mixing processes [4–6]. Only in the work of Paul et al. [7] is there mention of a significant increase in the forces acting on the agitator as the liquid surface passes through it. However, this has not been fully explained so far.

Detailed studies [8] only provide information on the possible increase in mixing power after activating the impeller while stirring the suspension, when the solid particles lifted from the bottom reach the stirrer level. This effect is most likely due to changes in the density of the slurry near the impeller.

In the course of our research on the phenomenon of an increase in mixing power when emptying the tank with a working pitched blade turbine (PBT) set to pump liquid downwards, it was established [9,10] that for a given geometric system, the higher the rotational frequency of the impeller, the lower the increase in mixing power as the liquid surface passes through the impeller. In the case of turbine-blade impellers, the influence of the blade inclination angle on the observed increase in mixing power was also noted. In this case, the greater the angle of inclination, the smaller the increase in power, and for the flat blade turbine (FBT) mixers no increase in power was observed at all. Thus, this phenomenon must be related to the hydrodynamics of the liquid in the mixer. Based on visual observations when emptying the mixer, changes were found in the liquid circulation in the tank. At the crucial moment—corresponding to a power surge—the PBT impeller stopped pumping liquid downwards. At the same time, it was found that the phenomenon

of an abrupt increase in the mixing power does not occur when filling the tank. If the impeller rotates at a constant angular velocity, then the torque applied to it is transferred by blades to the liquid stream pumped by the stirrer and increases the momentum (angular momentum) of the liquid.

#### **2. Materials and Methods**

#### *Theoretical Background*

**—**

This can be described by the equation [11]: = ∙ ∙ ∙

$$M = \rho \cdot V\_p \cdot \mathcal{R}\_m \cdot \mathcal{C}\_u \tag{1}$$

where: *M*—torque (Nm), *ρ*—liquid density (kg/m<sup>3</sup> ), *Vp*—liquid stream flowing (m3/s), *R<sup>m</sup>* = *D*/2 –impeller radius (m), *D* –impeller diameter (m), *C<sup>u</sup>* = *k*·*U*—tangential velocity component at the exit of the impeller (m/s), *k*—coefficient, *U* = *π*·*N*·*D*—tangential speed of the end of the stirrer blade (m/s). The above formula is true assuming that the liquid entering the agitator has no circumferential (tangential) component (i.e., it does not make a circular motion like at the inlet of a centrifugal pump [12,13]). This means that the momentum for this component can be neglected. The mixing power is determined based on the known relationship = 2⁄ **– –** = ∙ **— —** = ∙ ∙ **—** = ∙ = 2 ∙ ∙ ∙

$$P = M \cdot \omega = 2 \cdot \pi \cdot N \cdot M \tag{2}$$

where: *ω*—angular velocity (rad/s), *N*—rotational frequency of the impeller (s −1 ). It is worth noting that the relationship (2) is universal and is applicable in the description and analysis of other unit processes, e.g., mixing of granular materials and granulation [14–16]. **–**

The liquid stream flowing through the impeller with blades inclined in relation to the plane *z* = const at the angle *α* = const (the angle does not vary along the radius *r*) can be estimated based on theoretical considerations. Figure 1 shows the components of the velocity vector in the radial and axial directions (*b*—the width of the shoulder blade, *α*—the angle of inclination of the blade relative to the plane of movement, *U* = *ω*·*r* –tangential speed of the blade). *α* **—** *α* *ω* **–**

**Figure 1.** Distribution of velocity vectors for an inclined blade.

( − ) ∙ = (1 − ) ∙ ∙ (1 − ) ∙ ∙ ∙ <sup>2</sup> (1 − ) ∙ ∙ ∙ sin ∙ cos . ∙ ∙ ∙ = ∙ ∙ The starting point for calculating the velocity components is the difference between the tangential speed of the blade and the tangential velocity of the liquid (*ω* − *ωc*)·*r* = (1 − *k*)·*ω*·*r*, *k*, which acts as the tangential velocity on the paddle in the plane of stirrer motion *z* = const. This speed can be broken down into its components: radial (1 − *k*)·*ω*·*r*·*cos* 2*α* and axial (1 − *k*)·*ω*·*r*· sin *α*· cos *a*. Therefore, the radial flux for a cylindrical surface *π*·*b*·*D* for the condition *ω*·*r* = *π*·*D*·*N* is calculated as follows.

$$V\_{pr} = \pi^2 \cdot (1 - k) \cdot b \cdot N \cdot D^2 \cdot \cos^2 \alpha \tag{3}$$

Axial flux for the cross-section *<sup>π</sup>*·*D*2/4 is calculated by integration, taking the elementary section 2·*π*·*r*·*dr* and lifting speed *ω* = 2·*π*·*N*·*r* for specific radius. Hence:

$$V\_{pz} = (1 - k) \cdot 2 \cdot \pi \cdot N \cdot \sin a \cdot \cos a \cdot 2 \cdot \pi \cdot \int\_0^{D/2} r^2 \cdot dr \tag{4}$$

After integration you receive:

$$V\_{pz} = \pi^2 \cdot (1 - k) \cdot N \cdot \sin \alpha \cdot \cos \alpha \cdot \frac{D^3}{6} \tag{5}$$

The relationships describing the pumping of liquids through axial impellers can also be found in other papers [17,18].

For normal operation of turbine mixers with inclined blades (*H* = *D* or *H* >> *hm*) it can be assumed that axial flow only occurs through the liquid and the radial flow is negligible (*V<sup>p</sup>* ≈ *Vpz*, *Vpr* ≈ 0). However, it should be noted that Equation (5) also shows the dependence of the liquid stream flowing through the stirrer on the component of the peripheral velocity. Therefore, a dependence of the mixing power on this component in the area of the agitator should be expected. It is justified because the resistance force of the blades during their rotation in the liquid comes mainly from this component. This force can be calculated from these dependencies [19]:

$$F\_l = \frac{P \cdot B\_l \cdot \sin \alpha}{z \cdot \omega \cdot A} \tag{6}$$

where: *P*—power used for mixing (W), *ω*—angular velocity of the impeller (rad/s), *z* number of impeller blades, *α*—the angle of inclination of the blade relative to the horizontal, *B<sup>i</sup>* = *hi* 3 *R* 3 *<sup>i</sup>* − *r* 3 *i* —for the rectangular *i*-th impeller element, *A<sup>i</sup>* = *n* ∑ *i*=0 *hi* 4 *R* 4 *<sup>i</sup>* − *r* 4 *i* —for all rectangular elements of the impeller blade. The aim of the work is to determine the effect of changes in the liquid flow in the mixer on the mixing power during emptying with the mixer working.

The tests were carried out in a flat-bottomed glass tank with a diameter of *T* = 292 mm, equipped with four baffles with a width of *B* = 0.1·*T*. A six-blade pitched blade turbine with diameter *D* = 100 mm and blade width *b* = 20 mm was placed at height *h<sup>m</sup>* = 100 mm (*h<sup>m</sup>* ≈ *T*/3) above the bottom of the tank. Impellers with a blade inclination angle were used, at 45◦ (PBT45—Figure 2a) and 60◦ (PBT6—Figure 2b). This type of axial impeller provides the shortest mixing times compared to other axial mixers, but with the highest mixing power [20–23]. The tank was filled with distilled water (*t* = 20 ◦C) up to *H* = 300 mm (*H* ≈ *D*). Medium diameter glass tracer particles of 10 µm were added to the water. In order to reduce optical distortions, the cylindrical tank was placed in a rectangular tank, and the space between the walls of the tanks was filled with water. Based on the analysis of the data on the mixing power, the speed measurements were limited to only two rotational frequencies of the impeller *N* = 90 min−<sup>1</sup> (corresponding to the value of the number Froude *Fr* = *N*<sup>2</sup> ·*D*/*<sup>g</sup>* <sup>=</sup> 0.023i and Reynolds number *Re* <sup>=</sup> *<sup>N</sup>*·*D*<sup>2</sup> ·*ρ*/*η* = 15, 000) and *N* = 240 min−<sup>1</sup> (*Fr* = 0.163, *Re* = 40,000). The direction of rotation of the impeller was such that the axial flow of liquid generated by the impeller was directed to the bottom of the tank, as is usual when mixing suspensions.

**Figure 2.** Tested impellers (**a**) PBT45, (**b**) PBT60 and the position of the light knife during the measurements, (**c**) vertical: measurement of radial and axial components, (**d**) horizontal: measurement of tangential and radial components.

The measurements were performed using the LaVision PIV Particle Image Velocimetry measurement system [24–27] with a two-pulse laser with a maximum power of 135 mW and an ImagePro camera with a resolution of 2048 px × 2048 px with a Nikkor 1.8/50 lens. The lens aperture was stopped down to the value ensuring the maximum resolving power (i.e., the aperture value was 5.6 [28]).

ܰ∙ܦ∙ߨ=ܷ In order to determine the tangential and radial velocities, a 1 mm thick light knife was placed at the height of the stirrer. In the measurements of radial and axial velocities, the plane of the light knife was located about 2◦ in front of the baffle. A diagram showing the positions of the light knife is shown in Figure 2c,d. The measurement field was approximately 180 mm × 180 mm in the first case and approximately 190 mm × 190 mm in the second case. The laser frequency (pulses) was 2.7 Hz. Thus, for both configurations, the images were recorded for different positions of the blades with respect to the plane of symmetry between the baffles, although in the PIV method it is possible to synchronize the laser flashes with a specific position of the stirrer blade by using an external trigger [29] or selecting the frequency of the flashes [30].

Measurements were made for the height of the liquid in the tank equal to *h<sup>w</sup>* = 140 mm, 135 mm, 130 mm, 125 mm, 120 mm, 115 mm, 110 mm, and 105 mm. For each combination of rotational frequency and liquid height, 100 duplicates were taken to average the results. The proprietary DaVis 7.2 program was used for data processing. Two-pass data processing

was used with the final size of the analyzed field 32 px × 32 px (i.e., approximately 2.8 mm × 2.8 mm) without overlapping.

In order to facilitate comparisons, dimensionless velocities were used in the further part of the work, i.e., the velocity of the liquid was divided by the peripheral velocity of the end of the impeller blade: *U* = *π*·*D*·*N*.

#### **3. Results**

#### *3.1. Changes in Fluid Circulation during Changes in the Height of the Liquid in the Tank*

The liquid circulation method for PBT impellers is shown in Figure 3. At higher levels of liquid in the vessel, it is pumped down towards the bottom of the tank. After leaving the rotor, the liquid flows obliquely, so that centrally under the impeller there is a conical space in which the liquid flows upwards at a slow speed, with the apex angle of the cone being greater for a larger blade inclination angle (Figure 3a,b). The flow patterns obtained for large heights of liquid in the tank are consistent with the literature information [31–36]. After exceeding the critical height, the flow direction changes, the liquid under the impeller flows upwards and is radially directed over the impeller towards the tank wall, and the rising cone disappears (Figure 3c,d). From a height of *h* = 50 mm, the liquid flows practically in the axial direction, but with a uniform radial distribution. At the same time, the circulation core moves up to the level of the lower edge of the blades.

*α α α α* **Figure 3.** Liquid flow before the partition for the PBT45 and PBT60 impellers: (**a**) *h<sup>w</sup>* = 140 mm, *α* = 45◦ ; (**b**) *h<sup>w</sup>* = 140 mm, *α* = 60◦ ; (**c**) *h<sup>w</sup>* = 120 mm, *α* = 45◦ ; (**d**) *h<sup>w</sup>* = 120 mm, *α* = 60◦ .

ܸ = ܸ௭

Analysis of Figure 3 shows that pumping of the liquid through the impeller only takes place in the axial direction, i.e., *V<sup>p</sup>* = *Vpz* and, as assumed in the introduction, there is no radial discharge at the height of the stirrer. As Equation (1) shows, changes in mixing power should be correlated with changes in pumping efficiency. To specify numeric values *V<sup>p</sup>* and *Vpz*, appropriate measurements of the distribution of axial and radial velocities were performed using the PIV system. After decomposing the velocity into the axial and radial components, the velocity profiles can be determined by interpolation in the program Origin, as shown in Figure 4. The obtained profiles agree with the literature information [37,38].

− **Figure 4.** Map and profile of axial velocity at a height of *h* = 85 mm above the bottom for *h<sup>w</sup>* = 140 mm and *N* = 90 min−<sup>1</sup> (PBT45 impeller). −

ܸ = ∑ ܸ௭ ݀∙ߨ∙ ∙ ܿ = ܭ ܸ ሺܰ∙ܦ<sup>ଷ</sup> ⁄ ሻ ሺℎ<sup>௪</sup> − ℎௗ ሻ⁄ܶ ℎௗ = ℎ − 0.5 ∙ ܾ ∙ ݏ݅݊ߙ On the basis of the velocity profiles obtained, the pumping capacity was determined in MathCAD *V<sup>p</sup>* = ∑ *i Vzi* ·*π*·*d<sup>i</sup>* ·*c* below the stirrer (*h* = 85 mm, *d<sup>i</sup>* = 1, 3 . . . 99 mm, *c* = 2 mm) assuming the invariability of individual velocity components in the circumferential direction. The results obtained in the form of dimensionless pumping numbers *K<sup>p</sup>* = *Vp*/ *<sup>N</sup>*·*D*<sup>3</sup> are shown in Figure 5 and depend on the dimensionless parameter (*h<sup>w</sup>* − *hd*)/*T,* in which *hw*—liquid level, *h<sup>d</sup>* = *h<sup>m</sup>* − 0.5·*b*·*sinα*—distance of the bottom edge of the agitator from the bottom. ܸ = ∑ ܸ௭ ݀∙ߨ∙ ∙ ܿ = ܭ ܸ ሺܰ∙ܦ<sup>ଷ</sup> ⁄ ሻ ሺℎ<sup>௪</sup> − ℎௗ ሻ⁄ܶ ℎௗ = ℎ − 0.5 ∙ ܾ ∙ ݏ݅݊ߙ

**Figure 5.** Pumping capacity depending on the height of the liquid in the tank.

Lines (sections) connect the points between which the direction of the liquid flow through the impeller changes. After changing the pumping direction, no significant differences in the absolute values of the pumping numbers are observed. Moreover, when pumping upwards, in some cases the pumping capacity is even slightly reduced. This means that the mixing power should remain constant or it should decrease minimally when

∙ ሺ1−݇ሻ ∙ sin ߙ ∙ cos ߙ

∙ ሺ1−݇ሻ ∙ sin ߙ ∙ cos ߙ

= ܭ

= ܭ

 ே∙<sup>య</sup> = గ మ 

 ே∙<sup>య</sup> = గ మ 

*α α*

*α α*

changing the pumping direction. Therefore, the source of the increase in mixing power should be sought in the behavior of the peripheral velocity component. The theoretical value of the pumping number can be determined by transforming the Equation (5).

$$K\_p = \frac{V\_p}{N \cdot D^3} = \frac{\pi^2}{6} \cdot (1 - k) \cdot \sin \alpha \cdot \cos \alpha \tag{7}$$

For *k* = 0 i *α* = 45◦ we obtain *K<sup>p</sup>* = 0.822, and for *α* = 60◦ *K<sup>p</sup>* = 0.712 and similar values can be found in the literature [39]. The values obtained are greater than those measured, because in fact the peripheral velocity of the liquid is lower than the speed of the blade, i.e., *k* > 0. Even more value *K<sup>p</sup>* = 1.167 dla *h*/*T* = 0.33 is obtained from the correlation given by Foˇrt [40] for mixers with a blade inclination angle *α* = 45◦ ř *α*

$$K\_p = 0.947 \cdot \left(\frac{h}{T}\right)^{-0.19} \tag{8}$$

−

*α α*

#### *3.2. Tangential Velocity Profiles*

Based on the data obtained from the PIV system, the tangential velocity profiles were determined in the program Origin at the height of the impeller in the plane of symmetry between the baffles. The results in the form of dimensionless velocities *U*∗ *t* are shown in Figure 6. ܷ௧ ∗

<sup>−</sup> *α* <sup>−</sup> *α* <sup>−</sup> *α* <sup>−</sup> *α* **Figure 6.** Tangential velocity profiles at the height of the impeller *hm*. (**a**) *N* = 90 min−<sup>1</sup> , *α* = 60◦ ; (**b**) *N* = 240 min−<sup>1</sup> , *α* = 60◦ ; (**c**) *N* = 90 min−<sup>1</sup> , *α* = 45◦ ; (**d**) *N* = 240 min−<sup>1</sup> , *α* = 45◦ .

*α*

For the smallest of the analyzed rotational frequencies *N* = 90 min−<sup>1</sup> , an increase in velocity in the area of the impeller at the moment of changing the pumping direction is visible (marked in the figure). The greater difference occurs in the case of a smaller blade inclination angle *α* = 45◦ . Increasing the rotational frequency results in smaller speed variations when the fluid flow direction is changed.

The ratio of the maximum velocity values before and after the change of the circulation method is approximately 1.75 for the inclination angle *α* = 45◦ and 1.46 for *α* = 60◦ . These values are close to the multiplicity of the mixing power increase, 2 and 1.5 respectively. Thus, it can be assumed that the increase in mixing power is caused by the change in the peripheral speed of the liquid in the area of the impeller.

#### *3.3. Estimating the Mixing Power*

The relationship (1) presented at the beginning is less accurate than the direct measurement of the torque due to the need to experimentally determine the velocity of the liquid in the area of the impeller. Moreover, in the PIV method it is very difficult to estimate the measurement error, and the importance of this is evidenced by the information about new algorithms appearing in the literature [40–42]. Nevertheless, it should reflect the behavior of the system during hydrodynamic changes taking place in it. The results of calculating the power number using Equation (1) are shown in Figure 7, where the mixing power number is placed on the ordinate axis: *Eu* = *Po* = *P*/ *N*3 ·*D*5 ·*ρ* <sup>ଷ</sup>ܰሺ ܲ = ܲ = ݑܧ . ሻߩ ∙ ⁄ <sup>ହ</sup>ܦ ∙

**Figure 7.** The power number calculated using Equation (1).

− − − For pumping the liquid down (towards the bottom) at high liquid heights in the tank, low values of the mixing power were obtained. For the PBT45 impeller, direct measurements gave *Eu* = 1.53, and for the PBT60 impeller, *Eu* = 2.18. These results are consistent with the data in the literature [43,44]. The tangential velocity of the liquid at the outlet of the agitator has a great influence on the results obtained. For example, for the PBT45 impeller under the conditions of *N* = 90 min−<sup>1</sup> , *h<sup>w</sup>* = 140 mm, the measurements obtained the value of *Eu* = 1.05 for *C<sup>u</sup>* = 0.09 m/s, but at a distance of *R* = 48.4 mm from the impeller axis the tangential velocity of the liquid is 0.132 m/s and the calculated power number value is *Eu* = 1.535. Unfortunately, it is practically impossible to determine the measurement error in the PIV method [45]. In addition, in asynchronous measurement, when the position of the blades in relation to the velocity profile determination line (plane) changes, the initial position of the blade may affect the results obtained. This is illustrated in Figure 8 showing the results of five consecutive measurements made to test this thesis. The differences in the values of the tangential velocity of the liquid for the radius of the stirrer *R<sup>m</sup>* = 50 mm may reach about 0.05 of the velocity of the end of the stirrer blade. For the profiles from Figure 8, the values of the power numbers are obtained from *Eu* = 1.195 to *Eu* = 1.445 for *N* = 90 min−<sup>1</sup> and from *Eu* = 1.888 to *Eu* = 2.145 for *N* = 240 min−<sup>1</sup> .

**Figure 8.** Profiles for five consecutive measurements (PBT45, *h<sup>w</sup>* = 140 mm).

The multiplicity of the increase in mixing power is greater than the values obtained in direct measurements. Figure 7 shows that for blades set at an angle of 45◦ there should be a threefold increase, and for a 60◦ angle, a two-fold increase in power. In the measurements of torque for PBT45, a two-fold increase in power was achieved; for PBT60 this increase was 1.5 times, which can be read from Figure 9 presenting the results of previous studies [10]. These differences may result from incomplete fulfillment of the condition (assumption) that the liquid influencing the agitator impeller does not rotate.

**Figure 9.** Increase in mixing power when emptying the tank for various sizes of impellers.

#### **4. Discussion**

The results of the experiments presented in the paper allow for a preliminary hypothesis concerning the mechanism of increasing mixing power when emptying the mixers during the operation of the axial impeller while pumping the liquid down the tank [46]. The critical moment of the mechanism analyzed is undoubtedly the moment of changing the direction of the liquid flow through the impeller area, despite the unchanging parameters of the impeller itself. According to results from the analysis of the velocity distributions shown in Figure 3 for the liquid height in the tank *h<sup>w</sup>* = 140 mm, the liquid flows in the direction of liquid pumping through the rotating impeller (Figure 3a,b), and for *h<sup>w</sup>* = 120 mm the liquid flows through the area of the impeller in the opposite direction, i.e., to the bottom of the tank. This occurs when the liquid height above the upper edge of the impeller is approximately 10–15 mm. With high probability, it can be assumed that at this point the liquid layer above the impeller is so small that there is no possibility for secondary circulation lines, i.e., axial-radial circulation, to close within it. The rotating impeller starts to work like a radial-circumferential agitator (Figure 6). The impeller accumulates the

liquid in front of the paddle, which increases the resistance to motion and increases the tangential velocity. At the same time, the stream of liquid ejected from the area of the impeller at a relatively high speed (Figure 9) begins to flow towards the bottom of the tank at the wall, thus changing the direction of circulation, which is shown in Figure 3c,d. It should be emphasized that this is a working hypothesis and a more extensive cycle of tests should be performed to confirm it. Figure 10 Radial represent the velocity maps: (**a**) *h<sup>w</sup>* = 140 mm; (**b**) *h<sup>w</sup>* = 120 mm.

**Figure 10.** Radial velocity maps: (**a**) *h<sup>w</sup>* = 140 mm; (**b**) *h<sup>w</sup>* = 120 mm.

#### **5. Conclusions**

Due to the incomplete fulfillment of the conditions, relationship (1) can be used to determine energy changes (mixing power) in a system with a mechanical impeller and a six-blade pitched blade turbine during hydrodynamic changes of the centrifugation of the liquid flowing into the impeller. Furthermore, this allows achievable accuracy of velocity measurements in the area of the impeller taking place when emptying the tank.

The increase in the mixing power when emptying the tank with the impeller working is determined by the abrupt increase in the tangential velocity component in the area of the impeller after changing the direction of liquid circulation. The increase in the value of the tangential velocity depends on the angle of the blades' inclination and the rotational frequency of the impeller and is correlated with the changes in the mixing power when emptying the tank. As in the case of mixing power, smaller increments are observed for larger blade angles. Furthermore, increasing the rotational frequency (at the same angle of inclination) results in smaller increases in tangential velocity. In the paper, it is stated that it is practically impossible to determine the measurement error in the PIV method. According to Lehr and Boelcs [47] the standard measurement uncertainty of PIV velocity measurements for the mean velocity field is less than 4%, and in the regions of strong velocity gradients it is smaller than 5% when the test-section is quasi-two-dimensional and the out-of-plane components of the vectors cause only minor errors.

**Author Contributions:** Conceptualization, J.S. and C.K.; methodology, J.S., C.K., S.S., T.J., and F.R.; validation, J.S., C.K., S.S., T.J., and F.R.; formal analysis, J.S., C.K., S.S., T.J., and F.R.; investigation, J.S., C.K., S.S., T.J., and F.R.; resources, J.S., C.K., S.S., T.J., and F.R.; data curation, J.S., C.K., S.S., T.J., and F.R.; writing—original draft, J.S., C.K., S.S., T.J., and F.R.; writing—review and editing, J.S., C.K., S.S.; visualization, J.S., C.K., S.S., T.J., and F.R.; supervision, J.S., C.K., S.S., T.J., and F.R.; project administration, J.S., C.K., S.S., T.J., and F.R.; funding acquisition, J.S., C.K., S.S., T.J., and F.R. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by Ministry of Education, Youth and Sports of the Czech Republic: OP RDE CZ.02.1.01/0.0/0.0/16\_019/ 0000753.

**Institutional Review Board Statement:** Not applicable.

**Informed Consent Statement:** Not applicable.

**Data Availability Statement:** Not applicable.

**Acknowledgments:** The work was created as part of the statutory activity of the Department of Chemical Engineering of Lodz University of Technology and the grant OP RDE CZ.02.1.01/0.0/0.0/16\_019/ 0000753 financed by the Ministry of Education, Youth and Sports of the Czech Republic.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


### *Article* **New Design of the Reversible Jet Fan**

### **Miroslav H. Benišek, Ðorde S. ¯ Cantrak \* ˇ , Dejan B. Ili´c and Novica Z. Jankovi´c**

Faculty of Mechanical Engineering, University of Belgrade, Kraljice Marije 16, 11120 Belgrade 35, Serbia; mbenisek@mas.bg.ac.rs (M.H.B.); dilic@mas.bg.ac.rs (D.B.I.); njankovic@mas.bg.ac.rs (N.Z.J.)

**\*** Correspondence: djcantrak@mas.bg.ac.rs

Received: 18 November 2020; Accepted: 15 December 2020; Published: 17 December 2020 -

**Abstract:** This paper presents two designs of the axial reversible jet fan, with the special focus on the impeller. The intention was to develop a reversible axial jet fan which operates in the same way in both rotating directions while generating thrust as high as possible. The jet fan model with the outer diameter 499.2 ± 0.1 mm and ten adjustable blades is the same, while it is in-built in two different casings. The first construction is a cylindrical casing, while the second one is profiled as a nozzle. Thrust, volume flow rate, consumed power and ambient conditions were measured after the international standard ISO 13350. Results for both constructions are presented for three impeller blade angles: 28◦ , 31◦ and 35◦ , and rotation speed in the interval *n* = 400 to 2600 rpm. The smallest differences in thrust, depending on the fan rotation direction, as well as the highest thrust are achieved for the first design with the cylindrical casing and blade angle at the outer diameter of 35◦ . Therefore, it was shown that fan casing significantly influences jet fan characteristics. In addition, the maximum thrust value and its independence of the flow direction is experimentally obtained for the angle of 39◦ in the cylindrical casing.

**Keywords:** axial fan; reversible; jet; design; thrust; energy characteristics

#### **1. Introduction**

Reversible jet fans are present in road tunnels ventilation and garages, underground car parks, fire protection, good air quality systems, etc. They are designed to operate efficiently in both directions and produce adequate jets. Tunnel jet fans are, in fact, a substantial, i.e., core part of the tunnel ventilation, as well in smoke extraction systems. They should combine the highest technical requirements like efficiency and performance, as well as noise emission. Numerous CFD calculations have been performed in order to study the road tunnel ventilation and firefighting systems [1–8]. One of the choices for impulse ventilation of the tunnels is jet fan. "Impulse ventilation of tunnels involves the application of one or more jets of air into a tunnel, to drive the airflow in a desired direction. In essence, the kinetic energy of a high-velocity jet is transferred, with various degrees of efficiency, into the kinetic energy of slower-moving tunnel air" [4]. Therefore, the role of the jet fans is to provide an impulse to the air flow. "The average jet velocity is in the range of 30 to 40 ms−1" [4].

Experimental determination of tunnel ventilation axial ducted fan performance using a two-sensor hot wire X-probe with added pair of near-wall positioning pins is presented in [9]. Experimental results, obtained in the laboratory in the 1:19 scale tunnel, are used for ventilation performance of CFD test in a uni-directional traffic road tunnel [3,9,10]. Proposal for the improvement of CFD models of the tunnel fire development based on experimental data are also reported [7]. Improvement of the aerodynamic performance of a tunnel ventilation jet fan is performed by the application of multiobjective optimization technique [11].

Contemporary CFD tools include aerodynamic optimization of axial fan impeller with its blade geometry, guide vanes if they exist, casing and nozzle shapes, etc. Fan energy characteristics, i.e., the aerodynamic fan curves, prior to experiments, could be estimated numerically. Experimental validation could be done according to the international standard ISO 13350 [12].

Three high pressure reversible fan concepts, like a two-stage counter rotating fan, a single-stage high speed fan and a two-stage fan with a single motor and impeller on each end of the motor shaft are presented in paper [13].

Paper [14] presents the designed reversible jet fan, obtained experimental data and CFD results. Reversible aerodynamic design, in fact, limits the maximum fan pressure side [13]. Paper [15] presents a numerical optimization procedure for performance improvement of a jet fan. Authors in [16] point out that aerodynamically desirable axial fan rotor blades, which would have identical aerodynamic performances in both flow directions, are still insufficiently developed. They present a method to profile these blades.

This paper presents a design of the reversible jet fan, geometries of two versions of the casings and experimentally obtained data. The axial fan impeller is the same in both cases, while casings are different. Experimentally determined thrust, after ISO 13350 [12], power and volume flow rates for various fan rotation speeds in both rotating directions are presented in this paper. The intention was to design the impeller with good characteristics in both rotating directions, so the automatic fan speed control system could adopt the rotation direction depending on draft direction in the car tunnel. This should result in better maintenance of environmental conditions in car tunnels.

#### **2. Reversible Jet Axial Fan Designs**

The design is developed in cooperation of the Hydraulic Machinery and Energy Systems Department (HMESD) University of Belgrade Faculty of Mechanical Engineering (UB FME) and company Rudnap Group Minel Kotlogradnja from Belgrade, Serbia, where it was also manufactured. The demand from industry was to develop jet fan prototype with the following characteristics: volume flow rate—*Q<sup>p</sup>* = 17 m<sup>3</sup> s −1 , impeller outer diameter—*Da,p* = 0.71 m, fan rotation speed *n<sup>p</sup>* = 2950 rpm, fan motor power—*P<sup>p</sup>* = 39 kW and axial force, i.e., thrust—*Fz,p* = 938 N. Here, index "p" denotes "prototype". Axial thrust is calculated using the Equation (4). According to the reference [4]: "The average jet velocity is in the range of 30 to 40 m/s." This is, also, fulfilled for this prototype. These conventional jet fans are aligned parallel to the tunnel axis. The maximal achievable thrust (*Fz,p,max*) is calculated using Equation (6) in [4]. This relation could be simplified for the axial fan impeller in a free stream in the following way:

$$F\_{\mathbf{z},\mathbf{p},\text{max}} = \rho A\_{\mathbf{j}} c\_{\mathbf{z},\mathbf{j}} (c\_{\mathbf{z},\mathbf{j}} - c\_{\mathbf{z},\mathbf{j}\mathbf{s}}) . \tag{1}$$

where ρ is air density, *A<sup>j</sup>* is the jet fan outlet cross section, *cz,j* is the jet axial average velocity and *cz, fs* is the free stream velocity, i.e., air velocity in the tunnel in the region without jet fan influence. Of course, the effective thrust is lower and calculated as follows:

$$F\_{\mathbf{z},\mathbf{p}} = \rho A\_{\mathbf{j}} c\_{\mathbf{z},\mathbf{j}} (c\_{\mathbf{z},\mathbf{j}} - c\_{\mathbf{z},\mathbf{j}\mathbf{s}}) \eta\_{\mathbf{p}} \eta\_{\mathbf{p},\mathbf{inst}} \tag{2}$$

where η*<sup>p</sup>* is the jet fan efficiency, and η*p,ins* is the jet fan installation efficiency. In some cases, it could be assumed that η*<sup>p</sup>* = 1 [4]. Installation efficiency depends on the jet fan position in the tunnel. It could be assumed that η*p,ins* = 1, if the jet fan is positioned in the middle of the tunnel, without the influence of other fans, other obstacles, as well as tunnel surfaces [4]. However, influence of the wall on the propulsion jet is studied in [16]. Therefore, the installation efficiency (η*p,ins*) could be estimated on the basis of Equation (9) in [4], which is derived using the experimental data presented in [17]. In the case of the presented constructions, the guide vanes and slanted silencers do not exist, so the regulation could be performed only by the fan speed rotation number. For the flow direction purpose, the flow straighteners in the "cross" shape are in-built in both silencers. The flow straighteners need to eliminate or, at least, minimize the turbulent swirling flow, which occurs behind the axial fan impellers [18], and maximize the axial velocity component which generates thrust. The sound power level according to the A-weighting was not experimentally determined.

Jet fan head, i.e., pressure rise, could be determined in the following way:

$$
\Delta p\_{t,p} = P\_p \eta\_p \% \text{Q}\_p = \\$9 \cdot 10^3 \cdot 0.55/17 \approx 1262 \text{ Pa}\_{\prime} \tag{3}
$$

where the jet fan efficiency could be estimated as η*<sup>p</sup>* = 55%. Besides Equation (2), thrust could be also determined as follows:

$$F\_{z,p} = \rho Q\_p c\_{z,p} = \rho Q\_p^{\;/^2} / \text{A} = 938 \text{ N},\tag{4}$$

where *cz*,*<sup>p</sup>* is average axial velocity calculated as *cz*,*<sup>p</sup>* = *Qp*/*A* and surface of the cross-section.

The jet fan model parameters are determined on the basis of the similarity law and equality of coefficients such as flow (ϕ), head (ψ), power (λ) and efficiency (η). Reversible jet fan model is developed using the following parameters: *D<sup>a</sup>* = 0.5 m (punctually 499.2 mm ± 0.1) and fan power *P* = 3 kW. By introducing power coefficient (λ) as follows:

$$
\lambda\_p = P\_p / (D\_{a,p} \, ^2 \mu\_p \, ^3),
\tag{5}
$$

where *u<sup>p</sup>* is circumferential velocity on diameter *Da*,*p*. Equality of these coefficients for the prototype and model lead to the equation:

$$m = n\_p \text{ (P/P}\_p(\text{D}\_a/\text{D}\_{a,p})^5\text{)}^{1/3} = 2251 \text{ rpm}.\tag{6}$$

Flow coefficient is derived, on the basis of kinematic similarity, as follows:

$$\varphi = 4Q \langle \left[ u\_a \left( D\_a^{\;\;\;2} - D\_i^{\;\;2} \right) \pi \right] \rangle \end{pmatrix} \tag{7}$$

where *D<sup>i</sup>* is hub diameter.

Flow coefficients for the model and prototype are equal:

$$
\varphi = \varphi\_p \tag{8}
$$

It is assumed that non-dimensional diameter (ν), defined as ν = *D<sup>i</sup>* /*Da*, is equal for the model and prototype:

$$\boldsymbol{\nu} = \boldsymbol{\nu}\_p \tag{9}$$

Volume flow rate of the jet fan model could be determined on the basis of Equations (7)–(9) as follows:

$$Q = Q\_p \cdot \left(\frac{D\_d}{D\_{a,p}}\right)^3 \cdot \frac{n}{n\_p} = 17 \cdot \left(\frac{500}{710}\right)^3 \cdot \frac{2251}{2950} = 4.53 \text{ } \frac{\text{m}^3}{\text{s}}.\tag{10}$$

Head coefficient (ψ) is defined after the dynamic similarity as follows:

$$
\psi = \text{2Y/}u\_a^{\text{-}2}.\tag{11}
$$

where *Y* is fan head defined in the following way:

$$Y = \Delta p\_t / \rho\_\prime \tag{12}$$

where ∆*p<sup>t</sup>* is difference of total pressures after and before the fan, i.e., total pressure rise in the jet fan.

Applying Equations (11) and (12), as well as introducing the equality of model and prototype head coefficients lead to the following expression:

$$
\Delta p\_l = \Delta p\_{l,p} \cdot \left(\frac{D\_d}{D\_{a,p}}\right)^2 \cdot \left(\frac{n}{n\_p}\right)^2 = 1262 \cdot \left(\frac{500}{710}\right)^2 \cdot \left(\frac{2251}{2950}\right)^2 = 364.41 \text{ Pa.}\tag{13}
$$

Using Equations (4) and (7), the following expression is derived:

$$\frac{F\_z}{D\_a^4 \cdot n^2} = \pi^3 \cdot \rho^2 \cdot \rho \cdot \frac{\left(1 - \nu^2\right)^2}{120^2}.\tag{14}$$

Right hand side of the Equation (14), by assuming that air density is equal, depends only on flow coefficient and dimensionless radius, which are identical for the model and prototype, so the following equation for thrust could be derived:

$$F\_z = \left(\frac{D\_a}{D\_{a,p}}\right)^4 \left(\frac{n}{n\_p}\right)^2 F\_{z,p} = \left(\frac{500}{710}\right)^4 \left(\frac{2251}{2950}\right)^2 \cdot 938 = 134.32 \text{ N}.\tag{15}$$

In this way, all necessary data for jet fan model design are determined. , 500 2251 = = 938 = 134.32N. 710 2950 

The greatest challenge was to develop axial fan impeller geometry to provide the same energy characteristics in both directions. It is even more important for the reversible axial fan functionality in traffic tunnels where pressure could vary in regions close to the inlet, i.e., exit. In this case, due to the fact that the complete fan construction cannot be rotated, or simpler geometries where blade angles cannot be adjusted, it is clear that axial fan impeller geometry must be symmetrical. This would result in the axial fan impeller with symmetrical blades. They should be designed in the way to use symmetrical airfoil and to be symmetrical to the axis normal to the chord, i.e., in this case, also camber line, which divides it in two halves. The fan is designed after the law of constant head in the radial direction, i.e., constant circulation in order to achieve higher energy efficient fans, i.e., equal energy distribution along the radius. The result is the twisted blade presented in Figure 1a. Threaded connection M20 is used for blade positioning in the axial fan hub. Six symmetrical profiles and their geometry are shown in Figure 1a. Geometry parameters for the first and sixth one are presented in Table 1, where r-radius measured from the axial fan rotation axis, R1—radius at the blade leading/trailing edge, R2—radius of the profile pressure/suction side, β—profile angle measured from the fan rotation axis and ymax—maximum thickness. Profile maximum thickness is positioned in the center of the straight camber line, which has constant length along the blade *L* = 106 mm. , *β*

**Figure 1.** *Cont*.

**Figure 1.** (**a**) Geometry of the impeller symmetrical blade and (**b**) Reversible jet axial fan with specified normal and reverse flow directions.

*β* **⁰ Table 1.** Table of the geometry parameters of the symmetrical blade profiles (No. 1 and 6).


Geometry of the whole construction of the reversible jet axial fan, with specified normal and reversible flow directions, is presented in Figure 1b, where: 1—impeller, 2—AC motor, 3—impeller casing, 4—profiled impeller hub cap, 5—silencer (sound suppressor), 6—flow straighteners, 7—AC motor support and 8—AC motor cable casing (pipe form). Flow straighteners are not specially profiled, due to the intention to obtain similar flow characteristics in both directions. They are only sheet metal parts which form the "cross" geometry.

Asynchronous electric motor with two poles is placed in the casing in the way not to disturb fluid flow. Axial fan casing with a hub and carrier is designed in the way to stabilize operation and connection with the electromotor.

− *ν* The jet fan has profiled bell-mouth inlet, and casings have inner diameter of 500 mm, while outer is 584 mm (Figure 1b). Casing consists of perforated plate, mineral wool and steel plate envelope, which minimize noise. Flow straighteners (Figure 1b, position 6) decrease generated turbulent swirling flow jet and direct the flow. Namely, the main role is to improve generated jet strength, i.e., maximize thrust and fan efficiency.

The jet fan model is designed for the following parameters determined above: fan rotation speed—*n* = 2251 rpm, volume flow rate—*Q* = 4.53 m<sup>3</sup> s −1 , impeller outer diameter—*D<sup>a</sup>* = 0.5 m and axial force—*F<sup>z</sup>* = 130 N. It has ten adjustable blades and dimensionless ratio ν = *D<sup>i</sup>* /*D<sup>a</sup>* = 0.5. The manufactured jet fan model is presented in Figure 2.

**Figure 2.** Developed axial fan impeller with its casing and AC electric motor.

The reversible jet fan 3D model was developed in academic software package CATIA V5R18 (64 bit) for the flow analysis. This model had certain level of "intelligence" based on the CATIA Knowledge tools, which provided blade angle easy variation and blade shape variation according to its angle position. In this way, clearances are minimized.

The second construction is with nozzles and flow straighteners as shown in Figure 3. It has nozzles with inner diameter 440 mm (Figure 3b).

**Figure 3.** The second construction of the casing: (**a**) at the thrust measurement table and (**b**) nozzle geometry.

#### **3. Experimental Test Rig**

Experimental investigation of the designed jet fan was conducted on the designed and manufactured thrust measurement table in the Laboratory of the Hydraulic Machinery and Energy Systems Department at the Faculty of Mechanical Engineering University of Belgrade (Figure 4).

**Figure 4.** Thrust measurement table in the laboratory: (**a**) 3D model for calibration and (**b**) real model.

С The test rig (Figure 4), i.e., the thrust measurement table, is composed of numerous elements. The fundament of the test rig construction is manufactured with massive steel U-shaped profiles (Figure 4a, position 1). It is heavy and provides operating stability important for obtaining precise measuring results. Rails are assembled with the steel plate to the fundament (Figure 4a, position 2) so that axial fan with wheel chair could safely move along the rails and enable axial force, i.e., thrust measurements (Figure 4a, position 3). On the measurement table, a wheel fundament is attached, also made of steel. This wheel (pos. 5) is positioned on the wheel fundament (pos. 4) by the axle. Wheel rotation is possible by the use of radial rolling one-row bearing. Steel chrome polished cable with 3 mm in diameter (pos. 6) moves over it and connects weights carrier (pos. 7) with calibrated weights (pos. 8) and wheel chair. Weight carrier has two parts, of which the lower one is used for holding calibrated weights and the upper one is a hook for hanging on the steel rope. It is also calibrated and made of steel. Wheel chair is, on the other side, connected via measuring tape, with a force transducer (pos. 9). This is a construction for force transducer calibration. Calibration preceded each measurement. During measurements the steel cable is dismounted. However, the force transducer is always connected via measuring tape (pos. 11) with the wheelchair, and it is mounted on the steel carrier (pos. 10), which provides appropriate axial force measurements. The Vishay force transducer model 355, type C3, hermetically sealed, was used (Figure 5, pos. 1). Specified total error is ±0.02% of rated output, which is here for C3, 50 kg, i.e., ±10 g.

A force transducer was carefully calibrated at the thrust measurement table by first loading up to 45 kg and afterwards unloading due to hysteresis determination. A linear characteristic is obtained. A measuring tape transfers axial force from the axial fan to the force transducer. It provides stable work and precise measurements. A signal conditioner is used for the axial force transducer signal conditioning and acquisition. A frequency regulator is used to control the axial fan rotation speed. A digital frequency regulator DS2000, company MOOG, Serbia, was used. It has a three-phase regulator which works over the voltage interval from 65 V till 506 V and frequencies from 50 till 60 Hz. Working temperature interval is 0 till 40 ◦C. A multifunctional measuring device Testo 450 with appropriate probes was used in these experiments for measuring air temperature and humidity, as well as for velocity measurements with attached vane anemometer probe. On the basis of the velocity measurements, in positions specified by ISO 5801 [19], the volume flow rate was determined. It is compared with the ones calculated on the basis of the measured axial velocity in the following way: *Q* = *D<sup>a</sup>* (*Fz*π/ρ) 0.5/2, where ρ is air density. A mercury barometer measured atmospheric pressure before each test. Fan rotation speed was determined by a stroboscope DRELLOSCOP 3009.

**Figure 5.** Connection of the force transducer with wheel chair: **1**—force transducer, **2**—force transmitter carrier, **3**—measuring tape, **4**—wheel chair, **5**—axial fan, **6**—rails, **7**—steel plate for connection of rails with wheel chair loaded with reversible jet fan and **8**—fundament. 0 5 2 *ρ*

#### **4. Experimental Results and Discussion**

In the conducted experiments, the following physical values have been measured: axial force, i.e., thrust, velocity field at the fan inlet and outlet, fan rotation speed, electromotor power, air temperature, humidity and atmospheric pressure. Measurements were performed for various angle positions of both blade impeller sets, controlled at the outer diameter *Da*: β*Ra* = 28◦ , 31◦ , 33◦ , 35◦ , 39◦ and 45◦ as well as for various fan rotation speeds *n* = 400, 800, 1200, 1600, 2080, 2200, 2500 and 2565 rpm. Measurements have also been performed for both fan rotating, i.e., flow directions and are presented in Figure 6. *β*

**Figure 6.** Reversible jet fan characteristics in the function of the fan rotation speed and angle *<sup>β</sup>* β*Ra* for both flow directions: (**a**) volume flow rate, (**b**) internal consumed power, (**c**) thrust and (**d**) efficiency.

The fan efficiency is calculated, only after the contribution of the kinetic energy at the fan outlet, i.e., in the jet, as follows:

$$
\eta = Q \rho c^2 / 2P\_s \tag{16}
$$

where *c* is velocity at the fan outlet and ρ air density. It is assumed that the inlet velocity is zero. It is calculated on the basis of the approximated internal power, presented in Figure 6b. *η ρ ρ*

All fan characteristics, normally, increase with the fan rotation speed. Hierarchy of increasing the volume flow rate and thrust with increasing the blade angle, up to the angle 39◦ , is obvious. Fan characteristics depend on flow direction for all angles, but the smallest difference is obtained for angle 39◦ .

The best angle position (β*Ra*) of the blade impeller blades is determined on the basis of a large amount of experimental data (Figure 6). Measuring results for the angle position at the outer diameter β*Ra* = 39◦ are presented in the following charts (Figure 7). *β β*

*β* **Figure 7.** Reversible jet fan characteristics in the function of the fan rotation speed for both flow directions and angle β*Ra* = 39◦ : (**a**) volume flow rate, (**b**) internal consumed power, (**c**) thrust and (**d**) efficiency.

*β β η η* Small differences of thrust are obtained for angle β*Ra* = 39◦ depending on the flow direction in fan (Figure 7c). It is almost independent of the flow direction. This was the aim of this design. In this case, the maximum thrust is achieved in both directions (Figures 6c and 7c). The fan was also tested for β*Ra* = 45◦ , but thrust started to decrease, i.e., is significantly lower for normal flow direction. In addition, the highest fan efficiency, calculated after fan contribution to the jet kinetic energy, is reached for angle 39◦ (Figures 6d and 7d), and it is almost the same for both flow directions η*I,max* = 41.45% and η*II,max* = 41.94%.

Obtained experimental results could be scaled-up to the prototype on the basis of the procedure presented in [14]. This procedure involves equality of the turbomachinery coefficients for flow, head and power. It is shown here that designed thrust of 134.32 N for rotation speed 2251 rpm after Equation (15) is achieved for angle 39◦ . Obtained values are *F<sup>z</sup>* = 133 N for *n* = 2266.8 rpm.

*β* In addition, axial fan impeller was tested in two casing constructions. The first construction is a cylindrical casing, while the second one is profiled as a nozzle. Results for both models are presented and compared in Figure 8. This design was tested for β*Ra* = 28◦ , 31◦ and 35◦ .

*β* **Figure 8.** Comparison of the fan thrust in cylindrical (1) and nozzle (2) profiled casings for various angles β*Ra* and rotational directions (I-normal and II-reversible flow directions) in the function of the fan rotation speed: (**a**) 28◦ , (**b**) 31◦ and (**c**) 35◦ .

*β β β* Angle β*Ra* variation leads to good thrust in normal, while to worse ones in reversible flow direction (Figure 8). In all cases, the highest thrust values are reached for the highest fan rotation speed, what was expected. The smallest differences in thrust are achieved for β*Ra* = 35◦ and presented in Figure 8c. This is obvious for the model 1 with cylindrical casing. The highest values of thrust are also achieved for this angle β*Ra* = 35◦ .

*β β* Influence of the flow direction in the reversible axial jet fan is more obvious for the second model with profiled nozzle. For this case significantly lower values of thrust are achieved for all angles β*Ra*. This is obvious for the highest presented angle β*Ra* = 35◦ (Figure 8c). It could be concluded that this nozzle casing was not properly designed for the tested fan. Construction of model 2 resulted in a lower flow rate and thrust.

Analysis of sources of error and of uncertainty evaluation for the thrust measurement is provided for the one measurement point (*n* = 2266.8 rpm) which is close to the designed fan rotation speed (*n* = 2251 rpm). Calibration uncertainty of axial force (thrust) calibration, i.e., weights used for calibration, is ±0.54 g. Systematic uncertainty combines the uncertainty of transducer and calibration by the root-sum-square method and is ±0.075%. Random uncertainty of thrust measurements at 95% confidence level is 1.689 %, and total uncertainty of thrust measurement is 1.7%. This is in accordance with the used standard ISO 13350.

#### **5. Conclusions**

This paper presents the design of the axial jet fan impeller with symmetrical and adjustable blades and experimental results of the testing on the test rig following ISO 13350. Two designs of fan casings are presented too. Axial fan was tested for various angles and rotation speeds in both cases. These fans work in pairs for the case of bigger tunnels, and the distance between two pairs of fans is, among other things, defined by the experimentally determined thrust. It could be concluded the following:

• Herein, the procedure is presented for determination of the jet fan model parameters on the basis of the parameters demanded for the prototype. This procedure is based on the geometry, kinematic

and dynamic similarity law. Anyhow, this approach does not result in the same Reynolds number (Re), so ∆Re is incorporated in the equation of recalculation/conversion, i.e., efficiency scale-up from a model to the prototype which is treated in IEC 60193. This is not discussed in the used standard here ISO 13350 [12].


**Author Contributions:** Conceptualization and methodology, all authors; validation, Ð.S.C., N.Z.J. and D.B.I.; ˇ formal analysis, investigation and writing, all authors; All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by the Ministry of Education, Science and Technological Development, Republic of Serbia (MESTD RS), contract number 451-03-68/2020-14/200105 (subproject TR 35046) and by the Bilateral project "Joint Research on the Development Technology of Low-head Run-of-the-river Hydropower", between MESTD RS and Ministry of Water Resources in China and Renewable Energy and Rural Electrification Zhejiang International Science Center, contract number 401-00-00588/2018-09, which authors hereby gratefully acknowledge.

**Acknowledgments:** This article is partially based on a paper presented at the 40th International HVAC congress, 2009, "Fan for Ecological Condition Sustain in Tunnels" held on 18–19 September 2009 in Belgrade, Serbia, so authors are thankful for technical support to M. Pajni´c and M. Begovi´c from Rudnap Group; Minela Kotlogradnja, Belgrade, Serbia.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

© 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (http://creativecommons.org/licenses/by/4.0/).

### *Article* **Numerical and Experimental Study on Waviness Mechanical Seal of Reactor Coolant Pump**

#### **Xiaodong Feng 1,2,\*, Wentao Su <sup>1</sup> , Yu Ma <sup>3</sup> , Lei Wang <sup>2</sup> and Heping Tan <sup>1</sup>**


Received: 10 October 2020; Accepted: 4 December 2020; Published: 7 December 2020

**Abstract:** Based on the fluid hydrodynamic lubrication theory, a mathematical model of liquid film lubrication was established for the waviness hydrodynamic mechanical seal of a reactor coolant pump. The influences of the waviness amplitude and pressure on the sealing performance were investigated by the numerical simulation. The numerical results showed that the leakage rate increases linearly as the pressure and waviness amplitude increase under the force balance condition. The minimum liquid film thickness decreases first and then increase as the pressure increases. Stationary slide rings with three different waviness amplitudes were processed using the pre-deformation method and tested at different pressure and temperature. The experiments showed that all the three kinds of seal have good stability under different pressure conditions. The experimental results showed that the leakage rate is influenced by the pressure, waviness amplitude, and temperature, and the leakage rate increases as the pressure increases. The comparison between experimental and numerical results showed that both the temperature and pressure affect the seal performance, and tends to a smaller leakage rate, which is quite different from the numerical values. Therefore, the multi-physics coupling effect should be considered in the numerical analysis of seal performance, and this will be studied in the further works.

**Keywords:** reactor coolant pump (RCP); waviness; mechanical seal; leakage rate; liquid film

### **1. Introduction**

The reactor coolant pump (RCP) is one of the most critical pieces of primary equipment in a nuclear power plant, and the only rotating equipment in the nuclear island which suffers both high temperature and pressure [1]. The RCP's shaft seal consists of three stages identical hydrodynamic mechanical seals in series to prevent the leakage of primary medium from the outside of the RCP. The mechanical seal is designed to operate normally under 17.3 MPa for 10 h. Compared with the ordinary mechanical seals, the hydrodynamic mechanical seal realizes the non-contact between the sealing surfaces by using the closing force caused by the hydrodynamic effect between the sealing end faces, with a variety of grooves on the sealing surface. This characteristic greatly reduces the wear of the sealing surface and improves the reliability and lifespan [2,3]. Two types of mechanical seal are always used in the shaft-sealed RCP, including the waviness end face [4–6] mechanical seal and ordinary mechanical seal [7,8], where the former has a longer lifespan due to its hydrodynamic characteristics. Due to its excellent hydrodynamic effect and good controlled leakage ability, the waviness end face has been widely applied in the field of the RCP. By utilizing the hydrodynamic effect, the waviness mechanical seal can form a micro-scale thin layer of fluid film between the end faces, which avoids the direct contact between the seal pairs, reduces

the wear and prolongs the life [9]. Because of these outstanding advantages, many studies on the waviness end face mechanical seal have been made [10–14]. The wavy tilt dam (WTD) as one type of the waviness surface was studied by many researchers. The concept of WTD was first proposed by Lebeck and Young [15] who suggest that the hydrostatic and hydrodynamic effects are produced by the radial taper and the circumferential waviness of the end face, respectively, which leads to sufficient opening force and liquid film stiffness, and is suitable for high-parameter conditions. The stability researches of WTD mechanical seal are mainly focus on several aspects. Etsion et al. [13] established a closed analytical solution for the mechanical seal model to study the lubricating film pressure and the axial separating force, whereby the face geometry is combined with waviness and coning. To improve the leakage rate control, Salant et al. [16] simulated the hydraulically controlled RCP's seal under different deformations and geometries of the end face by changing the pressure in the cavity of non-rotating seal ring. In addition to the independent hydrodynamic research, some coupling simulations were also applied to analyze the coupled thermo-hydrodynamic characteristics. To study the 3D detailed behavior of the WTD mechanical seal, based on the Reynolds equation [17,18], Liu et al. [14,19–21] simulated and analyzed the WTD seal based on the three-dimensional thermal elastic hydrodynamic model, and the results showed that the sealing mechanism was the combined effect of hydrodynamic and hydrostatic. The film cavitation occurs at the high velocity region, and the hydrostatic effect prevailed at the high-pressure region. Djamaï et al. [22] established a numerical model of thermo-hydrodynamic mechanical face seals based on the coupling Reynolds equation and energy equation to analyze the influence of operating and design parameters. Brunetière et al. [23] analyzed the influence of the design and operating parameters on the thermo-hydrodynamic behavior of the mechanical end face seals in steady and dynamic tracking modes. To research the influence factors of cavitation starting and evolution, Li et al. [24] analyzed the effects of different waviness amplitudes, numbers and tapers on the cavitation characteristics. The results indicated that the start and evolution of the cavitation were affected by both the waviness and radial taper, and the change of the cavitation region along the circumferential direction was influenced by the waviness, while that along the radial direction depended on the taper.

As for the manufacture of the waviness groove on the sealing end face, the normal processing methods used mainly include the milling, electric spark processing, grinding and etc. Huo et al. [25–27] proposed a three-axis, ultra-precision grinding method using line contact kinematics for machining the WTD seal rings, which can achieve high form accuracy and low surface roughness of the waviness end faces. Han [28] researched the super precision milling process for the waviness end face of the tungsten carbide seal ring. The surface roughness could reach about 7 nm. Wang [29] used the electric spark processing method to pre-machine the waviness end face of the static ring. However, this work should be improved. On one hand, this method has suffers from a long processing time and serious carbon deposits, and on the other hand, the surface roughness cannot meet the requirements of less than 0.4 µm. Recently, Feng et al. [30] proposed a new grinding method through extrusion deformation of the seal ring. The extrusion deformation tooling and metal gaskets were used to deform the sealing ring into a waviness shape. After grinding, the required waviness shape was formed. The experimental results showed that the seal completely satisfies the requirements of nuclear power plant, while it can obtain high accuracy surface roughness and high reliability. In short, as for the field of waviness end face mechanical seal research, the main focus is on the predicting sealing performance by using theoretical models and cavitation characteristics, which are relatively rare in experimental research. The forming of the waviness end face limited to the equipment conditions and process methods is only focused on the research method of the contractible scale model. The leakage of reference work for the research of the prototype leads to a disconnection between the theoretical research and the experimental results.

In view of the above problems, this work, based on the Reynolds equation of liquid film lubrication, combined with the actual processing waviness end face, establishes a liquid film lubrication mathematical model of the mechanical seal which can represent waviness groove. The influences of waviness amplitude, temperature and pressure on the leakage rate of the mechanical seal systematically were studied by comparing the numerical results with experimental results. Moreover, it obtains the difference between theoretical analysis and experimental research, which provides a reference for the parameter optimization design of the seal end face and the coupling study of multiple physical fields.

#### **2. Numerical Analysis**

The mechanical seal of RCP mainly consists of stationary base ring (SBR), rotating slide ring (RSR), stationary slide ring (SSR) and rotating base ring (RBR), as shown in Figure 1a. The structure of SSR is as in Figure 1b.

**Figure 1.** Schematic of the mechanical seal, including (**a**) mechanical seal configuration and (**b**) stationary slide ring (SSR).

#### *2.1. Geometric Model*

The geometric model is composed of rotating slide ring (RSR) and stationary slide ring (SSR), as shown in Figure 2. The lubrication film lies between rotating slide ring and stationary slide ring. Rotating slide ring has an ideal plane on the sealing end face. A uniform circumferential waviness lies on the end face of the stationary slide ring, and a flat dam lies at the inner diameter. The thickness of the liquid film at any position can be expressed as follows:

$$h(r, \hat{\theta}) = \begin{cases} h\_i & , R\_i \le r \le R\_d \\ h\_i + \frac{r - R\_d}{R\_o - R\_d} h\_d (1 - \cos(z \times \hat{\theta})) & , R\_d \le r \le R\_o \end{cases} \tag{1}$$

where the inner and outer radius of the sealing end face are *R<sup>i</sup>* and *Ro*, respectively, the dam radius of the sealing end face is *Rd*, the minimum distance between rotating slide ring and stationary slide ring is *h<sup>i</sup>* , and the waviness amplitude is *ha*. θˆ is the coordinates of the rotating direction.

#### *2.2. Mathematical Model*

In order to establish the mathematical model, the following basic assumptions are listed:


3. The pressure variation along the direction of the film thickness is not considered. This is the basic assumption of Reynolds equation.

**Figure 2.** Model of the sealing gap.

The governing equation of the lubrication film in rectangular coordinates can be expressed by the steady-state Reynolds equation considering cavitation of the liquid film, and the expression is expressed as follows:

$$\frac{\partial}{\partial \mathbf{x}} (\frac{h^3}{12\mu} \frac{\partial p}{\partial \mathbf{x}}) + \frac{\partial}{\partial y} (\frac{h^3}{12\mu} \frac{\partial p}{\partial y}) = \frac{1}{2} \mathcal{U}\_\mathbf{x} \frac{\partial (\theta h)}{\partial \mathbf{x}} + \frac{1}{2} \mathcal{U}\_y \frac{\partial (\theta h)}{\partial y} \tag{2}$$

where µ is the dynamic viscosity, which is defined as:

$$
\mu = \mu\_0 e^{-\beta(T - T\_0)} \tag{3}
$$

where µ<sup>0</sup> is the dynamic viscosity under the reference temperature *T*0; *T* is the local temperature of the fluid film and β is the viscosity-temperature coefficient; *p* is the pressure; *U<sup>x</sup>* and *U<sup>y</sup>* are the shear velocity in the *x* and *y* directions; θ is the ratio of the density of the liquid film during cavitation to that in the liquid state, and when the flow is in full liquid film, θ = 1. When 0 < θ < 1, the flow is in cavitation state.

In order to solve Equation (2), two kinds of boundary conditions need to be added, among which the JFO cavitation boundary conditions for liquid film cavitation is defined as follows:

$$\begin{cases} \ p = p\_{c\prime} 0 < \theta < 1 & \text{in non-cavitation zone} \\ \ p > p\_{c\prime} & \theta = 1 \quad \text{in cavitation zone} \end{cases} \tag{4}$$

The pressure boundary condition is defined as follows:

$$\begin{cases} \ p = p\_l \ r = R\_l\\ \ p = p\_o \ r = R\_o \end{cases} \tag{5}$$

In Equations (4) and (5), *p<sup>c</sup>* is the cavitation pressure of the liquid film and is set to 0 MPa in this work because of the large sealing pressure. Pressure *p<sup>i</sup>* and *p<sup>o</sup>* are respectively the medium pressure at the inner and outer radius of the sealing end face.

The governing equation is calculated using the finite element method (FEM) due to its complication. The convection-diffusion Equation (2) will be convective dominant when the speed of the sealing ring is large, which will lead to numerical oscillation of Galerkin FEM. Therefore, the streamline

upwind/Petrov–Galerkin (SUPG) technology described in reference [31] is used to solve the lubrication Equation (2), and the relevant sealing performance parameters could be calculated after obtaining the liquid film pressure. In order to obtain the sealing performance in the force balance state of the stationary slide ring, the axial force balance equation is solved by using dichotomy method to obtain the minimum film thickness. The axial force balance equation is written as:

$$F\_o = G + F\_s \tag{6}$$

where *F<sup>o</sup>* is the axial opening force, *G* is the gravity of static ring, and *F<sup>s</sup>* is the downward spring force.

The triangular mesh configuration is used in this simulation, and a perturbation term is added to the weight function in the streamline direction, which can suppress the diffusion perpendicular to the flow direction in advance and overcome the false diffusion problem of the upwind discretization. The weak integral form of lubrication control Equation (2) can be written as:

$$\begin{split} & \int\_{\Omega} \left[ \frac{\hbar^{3}}{6\mu} \left( \frac{\partial w}{\partial \mathbf{x}} \frac{\partial p}{\partial \mathbf{x}} + \frac{\partial w}{\partial y} \frac{\partial p}{\partial y} \right) \right] d\Omega - \\ & \int\_{\Omega} \left[ w \Big( \mathcal{U} \frac{\partial(\theta \boldsymbol{h})}{\partial \mathbf{x}} + V \frac{\partial(\theta \boldsymbol{h})}{\partial y} \Big) + \frac{1}{2} \tau^{\text{SIIPC}} \Big( \mathcal{U} \frac{\partial w}{\partial \mathbf{x}} + V \frac{\partial w}{\partial y} \Big) \Big( \mathcal{U} \frac{\partial(\theta \boldsymbol{h})}{\partial \mathbf{x}} + V \frac{\partial(\theta \boldsymbol{h})}{\partial y} \Big) \right] d\Omega = 0 \end{split} \tag{7}$$

where *w* is the weight function and Ω is the calculation domain and τ SUPG is the coefficient of stability. By defining the FEM variables as: *w* = *wiN<sup>i</sup>* , *p* = *piN<sup>i</sup>* , θ = θi*N<sup>i</sup>* with *N* being the interpolation function of element, the Equation (7) can be rewritten as:

$$K\_{i\dot{j}}^p p\_{\dot{j}} - K\_{i\dot{j}}^\partial \theta\_{\dot{j}} = 0 \tag{8}$$

$$\begin{cases} \begin{aligned} K\_{ij}^{\eta} &= \int \frac{\hbar^{3}}{6\mu} \Big( \frac{\partial N\_{i}}{\partial x} \frac{\partial N\_{j}}{\partial x} + \frac{\partial N\_{i}}{\partial y} \frac{\partial N\_{j}}{\partial y} \Big) d\Omega\\ K\_{ij}^{\theta} &= \int \hbar N\_{i} \Big( \mathcal{U} \frac{\partial N\_{j}}{\partial x} + V \frac{\partial N\_{i}}{\partial y} \Big) d\Omega - \int \frac{1}{2} \pi^{S\underline{I}\underline{I}\underline{P}} h \Big( \mathcal{U} \frac{\partial N\_{i}}{\partial x} + V \frac{\partial N\_{i}}{\partial y} \Big) \Big( \mathcal{U} \frac{\partial (\hbar N\_{j})}{\partial x} + V \frac{\partial (\hbar N\_{j})}{\partial y} \Big) d\Omega \end{aligned} \end{cases} \tag{9}$$

To solve Equation (8), the switch function *F* is introduced, and the unknown variable *p* and θ can be expressed using the general variable Φ as:

$$
\Phi = Fp + (1 - F)\theta \tag{10}
$$

For the liquid film intact area, *F* = 1 and Φ = *p*, while for the cavitation area, *F* = 0 and Φ = θ. Substituting Equation (9) into Equation (7), one obtains:

$$A\_{i\uparrow} \Phi\_{\uparrow} = \mathsf{K}\_{ij}^{\theta} F\_{\uparrow} \tag{11}$$

where

$$A\_{i\bar{j}} = K\_{i\bar{j}}^{p} \mathbb{C}\_{i\bar{j}} - K\_{i\bar{j}}^{\theta} (I\_{i\bar{j}} - \mathbb{C}\_{i\bar{j}}) \tag{12}$$

with *I* being the unit matrix; *C* is a matrix whose other areas are 0 except for the same value as *F* on the diagonal. After obtaining the film pressure *p*, the sealing performance parameters such as liquid film bearing capacity, leakage rate and friction coefficient can be calculated.

Since the static seal ring is in floating state, the thickness of the lubricating oil film is determined by the balance between the bearing capacity of the lubricating liquid film and the gravity of the static seal ring, spring force and the static pressure of the sealing medium. Therefore, the balance film thickness of the liquid film needs to be obtained by solving the force balance equation of the static seal ring as:

$$\int p d\Omega - F\_c = 0\tag{13}$$

where *F<sup>c</sup>* is the closing force of the static ring, which is the summation of the gravity *G* of the static ring, the spring force *F<sup>s</sup>* , and the hydrostatic pressure in the sealed cavity.

#### *2.3. Calculating Results and Analysis*

Table 1 shows the geometric and operating parameters used in this work and the materials of the friction pair are carbon and tungsten carbide (WC). Except for special instructions, all the parameters taken in this work are shown in Table 1. The listed waviness amplitude is the actual measured value of the end face of the stationary slide ring manufactured, and is corresponds to Section 2. The simulating parameters are the same as the experimental parameters.


**Table 1.** Geometric and operating parameters.

In Figure 3, it shows the variation law of the minimum liquid film thickness *h<sup>i</sup>* and the leakage rate *Q* with the pressure in balance state. As can be seen from Figure 3a, the minimum liquid thickness decreases first and then increases with the increase of pressure, which is consistent with the research results in literature [5], which is due to the cavitation of the lubrication film under the small film thickness that leads to the enhancement of the hydrodynamic effect of the liquid film. Under the same pressure, the larger waviness amplitude leads to higher minimum liquid film thickness. The hydrostatic effect of the liquid film increases with the waviness amplitude increases. As can be seen from Figure 3b, the leakage rate increases approximately linearly with the increase of the pressure, and the larger waviness amplitude leads to larger leakage rate. Moreover, the upward trend of the leakage rate curve is more obvious.

**Figure 3.** Comparison of minimum fluid film thickness *h<sup>i</sup>* (**a**) and leakage rate *Q* (**b**), including waviness amplitude *<sup>h</sup>a*. The viscosity is taken as 1.003 <sup>×</sup> <sup>10</sup>−<sup>3</sup> kg/(m·s).

#### **3. Experimental Research**

#### *3.1. Manufacture and Experiment of the Sealing Rings*

According to the method and process described in literature [17], three kinds of the morphologies with different waviness amplitude on seal end face of the stationary slide rings are ground by using the metal gaskets with different thickness (δ = 0.12 mm, 0.15 mm and 0.20 mm). In order to make the surface roughness of the sealing end face satisfy the requirement, the grinding powder F1200 named boron carbide (B4C) is used for grinding. Its particle size is 1–7 µm and Vickers hardness is 31 GPa. The final roughness of the sealing end face of the stationary slide ring is about 0.0572 µm. The three stationary slide rings are shown in Figure 4.

**Figure 4.** Manufacture status of the stationary slide rings, including (**a**) δ = 0.12 mm, (**b**) δ = 0.15 mm, (**c**) δ = 0.20 mm.

Each wave groove of the static ring is divided equally in the radial direction, and the detection is recorded by moving slowly from the outer circle of the static ring along the inner circle. The nine waves are measured in nine groups, namely: M1–M9. The 9 waves of each static ring are made of the same metal gasket by compression deformation, which can ensure the same wave amplitude, and the single wave is also the same. The central section of each waviness is used as the measurement section of the waviness amplitude. The height of the waviness is measured and recorded by sliding from the outside to the inside of the sealing end face of the stationary slide ring to obtain the waviness amplitude *ha*. It can be seen from the Figure 5 that the processed waviness has good variation consistency. According to Equation (1), the waviness amplitude *h<sup>a</sup>* of the corresponding metal gasket thickness of 0.12 mm, 0.15 mm, and 0.20 mm is about 5.0 µm, 6.3 µm, and 6.9 µm, respectively.

#### *3.2. Performance Test*

Figure 6 shows the test rig, which consists of the testing device, motor, oil supply unit, charge pump, water reservoir, water deionization system, cooling water cycle, PLC cabinet, DAQ cabinet, cooling water basin, and other components. The test medium is purified tap water (6–8 pH, conductivity ≤ 20 µS/cm) which supplied by the water deionization system and stored in the water reservoir. The high-pressure charge pump supplies the testing device with pressurized barrier water, which is necessary for test rig operation, and is fed directly from the water reservoir. The process water returns from the testing device to the water reservoir via multiple leakage water pipes. The oil supply unit ensures the necessary lubrication of the upper roller bearing of the testing device, and the lower bearing of the testing device is a medium lubricated hydrodynamic bearing. A cooling water basin supplies the water for the cooling pump and should be situated outside of the test bench room. The constant temperature of the water from the cooling water basin ensures the thermal stability of the testing device. The operation and control of the test rig are regulated and controlled by the PLC unit in the

PLC cabinet. The DAQ switching cabinet contains components necessary to collect, record and display data during a test run. The measurement point data collected by the measuring instrument (see Table 2) are fed back to the DAQ unit.

As for the above three kinds of waviness sealing end faces, the measurement of the leakage rate under different temperature and pressure are performed. During the test, the speed of the shaft is 1485 rpm, the pressure is gradually increased to the highest and then decreased (the pressures are 2.0 MPa, 5.3 MPa, 10.6 MPa, and 15.9 MPa respectively). The medium temperature in the sealing chamber and leakage rate of the low-pressure side are recorded in per second. In order to consider the different working pressure, the pressure increase and decrease is applied via three steps. Beginning with about 2.0 MPa, the pressure is increased to 5.3 MPa rapidly (representing normal operation of a 3-stage application). After about 10 min, the pressure goes up to 10.6 MPa (representing normal operation of a 2-stage application), and after 20 min, it goes up to 15.9 MPa (representing accidental load on one stage). Finally, the reduction of the pressure is realized via the same steps within 15 min. The system pressure is changed slowly by adjusting the opening of the ball valve during the whole process to ensure not damaging the test loop and mechanical seal.

**Figure 5.** Measurement of the waviness amplitude, including (**a**) δ = 0.12 mm, (**b**) δ = 0.15 mm, (**c**) δ = 0.20 mm.

**Figure 6.** Test rig.

Figure 7 shows the leakage rate with different waviness amplitudes. The sealing end faces with waviness amplitude 5.0 µm have similar law with the other two (the waviness amplitude is 6.3 µm and 6.9 µm respectively), which will not be repeated here. From these figures, it can be seen that the leakage rate of the seal increases with the increase of the pressure. The leakage rate increases slowly at the beginning of each stage (the slope of leakage rate plot is very small) due to the leakage hysteresis on seal faces, and then increases rapidly in about 200 s (the slope of leakage rate plot is very large). After that, it remained at a stable value. At 2700 s, the pressure instantly dropped from 15.9 MPa to below 10.6 MPa, and the leakage rate did not change suddenly with the instantaneous rapid pressure drop, but slowly decreased. It can be predicted that, if the pressure maintenance time is enough during the pressure relief, the leakage rate can also be at a stable value. Due to the occasional air bubbles in the medium during the test, the measured value will suddenly change after passing through the low-pressure leakage measuring instrument, but then it returns to a stable value. The experimental results show that the waviness end face seal has excellent stability under the constant working conditions. In comparison, the temperature in the seal chamber gradually increases as the test progresses under a lower medium temperature as shown in Figure 7a,b. Although the pressure increases step by step and then decreases during the test, the temperature presents an obvious step change. As shown in Figure 7c, the measured temperature does not increase significantly under a higher medium temperature, which may be caused by the heat generation of the sealing end face that is in equilibrium with the heat dissipation of the test system. Moreover, the high capacity of the tank may also suppress the increase of measured temperature.



**Figure 7.** The leakage rate with different waviness amplitudes, including (**a**) *h<sup>a</sup>* = 5.0 µm, *T* = 30 ◦C, (**b**) *h<sup>a</sup>* = 5.0 µm, *T* = 40 ◦C, (**c**) *h<sup>a</sup>* = 5.0 µm, *T* = 60 ◦C, (**d**) *h<sup>a</sup>* = 6.3 µm, *T* = 30 ◦C, (**e**) *h<sup>a</sup>* = 6.3 µm, *T* = 40 ◦C, (**f**) *h<sup>a</sup>* = 6.3 µm, *T* = 60 ◦C, (**g**) *h<sup>a</sup>* = 6.9 µm, *T* = 30 ◦C, (**h**) *h<sup>a</sup>* = 6.9 µm, *T* = 40 ◦C, (**i**) *h<sup>a</sup>* = 6.9 µm, *T* = 60 ◦C.

#### *3.3. Test Comparative Analysis*

Figure 8 shows the variation trend of measured leakage rate under different waviness amplitudes, pressures and temperatures, which are mean values for all 9 cases. Since the temperature gradually increases with the work of the motor and the seal, it is difficult to maintain a constant during the test period of one minute. The temperature corresponding to the test is an approximate value. Figure 8a shows that, under the same pressure, the leakage rate reaches the maximum and minimum values at 40 ◦C and 60 ◦C, respectively. As shown in Figure 8b, when *h<sup>a</sup>* = 6.3 µm, under the same pressure, the leakage rate reaches the maximum and minimum values at 40 ◦C and 30 ◦C, respectively. Figure 8c shows that when *h<sup>a</sup>* = 6.9 µm, determining the pressure difference ∆*p* at 10.6 MPa or 15.9 MPa, the leakage rate reaches the maximum and minimum values at 60 ◦C and 30 ◦C, respectively. When ∆*p* = 5.3 MPa, the leakage rate is the largest at *T* = 40 ◦C, and is the smallest at *T* = 60 ◦C. According to these conditions, for these three kinds of waviness end face seals, their leakage rates all increase along the increases of pressure. Although the temperature also has a large effect on leakage rate, the change of temperature shows a non-obvious influence on these three waviness end faces, which may be caused by the unstable state of temperature distribution and the large influence of thermal effect on deformation of the end faces of the rotating and stationary slide ring for the mechanical seals. Generally, the increase of temperature will lead to the decrease of viscosity of the lubricating liquid film, and enhances the leakage ability of the liquid film. However, the effect of the temperature on the deformation of the seal end face is not obvious, which affects the actual distribution of the liquid film thickness. Therefore, the influence of temperature on leakage rate still needs to be further analyzed based on thermal elastohydrodynamic theory.

**Figure 8.** The comparison of the leakage rate at different temperature, including (**a**) *h<sup>a</sup>* = 5.0 µm, (**b**) *h<sup>a</sup>* = 6.3 µm, (**c**) *h<sup>a</sup>* = 6.9 µm.

Figure 9 shows the effect of the waviness amplitude *h<sup>a</sup>* on the leakage rate *Q* at the same temperature. When the temperature *T* is 30 ◦C and 40 ◦C and <sup>∆</sup>*p* <sup>≤</sup> 10.6 MPa, the smaller waviness amplitude leads to the larger leakage rate. When ∆*p* = 10.6 MPa, the leakage rate of the waviness amplitude *h<sup>a</sup>* = 6.3 µm suddenly increases, which indicates that the pressure effect on the deformation is obvious under this waviness amplitude state. When the temperature *T* = 60 ◦C, the deformation of the seal rings with different waviness amplitudes varies greatly due to the combined effects of the temperature and pressure.

**Figure 9.** The comparison of the leakage rate at different waviness amplitude, including (**a**) *T* = 30 ◦C, (**b**) *T* = 40 ◦C, (**c**) *T* = 60 ◦C.

#### **4. Comparisons of Test and Simulation Results**

Table 3 shows the comparisons of the test measured and calculated leakage rates under different pressures. It can be seen that the test value is in good agreement with the calculated value for the seal end face with a waviness amplitude *h<sup>a</sup>* = 5 µm, and the calculated values are significantly greater than the test values for the seal face with the larger waviness amplitudes *h<sup>a</sup>* = 6.3 µm and *h<sup>a</sup>* = 6.9 µm.


**Table 3.** Calculation and test results comparison at the different pressures.

The higher sealing pressure leads to the greater deviation between the test and the calculation, since the thermal deformation of the rotating and stationary slide rings for the mechanical seals is not considered in the theoretical model. In addition, under the high sealing pressure and the large waviness amplitude conditions, the seal end face is more likely to generate a non-uniform circumferential liquid film pressure distribution. The pressure distribution causes the ignored axial deformation, which affects the thickness of the lubricant liquid film. Therefore, in order to accurately predict the leakage rate under the high-pressure conditions, it is necessary to consider the thermo-mechanics coupling effect of the entire system, including the sealing rotating slide ring, stationary slide ring, lubricant liquid film, and base rings, and to establish a multi-field coupling model of mechanical seal for analysis.

#### **5. Conclusions**

In the paper, a mathematical model of the waviness mechanical seal for RCP is established to simulate the leakage rate and minimum liquid film thickness. The SUPG finite element method is applied to solve the lubrication equation considering the mass-conservation with JFO cavitation boundary. The predicted leakage rate was taken under different conditions (such as waviness amplitude, pressure, temperature). Three waviness seals were manufactured and tested. Through the comparison of the results between calculation and test, the following conclusions are obtained.


**Author Contributions:** X.F.: conceptualization, methodology, software, validation, formal analysis, data curation, visualization, writing—original draft, writing—review & editing; W.S.: supervision, formal analysis, investigation, resources, project administration, funding acquisition; Y.M.: conceptualization, validation, formal analysis, investigation, resources, data curation, writing—review & editing, project administration, funding acquisition; L.W.: software, validation, formal analysis, data curation; H.T.: formal analysis, investigation, writing—review & editing. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by Natural Science Foundation of Heilongjiang Province of China, Grant number E2018018; National Natural Science Foundation of China, Grant number 51976043 and National Natural Science Foundation of China, Grant number 11875330.

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **References**


**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

© 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (http://creativecommons.org/licenses/by/4.0/).

### *Article* **Numerical Investigation of an Open-Design Vortex Pump with Di**ff**erent Blade Wrap Angles of Impeller**

**Xiongfa Gao 1,\*, Ting Zhao <sup>1</sup> , Weidong Shi 1,2,\*, Desheng Zhang <sup>1</sup> , Ya Shi <sup>1</sup> , Ling Zhou <sup>1</sup> and Hao Chang <sup>1</sup>**


Received: 29 October 2020; Accepted: 1 December 2020; Published: 4 December 2020

**Abstract:** The blade wrap angle of impeller is an important structural parameter in the hydraulic design of open-design vortex pump. In this paper, taking a vortex pump with a cylindrical blade structure as the research object, two kinds of different blade wrap angle of vortex pump impellers are designed. The experiment and numerical simulation research is carried out, and the results of external characteristics and internal flow field are obtained under different flow rate. The results show that when ensuring that other main structural parameters remain unchanged, the efficiency and head of open-design vortex pump increase with the blade wrap angle decreases. In the case of blade wrap angle increasing, the length of rotating reflux back from lateral cavity to inlet is longer. For the same type of vortex pump, the length of rotating reflux to inlet decreases with the increase of flow rate. At the inlet area of impeller front face, there is an area where liquid flows back to the lateral cavity. The volute section shows that after passing through the impeller and lateral cavity, the liquid is discharged to the pump outlet with strong spiral strength. It is found that the blade wrap angle decreases and the shaft power increases, while the pump efficiency increases. The impeller blade wrap angle of vortex pump can be considered to select a smaller value.

**Keywords:** numerical simulation; vortex pump; lateral cavity; open-design; spiral flow

#### **1. Introduction**

Vortex pump is widely used in sewage treatment, slurries, and large particle transportation along with continuous development of industrial and agricultural production. The impeller is installed on one side of the pump cavity, and it has a wide lateral cavity, there are flow of through flow and circulation flow in the pump cavity simultaneously under the rotation of the impeller. This type of pump anti-clogging performance is better. However, this equipment exhibits disadvantages, which include low efficiency and high energy consumption [1]. At present, detailed information is still unavailable for flow fields in vortex pumps. Schivley [2] put forward a flow model to investigate internal flow of vortex pumps and pointed out that fluids can be sucked into pumps under effects of atmospheric pressure when static pressure is negative at central region of the vortex. There is a lateral cavity in the vortex pump, and the impeller has no front cover. Hence, the vortex pump anti-clogging performance is better than that of general centrifugal pumps. However, the pump efficiency is relatively low [3–5].

Numerical simulations of different end clearance conditions were carried out while ensuring that other design parameters remain unchanged.

The influence of pump structure on its performance was experimentally studied by Zheng [6]. A new method was developed in which the volumetric ratio of the lateral cavity to the impeller was used to design vortex pumps. According to the statistics of a number of experimental data,

the authors believe that the pump can get a good performance in the ratio between 3 and 5. Sha et al. [7] combined theory and experiment to derive a unified experience coefficient for use of hydraulic design method on vortex pump, further analyzed the hydraulic model, and inferred experience coefficient for least-square equation of centrifugal slurry and vortex pumps. Liu et al. [8] obtained the influence of the special volute structure of the vortex self-priming pump on its self-priming performance through 2D PIV and numerical calculation. The results show that the combination of the guide wall and the impeller outlet promotes the gas-water mixing and the formation of bubble flow, and improves the self-priming performance. To understand flow conditions in vortex pumps, Alexander Steinmann carried out numerical and experimental investigations [9], with further objective of investigating URANS-CFD (Unsteady Reynolds-Averaged Navier–Stokes -Computational Fluid Dynamics) method using cavitation model for numerical stability and accuracy.

The experiments on changing the axial location of impeller by Sha et al. [10,11], and measurement of flow field in lateral cavity with five-hole probe were conducted on a self-built vortex pump. Based on the experiments, the characteristic performance curves and the absolute velocity, the circumferential velocity, the radial velocity, the axial velocity, and the flow static pressure were obtained. The experimental results proved that the cavitation characteristic curve showed opposite tendency in the operating conditions of small charge compared with centrifugal pump and anti-cavitation were improved with the increase of the scale that impeller was inserted into lateral cavity. In order to study the influence of end clearance of impeller on the performance of a multi-stage pump, a change end clearance of impeller method was studied through CFD by Zhou et al. [12] to analyze performances of pump. The results show that the existence of end clearance, which leads to the flow aggravation separation in the diffuser passage, and further reduces the performance of the pump. The wear characteristics of slurry pump are studied based on particle model under low flow conditions by Peng et al. [13]. The results showed that there was serious local wear in the interface between the sheath and the rotor near the tongue under small flow condition. By removing the front and rear back blades, the wear degree at the junction can be effectively reduced, but the wear of the inner side of the front guard board will be intensified. The author established the apparatus first for measuring the velocity distribution on the axial vertical profile in vortex pump impeller and pressure distribution on blade surface [14]. The measuring methods are explained in more detail and the measured results are presented. An exploratory study on numerical calculation of solid–liquid two-phase flow by Gao et al. [15], the numerical calculation of vortex pump base on CFD-DEM (Discrete Element Model) coupling calculation method, and numerical simulation was carried out under different particle sizes and concentrations, then the rapeseed was used for solid particles to the experiment, and obtained that the values of inlet rotating reflux length under different flow rate conditions. The slurry pump was used to investigate into influences of blade camber profile on pump hydraulic performance and impeller wear characteristic in terms of limestone-water slurry as transported medium [16]. The relationships of both hydraulic performance and wear characteristic with blade camber profile were analyzed numerically in Fluent 16.0 by using discrete phase model (DPM) model. The results show that the cylindrical blade designed by the logarithmic spiral method with variable angle can improve hydraulic efficiency, but will lead to a slight reduction in the head. Wear characteristics in centrifugal pump simulation method are based on DPM model and semi empirical wear model by Zhao et al. [17]. The main wear positions of the centrifugal pump structure components are obtained.

At present, the research on this kind of vortex pump with special structure is scarce. Especially in the open-design vortex pump, if the improper blade wrap angle of impeller was chosen, impeller passage partial blockage and wear will occur, causing performance reduction. Even the pump passage will be blocked and operation is stopped. Therefore, the appropriate blade wrap angle of impeller is crucial for the performance and operation of the vortex pump. This article took a typical open-design vortex pump as the research object, and designed two different type of blade wrap angle of impeller. Numerical simulations of different blade wrap angle of impeller conditions were carried out. The test

validated the effect of impeller blade wrap angle on vortex pump performance and also provided a reference for impeller design and engineering application.

#### **2. Calculation Model**

#### *2.1. Physical Model*

An open-design vortex pump with a specific speed of 166 was selected as the research object. The design flow rate was *Q*des = 400 L/min; rated speed *n* = 1485 r/min. The main impellers structural parameters are shown in Table 1. Figure 1 shows the vortex pump two-dimensional assembly. The blade wrap angle of impeller as shown in Figure 2. In order to facilitate comparative analysis, numerical simulations of different impeller blade wrap angle conditions were carried out with the main impeller parameters unchanged.


**Table 1.** Parameters of impellers.

**Figure 1.** Simple diagram of pump section model.

#### *2.2. Grid Independence Verification*

The computational domains were formed in Unigraphics NX 10.0 software by 2d hydraulic design drawing, as shown in Figure 3, The entire mesh generation was carried out in ICEM 19.0 software, as shown in Figure 4. In theory, with increase in grid element number, errors caused by grid will reduce gradually until they disappear. However, the number of grid elements cannot be too large for the reason of considering computer performance and computer time [18–21].

In this paper, model pump 1 is used for grid independence verification. The structured mesh of computational domains was built based on ANSYS-ICEM 19.0 software (Customer Number: 1079741, NASDAQ:ANSS, Cannonsburg, PA, USA). Four calculation schemes were created with different grid numbers in this paper. The efficiency and head of the pump were taken as grid independence indicators, as shown in Table 2. The values of efficiency and head of Scheme 1 and Scheme 2 are lower than that of other schemes. The efficiency and head value of Scheme 3 are close to that of Scheme 4 as the grid increased, which means that Scheme 3 had achieved the requirement of numerical precision. Hence, considering the calculation performance and calculation time of the computer, Scheme 3 was selected

as the final grid scheme for numerical computation. Meanwhile, the entire computational domain 30 < y+ < 100 was ensured to meet the requirement of standard wall functions [22,23], and the y+ contour of the impeller as shown in Figure 5, and the mesh quality as Table 3. The mesh quality is shown in Table 3, when the value of mesh quality is >0.4, the percentage of the mesh is >99.9%, while the value of mesh quality is >0.67, the percentage of the mesh is >90%.

*ψ β β*

**Figure 2.** Blade wrap angle of impeller. (**a**) Impeller 1, (**b**) impeller 2.

lateral cavity

**Figure 4.** Sketch of the structured mesh: (**a**) impeller; (**b**) close-up view of near the trailing edge; (**c**) volute.


**Table 2.** Grid independence analysis.

**Figure 5.** y+ contour of the impeller.


#### *2.3. Numerical Algorithm*

The calculation domain of pump is divided into two types of subdomains in CFD numerical simulation, which includes a total of five subdomains as shown in Figure 3, namely inlet section, lateral cavity, impeller, volute, and outlet section, and the interfaces are formed between different subdomains. The first type of subdomain includes the inlet section, the lateral cavity, the volute, and the outlet section. The equations for this type of region are solved in a stationary framework. The second type of subdomain is the impeller, which is attached to the rotating frame and solved in a rotating framework via the multiple reference frame (MRF), and the rotational speed was set as 1485 r/min [23].

The flow through the model pump was simulated with the commercial code ANSYS-Fluent 19.0, which uses the finite volume method to solve the Reynolds averaged Navier-Stokes equations for 3D incompressible steady flow. Second order upwind discretization was used for the convective

and the diffusive terms. The time dependent term scheme was second order implicit [24]. The pressure–velocity coupling was calculated by means of the SIMPLE algorithm, and the convergence precision was set to 10−<sup>5</sup> .

The mass-flow rate was specified at the inlet of the CFD domain, and the outlet boundary was assumed to be outflow. At the exit, there is an unavoidable effect on the final flow solution as a result of the boundary conditions. A reasonable length was added to the real machine geometry to avoid this effect as much as possible. At the outlet, which is roughly four impeller-diameters, the gradients of the velocity components are assumed to be zero, and all physical surfaces of the pump were set as the no-slip wall.

The maximum number of iterations is set to 20, and the convergence precision is set to 10−<sup>5</sup> . In the process of iteration, if the convergence accuracy is reached, the next iteration will be carried out. If the convergence accuracy is not reached after 20 iterations, it is also considered to have reached the convergence accuracy and automatically jumps to the next step.

#### *2.4. Turbulence Model*

Predicting the performance of fluid machinery based on CFD, different turbulence models were used to calculate the fluid machinery, and the predicted results were different. There is no universally valid turbulence model which will yield optimum results for all applications [25–27]. It needs to select a turbulence model most suitable for vortex pump to be calculated, and comparing the numerical results with the experimental results for validate. Five turbulence models were selected to calculate in the design condition, namely, the standard *k-*ε model, RNG (Re-normalization group) *k-*ε model, realizable *k-*ε model, standard *k-*ω model, and SST (Shear stress transfer) *k-*ω model.

In Table 4, the test results and the numerical results with different turbulence models were compared. Generally speaking, the RNG *k-*ε and SST *k-*ω models predict the highest pump efficiency and head, and the standard *k-*ε model has the lowest and most close predicted value. Thus, the standard *k-*ε model is chosen for the following numerical calculation. It is should be noted that the standard *k-*ω model also has good predicted accuracy and the lowest computational time. There is around a 10% error with the test data, the reason for the increase in calculation results was probably the neglect of mechanical and leakage losses. The calculated losses in numerical simulation are considered less than the actual losses. The difference may be that in the numerical simulation in this paper, the fluid flow in the gap of rear cover plate is simplified, neglecting the volume losses caused by gap flow.


**Table 4.** Numerical results with different turbulence models at *Q*des.

#### **3. Results and Discussion**

#### *3.1. Pump Performance Test*

In this paper, two impellers with different blade wrap angles are processed by polymethyl methacrylate, as shown in Figure 6. In order to continue the research later, the inlet pipeline is also processed into transparent polymethyl methacrylate. Test rig comprises two parts, namely, data acquisition system and water circulation system [28]. The open test bench is shown in Figure 7, which has the identification from the technology department in Jiangsu province of China. Test facilities and measurement methods abide by measurement requirements described [29]. It includes flow control device, data acquisition device, and data processing device. During the experiment, the flow and pressure were measured by LBBE-50S-M2X102-25 electromagnetic flowmeter (Wuxi Dihua Automation Equipment Co. Ltd., Wuxi, China) and WT2000 pressure sensor (Shanghai Welltech

Automation Co., Ltd., Shanghai, China), and the shaft power was measured by JN338-20A shaft power tester (Wuxi Antok Automation Technology Co. Ltd., Wuxi, China). The range of LBBE-50S-M2X102-25 electromagnetic flowmeter is 30 L/min–850 L/min, the range of JN338-20A shaft power tester is 0–20 N m, the range of inlet pressure transmitter is −100 kpa–100 kpa; the range of outlet pressure transmitter is 0–100 kpa. Then, under the valve opening adjustment, we measure the inlet and outlet pressure and shaft power at different flow rates, and input all the signals into the computer software for calculation. *η*

PS

PS

gQH

gQH

−

−

100

100

**Figure 6.** Impeller of open-design vortex pump. (**a**) Impeller 1; (**b**) Impeller 2.

**Figure 7.** Testing system. 1. Motor; 2. rotational speed meter; 3. test pump; 4. inlet pressure sensor; 5. inlet valve; 6. turbine flowmeter; 7. outlet valve; 8. outlet pressure sensor.

In the pump performance test, pump efficiency is defined as follows [30]:

$$
\eta = \frac{\rho gQH}{P\_S} \times 100\% \tag{1}
$$

where η is pump efficiency, *Q* is flow rate (m<sup>3</sup> /s), *H* is pump head (m), and *P<sup>s</sup>* is output power of motor (*W*).

$$H = \frac{p\_{\rm out} - p\_{\rm in}}{\rho \text{g}},\tag{2}$$

where *pin* is inlet total pressure, and *pout* is outlet total pressure (*pin* and *pout* unit is Pa).

In this paper, experimental and numerical uncertainty analysis was performed [26,31,32]. The experimental total uncertainty is the combination of random uncertainty and systematic uncertainty, while the numerical uncertainty is caused by discretization in CFD applications. The numerical results compared to experimental results are shown in Figure 8. The performance tests under the wrap angle of the two types of impeller blades show that the efficiency and head of the impeller 1 are higher than that of the impeller 2. The numerical calculation results are in good agreement with the experimental

results, and the experimental results are lower than the numerical calculation results, but the error is less than 5%. The change trend is the same under different flow. Therefore, this research method is credible. The reason for the decrease in the calculation result may be that in the numerical simulation in this paper, the fluid flow in the gap of the rear cover plate is simplified, neglecting the volume losses caused by gap flow. According to the references below, the experimental uncertainty in this study was estimated as 2.8%, the numerical uncertainty in this study was estimated as 2.1%.

**Figure 8.** Comparison of pump performance between numerical and experimental results. (**a**) Model pump 1; (**b**) model pump 2.

#### *3.2. Flow Field Analysis*

#### 3.2.1. The Influence of Blade Wrap Angle on Inlet Backflow

At present, there are many studies on the covered design vortex pump. From the existing research conclusions, the vortex pump has both circulating flow and through flow inside. The structure of the open-design vortex pump is different from the impeller design of the covered design vortex pump. The impeller of the open-design vortex pump does not retract to the rear pump cavity, but is on one side of the pump cavity, and its internal flow mode shows different flow characteristics. In this paper, two types of vortex pump models with different impeller blade wrap angles are analyzed by numerical simulation of the full flow field.

Figures 9–11 shows the flow field in inlet region of two model pumps at the flow rates of 0.6*Q*, 1.0*Q*, and 1.4*Q*. It can be seen from the figure that part of the medium flows backwards from the pump cavity to the inlet section along the inlet wall. The direction of rotation of the backflow is consistent with the direction of rotation of the impeller, and it enters the inlet section in a spiral form adjacent to the wall of the inlet pipe, and is constantly mixed with the incoming flow of the inlet, causing the return flow energy to gradually weaken, and finally the return flow and the incoming flow reach equilibrium and stop at a certain position. After analysis, it is found that this backflow into the inlet pipe is caused by the unique structure of the vortex pump. The unique lateral cavity of the vortex pump, and the inlet diameter of the vortex pump is larger than that of the ordinary centrifugal pump, driven by the rotation of the impeller, the lateral cavity produces a circulating flow, driven by the strength of the circulating flow, part of the backflow flows into the pump inlet segment. This part of the backflow causes a large energy loss in the vortex pump.

**Figure 9.** 0.6*Q*des condition. (**a**) Impeller 1; (**b**) Impeller 2.

**Figure 10.** 1.0*Q*des condition. (**a**) Impeller 1; (**b**) Impeller 2.

The values of inlet rotating reflux length under different flow rate conditions are shown in Figure 12. Through the comparison of 3 different working conditions, it can be clearly seen that the stop position of the spiral reflux moves toward the pump cavity under the large flow working condition, which is mainly caused by the increase of the flow speed and the increase of kinetic energy under the large flow working condition. At the same time, the interference degree of the flow characteristic in the middle area of the inlet pipe also decreases as the flow rate increases. Under the same flow condition, when the blade wrap angle is 35◦ , the value of *L* is longer than that of the value of blade wrap angle is 65◦ . Under large flow, the change of the wrap angle of the impeller blade has no obvious effect on the stop position of the inlet spiral reflux.

Blade

Blade 3

Blade 5

**Spiral** 

**Figure 11.** 1.4*Q*des condition. (**a**) Impeller 1; (**b**) Impeller 2.

**Figure 12.** The values of inlet rotating reflux length under different flow rate conditions.

3.2.2. The Influence of the Blade Wrap Angle on the Flow Characteristic of the Impeller Front Face

In order to further explore the development process of the circulating flow in the pump cavity, focusing on the flow characteristics of the lateral cavity and the impeller, the axial velocity distribution at the impeller front face is analyzed under the two impeller blade wrap angles. The blade number is defined in Figure 13. Take the intersection line of the front face of the blade with the pressure side and the suction side respectively, and name them from blade 1 to blade 10 in turn according to the rotation direction of the impeller, and the blade 1 is located at the first section under the tongue. In Figures 14–16, ps represents the intersection line of pressure side and the front face, ss represents the intersection line of the suction side and the front face. Since the positive direction of the Z-axis is set to be opposite to the inlet flow velocity during modeling, a negative axial velocity means fluid flows into the impeller, and a positive axial velocity means fluid flows from the impeller into the pump cavity. The ratio of the position of a point on the intersection line to the radius of the impeller are treated as dimensionless to indicate the relative position of the data point, that is the length–diameter ratio r/R (r represents the vertical distance from a point in the pump to the axis, R represents the radius of the impeller). The relative velocity of a point on the intersection line can be obtained by numerical simulation as shown in Figures 14–16.

**Z** 

Blade 9

Blade 7

ps1 ss1

**(m/s)**

0.4 0.6 0.8 1.0 1.2 1.4 1.6

des

 Model Pump 1 Model Pump 2

Rotating reflux length

/mm

**Figure 13.** Schematic of blade number.

ps1 ss1

**0**

**Figure 14.** 0.6*Q*des condition. (**a**) Model pump 1; (**b**) model pump 2.

**Figure 15.** 1.0*Q*des condition. (**a**) Model pump 1; (**b**) model pump 2.

**Figure 16.** 1.4*Q*des condition. (**a**) Model pump 1; (**b**) model pump 2.

Due to the existence of lateral cavity, the flow characteristic in the pump cavity is more complicated than that of ordinary centrifugal pumps. The main reason is that the impeller is semi-open and has no front cover. The front face of the impeller is connected with the lateral cavity. This special structure makes the impeller area and the lateral cavity have fluid exchange flow, and the internal flow characteristic is very complicated.

A part of the fluid in the impeller passage enters the lateral cavity directly from the impeller front face. This part of the fluid contains large circumferential kinetic energy due to the rotation of the impeller, which can further drive the fluid in the pump cavity to do circumferential movement, and also affects the flow of the inlet section of pump.

It can be clearly seen from Figures 14–16 that under 0.6*Q*des, 1.0*Q*des, and 1.4*Q*des flow rate conditions, the axial velocity of the fluid at the pressure side of the impeller front face changes from negative to positive, which indicates that the fluid in the latter half of the blade begins to flow out into the lateral cavity. The flow characteristics are mainly concentrated in the middle and rear sections of the blade pressure side. Due to the large inlet pipe diameter of this type of vortex pump, the ratio of pump inlet radius to impeller radius r/R is 0.74, and the inlet flow has a greater impact on the front end of the impeller. Therefore, the value of r/R of the impeller front face is about 0.74, where the area becomes a boundary area for liquid in and out. For the suction side, except for the area after value of r/R 0.95, the values of axial velocity are negative, indicating that the liquid flow from the lateral cavity into the impeller at the entire suction side area. The axial velocity of the suction side of the blade tail turned from a negative value to a positive value, there is liquid entering the lateral cavity in this area. This phenomenon may be caused by the rotation of the impeller and the existence of circulating flow in the lateral cavity.

From the two model pumps, under small flow conditions, in the transition area between the impeller front face and the lateral cavity, the axial velocity values of the blade pressure sides show large differences, such as intersection lines of ps1, ps3 and ps5, indicating that in this area, axial velocity is disordered, while the axial velocity value of the intersection lines of suction side is relatively stable. With the increase of the flow rate, the circumferential velocity trends of the pressure side and suction side of each intersection line in the impeller front face are basically the same.

At 0.6*Q*des condition, the r/R value of model pump 1 and model pump 2 is about 0.55, the liquid starts to flow out from the impeller pressure side to the lateral cavity. For model pump 2, when the value of r/R is about 0.6, the liquid starts to flow out of the impeller pressure side into lateral cavity. When the flow rate increases to 1.4*Q*des, the r/R value of the model pump 1 and model pump 2 are 0.6

**(m/s)**

and 0.7, respectively, the liquid from the pressure side flow out to the lateral cavity. Thus, with the flow rate increases the r/R value, where liquid from the pressure side flow into the lateral cavity increases.

**0**

**(m/s)**

**0.4 0.5 0.6 0.7 0.8 0.9 1.0**

**0**

 ps1 ss1 ps3 ss3 ps5 ss5 ps7 ss7 ps8 ss8 ps9 ss9 ps10 ss10

3.2.3. The Influence of Blade Wrap Angle on the Flow Characteristic inside the Volute

**0.4 0.5 0.6 0.7 0.8 0.9 1.0**

 ps1 ss1 ps3 ss3 ps5 ss5 ps7 ss7 ps8 ss8 ps9 ss9 ps10 ss10

The vortex pump has lateral cavity and the volute is asymmetric, so it is very important to analyze the flow characteristic in the volute. In this paper, four sections of the volute were selected as shown in Figure 17, namely sections I, III, V, and VII, and analyzed for streamline velocity.

**Figure 17.** Volute sections.

The velocity streamline contours of the four sections in volute are shown in Figures 18–20. The relative velocity in the volute chamber presents non axisymmetric distribution, and the velocity in the volute decreases gradually from the first section of the volute to the outlet of the volute, which shows that the dynamic energy is gradually transformed into the pressure energy. From the first section of the volute to the outlet, the liquid entering from the impeller and the lateral cavity is discharged out of the volute outlet in a spiral flow state. Section I is at the volute tongue. Due to the blocking effect of the tongue, there is no spiral flow in the section, the spiral flow is gradually formed from the section I to the outlet of the volute. For the model pump 1, under small flow and rated flow conditions, it is found from the streamline velocity contour of section III that two spiral vortices of different sizes occur, the spiral vortex on the left is in a counterclockwise direction, the spiral vortex on the right flows in a clockwise direction. With the sectional area of the volute increases, these two spiral vortices increase. When the sectional position of the volute increases to VII, the spiral vortex on the left disappears, and the strength of the spiral vortex on the right increases to occupy the entire volute. Under the large flow rate condition, only the right side (The corresponding side of the impeller) of the volute forms a spiral vortex.

Under the same flow rate condition, the model pump 2 streamline velocity contour compares to model pump 1, it is found that at 0.6*Q*des condition, there is a small spiral vortex near the wall in the left side of the III, V section, and the spiral vortex is smaller than that of model pump 1. Under the conditions of 1.0*Q*des and 1.4*Q*des, there is only a large spiral vortex generated on the right side of the volute. The spiral vortex on the right moves to the middle area of the volute with the increase of the volute section. When the volute section is larger than the seventh section, the spiral vortex occupies the whole volute space, and the liquid is flow to the pump outlet in a spiral shape.

**Figure 18.** 0.6*Q*des streamline diagram of volute section. (**a**) Model pump 1; (**b**) model pump 2.

**Figure 19.** 1.0*Q*des streamline diagram of volute section. (**a**) Model pump 1; (**b**) model pump 2.

Generally speaking, there is a large vortex area in the volute, which mainly occurs in the corresponding side of the impeller. Under the same flow rate condition, the velocity of the volute in model pump 2 is lower than that of model pump 1, this is consistent with the result that the head of model pump 1 is higher than that of model pump 2, which is consistent with the previous comparison and analysis of external characteristics, the previous performance curve also shows this.

As the blade wrap angle increases, the flow passage of impeller becomes narrower, and the binding force of the blade to the liquid in the passage increases, while the pump efficiency decreases. The reduced blade wrap angle can widen the flow passage and weaken the blade's binding force to the liquid in the flow passage. It will also increase circulating flow in the lateral cavity and improve the efficiency. It is suggested that a smaller blade wrap angle should be considered.

ൌ

 ൌ ଵ ଶ ሺ డ௨ డ௫ೕ െ డ௨ೕ డ௫ ሻ

 Ω ൌ ଵ ଶ ሺ డ௨ డ௫ೕ డ௨ೕ డ௫ ሻ

 Q ൌ <sup>ଵ</sup> ଶ ሺ∣∣ Ω<sup>ଶ</sup>

Ω

∙Ω |||Ω|

∣∣ െ∣∣ <sup>ଶ</sup>

∣∣ሻ

s ିଶ −

*Processes* **2020**, *8*, 1601

**Figure 20.** 1.4*Q*des Streamline diagram of volute section. (**a**) Model pump 1; (**b**) model pump 2.

#### 3.2.4. Vorticity Analysis in the Volute

− In this paper, the regularized helicity *H<sup>n</sup>* is used to determine the vortex core [33]. This method mainly captures the position of the vortex core according to the angle between the velocity vector and the vorticity. It is defined as the modeling of the point product of the velocity and the vorticity, which is used to judge the rotation direction of the vortex core. The value is [−1, 1], the vortex turns counterclockwise with positive *Hn*, while it turns clockwise with negative *H<sup>n</sup>* [33].

$$H\_{\rm nl} = \frac{w \cdot \Omega}{|w||\Omega|}\tag{3}$$

Ω where *w* is relative velocity, Ω is absolute vorticity.

$$S\_{ij} = \frac{1}{2} (\frac{\partial u\_i}{\partial \mathbf{x}\_j} - \frac{\partial u\_j}{\partial \mathbf{x}\_i}) \tag{4}$$

$$
\Omega\_{ij} = \frac{1}{2} (\frac{\partial u\_i}{\partial \mathbf{x}\_j} + \frac{\partial u\_j}{\partial \mathbf{x}\_i}) \tag{5}
$$

$$Q = \frac{1}{2} \left( \|\Omega^2\| - \|\mathbb{S}^2\| \right) \tag{6}$$

where *S* is the strain rate tensor.

s ିଶ The *Q* criterion is selected to identify the vortex in this paper. The imaging vortex structure in the pump cavity is shown in Figure 21a,b. When *Q* = 54,288 s −2 , the strong vortex structure is observed in the areas of the impeller outlet volute tongue. The vortex structure of the impeller rim area is symmetrical, and there are obvious vortices in the lateral cavity near the pump inlet area. With the *Q* value increases to 5301 s −2 , strong vortices appear inside the volute, especially on the Sections I to V of the volute. The vortices are widely distrusted in the lateral cavity, and the vortex strength is greater near the pump inlet. The reason of the strong vortices occurring in the lateral cavity is mainly attributed to the rotation of the main flow in the cavity driven by the spinning impeller. There is a strong and wide vortex area in the entire pump cavity, mainly because the vortex pump has lateral cavity and there is circulating flow in the lateral cavity. The asymmetry of volute leads to the wide and complex vortex area in the whole pump cavity. In addition, a strong vortex appears in the tongue area and it flows to the exit of the volute due to the through flow.

ଶ

s ିଶ

s ିଶ

s ିଶ

s ିଶ

<sup>−</sup> <sup>−</sup> **Figure 21.** Vortex structures of pump cavity: (**a**) *Q* = 54,288 s−<sup>2</sup> ; (**b**) *Q* = 5301 s−<sup>2</sup> .

Figure 22a show the vortex distribution in the volute diffuser region with *Q* = 5301 s −2 . Five section faces are made at an average interval of 22 mm in the volute diffuser region. It is found that there is a strong vortex flow in the diffusion region. The vortex flow occurs in the front of the volute diffuser region and moves vertically to the outlet of the volute. The formation of vortex flow may be caused by the existence of a tongue and lateral cavity. The *H<sup>n</sup>* of the volute diffuser region is shown in Figure 22b, and the vortex core distribution in the volute diffuser region is relatively disordered. In particular, the vortex cores in the tongue region, and both clockwise and counterclockwise rotating vortices occurred, especially the counterclockwise rotating vortices were produced in lager area of volute diffuser region. The clockwise rotating vortices occurred in the front wall of the volute diffuser region, and the vortex cores move from the front side of the tongue to the middle side of the outlet. It was found that the liquid is discharged to the volute outlet in the form of a spiral by analyzing Figure 22. − −

**Figure 22.** Vortex structure of volute diffusion section: (**a**) Module distribution of vorticity; (**b**) *Hn*.

#### **4. Summary**

In this paper, two types of vortex pumps with different impeller blade wrap angles have been numerically simulated and experimentally studied under different flow conditions. Through numerical simulation and experiments, performance curves and internal flow field results have been obtained. The conclusions include the following aspects.


flows out from the back half of impeller into the lateral cavity. In the suction side, the fluid in the lateral cavity flows back to the impeller. It shows that fluid flows in and out of the front face of the impeller, which leads to a decrease in hydraulic performance.

(3) Since the impeller is installed on one side of the pump cavity, as the blade wrap angle increases, the flow passage of impeller becomes narrower, and the binding force of the blade to the liquid in the passage increases, while the pump efficiency decreases. The reduced blade wrap angle can widen the flow passage and weaken the blade's binding force to the liquid in the flow passage. It will also increase circulating flow in the lateral cavity and improve the efficiency. It is suggested that a smaller blade wrap angle should be considered.

**Author Contributions:** Conceptualization, X.G. and W.S.; methodology, X.G. and W.S.; software, Y.S.; validation, H.C. and W.S.; formal analysis, X.G.; investigation, D.Z.; resources, X.G.; data curation, T.Z.; writing—original draft preparation, X.G.; writing—review and editing, W.S. and H.C.; visualization, L.Z.; supervision, W.S.; project administration, W.S.; funding acquisition, X.G. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was funded by the National Natural Science Foundation of China (Grant No. 51909108), National Natural Science Foundation of China (Grant No. 51979138).

**Conflicts of Interest:** The authors declare no conflict of interest.

#### **Nomenclature**


#### **References**


**Publisher's Note:** MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations.

© 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (http://creativecommons.org/licenses/by/4.0/).

*Article*
