**The E**ff**ect of Root Clearance on Mechanical Energy Dissipation for Axial Flow Pump Device Based on Entropy Production**

#### **Yanjun Li <sup>1</sup> , Yunhao Zheng <sup>1</sup> , Fan Meng 1,\* and Majeed Koranteng Osman 1,2**


Received: 8 October 2020; Accepted: 17 November 2020; Published: 20 November 2020

**Abstract:** The axial flow pump is a low head, high discharge pump usually applicable in drainage and irrigation facilities. A certain gap should be reserved between the impeller blade root and the impeller hub to ensure the blade adjustability to broaden the high-efficiency area. The pressure difference between its blade surface induces leakage flow in the root clearance region, which decreases hydraulic performance and operational stability. Therefore, this study was carried out to investigate the effect of root clearance on mechanical energy dissipation using numerical simulation and entropy production methods. The numerical model was validated with an external characteristics test, and unsteady flow simulations were conducted on the axial flow pump under four different root clearance radii. The maximum reductions of 15.5% and 6.8% for head and hydraulic efficiency are obtained for the largest root clearance of 8 mm, respectively. The dissipation based on entropy theory consists of indirect dissipation and neglectable direct dissipation. The leakage flow in the root clearance led to the distortion of the impeller's flow pattern, and the indirect dissipation rate and overall dissipation of the impeller increased with increasing root clearance radius. The inflow pattern in the diffuser was also distorted by leakage flow. The diffuser's overall dissipation, indirect dissipation rate on the blade surface, and indirect dissipation rate near inlet increased with increasing root clearance radius. The research could serve as a theoretical reference for the axial flow pump's root clearance design for performance improvement and operational stability.

**Keywords:** axial-flow pump; root clearance radius; computational fluid dynamics; entropy production; energy dissipation

#### **1. Introduction**

The axial flow pump is a high flow rate pump with a low head, usually applied in drainage and irrigation engineering [1,2]. In this pump, the fluid approaches the impeller axially and leaves but with a swirling motion resulting from the impeller rotation. To effectively improve on its performance characteristics, an adjustable blade angle has been proven to widen the operating range of the axial flow pump, with an impeller tip clearance (radial clearance between impeller rim and impeller housing) [3–5] and root clearance (radial clearance between impeller hub and impeller root) [6]. However, the pressure difference between the suction side and the blade's pressure side induces leakage flow in the tip clearance [7,8] and root clearance regions. This can generate flow blockage within the impeller passage [9,10], resulting in decreased hydraulic performance and operational stability [11–13]. In comparison, the tip clearance region is more susceptible to cavitation and clearance leakage vortices due to the large internal velocity circulation compared to the root clearance.

Laborde et al. [14] studied the effect of clearance geometry, clearance height, and the operating condition on tip vortex cavitation in an axial flow pump by visual experiment. Farrell et al. [15] built a correlation of variables to predict the vortex minimum pressure. This was validated by experimental tests and other existing data from the literature. Zhang et al. [16] analyzed tip leakage flow structure and the evolution of tip vortex based on a modified filter-based turbulence model. Wu et al. [17,18] performed the particle image velocimetry test to study the tip leakage flow structure and the formation process of tip leakage vortex in the water-jet pump. Although circumferential velocity was low, and the flow was relatively stable in the axial flow pump's root clearance, excessive root clearance would also significantly impact the hydraulic performance. If the blade root clearance were rather too small, the blade's adjustability would be affected, resulting in a reduction of the high-efficiency operation range. Considering the state of the art, the root clearance of the axial flow pump has not been extensively researched, and therefore there is the need to investigate further the flow losses and loss mechanisms in the blade root clearance of the axial flow pump.

In identifying and evaluating hydraulic loss distributions in pumps, entropy production analysis has become very popular since it can help the pump designer improve hydraulic performance. In the past, local entropy production based on empirical correlations was applicable to laminar flow problems only [19,20]. However, in 2003, Kock et al. [21,22] proposed a calculation model of local entropy production suitable for turbulent shear flows by Reynolds-averaging the entropy generation equation. The local entropy could be estimated from calculation results from Computational Fluid Dynamics (CFD) using a proposed calculation model without solving the transport equation. This method has been widely used to obtain the spatial distribution of hydraulic losses in pumps [23–25].

In this paper, the root clearance radius on energy dissipation in the axial flow pump was studied. The axial flow pump's external characteristic test was first performed at two root clearance radii (0 mm and 2.7 mm) to validate the numerical model. The theory of entropy production was then applied to the unsteady calculation results with 4 root clearance radii (0 mm, 2.7 mm, 5 mm, and 8 mm) to identify the effect of the flow rate and root clearance radius on energy losses for each hydraulic component. Finally, the loss distribution and mechanism resulting from indirect dissipation within the impeller and diffuser were analyzed, and a reference was established for root clearance design in the axial flow pump.

#### **2. Numerical Simulation**

#### *2.1. Computational Domain*

Figure 1 shows that the axial flow pump model consists of an elbow inflow runner, an axial flow impeller, a diffuser, and an outflow runner. In this paper, the pump performance, and four kinds of root clearance radius (0 mm, 2.7 mm, 5 mm, 8 mm) of impeller were designed. The main design and geometry parameters of the pump model are shown in Table 1, and the specific speed was calculated based on Equation (1) [26]:

$$m\_s = \frac{3.65nQ\_{\rm des}^{0.5}}{H\_{\rm des}^{0.75}}\tag{1}$$

where *n<sup>s</sup>* and *n* stand for the specific speed and shaft rotational speed, respectively, *Q*des presents the design volume flow rate, and *H*des is the design pump head.

In order to precisely analyze the detailed flow loss distributions within the gap position, ANSYS ICEM was used to generate high-quality structural hexahedral grids for the inflow runner, impeller, and outflow runner. Turbogrid was used to generate grids of the diffuser automatically. Figure 2 presents the mesh of the calculation domain. The average Y<sup>+</sup> of impeller and diffuser were 10.1 and 10.9, respectively. For the inflow runner and outflow runner, the average Y<sup>+</sup> values were 5.0 and 15.4, respectively. In ensuring the simulation's speed and accuracy, a grid independence analysis of the pump was conducted in Figure 3. When the total number of grid nodes of pump exceeded 5.6 million, the calculation results were seen to be stable, and the relative error of the efficiency was

within 0.15%. Therefore, to ensure the calculation accuracy and save calculation resources, the number of grid nodes of inflow runner, impeller, guide vane, and outflow runner was finally controlled at 1.8 million, 1.2 million, 1.5 million, and 1.5 million, respectively.

**Figure 1.** 3D model of the axial flow pump device.


**Table 1.** Main parameters of the axial flow pump device.

of impeller and diffuser

ij i

( )

)

[( ) ] +

**Figure 2.** Mesh of axial flow pump device.

381.8 467.9 560.8 671.9

Nodes number /(×10<sup>4</sup>

j j 0

j i j j

i j i i

*ω ω*

j j 3j

( ) ( )

j

( ) ( ) <sup>t</sup>

*ω*

76.0

77.0

78.0

*ƞ*/%

79.0

<sup>ᇱ</sup> ᇱ *Processes* **2020**, *8*, 1506

**Figure 3.** Grid independence of pump device without root clearance.

#### *2.2. Boundary Condition*

In this study, 25 ◦C was chosen as the temperature of the working fluid. The governing equation was Reynolds Averaged Navier–Stokes (RANS) equation, which is defined as follows:

$$\frac{\partial \overline{v}\_{\overline{\}}}{\partial \mathbf{x}\_{\overline{\}}} = \mathbf{0} \tag{2}$$

 Middle section grid of impeller and diffuser

$$\frac{\partial(\rho \overline{v}\_{\text{i}})}{\partial t} + \frac{\partial(\rho \overline{v}\_{\text{i}} \overline{v}\_{\text{j}})}{\partial \mathbf{x}\_{\text{j}}} = -\frac{\partial \overline{p}}{\partial \mathbf{x}\_{\text{i}}} + \frac{\partial}{\partial \mathbf{x}\_{\text{j}}} (\mu \frac{\partial \overline{v}\_{\text{i}}}{\partial \mathbf{x}\_{\text{j}}} - \overline{\rho v'\_{\text{i}} v'\_{\text{j}}}) + \rho f\_{\text{i}} \tag{3}$$

j i j j where *<sup>i</sup>* and *<sup>j</sup>* stand for cartesian direction; <sup>∂</sup>*v*<sup>j</sup> ∂*x*j = 0 and *p* present the time-average speed and time-average pressure, respectively; ρ and µ stand for the fluid density and the dynamic viscosity. ρ*v* ′ i*v* ′ j is the Reynolds stress and ρ *f*<sup>i</sup> is the source item.

<sup>ᇱ</sup> ᇱ *ω* The *SST k-*ω turbulence model [27,28] was used to enclose the Equation. It was a Baseline (BSL) *k-*ω model with a limiter to the formulation of eddy-viscosity. The Baseline (BSL) *k-*ω model can be described as follows:

*ω ω*

$$\frac{\partial(\rho k)}{\partial t} + \frac{\partial(\rho v\_{\text{j}} k)}{\partial \mathbf{x}\_{\text{j}}} = \frac{\partial}{\partial \mathbf{x}\_{\text{j}}} [ (\mu + \frac{\mu\_{\text{t}}}{\sigma\_{k3}}) \frac{\partial \mathbf{k}}{\partial \mathbf{x}\_{\text{j}}} ] + P\_{\text{k}} - \beta' \rho k w + P\_{k\text{b}} \tag{4}$$

$$\frac{\partial(\rho\omega)}{\partial t} + \frac{\partial(\rho v\_j\omega)}{\partial \mathbf{x}\_j} = \frac{\partial}{\partial \mathbf{x}\_j} [ (\mu + \frac{\mu\_l}{\sigma\_{a3}}) \frac{\partial \omega}{\partial \mathbf{x}\_j} ] + 2\rho (1 - F\_1) \frac{1}{\sigma\_{a2}\omega} \frac{\partial k}{\partial \mathbf{x}\_j} \frac{\partial \omega}{\partial \mathbf{x}\_j} + a\_3 \frac{\omega}{k} P\_k - \beta\_3 \rho \omega^2 + P\_{ab} \tag{5}$$

The coefficient σ*k*<sup>3</sup> is a linear combination of σ*k*<sup>1</sup> and σ*k*<sup>2</sup> ; σω<sup>3</sup> is a linear combination of σω<sup>1</sup> and σω2; α<sup>3</sup> is a linear combination of α<sup>1</sup> and α2; β<sup>3</sup> is a linear combination of β<sup>1</sup> and β2. *Pkb* and *P*ω*<sup>b</sup>* are buoyancy production terms; µ<sup>t</sup> is turbulence viscosity.

The calculation method of linear combination is as follows:

$$
\Phi\_3 = F\_1 \Phi\_1 + (1 - F\_1) \Phi\_2 \tag{6}
$$

where σ*k*<sup>1</sup> = 1.176, σω<sup>1</sup> = 2, β<sup>1</sup> = 0.075, α<sup>1</sup> = 5/9, β′ = 0.09, σ*k*<sup>2</sup> = 1, σω<sup>2</sup> = 1/0.856, α<sup>2</sup> = 0.44, β<sup>2</sup> = 0.0828. The *F<sup>1</sup>* is a blending function of the wall distance, the value of which is 1 near the wall and decreases to 0 outside the boundary layer.

In order to improve the prediction accuracy of *k*-ω model for 3D flows, the shear stress transfer model (*SST*) should be applied to limit the formulation of eddy-viscosity.

$$\upsilon\_{\text{l}} = \frac{\alpha\_{\text{l}} k}{\max(\alpha\_{\text{l}} \omega\_{\text{}} S \mathcal{F}\_{\text{2}})} \tag{7}$$

$$\nu\_{\rm t} = \frac{\mu\_{\rm t}}{\rho} \tag{8}$$

where *F<sup>2</sup>* is a blending function similar to *F1*.

Inlet and outlet boundary conditions were set as "Mass flow rate" and "Opening", respectively. The reference pressure was 1 atm, and the outlet relative pressure was 0 atm. The no-slip wall and automatic wall function [29] was adopted as the wall condition for each hydraulic component. In addition, the roughness of the impeller and diffuser was set as 0.0125 mm, and that of the inflow runner and outflow runner was set as 0.05 mm.

Five flow conditions, 0.8 *Q*des 0.9 *Q*des 1.0 *Q*des 1.1 *Q*des and 1.2 *Q*des were analyzed based on unsteady calculation. The time step and total time were set as 0.000373134s and 0.447761s, respectively. The interface condition between rotor and stator was set as "Transient rotor stator" [30], and the interface condition between stators was set as "None". In each time step, when the residual value of convergence was less than 5 <sup>×</sup> <sup>10</sup>−<sup>5</sup> or the number of iteration steps reached 10, the calculation would stop. In addition, the advection scheme and transient scheme were set as "Upwind" and "second order Backward Euler."

#### *2.3. Entropy Production Theory*

The entropy production model's derivation was based on the entropy transport equation (Equation (9)), which was applied to the single-phase incompressible fluid [27].

$$\rho(\frac{\partial \mathbf{s}}{\partial t} + v\_1 \frac{\partial \mathbf{s}}{\partial \mathbf{x}} + v\_2 \frac{\partial \mathbf{s}}{\partial y} + v\_3 \frac{\partial \mathbf{s}}{\partial z}) = \text{div}(\frac{\vec{q}}{T}) + \frac{\phi}{T} + \frac{\phi\_\theta}{T^2} \tag{9}$$

where *s* is the specific entropy; *v*1, *v*2, *v*<sup>3</sup> are the velocity components in Cartesian direction: *x*, *y*, *z*; *T* is the temperature. div( → *q T* ) stands for reversible heat transfer term. <sup>φ</sup><sup>θ</sup> *<sup>T</sup>*<sup>2</sup> and <sup>φ</sup> *T* present the entropy production by heat transfer and the entropy production by dissipation.

An isothermal heat transfer rate was set to render the system into a thermal equilibrium state. Hence, <sup>φ</sup><sup>θ</sup> *<sup>T</sup>*<sup>2</sup> and div( → *q T* )were neglected.

Because all calculated results were based on RANS equation. <sup>φ</sup> *T* should be time-averaged. ( φ *T* ) can be divided into the entropy production by direct dissipation <sup>φ</sup>*<sup>D</sup> T* and entropy production by indirect dissipation <sup>φ</sup>*<sup>I</sup> T* . φ*<sup>D</sup> T* and <sup>φ</sup>*<sup>I</sup> T* are defined as follows.

$$\overline{\left(\frac{\partial \mathbf{\bar{D}}}{\overline{T}}\right)} = \frac{\mu}{\overline{T}} \cdot \left[ 2 \left( \left(\frac{\partial \overline{\mathbf{v}\_1}}{\partial \mathbf{x}}\right)^2 + \left(\frac{\partial \overline{\mathbf{v}\_2}}{\partial \mathbf{y}}\right)^2 + \left(\frac{\partial \overline{\mathbf{v}\_3}}{\partial z}\right)^2 \right) + \left(\frac{\partial \overline{\mathbf{v}\_1}}{\partial \mathbf{y}} + \frac{\partial \overline{\mathbf{v}\_2}}{\partial \mathbf{x}}\right)^2 + \left(\frac{\partial \overline{\mathbf{v}\_3}}{\partial \mathbf{x}} + \frac{\partial \overline{\mathbf{v}\_1}}{\partial z}\right)^2 + \left(\frac{\partial \overline{\mathbf{v}\_2}}{\partial z} + \frac{\partial \overline{\mathbf{v}\_3}}{\partial \mathbf{y}}\right)^2 \right] \tag{10}$$

$$\overline{\left(\frac{\phi\_1}{T}\right)} = \frac{\mu}{T} \cdot \left[ 2 \overline{\left(\frac{\partial v'\_1}{\partial \mathbf{x}}\right)^2} + \overline{\left(\frac{\partial v'\_2}{\partial y}\right)^2} + \overline{\left(\frac{\partial v'\_3}{\partial z}\right)^2} \right] + \overline{\left(\frac{\partial v'\_1}{\partial y} + \frac{\partial v'\_2}{\partial x}\right)^2} + \overline{\left(\frac{\partial v'\_3}{\partial \mathbf{x}} + \frac{\partial v'\_1}{\partial z}\right)^2} + \overline{\left(\frac{\partial v'\_2}{\partial z} + \frac{\partial v'\_3}{\partial y}\right)^2} \right] \tag{11}$$

where *v*1, *v*2, *v*<sup>3</sup> are time-average velocity; *v* ′ <sup>1</sup>, *v* ′ <sup>2</sup>, *v* ′ <sup>3</sup> are instantaneous velocity fluctuation.

Because the *v* ′ <sup>1</sup>, *v* ′ <sup>2</sup>, *v* ′ <sup>3</sup> cannot be obtained when solving the RANS equation, Kock et al. [22] proposes another method and the <sup>φ</sup><sup>I</sup> *T* can be calculated as follows:

$$\frac{\rho\_{\rm I}}{\overline{T}} = \frac{\rho\_{\rm \varepsilon}}{\overline{T}}\tag{12}$$

The overall dissipation of each hydraulic component can be obtained by integrating the dissipation rate over the whole fluid-producing domain as follows:

$$P\_{\rm D} = \int\_{V} \phi\_{\rm D}dV\tag{13}$$

*Processes* **2020**, *8*, 1506

$$P\_{\rm I} = \int\_{V} \phi\_{\rm I}dV\tag{14}$$

where *P*<sup>D</sup> represents direct power loss, and *P*<sup>I</sup> represents indirect power loss.

#### **3. Test Measurement**

#### *3.1. Test Equipment*

The closed test bench adopted a double-floor vertical structure, as shown in Figure 4. The flow meter was located on the −2.6 m floor, and the pressure transducers and torque meter were located on the 4.2 m floor. The basic parameters of test equipment are shown in Table 2. In addition, the flowmeter was arranged horizontally, and the length of straight pipes was greater than five times the pipe diameter. The test measuring point of the head was located on the inlet and outlet water tank.

**Figure 4.** Photo of the axial flow pump device.

**Table 2.** Basic parameters of test equipment.


#### *3.2. Test Validation*

௨௧

≤ Figure 5 shows the external characteristic test results of an axial flow pump with two different root clearance radii (0 mm and 2.7 mm). The hydraulic efficiency and head were defined as follows:

$$\eta = \frac{(P\_{\text{out}} - P\_{\text{in}})Q}{P\_{\text{m}}} \tag{15}$$

≤

$$H = \frac{P\_{\text{out}} - P\_{\text{in}}}{\rho \text{g}} \tag{16}$$

 = (௨௧ − ) <sup>୫</sup> = ௨௧ − where *Pout* and *Pin* present the total pressure at the outlet of outflow runner and inlet of inflow runner, respectively. *P*<sup>m</sup> stand for the motor input power, ρ and *g* are the fluid density and gravitational acceleration.

<sup>୫</sup>

65.0

0.0 2.0 4.0 6.0 8.0

0.8 1.0 1.2

t /mm

70.0

*η* /%

75.0

80.0

**Figure 5.** Comparison of simulated pump performance under different root clearance radii.

For the pump with a root clearance of 2.7 mm, the pump head was lower than that without root clearance under all flow rates, and the drop of performance parameters caused by root clearance increased with increasing flow rate. Under the part-load condition, the pump efficiency with 2.7 mm root clearance was slightly higher than that without root clearance, but the pump efficiency with 2.7 mm root clearance was significantly lower than that without root clearance under design condition and over-load condition. The experimental (EXP) results proved that the root clearance radius has a significant influence on hydraulic pump performance.

In order to verify the accuracy of numerical simulation, the experiment data with a root clearance of 0 mm was compared with calculated results in Figure 6. Under part-load flow rates, the simulated head and efficiency were lower than test data, but the simulated head and efficiency were higher than experiment data under design and over-load flow conditions. In addition, the maximum relative deviation between the measured results and the calculated data was less than 3% under the design flow rate. This shows that the numerical simulation results could accurately predict the pump's internal flow characteristics, and the numerical simulation results are reliable.

**Figure 6.** Comparison of pump performance between simulated data and test results (*R<sup>t</sup>* = 0 mm).

2.0

0.0 2.0 4.0 6.0 8.0

0.8 1.0 1.2

t /mm

3.0

4.0

/m

5.0

6.0

#### **4. Analysis of Calculation Results**

50.0

60.0

70.0

*η* /%

80.0

90.0

#### *4.1. Comparison of Pump Performance*

Figure 7 shows the hydraulic performance of the pump under different root clearance radii. As shown in Figure 7a, the hydraulic efficiency under 0.8 *Q*des did not fluctuate obviously with the increase of root clearance radius. However, the hydraulic efficiency under 1.0 *Q*des and 1.2 *Q*des decreased with increasing root clearance radius, and the maximum drop in efficiency was 2.5% and 6.8% at 1.0 *Q*des and 1.2 *Q*des, respectively. In Figure 7b, the pump head decreased with increasing root clearance radius under all flow conditions, while a head drop of 2.6%, 5.6%, and 15.5% occurred at 0.8 *Q*des, 1.0 *Q*des, and 1.2 *Q*des, respectively. In conclusion, under 0.8 *Q*des, the root clearance radius had no significant effect on the hydraulic performance of the axial flow pump device, but under 1.0 *Q*des and 1.2 *Q*des, the hydraulic performance decreased significantly as the root clearance radius increased. This was consistent with the test results above.

235.0 265.0 295.0 325.0 355.0 385.0

EXP-Efficiency CFD-Efficiency EXP-Head CFD-Head

/(L·s−1)

1.0

3.0

5.0

/m

7.0

**Figure 7.** Comparison of simulated (**a**) hydraulic efficiency and (**b**) head under different root clearance radii.

To illustrate why the hydraulic performance decreased with increasing root clearance radius, the entropy production theory was applied to the unsteady calculated results to analyze the additional energy losses caused by leakage flow in root clearance. Firstly, each hydraulic component's overall dissipation without root clearance under different flow rates was shown in Figure 8. Figure 8a shows the distribution of overall indirect dissipation *P*<sup>I</sup> . Due to the small rotational kinetic energy inside the inflow runner, the *P*<sup>I</sup> of this component was much lower than that of other hydraulic components. In addition, the *P*<sup>I</sup> of impeller and outflow runner was minimal near the design condition, and that of diffuser decreased with flow rate was increasing. Figure 8b shows the distribution of overall direct dissipation *P*D. As shown in the figure, the *P*<sup>D</sup> of the impeller was significantly higher than that of other hydraulic components, the effect of the flow rate had little influence on the *P*D. Compared with *P*I , the *P*<sup>D</sup> was so small that could be ignored, so the following section only analyzed the distribution of *P*<sup>I</sup> in axial flow pump.

Figure 9 shows the *P*<sup>I</sup> of four hydraulic components with four root clearance radii at 1.0 *Q*des. As shown in the figure, the *P*<sup>I</sup> of each hydraulic component from high to low is as follows: impeller, outflow runner, diffuser, and inflow runner. The effect of root clearance radius on *P*<sup>I</sup> in inflow runner was not obvious, and that of other hydraulic components increased with root clearance radius increasing, which explained why the hydraulic performance decreased with increasing root clearance radius. In addition, the maximum increases in *P*<sup>I</sup> in the impeller, diffuser, and outflow runner caused by the increase of root clearance radius were 3%, 5%, and 8%, respectively.

(**a**)

**Figure 8.** Distribution of (**a**) power loss due to indirect dissipation and (**b**) power loss due to direct dissipation of different hydraulic components without root clearance under five flow rates.

#### *4.2. Analysis of Inner Flow Dissipation*

Span=0.015

To understand the reason for the rise in overall dissipation with increasing root clearance radius, the internal velocity distribution and indirect dissipation rate within the impeller passage and diffuser

Span = ( − )/(<sup>௧</sup> − )

Impeller Diffuser

Span=0.015

<sup>௧</sup>

Velocity

0.0

100.0

200.0

300.0

I /W

400.0

500.0

passage were analyzed under different root clearance radii. Figure 10 shows the cylindrical cross-section for the impeller and diffuser at a specific blade height position Span, which is defined as follow:

Inflow runner Impeller Diffuser Outflow runner

Hydraulic components

0mm 2.7mm 5mm 8mm

$$\text{Span} = (r - r\_{\text{h}}) / (r\_{\text{t}} - r\_{\text{h}}) \tag{17}$$

where, *r* is the calculated ring radius, *r<sup>h</sup>* and *r<sup>t</sup>* are the the hub radius and radius of the impeller rim. <sup>௧</sup>

**Figure 10.** The cylindrical cross-section for impeller and diffuser.

Figure 11 shows the distribution of the relative velocity vector within the cross-section of the impeller passage with Span = 0.015 at 1.0 *Q*des. In the impeller passage without root clearance, the inlet angle matched the inlet edge of the blade better, and the fluid moved closer to the blade profile. There was only a small range of backflow at the trailing edge of the blade. The pressure difference between the pressure side and the blade's suction side causes the leakage flow to appear in the blade root clearance. In addition, the collision between the root leakage flow and the main flow leads to the deviation of the flow direction near the impeller inlet and outlet to the circumferential direction. The degree of deviation for the flow direction increased with the increasing root clearance radius.

**Figure 11.** Distribution of velocity vector at Span = 0.015 in impeller passage with varying root clearances *(R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

Figure 12 shows the relative velocity distribution in the cross-section of the impeller passage at Span = 0.015 under 1.0 *Q*des. In the impeller passage without root clearance, the low velocity caused by the wake vortex can be found near the trailing edge of the suction side, and the high velocity was

5 mm 8 mm

/(m·s-1) 2.7 mm

0 mm

obtained near the leading edge of the blade suction side. In the passage with root clearance, the low velocity near the trailing edge of the suction side was offset horizontally, causing leakage flow, thereby reducing the high-velocity area near the trailing edge of the suction side.

0 mm 2.7 mm

5 mm 8 mm

Figure 13 shows the distribution of indirect dissipation rate in the cross-section of impeller passage at Span = 0.015 under 1.0 *Q*des. In impeller passage without root clearance, the dissipation rate near the blade's trailing edge was higher due to the wake vortex, but there was no obvious high dissipation region. When the blade root clearance appeared in the impeller passage, a high dissipation region appeared near the trailing edge of the blade due to the impact of the leakage flow and the mainstream flow. The larger the clearance radius is, the greater the leakage velocity, resulting in a more obvious flow instability. Therefore, the area of the high dissipation region near the trailing edge of the blade increases with increasing root clearance radius.

**Figure 12.** Velocity contour at Span = 0.015 in impeller passage with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

**Figure 13.** Distribution of the indirect dissipation rate at Span = 0.015 in the impeller passage with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

The standard deviation of relative velocity represents the fluctuation and stability of velocity in the last period. It was defined as:

$$\overline{V} = \frac{1}{N} \sum\_{i=1}^{N} V\_i \tag{18}$$

/(W·m-3) 2.7 mm

0 mm

Indirect dissipation rate

where *V*<sup>i</sup> is the velocity at every time step; *V*. is the average velocity in a single rotation cycle; *V*sd is the standard deviation velocity in a single rotation cycle; *N* represents the sampling times of velocity data in a single rotation cycle.

Figure 14 shows the standard deviation of the velocity distribution within the impeller passage with four root clearance radii at Span = 0.015. In the impeller passage without root clearance, the internal flow field was relatively stable, and there was no high fluctuation intensity of velocity. In the impeller passage with 2.7 mm root clearance, the velocity fluctuation near the impeller outlet became stronger due to the influence of leakage flow in root clearance. When the root clearance continued to increase, the velocity fluctuation intensity in the blade passage decreased gradually, while the velocity fluctuation intensity at the impeller outlet increased. This result shows that the leakage flow in root clearance leads to the enhancement of rotor-stator interaction between the impeller and diffuser and worsens the diffuser's inflow condition. i 1 1 2 i 1 sd ( ) ത

Figure 15 shows the distribution of the velocity vectors in the guide vane passage with four root clearance radii. After passing through the impeller, the fluid generated a large amount of rotational kinetic energy, which caused some flow separation near the leading edge of the guide vane since the inlet angle of the guide vane was large. Furthermore, the inflow direction was obviously affected by the clearance radius of the blade root. The guide vane's inlet angle gradually deviated to the horizontal direction with increasing blade root clearance radius, which could affect the flow of the fluid between the guide vanes. The flow pattern inside the guide vane was expected to deteriorate with the increase of the root clearance radius, particularly at 5 and 8 mm, where an obvious backflow phenomenon at the inlet of the guide vane occurs.

**Figure 14.** Standard deviation of the velocity distribution at Span = 0.015 in the impeller passage with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

**Figure 15.** Velocity vectors at Span = 0.015 in guide vane passage with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

Figure 16 shows the distribution of indirect dissipation rate at Span = 0.015 in the diffuser passage at 1.0 *Q*des. When there is no root clearance in the diffuser passage, a high indirect dissipation rate occurred at the leading edge of the suction side as a result of flow separation. The backflow near the diffuser inlet could hinder the inlet flow of the guide vane into the blade passage, and the recirculation area near the diffuser inlet gradually increases with increasing root clearance. So, the indirect dissipation rate near the leading edge of the suction side and diffuser inlet decreased and increased with root clearance increasing, respectively.

5 mm 8 mm Indirect 0 mm 2.7 mm dissipation rate /(W·m-3) Figure 17 shows the distribution of indirect dissipation rate on the surface of the diffuser blades at 1.0 *Q*des. At the diffuser inlet, the blade surface's indirect dissipation rate gradually decreased from the leading edge of the blade towards the trailing edge, as shown in Figure 17a. Particularly near the hub, the indirect dissipation rate of the blade surface was very high. Since the leakage flow in the blade root clearance would worsen the inflow condition of the guide vane, thereby affecting the stability of the flow field in the guide vane channel, the area of the high dissipation zone near the hub is increased with increasing blade root clearance radius. For the diffuser outlet, the blade surface's overall indirect dissipation rate was low, and the indirect dissipation rate gradually decreased from the leading edge to the trailing edge, as shown in Figure 17b. In addition, the indirect dissipation rate near the guide vane hub was also low, and only a small area of high dissipation rate existed near the leading edge.

**Figure 16.** Indirect dissipation rate at Span = 0.015 in guide vane passage with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm 8 mm; *Q* = 1.0 *Q*des).

**Figure 17.** Distribution of indirect dissipation rate (**a**) from diffuser inlet and (**b**) from diffuser outlet on the surface of diffuser blades with varying root clearances (*R<sup>t</sup>* = 0 mm, 2.7 mm, 5 mm, 8 mm; *Q* = 1.0 *Q*des).

#### **5. Conclusions**

In this paper, the unsteady internal flow state of the axial flow pump under four root clearance radii (0 mm, 2.7 mm, 5 mm, 8 mm) was calculated to establish the influence of root clearance radius on hydraulic performance. The external characteristics test of an axial flow pump with root clearance radii 0 mm and 2.7 mm was completed to verify the numerical simulation method's reliability. In addition, the entropy production theory was adopted to determine the turbulence dissipation distribution within the flow domain in the axial flow pump. These conclusions were drawn to provide a reference for mixed flow pumps with similar specific speed:

In the axial flow pump, both the hydraulic efficiency and head decreased with root clearance radius increasing, and the decline magnitude rose with increasing flow rate. At 0.8 *Q*des, the effect of root clearance on hydraulic efficiency and the head was not obvious. With an increase in flow rate, the effect of root clearance became obvious. The maximum reductions in the head and hydraulic efficiency were 15.5% and 6.8%, with the root clearance of 8 mm at 1.2 *Q*des, respectively.

(1) The overall direct dissipation *P*<sup>D</sup> of each hydraulic component was negligible, compared with overall indirect dissipation *P*<sup>I</sup> . In addition, the *P*<sup>I</sup> of the inflow runner was much lower than that of the impeller, outflow runner, and diffuser. The *P*<sup>I</sup> of outflow runner decreased with decreasing flow rate, whereas that of impeller and diffuser reach a minimum value at 0.9 *Q*des and 1.1 *Q*des, respectively.


**Author Contributions:** Conceptualization, Y.L., and F.M.; data curation, Y.L., and Y.Z.; methodology, Y.L., and Y.Z.; project administration, Y.L., and F.M.; supervision, Y.L.; validation, F.M.; Writing—original draft, Y.L.; Writing—review & editing, Y.Z., and M.K.O. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research was supported by the Science and Technology Plan of Wuhan (Grant No.2018060403011350).

**Acknowledgments:** The authors sincerely thank the Science and Technology Plan of Wuhan.

**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* **E**ff**ect of Clearance and Cavity Geometries on Leakage Performance of a Stepped Labyrinth Seal**

**Min Seok Hur <sup>1</sup> , Soo In Lee <sup>2</sup> , Seong Won Moon <sup>1</sup> , Tong Seop Kim 1,\*, Jae Su Kwak <sup>2</sup> , Dong Hyun Kim <sup>3</sup> and Il Young Jung <sup>3</sup>**


Received: 11 October 2020; Accepted: 17 November 2020; Published: 19 November 2020 -

**Abstract:** This study evaluated the leakage characteristics of a stepped labyrinth seal. Experiments and computational fluid dynamics (CFD) analysis were conducted for a wide range of pressure ratios and clearance sizes, and the effect of the clearance on the leakage characteristics was analyzed by determining the performance of the seal using a dimensionless parameter. It was observed from the analysis that the performance parameter of the seal decreases as the clearance size increases, but it tends to increase when the clearance size exceeds a certain value. In other words, it was revealed that there exists a specific clearance size (Smin) which minimizes the performance parameter of the seal. To identify the cause of this tendency change, a flow analysis was conducted using CFD. It was confirmed that the leakage characteristics of the stepped seal are affected by the size of the cavity, which is the space between the teeth. Therefore, a parametric study was conducted on the design parameters related to the cavity size (tooth height and pitch). The results show that the performance parameter decreases as the tooth height and pitch decreases. Moreover, Smin increases as the tooth height increases and the pitch decreases.

**Keywords:** clearance; flow function; gas turbine; leakage; pressure ratio; stepped labyrinth seal

#### **1. Introduction**

The power and efficiency of gas turbines are being improved to meet the demands of users, leading to increased operating pressures and temperatures. However, the increased operating pressure and temperature increases the leakage flow at the blade tip, which disturbs the main flow and decreases turbine efficiency. Labyrinth seals are devices used to prevent such leakages and have benefits such as relatively simple structures and durability at high temperatures. Among the various geometric parameters of labyrinth seals, the parameter having the most dominant impact on the seal performance is the clearance size. The clearance size varies depending on the operating conditions (rotational speed and degree of thermal expansion of the blades) of the gas turbine. If the clearance is too large, the stage efficiency of the turbine decreases, and flow instability increases. In contrast, if it is too small, mechanical losses, such as wear, occur, thereby affecting the blade life [1]. Therefore, accurate predictions of the leakage characteristics of labyrinth seals according to the clearance are required.

Labyrinth seals are manufactured in various shapes by varying the arrangement of teeth to increase pressure loss and thereby reduce leakage. The commonly used geometries include straight seals with teeth arranged in a straight line on one side, stepped seals with teeth arranged in the form of steps, and staggered seals with teeth arranged in a staggered manner. Many studies involving experimental and numerical analyses have been conducted to understand the complex flow phenomenon inside labyrinth seals. The most basic research was conducted by Vermes [2]. He performed experiments using a labyrinth seal with the most basic configuration and developed an analytical model based on the experimental data. Stocker et al. [3,4] conducted an experimental study on various seal geometries. They also investigated the sealing characteristics of several seals, including honeycomb seals considering the design parameters. Witting et al. [5–7] conducted experimental studies on the leakage characteristics of the flow and on heat transfer, and they analyzed the influence of the scale of the experiment and the rotation effect on the results. Tipton et al. [8] summarized previous studies on leakage prediction and analyzed the effects of the main design parameters of seals on leakage. Research on the characteristics of labyrinth seals has been performed steadily with the development of experimental methods and performance prediction software programs based on existing data [9,10].

During the past couple of decades, studies comprehensively evaluating the flow characteristics inside labyrinth seals have increased owing to advancements in experimental techniques and numerical methods. Zimmermann et al. [11] analyzed the effects of various design parameters of straight/stepped seals on leakage and examined the changes in the leakage characteristics of the seals due to the wear of the tooth tip. Rhode et al. [12] researched labyrinth seals with added grooves and observed changes in the flow field inside the seals using the flow visualization technique. Schramm et al. [13,14] optimized the geometry of labyrinth seals and compared the leakage characteristics of honeycomb and solid land seals using computational fluid dynamics (CFD). Willenborg et al. [15] performed experiments in a wide range of Reynolds numbers and confirmed that the discharge coefficient depended only on the pressure ratio at high Reynolds numbers. Do ˘gu et al. [16] analyzed the leakage characteristics of mushroom-shaped labyrinth seals using CFD and confirmed that more leakage occurred due to shape changes, caused by rubbing. Yan et al. [17,18] conducted experiments and CFD analysis considering not only mushroom-shaped wear, but also deformation of teeth by bending. In addition, they conducted research on the hole-patterned labyrinth seal that arranged the holes regularly in the casing instead of honeycomb cells.

In recent years, experimental and numerical studies have focused on stepped labyrinth seals, which are themost common types of seals used to preventleakage at the turbine blade tip. Kim et al. [19–21] conducted an experimental study on the pressure ratio and clearance size for straight/stepped seals and analyzed the leakage characteristics using CFD. Kang et al. [22] conducted experimental and numerical studies on stepped labyrinth seals according to the number of teeth and clearance size. They also compared the leakage characteristics of solid and honeycomb seals and confirmed that solid seals exhibited better sealing performance. Zhang et al. [23] performed experiments using clearance sizes applied to actual engine blades to exclude the influence of the scale of the experiments on the results. They also numerically analyzed the influence of various design parameters of stepped labyrinth seals, such as the clearance size, step height, and the number of teeth.

According to several previous studies, the performance parameters of stepped labyrinth seals tend to decrease as the clearance size increases [19–24]. However, some studies have reported that this is not always true, and the performance parameters tend to increase again as the clearance size exceeds a certain value [25]. Nevertheless, these studies did not present comprehensive cause-and-effect analyses. Therefore, it is necessary to conduct basic research on the performance parameter according to the clearance size. In this regard, we conducted experiments and CFD analysis in this study to analyze the leakage characteristics of a stepped labyrinth seal, and the effect of the clearance size on leakage performance was analyzed thoroughly. The stepped seal geometry used at the tips of rotating blades in gas turbines was selected as the target and a diverging flow path in which the diameter increases in the flow direction was considered the leakage flow path as in real applications in the tip section of turbine blades. The minimum performance parameter was determined by observing the leakage characteristics according to the clearance

size. To explain the cause for tendency change in the performance parameter, the effects of several design parameters (tooth height and pitch) on leakage were analyzed.

#### **2. Labyrinth Seal and Experiment**

#### *2.1. Test Rig*

Labyrinth seals used in actual gas turbines are ring-shaped, and there is an empty space (i.e., clearance or gap) between the rotating and stationary parts. However, it has been widely accepted that the rotation effect on the leakage flow rate is important only when the rotational speed is very high [7] and thus a stationary two-dimensional (2D) rig provides almost the same results as those obtained using an axisymmetric three-dimensional (3D) rig [4]. Therefore, numerous studies including those surveyed in the introduction have used 2D test rigs and 2D CFD simulations to obtain fundamental flow physics and accumulate vast amounts of information. Accordingly, a 2D test rig was also used in our study.

Figure 1 shows the overall configuration of the test rig and Figure 2 illustrates the geometry of the labyrinth seal used in the test. To minimize the 3D flow effect due to the wall, the width of the test section, which is the depth of the test section into the page of Figure 2, was set to be sufficiently large (approximately 67 times the smallest clearance size) compared to the clearance size. The components of the test rig included the air tank, valve, mass flow meter, honeycomb panel, and the test section. The pressure of the air inside the tank was as high as 8.5 bar and the pressure ratio was adjusted from 1.1 to 3.0 using the control valve between the tank and the test section. The pressure ratio (PR) was defined as the ratio of total pressure at the inlet to static pressure at the outlet of the test section. The inlet pressure was measured using a pressure transducer (PX409-050GI, OMEGA, Norwalk, CT, USA). The flow rate at each PR was measured using a thermal electronic mass flow meter (KMSG-8040MT, KOMETER, Incheon, Republic of Korea), and the inlet temperature was measured using a thermocouple (T-type SCPSS-040E-6, OMEGA, Norwalk, CT, USA). In addition, a honeycomb panel was installed at the inlet of the test section for ensuring straight and uniform flow, and the test section was scaled up to the actual geometry to improve the accuracy of the test results.

**Figure 1.** Schematic diagram of the test facility.

θ

**Figure 2.** Seal geometry and parameters.

*θ* Table 1 summarizes the symbols and names of each design parameter and the non-dimensionalized expressions of the parameters of the labyrinth seal geometry. The test section was divided into an upper part and a lower part, which represent the stationary and rotating parts, respectively, in an actual turbine. The air comes into the test section from the left-hand side of Figure 2 and exits at the right-hand side, simulating a diverging flow path in actual turbine tip sections. The main geometric parameters of the stepped labyrinth seal include the clearance size (S), tooth thickness (b), tooth height (K), pitch (D), step height (H), and tooth angle (θ). In this study, numerical analysis and experiments were conducted by setting the range of the non-dimensionalized clearance size (step height ratio, S/H) from 0.2 to 1.2.


**Table 1.** Design parameters of the stepped labyrinth seal.

#### ሶ , , *2.2. Seal Performance*

The performance of the labyrinth seal was determined using the relationship between the PR and a performance parameter. The most commonly used performance parameter is the flow function, which is defined in Equation (1).

$$\phi = \frac{\dot{m}\sqrt{T\_{o,in}}}{A\_c P\_{o,in}} \tag{1}$$

where . *m* is the flow rate, *A<sup>C</sup>* is the throat area, *Po*,*in* is the inlet total pressure, *To*,*in* is the inlet total temperature. The flow function is the semi-dimensionless number which facilitates real leakage flow rate prediction for any arbitrary operating condition. The smaller the flow function is, the better the performance of the labyrinth seal becomes.

#### *2.3. Measurement Uncertainty*

The method proposed by Kline [26] was used to check the measurement uncertainty. The equation used for calculating the uncertainty of the flow function is given below.

$$
\Delta\phi = \sqrt{\left(\frac{\partial\phi}{\partial\dot{m}}\Delta\dot{m}\right)^2 + \left(\frac{\partial\phi}{\partial T\_0}\Delta T\_0\right)^2 + \left(\frac{\partial\phi}{\partial S}\Delta S\right)^2 + \left(\frac{\partial\phi}{\partial d}\Delta d\right)^2 + \left(\frac{\partial\phi}{\partial P\_0}\Delta P\_0\right)^2} \tag{2}$$

0 0

$$
\mu = \frac{\Delta\phi}{\phi} \tag{3}
$$

We used 0.3% of the measured flow rate as the uncertainty of the mass flow rate measurement (∆ . *m*) and 0.5 ◦C as that of the temperature (∆*T*0) according to the manufacturer's manual. The uncertainty of the tip clearance measurement (∆S) was set at 0.01 mm according to the least count of the gap gauge, and the uncertainty of the section width measurement (∆*d*) was set at 0.005 mm according to the least count of the Vernier calipers. The sum of 0.01% of the maximum measurable limit and 0.008% of the measured value was used as the value for the uncertainty of the pressure measurement (∆*P*0) according to the manufacturer's manual. Therefore, the uncertainty of the flow function (*u*) was calculated to be 3.4%. ∆ሶ ℃ ∆ ∆ ∆

#### **3. Analysis**

#### *3.1. Numerical Approach*

∆

ANSYS CFX (ver. 19.0, ANSYS Inc., Canonsburg, PA, USA, 2018) [27], a commercial software program, was used for CFD analysis. Figure 3 shows examples of the analysis domain and grid structure. As the 2D flow was secured in the experiment, the 2D calculations were also sufficient for CFD. However, as ANSYS CFX is based on 3D calculations, the 3D domain was set as shown in Figure 1; nevertheless, we ensured that the 3D was practically close to the 2D domain by setting the smallest width as far as we could and applied symmetry conditions to lateral faces. This method is recommended for 2D calculations according to the CFX manual [28]. ANSYS ICEM (ver. 19.0, ANSYS Inc., Canonsburg, PA, USA, 2018) was used for mesh generation. The grids of the overall leakage flow path were composed of unstructured meshes and only the wall portion was composed of prism layers so that y+ could be ≤2. Figure 3 shows an example of generated meshes. It is clearly shown that dense meshes were generated around the tip clearance. Grid dependence tests were performed to select appropriate numbers of meshes. Figure 4 illustrates an example for the case when the clearance to step height ratio (S/H) is 0.4. The results confirmed that the flow function, which was the target function, became almost constant when the number of meshes was 120,000 or more. Accordingly, 130,000 meshes were adopted in a specific case. Of course, the number of meshes generally increased as the clearance increased. It ranged from 130,000 to 150,000 when the S/H ratio increased from 0.2 to 1.2. ≤

**Figure 3.** Example of the computational domain and meshes (S/H = 0.4).

**Figure 4.** Example of grid dependence of the computational fluid dynamics (CFD) result (S/H = 0.4).

#### *3.2. Boundary Conditions and Validation*

− ω ε ε Inlet total pressure and temperature and outlet static pressure were used as boundary conditions to simulate the operating conditions of the test. Adiabatic and no-slip conditions were used for the solid surfaces, and the symmetry condition was used at the two side boundary surfaces (lateral faces). The high-resolution advection scheme was used, which adequately uses the first and second order scheme depending on the situation, satisfying both the numerical stability and accuracy of the analysis. In addition, the first-order turbulence numerics was selected. The residual value (RMS) of the flow parameter was set to less than 1.0 <sup>×</sup> <sup>10</sup>−<sup>4</sup> as the convergence condition for the analyses. Table <sup>2</sup> summarizes the numerical analysis method and boundary conditions. A turbulence model that accurately captures the flow characteristics inside the seal cavity is required because of a strong vortex flow which is one of the major causes of the pressure loss in the seal. Therefore, the SST turbulence model, which is known to predict the vortex size and separation point accurately [29,30], was adopted. Figure 5 compares the sample test run results obtained using the SST model with those obtained using other turbulence models (k–ω, k–ε and RNG k–ε models). Although there were no significant differences in the calculation results obtained using the various turbulence models, the SST model produced results closest to the experimental values with errors less than 3%. In addition, a comparison between the experimental and CFD results shown in Figure 6 confirms that CFD has sufficient accuracy for evaluating the leakage performance of the labyrinth seal.

**Figure 5.** Comparison of turbulence models (S/H = 1.0, K/H = 4, D/H = 4).

**1.0 1.5 2.0 2.5 3.0**

**PR**

**EXP - S/H = 0.333 CFD - S/H = 0.333 EXP - S/H = 0.666 CFD - S/H = 0.666 EXP - S/H = 1 CFD - S/H = 1**

**8**

**12**

**16**

 **(kg K 0.5kN s)**

**20**

**24**

**1.0 1.5 2.0 2.5 3.0**

**PR**

**EXP SST k k - RNG k -** 

 **(kg K 0.5kN s)**

**Figure 6.** Comparison between the CFD and experimental results (K/H = 4, D/H = 4).


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

#### *4.1. Leakage Characteristics According to Clearance Size*

Figure 7 shows the flow function obtained using CFD at different PR and S/H values. For all S/H values, the flow function increases as the PR increases and exhibited choking after a certain PR. For example, the choking pressure ratio is around 2.5 when S/H is 0.2. As well known, the fact that the flow becomes choked does not necessarily mean that the actual flow rate is constant. It varies with the inlet total pressure and temperature. In our cases, the actual mass flow rate increases in proportion to the inlet total pressure because a higher pressure ratio means a higher inlet total pressure: remember that the inlet total temperature and the outlet static pressure were fixed.

**Figure 7.** Variations in flow function with pressure ratio (PR) and S/H (K/H = 4, D/H = 4).

**EXP CFD**

**0.2 0.4 0.6 0.8 1.0 1.2**

**S / H**

**15**

**18**

**20**

**22**

 **(kg K 0.5kN s)**

**25**

**27**

**30**

An important observation was that change in flow parameter due to the increase in the clearance size clearly differs below and above S/H = 0.6. To intensively examine changes in the flow function according to the clearance, the flow function at the PR of 2.5 was plotted in Figure 8 and compared with the experimental values under the same conditions. As the clearance increases, the flow function decreases and then tends to increase again at a certain clearance size, as observed commonly in the CFD and experimental results. This result confirmed that the stepped labyrinth seal has a specific clearance size (Smin) that minimizes the flow function. It should be noted that the flow function does not represent the actual leakage flow rate but indicate relative leakage performance. Therefore, a lower flow function does not necessarily mean a lower flow rate but represents a better relative seal performance. The actual leakage flow rate increases as the clearance size increases in all the test cases in our study. **8 10 12 14 16 18 20 22 1.0 1.5 2.0 2.5 3.0 S / H = 0.2 S / H = 0.4 S / H = 0.6 S / H = 0.8 S / H = 1.0 S / H = 1.2 (kg K 0.5kN s) PR**

**24**

**Figure 8.** Variation in flow function with S/H (PR = 2.5, K/H = 4, D/H = 4).

To identify the cause of such changes in the flow function due to the increase in the clearance size, the flow inside the seal was analyzed using the details of the flow phenomena obtained by CFD. Figures 9 and 10 show the contours of the total pressure and static pressure, respectively, for various S/H ratios at the PR of 2.5. As S/H increases, the flow through the clearance develops a type of high-speed flow layer (see Figure 9). Figure 10 shows that the flow layer passing the clearance collides with the next tooth, resulting in a local increase in static pressure, which means that the kinetic energy of the leakage flow significantly dissipates. The collision point moves toward the tooth tip gradually as the S/H increases, and after S/H = 1.0, it is located at the tip of the tooth. In other words, in the specific S/H range in which the flow function decreased (S/H from 0.2 to 0.533), the flow rate gradually increases and the pressure loss due to collision with the tooth increases, improving the sealing performance. However, when the clearance continues to increase over the critical value of 0.533, most of the leakage flow through the previous clearance directs to the next clearance space without hitting the tooth, as shown in Figure 9. Accordingly, the kinetic energy loss caused by the collision reduced, resulting in a decrease in the sealing performance. In addition, it is seen from Figure 9 that the total pressure inside the cavity slightly increases as S/H increases from 0.2 to 0.533. This indicates that the leakage performance improves (i.e., the flow function decreases) as the flow trapped inside the cavity is increased by the flow layer moving at a high speed. However, after S/H = 0.533, the total pressure inside the cavity tends to decrease which means the flow trapped inside the cavity decreases. Figure 11 clarifies the change of the pressure inside the cavity with respect to S/H. It shows the variation in the averaged total pressure inside the cavity according to S/H, which clearly shows that total pressure decreases after the maximum point.

**Figure 9.** Total pressure contour plots for various S/H ratios (PR = 2.5, K/H = 4, D/H = 4).

**Figure 10.** Static pressure contour plots for various S/H ratios (PR = 2.5, K/H = 4, D/H = 4).

**Figure 11.** Variation in the averaged total pressure inside the cavity with S/H (PR = 2.5, K/H = 4, D/H = 4).

In summary, the tendency of the variations in flow function with clearance change at S/H = 0.533. In other words, when the clearance size is approximately half the step height, the maximum resistance to leakage flow occurs, leading to decreases in the flow function. As the clearance size further increases, the resistance to leakage flow decreases, leading to increases in the flow function.

#### *4.2. Parametric Study on the Impact of Cavity Size*

#### 4.2.1. Outline

Through the flow analysis, we identified two main reasons for the reduced flow function (i.e., enhanced leakage performance) of the stepped labyrinth seal. The first is the significant dissipation of the kinetic energy during the leakage flow that occurs as the fluid passing through the clearance collides with the next tooth. The second is the formation of a strong flow layer owing to the high-speed flow passing through the clearance and the subsequent confinement of the rotating flow inside the cavity. The identification indicates that the leakage characteristics of the stepped labyrinth seal are affected not only by the clearance size but also by the value of S/H relative to the cavity size. Based on this observation, a parametric study on the tooth height and pitch, which are geometrical parameters affecting the cavity size, was conducted using the CFD. Table 3 gives the analysis range set for each parameter.

**Table 3.** Variation range of the non-dimensional parameters.


#### 4.2.2. Tooth Height

Figure 12 shows the change in the flow function according to the values of S/H and K/H at the PR of 2.5. As the value of K/H decreases, the flow function decreases. The minimum value of the flow function is 8.4% lower at K/H = 2 and 5.9% higher at K/H = 6 compared to the reference value at K/H = 4. Figure 13 shows the velocity vector according to the K/H value at constant S/H and PR values. As the value of K/H decreases, the cavity size decreases, thereby increasing the velocity of the rotating flow in the cavity. Accordingly, a high-velocity flow layer is formed at the point where the flow in the axial direction (i.e., the throughflow) and the rotating flow inside the cavity joined. Following this, the joined flow collides with the tooth, increasing the local pressure, as shown in Figure 14. This indicates significant dissipation of the kinetic energy is induced by the leakage flow. In addition, as the velocity of the flow layer is higher, a larger separation occurs at the tooth tip, as shown in the velocity contour of Figure 15. This reduces the flow function because the effective area in which the flow can actually move is reduced. In addition, as the tooth height decreases, Smin slowly decreases owing to the reduced flow rate inside the cavity.

**Figure 12.** Variation in the flow function with S/H and K/H (PR = 2.5, D/H = 4).

**Figure 13.** Velocity vectors for various K/H ratios (PR = 2.5, S/H = 0.6, D/H = 4).

**Figure 14.** Static pressure contour plots for the smallest and largest K/H ratios (PR = 2.5, S/H = 0.6, D/H = 4).

**Figure 15.** Velocity contour plots for the smallest and largest K/H ratios (PR = 2.5, S/H = 0.6, D/H = 4).

The impact of S/H is summarized as follows. At S/H = 0.2 which is the smallest value in our study, the change in tooth height did not affect the flow function (see Figure 12) because the clearance is too small for the flow separation to be an important factor. As S/H increases, the influence of K/H increases, which means the favorable impact of a lower K/H increases. However, as S/H increases above the minimum flow function point, the influence of K/H increases again.

#### 4.2.3. Pitch

Figure 16 shows the flow function according to the S/H and D/H values at the PR of 2.5. As the value of D/H decreases, the flow function decreases. The minimum value of the flow function is 5.4 % lower at D/H = 3 and 0.7% higher at D/H = 5 compared to the reference value at D/H = 4. Figure 17 shows the streamlines when D/H is the highest and lowest at constant S/H and PR values. As D/H decreases, the velocity of the flow layer increases because the travel distance of the flow in the axial direction decreases. In addition, larger separation occurs because of the rapid movement of the flow in the radial direction. This reduces the effective area, thereby further increasing the leakage reduction effect (see Figure 18). In addition, as the pitch decreases, Smin tends to increase. This is because flow into the cavity continuously occurs despite the increase in cavity size owing to the reduction in the travel distance in the axial direction.

**Figure 16.** Variation in the flow function with S/H and D/H (PR = 2.5, K/H = 4).

**0.2 0.4 0.6 0.8 1.0 1.2**

**S / H**

**0.2 0.4 0.6 0.8 1.0 1.2**

**S / H**

**D / H = 3 D / H = 4 (ref.) D / H = 5**

**D / H = 3 D / H = 4 (ref.) D / H = 5**

**16**

**16**

**18**

**18**

**20**

**20**

 **(kg K 0.5kN s)**

 **(kg K 0.5kN s)**

**22**

**22**

**24**

**24**

**Figure 17.** Velocity streamline plots for the smallest and largest D/H ratios (PR = 2.5, S/H = 0.6, K/H = 4).

**Figure 18.** Velocity contour plots for the smallest and largest D/H ratios (PR = 2.5, S/H = 0.6, K/H = 4).

As with the case of the tooth height, when S/H = 0.2, the change in pitch does not affect the flow function because the clearance is too small for the flow separation to be an important factor. Despite the increase in the clearance size, changes in the flow function due to the pitch were hardly observed before Smin. Although the relative flow velocity decreases owing to the increase in the travel distance in the axial direction, there is almost no difference in the overall leakage performance because the flow rate into the cavity increases. However, as the clearance continues to increase, the flow rate inside the cavity sharply decreases, causing differences in the flow function owing to the difference in the velocity of the flow layer.

#### 4.2.4. Summary of the Parametric Study

The results obtained from analyzing the effects of the tooth height and pitch on leakage performance can be summarized as follows. Overall, changes in the tooth height cause more significant changes in leakage characteristics than changes in the pitch. The influence of the clearance change is also stronger according to the tooth height variation. In addition, when the clearance is considerably small, changes in the two design parameters have little influence on the flow function. However, as the clearance gradually increases, the flow function shows different tendencies owing to changes in the two design parameters before and after Smin. As the values of both the parameters decrease, the leakage performance improves (i.e., the flow function decreases), but Smin decreases as K/H decreases and D/H increases. As the tooth height decreases, Smin decreases owing to the reduction in the flow rate into the cavity. In contrast, as the pitch decreases, the flow rate into the cavity decreases, but Smin increases because the flow into the cavity continuously occurs despite the increase in the clearance size due to the relatively reduced travel distance in the axial direction.

### **5. Conclusions**

In this study, the leakage characteristics of a stepped labyrinth seal, which is mainly used for sealing at the blade tips of gas turbines, were analyzed through experiments and CFD simulations for a wide range of PRs and clearance sizes. We focused on determining the clearance size at which the tendency of the flow function changed owing to changes in the design parameters. The main results and conclusions of this study are summarized as follows:


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

**Funding:** This study was conducted with the support of the Korea Evaluation Institute of Industrial Technology (KEIT) at the Ministry of Industry, Commerce and Energy in 2020 (No. 20002700). The authors gratefully acknowledge this support.

**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*
