ZHU Bing, CHEN Hong-xun

Shanghai Institute of Applied Mathematics and Mechanics and Shanghai Key Laboratory of Mechanics in Energy Engineering, Shanghai University, Shanghai 200072, China, E-mail: klarke_zhu@163.com

(Received March 1, 2012, Revised May 11, 2012)

CAVITATING SUPPRESSION OF LOW SPECIFIC SPEED CENTRIFUGAL PUMP WITH GAP DRAINAGE BLADES*

ZHU Bing, CHEN Hong-xun

Shanghai Institute of Applied Mathematics and Mechanics and Shanghai Key Laboratory of Mechanics in Energy Engineering, Shanghai University, Shanghai 200072, China, E-mail: klarke_zhu@163.com

(Received March 1, 2012, Revised May 11, 2012)

This paper aims to clarify the cavitation suppression mechanism of the gap structure impeller based on the analysis of cavitation characteristics in a low specific speed centrifugal pump. In order to obtain reliable and consistent numerical results, some numerical considerations and modeling methodology were demonstrated and researched, and a check of the time and space resolution were also conducted. Hence the predicted cavitation performance of the two centrifugal pumps were investigated and compared with experimental results, and they were in qualitative agreement. It was confirmed that the new gap structure impeller has a very good characteristic of inhibiting cavitation, especially in large flow area, the present numerical method can effectively capture the major internal flow features in the centrifugal pump, through the comparison of the two type impeller flow fields, the cavitation suppression mechanism of the gap impeller may be the combination effects of the small vice blade?s guiding flow and gap tunnel?s auto-balancing of pressure.

Low Specific Speed Centrifugal Pump (LSSCP), gap drainage blade, cavitation suppression, numerical simulation

Introduction

The Low Specific Speed Centrifugal Pump (LSSCP) is widely used in various areas. At present, there often exist some tough issues for those LSSCPs produced with to the conventional design methods, such as relative low efficiency, instability of operation in lower flow region and overload for motor power in the larger flow region, etc.. Thus, it is of great significance to enhance the performance and operation stability of LSSCPs for energy saving and equipment safety.

In order to improve the characteristics of LSSCP, Zhang[1]summarized several modified design methods, mainly including the increase of volume flow design method, the non-overloading design method, the area-ratio design method and the splitter blade design method, etc.. These methods have been widely used in the design of LSSCP, and confirmed improving the performance of the pump to some extent.

Based on the idea of flow control, Chen et al.[2]put forward the primary impeller structure of gap drainage blades (gap) in the design of LSSCP. It was validated in experiments that this structure can increase the pump efficiency and broaden the stable operation range.

The hydraulic and cavitation performances are two important indexes measuring the characteristics of water pumps. This work aims to investigate the cavitation behavior of the LSSCP with the new gap structure impeller. Although some other measures were proposed to improve the cavitation performance of hydrodynamic machinery, such as adding structure of groove[3], accumulator[4]and active mass injection[5], etc., they are not always working well for the un-clarified mechanism of cavitation suppression.

Cavitation is a kind of complex flow phenomenon associated with unsteady flows, turbulence and phase change, etc.. The study in the aspects of theory, experiment or simulation is challenging. In recent years, with the development of theoretical modelingnumerical method and computer resources, many effective cavitation models were proposed and used in industry, such as Singhal?s full cavitation model[6], Zwart-Gerber-Belamri model[7]and Schnerr and Sauer model[8], etc.. From these we can see that the Computational Fluid Dynamics (CFD) has already become an important research method for the study of cavitation characteristics in hydraulic machinery. Bakir[9]developed a multiphase cavitation model based on a truncated Rayleigh-Plesset equation for bubble dynamics, which was validated on an inducer for a range of flow rates about the overall performance, head drop and the size and location of the cavitation bubble cloud. The results showed a good agreement between experiments and prediction. Liu et al.[10]studied the cavitation performance of a Francis turbine based on the twophase flow mixture model and the RNG k-ε turbulence model. The cavitation characteristics and the overload vortex rope at the draft tube inlet were reproduced reasonably when compared with the model test data. Medvitz[11]adopted a multi-phase CFD method to analyze centrifugal pump performance under developed cavitating conditions. The results indicated indeed capturing principal physical elements of cavitation breakdown in comparison of experimental and computed head coefficients versus cavitation number at design flow coefficient. Pouffary et al.[12]proposed a cavitation model based on the barotropic state law. The model was numerically validated for two inducers and a SHF impeller centrifugal pump with available experimental results, which showed that numerical simulations enable the characterization of the mechanisms leading to the head drop, and the visualization of the effects of the cavitation development in internal flows. Hejranfar[13]presented and assessed a numerical treatment for the prediction of cavitating flows. With the usages of the preconditioned multiphase Euler equations with appropriate mass transfer terms, and of a central difference finite volume scheme with suitable dissipation terms to account for density jumps across the cavity interface, it was shown to yield an effective method for solving the multiphase Euler equations. Frikh[14]researched the influence of different cavitation models on the simulation of cloud cavitation on 2-D foil section. The results showed some resemblance between most of the models, but the model constants change the cavity shape and structure. Dupont and Okamara[15]presented some experiences in predicting the pump cavitating performance based on the evaluation of model capabilities of different general commercial CFD software. All these practical examples tell us that CFD can be used to analyze the pump cavitating behavior through coupling the suitable turbulence and cavitation models.

In the present paper, two impellers of LSSCP will be first designed with conventional technique a[n2d

] new flow control technique proposed by Chen et al. . And then the cavitation performance will be predicted on the basis of reliable numerical studies. The comparison of concerned cavitation characteristics will be conducted for the two impellers between calculation and experiment. This work will help to verify the effectiveness of the new design method of LSSCP further and reveal the cavitation suppression mechanism of Gap structure.

1. Physical model and test rig

One type of impeller of LSSCP was designed by the conventional increasing flow design method. The designed parameters of pump head and flow rate are respectively 20 m and 14 m3/h. There are four cylindrical 2-D blades in the impeller with a blade inlet diameter (D1) of 0.0534 m, an outlet diameter (D2) of 0.255 m, an outlet width (b) of 0.00729 m and a rotating speed of 1 450 RPM. To ensure that all the main parameters were in the same conditions, a new structure of impeller was designed as suggested by Chen et al.[2]. The major difference is that a small vice blade was designed and put aside of the suction surface of the main blade at the leading edge. Thus a gap is formed between the overlap area of the main and vice blades. The major parameters and structures of the impellers were shown in Fig.1.

Fig.1 Scheme of gap impeller and conventional impeller

Fig.2 Centrifugal pump test rig

The two different impellers were made by ABS mate rial and processed by a 3-axis linkage numerical control machine, which were installed in the same centrifugal pump for easy comparison. The cavitation performance of the two impellers was tested on an open centrifugal pump rig, as shown schematically in Fig.2. The pump w as driv en by an asynchronous motor,governedbymeansofavariable-frequency d rive, allowing the adjustment of the motor?s rotational speed. The flow rate was measured with an electromagnetic flowmeter. The static pressure rise of the pump was obtained using two pressure sensors located at the suction and discharge manometer tubes. The rotational speed and the torque were measured with a tachometer and torquemeter, which was equipped on the shaft between the motor and pump. The sluice valves located close to the water tank should be adjusted carefully and patiently for the variation of flow rate in the cavitation testing. All the data can be captured and recorded in a computer automatically.

2. Numerical treatment and modeling

2.1 Computational model and grid generation

The computational model was generated accordingto the test pump, containing suction and discharge pipelines, impeller, volute, cavity between impeller and volute, mouth ring clearance, and the guide plate at the intake, as can be seen in Fig.3.

F ig.3 Simulation domain: Cross section, rotor blades and volute

To effectively control the grid distribution in centrifu gal pump, such as the mouth ring clearance, gap tunnel of the new impeller and wall boundary layer, the whole hexahedral meshing strategy was adopt in this paper. The simulation model was separated into three domains by the interfaces at the inlet and outlet locations of the impeller. The grid was generated for each part with the software of ANSYS ICEM CFD 12.1, and the grid distribution and number were guaranteed consistence at the interface transition. The O-type grid technology and local refinement method were adopted to control the near-wall mesh, which ensured the requirements of corresponding turbulence model at the near wall treatment. In order to obtain mesh-independent simulation results, the similar grid topology and distribution were kept for the two impellers, which would be discussed in Section 2.4.

Fig.4Grid distribution

The final impel ler grid nodes number is 1.52×106for conventional impeller and 1.69×106for gap impeller,sharing 1.19×106grid nodes number for other parts of the pump. The whole and local mesh distributions were illustrated in Fig.4. The structure and grid distribution of gap impeller were specially shown in Figs.4(d) and 4(e).

2.2 Computational methodology

In the p rese nt resear ch,all simulat ions w ere conductedwiththegeneralpurpose CFDcodeANSYSCFX 12.1. The three-dimensional viscous flow was modeled by the the Reynolds Averaged Navier-Stokes (RANS) equations discretized on the element-based finite-volume. The two-equations kε- based Shear-Stress-Transport (SST) turbulencel with automode matic near-wall treatment was used in the simulations, which can automatically switch from wall-functions to a low-Re near-wall formulation as the mesh is refined. Thhomogeneous multiphase flow model was

Tabble 1 Grid discretization error estimation of impeller

e applied in the cavitating simulation where all fluids shared the same fields. Bakir?s Rayleigh-Plesset cavitation model[9]was selected to calculate the interphase mass transfer rate when the saturation pressure and mean nucleation site diameter were given.

In order to decrease the numerical dissipation eithe r in steady or unsteady simulation, the secondorder high-resolution scheme and the second-order backward Euler scheme were used separately for the advection term and the transient term. A co-located (non-staggered) grid layout was used for the pressurevelocity coupling, thus the linear momentum and mass equation set could be solved together, which increased the robustness and efficiency of coupled solver.

The rotating and stationary domains were connected by the General Grid Interface (GGI) where the grid on either side of the two connected surfaces permits non-matching. The frozen rotor interface model was set for the steady simulation which treats the flow from one component to the next by changing the frame of reference while maintaining the relative position of the components. The transient rotor-stator interface model was set for the unsteady simulation which takes into account of all the transient flow characteristics and allows a smooth rotation between components.

The boundary conditions of a total pressure specified inlet an d a mass flow outlet were set, which are often more appropriate for the case that assume the pump is drawing fluid directly from a static tank. The non-slip wall was implemented for the wall boundary condition considering the effect of wall roughness (0.00007 m for ingot steel and 0.00003 m for ABS material). A steady simulation was modeled first for the initial condition of transient case, and a non-cavitation result was used as an initial guess of cavitation case. mean sq-5

The residual convergence criterion for the root

uare variables was set to 1×10 and the massmomentum imbalance target was smaller than 1%. For the transient case, the total time duration, time step size and computing resource consumption will be discussed specially.

2.3 Dimensionless coefficients

The calculat ed and measured characteristics of the analyzed centrifugal pump a re presented by means of th e dimensionless coefficients, which are defined as follows:

Flow coefficient

Cavitatn number

io

Net positive suction pressure whereV is average volume flow, Δptotstands for th e total pressure rise from the pump suction to discharge manometer tube, pt-inletis theinlet total pressure close to the tank, and pvis equal to 3 574 Pa which is the vapor pressureof water at 25oC.

2.4 Grid and time resolution

In order to establish grid-convergent r esults, a criterion based on the Richardson extrapolationtechnique[16]was used to improvegrid resolutionand systematically evaluate truncation error and accuracy. A representative grid size base on the element volume and the grid refinement factor were defined as follows

suggested greater than 1.3 based on experience.

Base on the conventional impeller, four sets of grids were created. The grid numbers (N1-N3) were selected to do an error evaluation, and N0was for a validation. Because the pump performance was the concern of this research, the water head coefficient (ψ) and efficiency (η) were determined as the key variables (φ). The values were based on the steady simulation at a flow rate close to the best efficiency point, as illustrated in Table 1. According to the variation of key variables, the grid monotonic convergence results were obtained. Based on the finer grid number N1, the head and efficiency relative errors were both below 0.2%, and the grid convergence index was estimated to be 4.03% for the water head and to be below 1% for the efficiency. Thus grid number N1was used as the final computation, which was referenced as the basis of other part grid generation of the centrifugal pump.

It is difficult to get convergent water head and efficiency in steady simulation when the pump is operated at part-load conditions. Besides, the steady results are strongly dependent on the relative locations of the impeller and volute for such a typical thickness blade impeller, as can be seen in Figs.1 and 5. Thus the unsteady simulation is necessary and the obtained data are regarded as the ultimate results.

Fig.5 Location dependency of steady simulation

Table 2 Time step size and time duration (φ=0.58, 1450 RPM)

In t ransient simulation, the time duration and time step size were studied, as shown in Table 2. In order to make a balance between the temporal accuracyand computing resource consumption, the time step size was set to 2×10-4(i.e., about rotating 1.7oeach step), and the total time was of 10 circles of the impeller rotating. This type of setting can keep convergence in each time step and the monitor variables appear periodically during the total time. The last circle results were averaged for post-processing. All simulations were carried out on the servers at Shanghai Institute of Applied mathematics and Mechanics (11CPUs*11nodes, 2.66 GHz). The computing time was of approximately 72 h with 11 CPUS for each transient simulation.

Fig.6 Cavitation performance

3. Results and discussion

3.1 Cavitation performance

The experimental cavi tation performances of the conventional and gap impeller centrifugal pump were displayed at two flow rates (one is at Best Efficiency Point (BEP), and another is atBEP1.35/QQ point) as shown in Fig.6. It is surprised that the gap impeller can greatly suppress the generating of cavitation, which is more obvious at larger flow rate. To ensure the same operating condition of the experiment at BEP, the Unsteady Reynolds Averaged Navier-Stokes (URANS) simulation results of cavitation match the experimental ones qualitatively. It means that the main cavitating flow characteristics in the centrifugal pump were captured.

Fi g.7 Iso-surfaces of water vapor volume fraction (α=0.1, σ=0.178)

3.2 Cavitation visualization

The calculated water vapor volume fractions (plotted with iso-surfaces, α=0.1) of the conventional and gap impeller at the same cavitation number (σ=0.178, see Fig.6) are given in Fig.7. It is obvious that the cavitation is fully developed and there is some blocking in the region close to the inlet and shroud of Conventional impeller, while there is only a primary cavitation on the main blade leading suction surface located in the controlled gap tunnel for the gap impeller.

Fig.8 Normalized relative velocity distribution (σ=0.178)

3.3 Discussion

In this section, we will research and an alyze the predicted internal flow features of the conventional and gap impelle r, and look for the cause of good anticavit aion performance in the gap impeller.

Figure 8 shows the comparison of normalized relative velocity distribution at the middle span of the two impellers. For the left conventional impeller, the flow first tends to be on the suction side at the blade entrance and then turns to the pressure side at the impeller exit. Also, there is a big vortex at the exit which blocks some part of the suction side tunnel. And instead for the right gap impeller, the flow is uniform and stable, which can also be observed from the streamline distribution shown in Fig.9. In addition, some fluid is draught from the pressure side to the suction side at the gap of the tandem blades.

Fig.9 Streamlines of gap impeller (σ=0.178)

Fig.10 Normalized static pressure distribution (σ=0.178)

The comparison of the normalized static pressure (defined as the head coefficient ψ) distribution for the two impellers is displayed in Fig.10. A large part of low pressure area exists in the fore part of the conventional impeller fluid tunnel, which promotes the cavitation generating and developing to a certain degree. However, most of the internal pressure is higher than the water vapor pressure in the whole gap impeller, which suppresses the cavitation generating.

Fig .11 Normalized turbulence intensity distribution (σ= 0.178)

The contrast of normalized turbulence intensity distribution is also exhibited in Fig.11. Because of the occurrence of cavitation in the conventional impeller, the t urbulence intensity is significantly higher than that in the gap impeller, which of course will cause major energy loss.

Therefore, based on the above analysis, we can see that the mechanism of gap impeller improving cavitation performa nce is due to the existence of the speci al designed aperture structure blades. The advantage is that the leading vice blade can guide the entrance flow speed more even and pull some through the gap from the pressure side to the suction side, another aspect is that the distributed pressure imbalance in the import region can quickly be compensated through the gap channel, while only one main blade isolates such a mechanism.

4. Conclusions

In this paper, based on the numerical reliability analysis, a numerical and experimental investigation of a LSSCP with conventional and gap impeller is presente d to examine the difference of the cavitation performance. It was confirmed that:

(1) The structure of gap impeller can effectively inhibit cavitation generating, which is more apparent in large flow area.

(2) The numerical prediction of cavitation performances agree well with experimental results qualitatively, and the cal culated critical point of cavitation char acteristics curve matches with the testing, which suggests that the main flow features are captured by the simulation.

(3) According to the analysis of the calculated internal flow behaviors, the anti-cavitation mechanism of the gap impelle r is discussed, which may be the guidi ng flow feature of the small vice blade and the pressure auto-balance effect of the gap tunnel.

This work provides a new concept of designing high anti-cavitation centrifugal pump, and also sets a successful example of the flow control theory guiding engi neering practices. In future, the cavitation visualization experiment will be conducted and the ways of reducing model errors will be researched.

Acknowledgement

This work was supported by the Graduate Student Innovation Foundation of Shanghai University (Grant No.SHUCX111010).

[1] ZHANG Jin-feng. Numerical forcast and research on the design method for centrifugal pumps with splitter blades[D]. Ph. D. Thesis, Zhenjiang: Jiangsu University, 2008(in Chinese).

[2] CHEN Hong-xun, LIU Wei-wei and JIAN Wen et al. Development of low specific-speed centrifugal pump impellers based on flow control technique[J].Chinese Journal of Drainage and Irrigation Machinery Engineering, 2011, 6(9): 466-470(in Chinese).

[3]SHIMIYA N., FUJII A. and HORIGUCHI H. et al. Suppression of cavitation instabilities in an inducer by J-Groove[J]. Journal of Fluids Engineering, 2008, 130(2): 021302.

[4] AKIRA F., SHINICHI M. and HIRONORI H. A Method for the suppression of rotating cavitation by an accumulator at the inlet of an inducer[J]. Journal of Fluid Science and Technology, 2008, 3(7): 838-845.

[5] CHANG N., GANESH H. and YAKUSHIJI R. et al. Tip vortex cavitation suppression by active mass injection[J]. Journal of Fluids Engineering, 2011, 133(11): 111301.

[6] SINGHAL A. K., ATHAVALE M. M. and LI H. Y. et al. Mathematical basis and validation of the full cavitation model[J]. Journal of Fluids Engineering, 2002, 124(9): 617-624.

[7] ZWART P. J., GERBER A. G. and BELAMRI T. A two-phase flow model for predicting cavitation dynamics[C]. The Fifth International Conference on Mul- tiphase Flow. Yokohama, Japan, 2004.

[8] SCHNERR G. H., SAUER J. Physical and numerical modeling of unsteady cavitation dynamics[C]. The Fourth International Conference on Multiphase Flow. New Orleans, USA, 2001.

[9] BAKIR F., REY R. and GERBER A. G. et al. Numerical and experimental investigations of the cavitating behavior of an inducer[J]. International Journal of Ro- tating Machinery, 2004, 10(1): 15-25.

[10] LIU S., ZHANG L. and NISHI M. et al. Cavitating turbulent flow simulation in a Francis turbine based on mixture model[J]. Journal of Fluids Engineering, 2009, 131(5): 051302.

[11] MEDVITZ R. B., KUNZ R. F. and BOGER D. A. et al. Performance analysis of cavitating flow in centrifugal pumps using multiphase CFD[J]. Journal of Fluids Engineering, 2002, 124(2): 377-383.

[12] POUFFARY B., FORTES PATELLA R. and REBOUD J.-L. et al. Numerical simulation of 3D cavitating flows: Analysis of cavitation head drop in turbomachinery[J]. Journal of Fluids Engineering, 2008, 130(6): 061301.

[13] HEJRANFARKazem,FATTAH-HESARYKasra. Assessment of a central difference finite volume scheme for modeling of cavitating flows using preconditioned multiphase Euler equations[J]. Journal of Hydrodynamics, 2011, 23(3): 302-313.

[14]FRIKHA S., COUTIER-DELGOSHA O. and ASTOLFI J. A. Influence of the cavitation model on the simulation of cloud cavitation on 2D foil section[J]. International Journal of Rotating Machinery, 2009, 2008: 146234.

[15] DUPONT P., OKAMURA T. Cavitating flow calculations in industry[J]. International Journal of Rotating Machinery, 2003, 9(3): 163-170.

[16] CELIK B. I., GHIA U. and ROACHE P. J. et al. Procedure for estimation and reporting of uncertainty due to discretization in CFD applications[J]. Journal of Fluids Engineering, 2008, 130(7): 078001.

10.1016/S1001-6058(11)60297-7

* Project supported by the National Science and Technology Foundation of China (Grant No. 51179100), the Key Research Projects of Shanghai Science and Technology Commission (Grant No.10100500200) and the Shanghai Program for Innovative Research Team in Universities.

Biography: ZHU Bing (1979-), Male, Ph. D.

CHEN Hong-xun,

E-mail: chenhx@shu.edu.cn