Grapsas V Etal_2006_experimental And Computational Study Of A Radial Flow Pump Impeller

2nd International Conference “From Scientific Computing to Computational Engineering” 2nd IC-SCCE Athens, 5-8 July, 2006 © IC-SCCE

EXPERIMENTAL AND COMPUTATIONAL STUDY OF A RADIAL FLOW PUMP IMPELLER Vasilios A. Grapsas*, Michalis D. Mentzos †, John S. Anagnostopoulos*, Andronicos E. Filios†, Dionisios P. Margaris† and Dimitrios E. Papantonis* *

Laboratory of Hydraulic Turbomachines School of Mechanical Engineering / Fluids Section National Technical University of Athens, Greece Heroon Polytechniou 9, Zografou, 15780 Athens, Greece e-mail: [email protected] †

Fluid Mechanics Laboratory Mechanical Engineering and Aeronautics Department University of Patras GR-26500 Patras, Greece e-mail: [email protected] Keywords: Experimental measurements, Impeller, Pump Characteristics, CFD. Abstract. Radial flow pumps are widely used in a wide range of applications. Although they have attained a high degree of perfection, both from the point of view of hydraulic behaviour and reliability, a lot more can be done. This paper describes an experimental investigation of a radial flow pump impeller with 2D curvature blade geometry.The experimental set up mainly includes a radial flow impeller inserted into a completely twodimensional space, limited by two transparent plexiglass plates, an electric drive motor, a storage tank and a control system. Investigation of the behaviour of the above impeller for a wide flow rate range and for various rotational speeds was carried out. The obtained experimental results were used to validate a precision check of numerical results. The flow simulation has been generated with a numerical code and a commercial CFD code. The viscous Navier-Stokes equations are handled with the control volume approach and the k-ε turbulence model. An unstructured Cartesian grid is applied and local refinement techniques were used to treat the curved boundary surfaces of the blade. Finally, experimental and numerical results concerning H-Q curve and performance behaviour were compared at different flow conditions. The results show good agreement, encouraging the extension of the developed methodology to the understanding of the unsteady behavior of cavitating flows. 1 INTRODUCTION The studies on flow characteristics of centrifugal pumps have attained new importance in recent times. Formerly it was sufficient for a designer to analyze the steady state operation of a pumping system. Now with the increasing complexity of pumping systems, experimental and theoretical analysis is desirable. Computational Fluid Dynamics (CFD) analysis is being increasingly applied in the design of centrifugal pumps and especially in order to illustrate fields which are difficult to be studied experimentally. With the aid of computational fluid dynamics, the complex internal flows in water pump impellers can be well predicted, facilitating thus the design of pumps. Numerous studies are available, on the static performance of centrifugal pumps, to the extent that the steady-state characteristics of the pumps can be predicted by available data with sufficient accuracy and many comparisons between CFD studies and experiments concerning the complex flow in all types of centrifugal pumps have been reported. The first systematic investigations of rotodynamics pumps on a scientific basis were commenced in 1890 at the works of Sulzer Brothers in Switzerland. This lead was followed by other factories that endeavored to become leading manufacturers of centrifugal pump design and in later years, in the design of helicoidal, diagonal and axial flow pumps. Since then, experimental data were used as a validation tool for the computation methods developed, till recently. Byskov et al.[1] investigated the flow field in a shrouded six bladed centrifugal pump impeller and their predictions were compared with experimental data obtained from particle image velocimetry. The computed flow fields at the exit of a mixed flow impeller with various tip clearances[2], including the shrouded and unshrouded impellers, were compared with experimental measurements[3], confirming by this way

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ the applicability of the incompressible version of the developed three dimensional Navier-Stokes code. In an other case [4], a three dimensional, incompressible Navier-Stokes solver was also developed to study the flow field through a mixed flow water pump impeller. The applicability of the original code was verified by comparing it with experimental results. More recently, the off-design pump performance was studied using the commercial software CFX-TASCflow and the predicted results were validated by revealing the experimental data over the entire flow range[5]. The present study consists on the experimental investigation of a centrifugal test pump impeller and the comparison of the experimental data with the numerical obtained by two numerical methods. Experiments were carried out at the National Technical University of Athens. Experiments were conducted on a radial flow pump the main characteristic of which is that the outlet of the impeller discharges on a vaneless radial diffuser. The predicted results for the head-flow curve in these cases are presented over the entire flow range. On the other hand, for the numerical simulation of the three dimensional flow through the radial impeller during design conditions, a commercial CFD code, called FLUENT® and a recently developed numerical algorithm by the Laboratory of Hydraulic Turbomachinery, of the National Technical University of Athens were used. 2 EXPERIMENTAL LAYOUT 2.1 Experimental apparatus and test procedure The experimental setup, established in the Laboratory of Hydraulic Turbomachinery of NTUA, is composed by the experimental radial flow pump recirculating the water of a storage tank, the capacity of which is of the order of 320m3, ensuring that the water temperature remains constant during the execution of the experiments. The flow rate regulation is obtained by throttling of the valve installed at the discharge pipe, as well as by the variation of the speed of rotation. The measuring equipment is composed by two differential pressure transducers, one for the head of the pump and the second for the flow rate (pressure difference across a calibrated orifice plate), a torsional torque meter installed at the shaft between the impeller and the motor and a digital counter for the speed of rotation. The experimental installation with the instrumentation system is shown in Fig. 1.

Fig. 1. Complete assembly of the experimental apparatus and the model pump. In order to generate a uniform circumferential pressure distribution at the impeller outlet, a vaneless radial diffuser was used instead of a volute. The diffuser itself was connected to the downstream system with twelve (12) Φ50 discharge pipes. Figure 2 shows a cross-sectional view of the pump with a vertical rotating shaft. The radial flow impeller is inserted into a completely two (2) dimensional space, limited by two transparent plexiglass plates playing the role of the vaneless diffuser. The so formed casing is axisymmetrical. The impeller shroud and the shroud sided casing was made of Plexiglas to enable direct observations of the impeller. Another characteristic is the parallel hub and shroud to get an almost 2-dimensional blade-to-blade channel with constant width. The flow-measuring probes can be placed at five radial sections of the ratio R=5, 10, 15, 20, 25 on the diffuser wall of the impeller shroud side. Flowing into the impeller, from an open tank, water is discharged to the pipes, at the lower part of the apparatus. The suction and delivery pressures are measured by semi-conductor type pressure transducers, which are installed in points “1” and “2” respectively. The actual places of the pressure transducers are selected according to ISO 5167 [6]. The pump was driven by a three-phase AC electric motor, the speed of rotation of which can be continuously varied by an inverter. The flow rate (operation condition) is controlled by a butterfly valve in the discharge pipe and can be set in the range of 0 to 30 l/s. The design parameters of the impeller geometry are determined by using classical calculation procedures[7]. The centrifugal impeller has nine (9) two-dimensional (non-twisted) blades with inlet and exit diameter D1=70 mm, D2=190 mm, exit width b2=9 mm as well as inlet width, and inlet and exit angle β1=26 deg, β2=49 deg. The blade thickness is fixed at s=5mm. The impeller blade geometry is illustrated in figure 2 and table 1. The geometry of the blade profile is described with a single circular arc whose radius is defined as:

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ R=

D 22 − D12 (1) 4 ⋅ (D 2 cos β 2 − D1 cos β 1 )

Impeller Technical Characteristics Blade shape Single arc method for constructing the blade profile Inlet diameter D1 70 mm Outlet diameter D2 190 mm Blade inlet angle β1 26o Blade outlet angle β2 49o Exit width b2 9 mm Blade thickness s 5 mm Number of blades z 9 Nominal Head H 47,5 m Nominal Discharge Q 62,5 m3/h Rotating speed n 3000 rpm Table 1. Design parameters of impeller The experiments were carried out at four different speeds (400, 500, 600 and 700 rpm) and were transformed at 3000 rpm. Head, flow rate and rotational speed are recorded.

800m m

2

1

190mm

Figure 2. Cross sectional view of the impeller.

2.2 Analog to Digital Card In the experiments, in order to evaluate the incoming signals, a human interface computer program is used.

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ All the analog signals from the transducers (4-20mA), after proper amplification, are transmitted to a computer where, via an A/D (Analog to Digital) interface card, are stored and processed in digital form. The A/D card samples the data from the different channels, where the analog signals are fed in, with the desired sampling rates and software gain for each channel, through software developed for the present experimental program. The actual program is written in Q-Basic language. The acquired data are then recorded on a data file in the computer. From the data, instantaneous rotational speed, flow rate and pressure rise in the pump are read out and plotted. The accuracy of A/D conversion in the data acquisition is 0,2 millivolt per volt. 2.3 Impeller head and power calculations Pumps are usually operated with constant speed, head and flow rate. A pump is, therefore, designed for one particular point of operation. Ideally, the duty point coincides with the maximum efficiency of the pump. In a pump, kinetic energy imparted to the fluid must be converted into pressure energy. The total head of pump or the energy gained by the fluid through the impeller, H is defined as the gain of the total energy of the fluids between the points “1” and “2” (Fig. 2): H = H

2

− H 1 = z2 + p2 +

c2 c 22 − ( z 1 + p 1 + 1 ) = (z 2 − z 1 ) + ( p 2 − p 1 ) + 2g 2g

where (z2-z1) is the elevation difference, c 2 =

c1 =

Q

πD12 / 4

⎛ c 22 − c 12 ⎜ ⎜ 2g ⎝

⎞ (2) ⎟ ⎟ ⎠

Q is the velocity at the radius r of the vaneless diffuser, 2πrb

the inlet velocity, denoting by Q the flow rate through the pump and p2 and p1 the static pressure

at points “2” and “1” respectively. Applying the momentum principle on the radial type impeller, from the Euler equation the theoretical head Hu for infinite number of blades, is defined as:

Hu =

1 (cu 2 u 2 − cu1u1 ) (3) g

where u represents the peripheral velocity and cu the tangential velocity. 3. COMPUTATION METHODS In order to predict the fluid behavior through the impeller, two computational methods were used. For the simulation of the incompressible, turbulent flow, with the numerical methods, the continuity and momentum equations can be written in the rotating coordinate system as follows: Continuity:

G ∇⋅w = 0

Momentum:

G G G G G ∇p G G G w ⋅ ∇w = −2ω × w − ω × (ω × w) − +ν ∇2w

(4) (5)

ρ

G

where p is the fluid pressure; ρ is the density; ν is the kinematic viscosity; w is the fluid velocity in the rotating system and ω is the rotation speed of the impeller. The governing equations are solved in a rotating reference frame, so including Coriolis and centrifugal forces. The computational domain for both methods is a periodically symmetric section of the centrifugal impeller. 3.1 Numerical Simulation with the commercial code FLUENT®. The simulation of the three-dimensional turbulent flow through the test pump was enhanced with the commercial CFD code FLUENT®. FLUENT is a software package available to predict laminar or turbulent flow which has been widely used in the field of turbomachinery and the simulation results have been proved by many researchers to be reliable[5,8]. Modeling the impeller numerically, all nine impeller passages should be included ideally, in order to simulate the true flow field and detect any asymmetry of the flow. However, due to the diffuser ring, the parallel shroud and hub of the radial pump impeller studied, and the geometrical symmetry of it, we have the opportunity to simulate accurately only one of the blade passage, with the enforcement of periodicity boundary conditions, as it is shown in figure 2. The computational grid is of structured type and it is generated with the Fluent preprocessor Gambit. The whole domain consists of a lot of subdomains or zones, in a way that the density and the quality of the cells in local flow field regions can be suitably controlled and handled depending on pressure gradients and velocities. Some of them are stationary while some other zones that incorporate the blades are moving with the applied rotational speed, i.e. 3000 rpm. The first zone represents the suction or inlet pipe and the last zone is the

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ discharge or outlet portion where the flow is fully developed with a less possible reacting outlet boundary condition. Structured hexahedral cells are used in the whole domain. The total number of cells is 321.000. The size of the resulting cells which are in the neighborhood of the walls is not adequate for a full boundary layer simulation; however it provides correct values for the pump performance and allows the analysis in details of the main phenomena involved. The resulting mesh for the entire computational domain under study is shown in figure 3a and a detail of the structured mesh is shown in figure 3b.

Y Z

X

Y Z

X

Figure 3. a) Computational mesh for the test impeller, and b) detailed view at the blade’s leading edge. The modeled boundary conditions are the ones considered with more physical meaning for turbomachinery flow simulations. At the inlet zone, the axial velocity is a constant based on the through flow for the pump. The absolute tangential velocity at the inlet is zero, which implies in the rotating frame the relative velocity is –rω, and the radial velocity is zero. The involved parameters regarding the turbulence intensity and the hydraulic diameter in the lack of realistic turbulent inflow conditions in industrial applications are estimated with values of 5% and D1/2 respectively. The only specification made at the outlet is that the static pressure in the absolute frame is uniform and is set to zero. This absolute condition is converted into the appropriate relative pressure in the rotating frame. Periodic boundaries are used upstream and downstream of the blade leading and trailing edges, respectively. For the rotating solid surfaces all of the relative velocity components are set to zero, imposing the non-slip condition. The flow and pressure field through the impeller results from the solution of the fully three-dimensional incompressible Navier-Stokes equations, including the centrifugal force source. Turbulence is simulated with the standard RNG k-ε model. Although grid size is not adequate to investigate local boundary layer variables, global ones are well captured. For such calculations, wall functions, based on the logarithmic law, are used. The pressure-velocity coupling is calculated through the SIMPLE algorithm. Second order, upwind discretizations is used for convection terms and central difference schemes for diffusion term. Aiming to smooth convergence, various runs were attempted by varying the under-relaxations factors. In that way a direct control regarding the update of computed variables through iterations was achieved. Initializing with low values for the first iterations steps and observing the progress of the residuals, their values were modified for accelerating the convergence. Also we have mentioned that we start our “runnings” with small rotational speed, and continue to increment it gradually until we reach the desired operating condition. The number of iterations has been adjusted to reduce the scaled residual below the value of 10-5 which is the convergence criteria. For each run, the observation of the integrated quantities of total pressure, at suction as well as at discharge surface was appointed for the convergence of the solution. In many cases this drives the residuals in lower values than the initially set value. Depending on the case, the convergence was achieved at difference iterations, as the result at a specific mass-flow was used to initialize the computations at another massflow. Since the problem involves both stationary and moving zones, the multiple reference frame model was selected. It is a steady-state approximation in which individual cell zones move at different rotational speeds. As the rotation of the reference frame and the rotation defined via boundary conditions can lead to large complex forces in the flow, calculations may be less stable as the speed of rotation and hence the magnitude of these forces increases. To control this undesirable effect, each run starts with a low rotational speed and then slowly is increased the rotation up to the desired level. In order to well suit the pump for CFD analysis, a front shroud was fitted and a mean camber line was adjusted in a way that the relative w-velocity varies linearly from the inlet section of the impeller to the outlet section. 3.2 Numerical Simulation with the code of NTUA In the specific numerical algorithm the system of the governing equations is numerically solved with the

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ finite volume approach and turbulence is modeled with the standard k-ε model. A pseudo-3D incompressible term in dimensional form is added to the continuity equation to simulate the actual velocity and pressure field in the 3D blade-to-blade domain. An unstructured Cartesian grid is applied and adaptive grid refinement techniques are incorporated [9,10]. The Cartesian grid is adaptively refined near the leading and trailing edges and along the pressure and suction sides, using two refinement levels. Local refinement of the computational grid in these regions of steep gradients, can significantly improve the accuracy of the results and of the blade geometry representation, without increasing considerable the computer storage and the CPU-time requirements. The main drawback of the Cartesian grid which is the simulation of irregular boundaries came over with a “partially blocked cell” technique [11] which makes possible the solution of the grid cells that are crossed by the blade surfaces and are solved with an almost second order accuracy. Calculations are typically started from a no-flow initial condition, with the impeller at standstill. The rotational speed is increased gradually until the final speed is reached. The first flow rate calculated has always been the nominal flow rate. Often the calculations for some flow rate can be started from the result of a neighbouring flow rate, without going through the procedure of gradual increase of the rotational speed.

Figure 4. a) Computational grid for the 2D pump impeller, and b) detailed view at the blade’s leading edge. 4 RESULTS The experiments were carried out at a constant speed of 400, 500, 600 and 700 rpm and were deducted to 3000rpm. In figure 7 the four series of measurements are presented for the H-Q curves. As observed, the headflow curves increase with the increase of the rotation speed. In order to train and test a series of older measurements of the current impeller with spiral casing were used, obtained in 3000 rpm. In figure 6, experimental data are presented for the radial impeller along with the older measurement. The H-Q curve for the impeller with the spiral casing is slightly lower of the current H-Q curve due to the lack of the volute which reduces the disk/friction losses through the pump. In figure 7 experimental measurements are plotted along with the numerical predictions from the two computational methods and the experimental Hu-Q curve. Both numerical methods are a bit higher than the experimental data and only near and below the Best Efficiency Point (Q=62,5m3/h) tend to overlap. After the BEP a 5% difference among the two computational methods is observed. This can be explained from the different numerical methods and the ignorance of the volute and the particularities of the testing apparatus which reduce the hydraulic losses. The theoretical head Hu is also higher from the H-Q computational curves, as expected, due to the ignorance of the losses inside the casing. Based on the numerical models the pressure contours for the flow fields were drawn, for the two computational methods. Fig. 8a shows the flow simulated with the Fluent Code. The flow has a tendency to separate at the inlet radius of the blade and a recirculation zone is illustrated at the suction side. Moreover, it can be seen clearly from the pressure relief map of fig. 8b that the pressure increases gradually in a stream wise direction and normally higher pressure is exceeded on the suction surface than on the pressure surface. Comparisons between the predicted static pressure fields for the two numerical methods are shown in Fig. 9 and 10 at the design point. As shown in these figures and as reveals the colour distribution representing the pressure field, the values predicted by both computations are very close. From figures 8a and 10a a recirculation zone is revealed in the blade’s pressure side. It is found from a detailed view of the pressure field in the vicinity of the leading edge that the region of the large pressure fluctuation appears in the pressure and suction sides just downstream from the leading edge (fig. 9b and 10b), where the flow accelerates and pressure minimizes.

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ 4 3.5 3

H (mΣΥ)

2.5 2 1.5 1 0.5 0 0

5

10

15

20

25

30

Q (m 3/h) H-Q (400rpm)

H-Q (500rpm)

H-Q (600rpm)

H-Q (700rpm)

Figure 5. Comparison of H-Q curves for 400, 500, 600 and 700 rpm. 70

60

H (mΣΥ)

50

40

30

20

10

0 0

20

40

60

80

100

120

Q (m 3/h) H-Q (400rpm)

H-Q (500rpm)

H-Q (600rpm)

H-Q (700rpm)

Impeller with Spiral Casing

Figure 6. Comparison between experimental data of the impeller in the parallel plates and with the spiral casing in 3000 rpm. 70

60

50

H (mΣΥ)

40

30

20

10

0 0

20

40

60

80

100

120

Q (m3/h) H-Q (400rpm)

H-Q (500rpm)

H-Q (600rpm)

NTUA

UPatras

Hu

H-Q (700rpm)

Figure 7. Comparison of experimental and computed results in 3000 rpm.

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________

Figure 8a. Pressure distribution and velocity isolines with Fluent code, 8b. 3D Pressure distribution.

Figure 9. Contour of the calculated static pressure fluctuation (nominal flow rate) with Fluent a. around the blade, b. near the leading edge.

Figure 10a. Pressure contours and flow streamlines in the computational domain of NTUA model.

Figure 10b. Details of the flow field around the normal edge of NTUA model.

5 CONCLUSIONS In this study are presented experimental results concerning the operating characteristics of a laboratory radial flow pump and their comparison with corresponding numerical results obtained by two numerical codes. A numerical code for the simulation of the 3D flow in the centrifugal pump impeller, based on the 3D code FLUENT, has been developed by University of Patras and a 2D numerical analysis code has been developed by the National Technical University. Both experimental and numerical results for the H-Q curve were presented at 3000 rpm and the pressure distributions within the impeller were also compared. The results obtained show good agreement and confirm the ability of the models to simulate the main features of 3D flows in rotating turbomachinery. REFERENCES [1]

Byskov, R.K., Jacobsen, C.B., and Pedersen N. (2003), “Flow in a centrifugal pump impeller at design and off-design conditions-Part II: Large Eddy simulations”, ASME Journal of Fluids Engineering, Vol. 124,

Vasilios A. Grapsas, Michalis D. Mentzos, John S. Anagnostopoulos, Andronicos E. Filios, Dionisios P. Margaris and Dimitrios E. Papantonis

___________________________________________________________________________ pp. 348-355. Goto, A., (1992), “Study of internal flows in a mixed-flow pump impeller at various tip clearances using three-dimensional viscous flow computations”, ASME Journal of Turbomachinery, 114, pp. 373-382. [3] Dawes, W., (1986), “A numerical method for the analysis of three dimensional viscous compressible flow in a turbine cascade: application to secondary flow development in a cascade with and without dihedral”, ASME Paper 86-GT-145, New York. [4] Benra, F.K. (2001), “Economic development of efficient centrifugal pump impellers by numerical methods”, World Pumps, May 2001, pp. 48-53. [5] Sun , J., and Tsukamoto, H. (2001), “Off-design performance prediction for diffuser pump”, Journal of Power and Energy, Vol. 215, pp. 191-201. [6] ISO 5167, (1980), “Measurement of fluid flow by means of orifice plates, nozzles and venture tubes inserted in circular cross-section conduits running full”. [7] Stepanoff, A.J. (1993), “Centrifugal and Axial Flow Pumps, Theory, Design and Application”, Krieger Publishing Company Malabar, Florida. [8] Gonzalez, J., Fernandez, J., Blanco, E., and Santlaria C. (2002), “Numerical Simulation of the dynamic effects due to impeller-volute interaction in a centrifugal pump”, ASME Journal of Fluids Engineering, Vol. 125, pp. 348-355. [9] Grapsas, V. and Anagnostopoulos, J. (2004), “Numerical optimization of the hydrodynamic shape of fluid flow systems”, Proceedings 1st IC-SCCE, Athens, Greece, 8-10 September. [10] Anagnostopoulos, J. (2003), “Discretization of transport equations on 2D Cartesian unstructured grids using data from remote cells for the convection terms”, Intl. J. for Numerical Methods in Fluids, 42, pp. 297-321. [11] Anagnostopoulos, J. (2005), “A numerical Simulation Methodology for Hydraulic Turbomachines”, 5th GRACM International Congress on Computational Mechanics, Limassol, Cyprus, 29 June-1 July. [2]