Mentzos M Etal_2004_a Numerical Simulation Of The Impeller-volute Interaction In A Centrifugal Pump

1st International Conference “From Scientific Computing to Computational Engineering” 1st IC-SCCE Athens, 8-10 September, 2004 © IC-SCCE

A NUMERICAL SIMULATION OF THE IMPELLER-VOLUTE INTERACTION IN A CENTRIFUGAL PUMP † * * * Michalis D. Mentzos , Andronicos E. Filios , Dionisios P. Margaris and Dimitrios G. Papanikas * Fluid Mechanics Laboratory, Mechanical Engineering and Aeronautics Department University of Patras GR-26500 Patras, Greece e-mail: [email protected] †

Fluid Mechanics & Turbomachines Laboratory, Mechanical Engineering Department, School of Pedagogical and Technological Education, GR-141 21 Athens, Greece e-mail: [email protected]

Keywords: Centrifugal pump, Computational fluid dynamics, Navier-Stokes code, Pump performance. Abstract. Pump designers are continually being challenged to provide machines that operate more efficiently, quietly, and reliably at lower cost. With the aid of the CFD approach, the complex internal flows in water pump impellers, which are not fully understood yet, can be well predicted, to speed up the pump design procedure. The present work describes a numerical simulation of the internal flow in a centrifugal pump. The object of the study is an industrial centrifugal water pump with backward curved blades, which is built within a vaneless single tongue volute. For the numerical simulation, the viscous Navier-Stokes equations are handled with a steady calculation utilizing the k-ε turbulence model and the multi reference frame technique is applied to take into account the impeller-volute interaction. With them, it is possible to simulate correctly the blade passage in front of the tongue and the flow and pressure distributions. The data obtained allow the analysis of the main phenomena existent in the pump, such as: pressure changes in the volute for different flow rates; and the incidence at the leading edge of the blade with different flow conditions. 1 INTRODUCTION The design of hydraulic turbomachines has reached the stage were improvements can only be achieved through a detailed understanding of the internal flow. The prediction of the flow in such equipment is very complicated due to the rotation and the curved three-dimensional shape of the impellers. Furthermore, the flow in turbomachines shows unsteady behaviour, especially at off-design conditions, as a result of interaction between impeller and pump casing. Considering these complexities, computer simulations will become increasingly important. Computational fluid dynamics (CFD) analysis is being increasingly applied in the design of centrifugal pumps. With the aid of the CFD approach, the complex internal flows in water pump impellers, which are not fully understood yet, can be well predicted, to speed up the pump design procedure. Thus, CFD is an important tool for pump designers. The use of CFD tools in turbomachinery industry is quite common today. Many tasks can numerically be solved much faster and cheaper than by means of experiments. Nevertheless the highly unsteady flow in turbomachinery raises the question of the most appropriate method for modeling the rotation of the impeller. Many CFD studies concerning the complex flow in all types of centrifugal pumps have been reported. Goto[1] presented a comparison between the measured and computed exit-flow fields of a mixed flow impeller with various tip clearances, including the shrouded and unshrouded impellers, and confirmed the applicability of the incompressible version of the three-dimensional Navier-Stokes code developed by Dawes[2] for a mixedflow centrifugal pump. Van Esh et al.[3] developed a numerical method based on a fully 3D finite element method for solving the inviscid, incompressible flow field in entire pump. The pump’s efficiency is determined applying Thwaites’[4] method along with Green’s “lag entrainment method”[5]. The capabilities of the proposed method are demonstrated by the analyses of the flow in two pumps. Zhou and Ng[6] and Ng et al.[7] also developed a three-dimensional time-marching, incompressible Navier-Stokes solver using the pseudocompressibility technique to study the flow field through a mixed-flow water-pump impeller. The applicability of the original code was validated by comparing it with many published experimental and computational results. Oh and Ro[8] used a compressible time marching method, a traditional SIMPLE method, and a commercial

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

program of CFX-Tascflow to simulate flow pattern through a water pump and compared the differences among these methods in predicting the pump’s performance. Recently, Kaupert et al.[9], Potts and Newton[10], Sun and Tsukamoto[11], and Byskov et al.[12] studied pump design and off-design performance using the commercial software CFX- Tascflow, Fluent, StarCD and Fine/Turbo, respectively. Although these researchers predicted reverse flow in the impeller shroud region at small flow rates numerically, some contradictions still existed. For example, Kaupert’s[9] experiments showed the simultaneous appearance of shroud-side reverse flow at the impeller inlet and outlet, but his CFD results failed to predict the numerical outlet reverse flow. Sun and Tsukamoto[11] validated the predicted results of the head-flow curves, diffuser inlet pressure distribution, and impeller radial forces by revealing the experimental data over the entire flow range, and they predicted back flow at small flow rates, but they did not show an exact back-flow pattern along the impeller outlet. Byskov et al.[12] investigated the flow field in a shrouded six bladed centrifugal pump impeller using LES and RANS simulations and their predictions are compared with experimental data obtained from particle image velocimetry. However, it is found that the two RANS models do not reproduce the stall phenomenon observed at quarter load and are incapable of detecting the difference between the two passages. From such literature, it was found that most previous research, especially research based on numerical approaches, had focused on the design or near-design state of pumps. Few efforts were made to study the offdesign performance of pumps. Centrifugal pumps are widely used in many applications, so the pump system may be required to operate over a wide flow range in some special applications. Thus, knowledge about offdesign pump performance is a necessity. On the other hand, it was found that few researchers had compared flow and pressure fields among different types of pumps. Therefore, there is still a lot of work to be done in these fields. In this work, the commercial CFD code Fluent, was used to study three-dimensional turbulent flow through a commercial water-pump during design and off-design conditions. Fluent is a software package that can predict laminar flow, turbulent flow, and heat transfer. It has been widely used in the field of turbomachinery, and the simulation results have been proven by many researchers to be reliable (Sun and Tsukamoto[11], Gonzalez et al.[13]). Fluent overcomes the meshing difficulties that arise in complex geometry by using a powerful CAD-based preprocessor, Gambit, which generates a surface mesh of triangles. This surface mesh is then converted into a volume mesh of tetrahedral elements. The selected commercial pump is the Norma 80-250 water-pump for which drawings were provided by the manufacturer[14]. In order to well suit the pump for CFD analysis, modifications were done. These concern the fitting of a front shroud and the adjustment of the mean camber line of the blades in a way that the relative w-velocity varies linearly from the inlet section of the impeller to the outlet section. The resulted CAD-model of the above pump is shown in Figure 1 and its main geometry and flow parameters are presented in Table 1.

Denomination

Value

Suction pipe diameter

Ds = 142,4mm

Impeller diameters Impeller widths Impeller angles Number of blades Flow rate in best efficiency point, rpm Specific speed (nq = n ·Q1/2/H3/4)

D1 = 157mm, D2 = 274mm b1= 31,0mm, b2= 20,8mm β1 = 10°, β2 =30° z=6 Q = 80m3/h, n = 1450rpm

Reynolds number at impeller exit (Re=U2·D2/ν) Figure 1. CAD-model of the commercial centrifugal pump under study.

nq = 22,86 Re = 2,84 ·106

Table 1: Geometric details and flow parameters of the centrifugal pump under study.

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

2 MODELS DESCRIPTION AND COMPUTATIONAL METHOD 2.1 Mathematical Models The code solves the fully 3D incompressible Navier-Stokes equations, including the centrifugal force source in the impeller and the unsteady terms. Turbulence is simulated with the standard 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, have been used. Basic Equations For three-dimensional incompressible, unsteady flow, the continuity and momentum equations can be written in the rotating coordinate system as follows:

∂ρ + ∇ ⋅ (ρU ) = 0 ∂t

(1)

and

(

(

))

∂ρU + ∇ ⋅ (ρU ⊗ U ) = ∇ ⋅ − pδ + µ eff ∇U + (∇U )T + S M ∂t

(2)

where vector notation has been used, ⊗ is a vector cross product; U is the velocity; p is the pressure; ρ is the density; δ is the identity matrix; and SM is the source term. For flows in a rotating frame of reference that are rotating at the constant rotation speed Ω, the effects of the Coriolis are modeled in the code. In this case, with r the location vector,

S M = − ρ [2 Ω ⊗ U + Ω ⊗ (Ω ⊗ r )]

(3)

k-ε Turbulence Model In Equation (2), µeff is the effective viscosity coefficient, which equals the molecular viscosity coefficient, µ, plus the turbulent eddy viscosity coefficient, µt :

µ eff = µ + µ t

(4)

The turbulent viscosity, µt, is modeled as the product of a turbulent velocity scale, Vt, and a turbulent length scale, lt, as proposed by Kolmogorov[15]. Introducing a proportionality constant gives

µ t = ρc µ ltVt

(5)

Both equation models take the velocity scale, Vt, to be the square root of the turbulent kinetic energy:

Vt = k

(6)

The turbulent kinetic energy, k, is determined from the solution of a semiempirical transport equation. In the standard k-ε two-equation model it is assumed that the length scale is a dissipation length scale, and when the turbulent dissipation scales are isotropic, Kolmogorov determined that

ε=

k3/ 2 lt

(7)

where ε is the turbulent dissipation rate. Therefore, the turbulence viscosity, µt, can be derived from Equations (5), (6), and (7) to link to the turbulence kinetic energy and dissipation via the relation

µt = Cµ ρ

k2

ε

(8)

where Cµ is a constant. Its value is 0,09. The values of k, ε come directly from the differential transport equations for the turbulence kinetic energy and turbulence dissipation rate:

∂ρk + ∇ ⋅ (ρUk ) − ∇ ⋅ (Γ k ∇k ) = p k − ρε ∂t

(9)

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

and

ε ∂ρε + ∇ ⋅ (ρUε ) − ∇ ⋅ (Γε ∇ε ) = (Cε 1 p k − Cε 2 ρε ) k ∂t

(10)

where the diffusion coefficients are given by

Γk = µ +

µt σk

(11a)

Γε = µ +

µt σε

(11b)

and

and Cε1=1,44; Cε2 =1,92; σk=1,0; and σε=1,3 are constants. The pk in Equations (9) and (10) is the turbulent kinetic energy production term, which for incompressible flow is

(

)

2 p k = µ t ∇U ⋅ ∇U + ∇U T − ∇ ⋅ U (µ t ∇ ⋅ U + ρk ) 3

(12)

Equations (1), (2), (9), and (10) form a closed set of nonlinear partial differential equations governing the fluid motion. Log-Law Wall Functions There are large gradients in the dependent variables near the wall. It is costly to fully resolve the solution in this near-wall region as the required number of nodes would be quite large. Thus a common approach known as “wall functions” is applied to model this region. In the wall-function approach (Launder and Spalding[16]), the near-wall tangential velocity is related to the wall shear stress by means of a logarithmic relation, which can be written as follows:

u+ =

1

κ

( )

(13)

ut uτ

(13a)

ρ∆yut µ

(13b)

τw ρ

(13c)

ln y + + C

where

u+ =

y+ =

uτ =

τw is the wall shear stress, ut is the known velocity tangent to the wall at a distance of ∆y from the wall, κ is the von Karman constant for smooth walls, and κ and C are constants, depending on wall roughness. However, this form of the wall-function equations has the problem that it becomes singular at separation points where the near-wall velocity, ut, approaches zero. In the logarithmic region, the alternative velocity scale, u*, can be used instead of u+:

u* = c µ1 / 4 k

(14)

This scale has the useful property of not going to zero if ut goes to zero (and in turbulent flow, k is never completely zero). Based on this definition, the following explicit equation for the wall shear stress is obtained:

τ w = τ visc

y* u+

(15)

where τvisc= µut/∆y; y*= ρu*∆y/µ; and u+ as given from equation (13). The recommended practice is to locate near-wall nodes such that y* is in the range of 20 to 50 for smooth walls. In the near-wall region, an estimate of the dissipation consistent with the log-law can be presented as

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

ε=

c µ3 / 4 k 3 / 2

(16)

u∆ y

The dissipation at the first interior node is set equal to this value. The boundary nodal value for k is estimated via an extrapolation boundary condition. The near-wall production of turbulent kinetic energy is derived to be

pk =

2 τ visc p k∗ µ

(17)

where 2

p k∗

 y ∗  du + = +   u  dy ∗  

(18)

2.2 Modeling details The computational grid was generated using the Fluent preprocessor Gambit. In a pre-step the walls of the impeller limiting the fluid flow space were separated with a CAD-tool and some additional inner faces were introduced. This was helpful since the complete unstructured grid was partially refined, as shown in fig. 2. The spiral casing with its circular symmetric cross section and the draft tube part directly upstream of the impeller inlet were quite difficult to mesh and this explains the adoption of the unstructured meshing, too. The resulting grid for the entire pump under study is shown in fig. 3. For the use with the fluent solver, two blocks with suitable boundary conditions form the complete computational domain. All parts of the pump rotating in the inertial frame are made part of the impeller fluid zone that is calculated in a rotating reference frame when using the FR-approach. The second fluid zone is steady, i.e. the spiral casing, the discharge nozzle that is extended almost three outlet diameters for a less reacting outlet boundary condition, as well as the two impeller side gaps. Grid interfaces are needed to couple fluid zones which are in relative motion to each other. The rotating fluid zone is constructed with 114.908 tetrahedral elements, while the stationary fluid zone comprises 204.326 tetrahedral elements.

Z Y

Z

X

Y X

Jul 08, 2004 Figure 3. Sketch of the pump unstructured mesh FLUENT 6.0 (3d, segregated, ske) Jul 08, 2004 Figure 2. Mesh structure in theFLUENT impeller. (outlet pipe portion is added). 6.0 (3d, segregated, ske)

Turbulence was modeled using the most popular and standard model for investigations not aiming at turbulence model validation, the standard k-ε model with standard wall functions for smooth walls. As inlet boundary condition the velocity according to the operating point flow rate was prescribed. Also, non-slip boundary conditions have been imposed over the impeller blades and walls, the volute casing and the inlet pipe wall. Turbulence intensity was not measured and estimated to 5%, the length scale to (Ds/2) mm. At the exit of the discharge nozzle, assuming a fully developed turbulent flow, a practical zero velocity gradients was set. Second order upwind schemes were chosen for space discretisation while the pressure correction equation was solved with the SIMPLE algorithm. Convergence is checked by residuals decreasing about two orders. For setting up the problem, a low rotational speed in the inputs for boundary conditions and for the angular velocity of the reference frame was used. The rotational speed in the first attempt was selected as 10% of the actual operating condition and gradually increased to 100%. A converged multi reference frame result needed about 2000 iterations, in a 3GHz Pentium IV PC, for the actual operating condition. The results are certainly may be used as an initial flow field for a transient calculation.

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

3

RESULTS FOR IMPELLER-VOLUTE INTERACTION

One rotational speed, 1450 rpm, was used in the computations. At this rotational speed, several different flow rates were specified at the inlet boundary so as to study design and off design flow patterns. The convergence criteria for each run were set to be 10-5 for root mean-square (RMS) residuals of mass/momentum equations and 10-4 for RMS residuals of k-ε equations. It was clearly evident that after several hundred time steps in each run, the above criteria could be satisfied, and the convergence was reached gradually. Figure 4 shows the profiles of static pressure in the rotational zone of the domain at the design point. As for pressure distribution, it can be seen clearly that the pressure increases gradually in a stream wise direction, and normally it has higher pressure on the pressure surface than on the suction surface on each blade. Figure 5 shows the w-relative velocity vectors through the impeller’s blade passages at the same operating conditions. From the last figure it is evident that the flow is smooth and no recirculation is in presence. Figures 6 and 7 show the static pressure profiles in the impeller-volute domain at the design point. In both figures, the maximum outlet pressure is reached at the entrance of the attached pipe outlet portion. Various volume flow rates were specified to study in constant rotational speed the off-design conditions. It was found that with the change of inflow rate even as much us 50% of the design flow rate, the flow patterns look similar to each other. 2.09e+00 1.98e+00 1.87e+00 1.76e+00 1.65e+00 1.54e+00 1.43e+00 1.32e+00 1.21e+00 1.10e+00 9.89e-01 8.80e-01 7.70e-01 6.60e-01 5.50e-01 4.41e-01 3.31e-01 2.21e-01 1.12e-01 1.83e-03 -1.08e-01 -2.18e-01 -3.27e-01 -4.37e-01 -5.47e-01 -6.56e-01

1.84e+01 1.77e+01 1.69e+01 1.62e+01 1.55e+01 1.47e+01 1.40e+01 1.33e+01 1.25e+01 1.18e+01 1.11e+01 1.03e+01 9.60e+00 8.86e+00 8.13e+00 7.39e+00 6.66e+00 5.92e+00 5.19e+00 4.45e+00 3.72e+00 2.98e+00 2.25e+00 1.51e+00 7.80e-01 4.47e-02

YZ

Z Y X

X

Figure 5. Relative velocity vector (m/s) through the impeller’s blade passages at the design point.

relative-velocity Colored By Velocity Magnitude (m/s)

Figure 4. Profiles of static pressure (atm).

Profiles of Static Pressure (atm)

Jul 08, 2004 FLUENT 6.0 (3d, segregated, ske)

Jul 08, 2004 FLUENT 6.0 (3d, segregated, ske)

2.09e+00 1.93e+00 1.78e+00

2.09e+00

1.63e+00

1.93e+00 1.78e+00

1.48e+00

1.63e+00

1.32e+00

1.48e+00

1.17e+00

1.32e+00

1.02e+00

1.17e+00

8.67e-01

1.02e+00

7.15e-01

8.67e-01

5.63e-01

7.15e-01

4.10e-01

5.63e-01

2.58e-01

4.10e-01

1.05e-01

2.58e-01 1.05e-01

-4.69e-02

-4.69e-02

-1.99e-01 -3.52e-01

-1.99e-01 -3.52e-01 -5.04e-01

YZ

-5.04e-01

X

-6.56e-01

Y Z

X

-6.56e-01

Contours of Static (atm) Figure 6.Pressure Contours of static pressure (atm) at the FLUENT 6.0 (3d, seg design point.

4

Figure 7. Contours of static pressure (atm) at the FLUENT 6.0 (3d design point.

Contours of Static Pressure (atm)

CONCLUSIONS

The commercially available 3D Navier-Stokes code called Fluent, which has a standard k-ε two-equation turbulence model, was chosen to simulate the internal flow of a commercial centrifugal pump. The complete centrifugal pump including impeller side gaps and discharge nozzle has been modeled and meshed with an unstructured grid. Quasi-steady calculations have been performed for the design point as well as for a range of volume rates with a deviation of 50% from the design value but with similar flow patterns. The predicted results are presented in terms of pressure profiles and velocity vectors. Having a closer look at the flow rates in a rotating impeller, the multiframe reference frame approach fails completely due to its fixed coupling formulation. However, the present approach is useful for basically understanding the flow states in various operating points. Certainly the scheduled transient calculations may serve as a real tool for understanding the interaction between impeller and spiral casing. Further work will focus on a detailed statement on the influence

Michalis D. Mentzos*, Andronicos E. Filios†, Dionisios P. Margaris* and Dimitrios G. Papanikas.

and a general validation of different turbulence models for use with pump calculation. REFERENCES [1] [2] [3] [4] [5] [6] [7]

[8] [9] [10] [11] [12] [13] [14] [15] [16]

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, Vol.114, pp. 373– 382. Dawes, W. N. (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: American Society of Mechanical Engineers. Van Esch, B.P.M., Kruyt, N.P., and Jonker J.B. (1997), “An inviscid-viscous coupling method for computing unsteady flows in entire pump configurations”, The ASME Fluids Engineering Division Summer Meeting, FEDSM’97, June 22-26, pp. 1-8. Thwaites, B.(1949), “Approximate calculation of the laminar boundary layer”, Aeronaut. Q., Vol. 1, pp. 245-280. Green, J.E., Weeks, D.J., and Brooman, J.W.F. (1972), “Prediction of turbulent boundary layers and wakes in compressible flow by a lag-entrainment method”, RAE Technical Report 72231, pp. 49-53. Zhou, W. D., and Ng, E. Y. K. (1998), “3-D viscous flow simulation of mixed-flow water pump impeller with tip-clearance effects”, Proceedings of the 4th International Conference and Exhibition on Pumps and Systems, pp. 189–198, Singapore, HQ Link Pte Ltd. Ng, E. Y. K., Zhou, W. D., and Chan, W. K. (1998), “Non-Newtonian effects on mixed-flow water pump using CFD approach”, Proceedings of the 19th International Association of Hydraulic Research Symposium, Section on Hydraulic Machinery and Cavitation, pp.735–749, Singapore, International Association of Hydraulic Research. Oh, J. S., and Ro, S. H. (2000), “Application of time marching method to incompressible centrifugal pump flow”, Proceedings of the 2nd International Symposium on Fluid Machinery and Fluid Engineering, pp. 219–225, Beijing: Tsinghua University Press. Kaupert, K. A., Holbein, P., and Staubli, T. (1996), “A first analysis of flow field hysteresis in a pump impeller”, ASME Journal of Fluids Engineering, Vol.118, pp.685–691. Potts, I., and Newton, T. M. (1998), “Use of a commercial CFD package to predict shut-off behavior of a model centrifugal pump: an appraisal”, IMechE Seminar Publication: CFD in Fluid Machinery Design, London: Institute of Mechanical Engineers. Sun, J., and Tsukamoto, H. (2001), “Off-design performance prediction for diffuser pumps. Journal of Power and Energy”, Proceedings of I. Mech. E., Part A, Vol. 215, pp. 191–201. 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. 125, pp. 73-83. Gonzalez, J., Fernandez, J., Blanco, E., and Santolaria C. (2002), “Numerical simulation of the dynamic effects due to impeller-volute interaction in a centrifugal pump”, ASME Journal of Fluids Engineering, Vol. 124, pp. 348-355. Drakos-Polemis S.A., Pump Catalogue. Kolmogorov, A. N. (1941), “Local structure of turbulence in incompressible viscous fluid for very large Reynolds number”, Doklady Akademyia Nauk SSSR, Vol. 30, pp. 9-13. Launder, B.E., and Spalding, D.B. (1974), “The numerical computation of turbulent flows”, Complete Methods of Applied Mechanical Engineering, Vol. 3, pp. 269-289.