Unsteady Numerical Simulations of the Flow Related to the Unstable Energy-discharge Characteristic of a Medium Specific Speed Double Suction Pump

Regions of positive slope in the pressure-discharge characteristics can result in a reduction or even lack of damping of system instabilities. They are therefore one of the major concerns in design and operation of centrifugal pumps as they are limiting the admissible operating range. The considered preliminary hydraulic design of an industrial double suction pump of medium specific speed ν = 0.410 (0.205 per impeller side) shows a marked saddle in the energydischarge characteristic associated to a sudden drop of efficiency versus discharge at part load. Unsteady RANS type flow simulations are performed using hexahedral meshes with 2.5 million nodes to model the inlet casing, the shrouded double sided impeller with 2 x 7 blades, the diffuser with 12 blades and the volute. In unsteady solution monitoring, low frequency (below blade passing frequencies) phenomena are noticed. Therefore, simulation times of up to 10 impeller revolutions at each flow rate are requested to achieve statistically steady behavior of the flow judged on global performance numbers and circumferential flow rate distribution. The numerical simulations emphasize a drop in the characteristic, though at a lower flow rate than found on the test rig. It is 1 shown to be associated to a one-sided separation in the diffuser, further leading to an unbalanced flow rate distribution of about 10% of flow rate between both sides of the impeller. There is a region of hysteresis, where both configurations with balanced and unbalanced flow rate distributions can be obtained for the same global flow rate. The asymmetric flow distribution leads to asymmetric velocity profiles at the impeller-diffuser interface which results in a strongly vortical flow in the diffuser channels, where an important amount of energy is dissipated in regions of increased viscous and turbulent shear. NOMENCLATURE C Fluid Velocity , [m/s] cp Pressure Coefficient, [-] fn Rotational Frequency, [Hz] p Pressure, [Pa] Q Flow Rate, [m3/s] y+ First Node Dimensionless Wall Distance, [-] φ Flow Coefficient, [-] ψ Energy Coefficient, [-] ρ Fluid Density, [kg/m3] Copyright c © 2007 by ASME A,B Side A, Side B r Loss evaluated by Area Integral of Energy Fluxes rv Loss evaluated by Volume Integral of Viscous Work vi Diffuser Channel i ∗ Normalized to Best Efficiency Point INTRODUCTION Positive slope in the energy-discharge characteristic of centrifugal pumps has been investigated for a long time. Both experimental investigations and steady numerical simulations have shown that high specific speed impellers experience flow separations when the performance curve exhibit instability (1, 2). Pedersen (3) identifies alternate stall in a 2D-Pump impeller without diffuser. Former experimental and numerical studies on a medium specific pump turbine (4) have shown a flow separation on the diffuser top wall extending back into the runner to be related to an undesirable performance drop. The intense rotor-stator interaction in centrifugal pump with small gaps between impeller exit and diffuser inlet leads to highly unsteady 3-dimensional flow patterns in the rotor stator-interaction zone and the downstream diffuser that can not reasonably be treated using steady approaches (5, 6). Unsteady RANS approaches (7) and LES simulations (8) have both shown good predictions of unsteady pressure in turbomachinery. Moreover, a part the periodic blade passing frequencies, lower frequency phenomena like alternate stall or rotating stall in the diffuser can occur, especially at part load (9). Sano et al. relate the apparition of diffuser stall to a flat part in the diffuser performance curve and show the influence of the radial impeller-diffuser gap on the onset of different diffuser stall forms (10, 11). With the aim of investigating an appropriate methodology for predicting pump instability, a rather old design of a double suction pump which exhibits a performance curve with a well marked saddle shape has been selected as a case study. We first introduce the numerical method and the case study geometry and present the obtained performance curve and conclude by a comparative analysis of the simulation results of two operating points. NUMERICAL METHOD The flow is simulated by solving the incompressible Reynolds-averaged Navier-Stokes Equations using a commercial finite-volume solver (CFX-5) and closing the turbulent stresses by the Menter-SST-Model. The computational domain consists of block-structured hexahedral meshes containing a few prismatic elements in swept prismatic blocks to avoid low element face angles or collapsed element edges (Fig. 1). The mesh refinement is chosen based on the experience gained on former test cases (4) and with respect to the number of operating points to investigate. 2 Table 1. MESH SIZES PER COMPUTING DOMAIN Domain Per Passage Total Inlet Casing (ic) 505’000 Impeller (a, b) 61’000 790’000 Diffuser (v) 79’500 824’000 Volute (sc) 417’000 Total 2’536’000 Inlet (I) Outlet (I) Figure 1. COMPUTATIONAL DOMAIN The boundary conditions and interfaces represented in Fig. 1 and 2 are specified in table 2. Table 2. BOUNDARY CONDITIONS Type Location Option Inlet ic (Ī) Constant Flow Rate Q Outlet sc (I) Zero Average Static Pressure Leak. Out (a, b) Flow Rate (0.8% Q per side) Leak. In (ic) Flow Rate, Cu = 0.5 u Walls No Slip Log Wall Functions (y+ = 100) Copyright c © 2007 by ASME