Unsteady Simulations of Impeller - Diffuser Interactions in a Centrifugal Pump

Introduction

Importance of Unsteady Effects in Hydraulic Machines

Fig. 1 - Geometry of a vaned diffuser

The flow in hydraulic machines (turbines, pumps) is inherently unsteady due to the relative motion between the different components of the machine, e.g. impeller blade passing in front of diffuser vanes (Fig. 1) or in front of the tongue of a volute (Fig. 2).

Fig. 2 - Geometry of a volute surrounding a centrifugal pump

Furthermore, in hydraulic machines the flow is fully turbulent, highly three-dimensional and spatially non-uniform. It is thus a veritable challenge to simulate accurately such complex flow fields. The computational resources required for the numerical simulation of unsteady phenomena in a pump or a turbine are large and exceed the resources available in industry for designing new machines. Presently, in the design process, each stage of a hydraulic machine is treated separately and steady simulations are performed for each component. Simulations of the impeller associated with a vaneless diffuser are used for designing the impeller form. The diffuser is designed by assuming that the flow entering it is completely mixed (circumferentially uniform inflow). In centrifugal pumps, the close proximity of the impeller blades and the diffuser vanes causes strong interactions between the components. The very small distance separating the trailing edge of the impeller blade to the leading edge of the diffuser vane, make it doubtful that the flow leaving the impeller has enough time to mix completely before entering the diffuser. Despite the simplifications used in the design process, the efficiencies reached by modern machines are probably very close to the optimum feasible. Furthermore, recent simulations performed on a pump-turbine, in pump mode, showed good agreement with detailed measurements, even if the diffuser vanes were omitted in the numerical simulation. Unsteady effects have probably a prominent importance at off design conditions, especially at part load operating conditions. For instance, stator-rotor interaction phenomena can modify the stability of the operating characteristic. They affect also the formation of rotating stall - fluid zones (cells) of low momentum that are rotating around the machine at a speed lower than the impeller velocity - and they influence the appearance of surge - variation in time of the average mass flow through the machine. In addition, stator-rotor interactions induce noise and vibrations, and if the unsteady pressure forces created by the interaction generate excessive loads, mechanical damage to the machine can occur. Therefore, even if it seems not necessary to account for stator-rotor interaction mechanisms for designing highly efficient machines, to assure a stable operation of the machines for a broad range of flow rates, and to improve the reliability of the machines, unsteady phenomena should be controlled.

Classification of Stator/Rotor Interaction Phenomena

Unsteady phenomena generated by stator/rotor interactions are classically divided into potential effects that propagate upstream and downstream, and wake effects that are convected downstream. Potential effects are geometry driven pressure unsteadiness due to the relative motion of the blades. In the simulation of a two-stage machine, the pressure field can be decomposed approximately into a steady uniform part, a non-uniform part that is steady in the stator frame and a non-uniform part that is steady in the rotor frame. The potential unsteady effects observed in the stator are caused by the motion of the non-uniform pressure field that is steady in the rotor frame. This unsteady pressure observed in the stator is like the unsteady variation recorded by a pressure probe moving uniformly across a non-uniform, steady, pressure field generated by an isolated airfoil. Similarly, the potential effects observed in the rotor are due to the non-uniform pressure field that is steady in the stator frame. Unsteady effects generated by wake/blade interactions are due to the slicing in pieces of the wakes, issued from the front blades, by the downstream blade row. Wakes are created by viscosity, but in axial machines, the dynamic of the wake/blade interaction is controlled mainly by inviscid mechanisms. Therefore, in order to reduce the computational expense of the simulations, a usual practice is to model the wake using specified unsteady inflow boundary condition, and to perform inviscid calculations on the downstream blade row. Potential stator/rotor interaction effects in the upstream blade row have been modeled also by unsteady pressure boundary conditions. (In the downstream blade row potential effects can be modeled by unsteady boundary conditions, but, since in the downstream stage the wake effects are at least as important as potential effects, modeling only potential effects is not very useful; furthermore, the modeling cannot be validated against experimental data.) A proper modeling of either the potential or wake stator/rotor effects by unsteady boundary conditions requires, however, the specification of appropriate boundary flow conditions. This may be difficult when the spacing between the blade rows is small. In this case, unsteady stator/rotor interaction mechanisms can be found only by calculating the coupled stator-rotor flow solution. There are in rotating machines other sources of unsteadiness, e.g. the unsteadiness can be generated by vortex shedding behind a blade, or caused by the vibration of the blades, but these unsteadiness are not linked directly to the relative motion of the stator and rotor blades.

Characteristics of the Flow at the Stage Junction

The flow leaving a rotating machine is fully three-dimensional and presents non-uniformities between the hub and the shroud as well as in the circumferential direction. These non-uniformities result from the secondary flow that develops in the machines. Under the action of the centrifugal and Coriolis forces low momentum fluid accumulates in the shroud-suction side corner. This migration of the low momentum fluid led to the so-called jet-wake model. This model was very popular in the past, but as detailed measurements became available, it appears that the model is too idealized. The flow at the outlet of a centrifugal machine is quite complex and the gradient between the high and low relative velocity regions is not invariably steep. Therefore, in view of the complexity of the outflow, it appears doubtful that a simple model can be used to construct the flow entering the downstream blade row, making the uncoupled unsteady approach (see above) not practical for designing any new rotating machine. In centrifugal pumps, how a vaned diffuser reacts to a non-uniform flow entering it is still debated. There is, however, some indication deduced from experimental measurements as well as from numerical simulations, that showed that at the best efficiency condition, the circumferential non-uniformities are less important than the hub-shroud non-uniformities. It has been observed also that the pressure fluctuations in the diffuser decay very rapidly. This insensitivity of the diffuser to the pulsating flow entering it explains why the design techniques are so successful even without accounting for stage interactions. However, the reasons of this insensitivity are not well understood.

Computational Difficulties for the Stage Interaction Simulations

From a computational point of view, one major difficulty in simulating stator-rotor flows arises because of the relative motion of the stator and rotor blades. The classical solution to this problem is to use several grids that move relative to each other. Typically, stationary grids are employed for partitioning the stator flow domain, and grids rotating with the blades are used in the rotor stage. Specialized boundary treatments are then employed at the grid interfaces to transfer information between them. Two classes of techniques were tried. The grids either slide along their common face, or the grids slide with some overlapping over part of the domain. For both techniques, the information transfer requires some interpolation. The overlapping technique necessitates, however, a three-dimensional interpolation scheme whereas only a two-dimensional scheme is needed for the face sliding technique. In addition, stability problems were reported with the overlapping technique. At midway between unsteady multiple stages sliding block simulation and uncoupled stage simulation, is the multiple stages mixing plane simulation. The underlying philosophy behind the mixing plane procedure is to suppress any dependency on the respective position of the components of the machine. By doing this, steady state computations can be made in the complete machine (the flow in the rotor being calculated in a rotating frame and the flow in the stator is calculated in a stationary frame). The removal of the dependency of the rotor position is done by averaging some quantities in the direction of the rotor motion.

Another difficulty associated with multi-stage simulations is that each stage has a different number of blades. For practical machines, if N_R and N_S are respectively the number of blades of the rotor and of the stator stages, neither N_R/N_S nor N_S/N_R has an integral value. Furthermore, the stator/rotor pitch ratio N_S/N_R is usually large (e.g. 20/9) which implies that the simulation must be undertaken using a large number of blades. (If the stator/rotor pitch ratio is 2/1, simulations could be performed on one rotor channel and two stator channels by applying simple periodic boundary conditions on the lateral boundaries.) Two techniques were developed to allow unsteady simulation to be conducted nevertheless on one stator and one rotor channel, even with large pitch ratio. These are the phase lag method and the time inclining method. In the phase lag method, periodicity at the lateral boundaries is not imposed at the present computing instant but at a previous time. The drawbacks of the technique are that it requires additional storage (the flow field near the boundaries must be stored over one period at least) and that the lagged procedure increases the length of the numerical transient phase. The phase lag technique assumes also periodicity in time which limits the validity of the calculations, since only frequencies multiple of the blade-passing frequency can be accounted for. Vortex shedding at the trailing edge of a blade could not be simulated correctly with this technique, as its frequency is not directly linked to the blade-passing frequency. The time inclining technique avoids this assumption. It has, however, a serious drawback, because the computations are performed in a transformed space-time frame. Thus, the flow quantities at each physical point are known at a different physical time, making the analysis of the unsteady solution very difficult, unless the solution is transformed back in the physical space-time frame. The backward transformation is possible but requires to store the complete unsteady solution. In addition, the forward and backward transformations introduce significant complexities. Therefore, the usual practice is to modify slightly the number of blades of the stages to reduce the stator/rotor pitch ratio. For instance, if 20 vanes are used to guide the flow in a turbine runner comprising 9 blades, by increasing the runner blade number to 10, computations on 2 guide vane channels coupled to 1 runner channel can be performed. If the rescaling of the stator/rotor pitch ratio is small, it is expected that the unsteady solution will not be significantly affected. It was shown, however, that even if the rescaling has little effect on the time-averaged pressure distribution, it may influence markedly the temporal variation of the flow quantities. In addition, as mentioned above, unsteady phenomena have mainly a significant importance at low mass flow rates. For these cases, the flow has the tendency to be different in the various channels (appearance of stalled cells). In such a situation, only the simulation of the complete machine or at least of a large number of channels can give correct flow predictions. Thus, none of the above simplification techniques are practical for simulating the interesting low mass flow rate cases.

The CTI Project

To investigate further the mechanisms involved in stator/rotor interactions, a research project has been established in collaboration with the Sulzer company under the auspices of the Commission pour la Technologie et l'Innovation (CTI). The flow inside a hydraulic centrifugal pump has been investigated, with the middle stage of a multi-stage pump chosen for this purpose. The middle stage is composed of an impeller having 7 blades and a diffuser having 13 vanes (Fig. 3). At nominal operating condition, the mass flow through the pump is Q = 70kg/s with an impeller rotating at w = 1000 rpm. The specific speed of the pump is n_q = 33. Detailed flow measurements using Laser Particle Tracking Velocimetry and Laser Doppler Anemometry have been performed at Sulzer Innotec [1] to improve the understanding of the interaction phenomena and to build a data base for validating the numerical flow simulations. Steady numerical simulations were performed on the different elements of the pump [2] and the unsteady flow in the vaned diffuser calculated using the measured unsteady profiles as inlet boundary conditions [3]. At the Fluid Mechanics Laboratory of the Institute for Hydraulic Machines and Fluid Mechanics (IMHEF) a computer program [4] has been developed for simulating unsteady phenomena generated by stator/rotor interactions.

Fig. 3 - Geometry of the Sulzer pump investigated

Characteristics of the Flow Computed and Objectives of the Investigations

Three-dimensional simulations of the Sulzer pump were undertaken, however, due to the complexity of the flow to be analyzed, it was decided that the research effort should be concentrated first on the response of the diffuser to a non-uniform, pulsating inlet flow. As circumferential non-uniformities were first investigated, only two-dimensional simulations were conducted. To reduce the computational cost, the number of diffuser vanes was raised to 14 in order to enable simulations to be performed on one impeller and two diffuser channels. Since the stator/rotor pitch ratio has been altered and since the hub-shroud variations are not accounted for in the two-dimensional simulations, it should not be expected that the computed solution represents accurately the real three-dimensional pump flow. Moreover, the inlet flow conditions used in the simulations make the flow solution of the two-dimensional pump very peculiar (Fig. 4); most of the fluid in the impeller is flowing in a jet and a massive separation is present in the diffuser. The objective of this work was not to simulate a real flow, but to study stator-rotor interaction flows by using the full potential of Computational Fluid Dynamics (CFD) for analyzing the computed flow. (A major advantage of CFD is that the numerical pump can be exhaustively instrumented.) The jet structure in the impeller observed in the numerical flow is almost ideal, because it gives a flow leaving the impeller with a significant non-uniformity in the circumferential direction. Furthermore, this jet flow can be perceived as a model of a real 3D flow leaving a centrifugal impeller with the jet-wake structure. The separation in the diffuser also can be representative of a 3D flow. The thick boundary layers growing on the walls may produce a mismatch in the vane incidence flow angle and therefore induce a separation, even at nominal flow rate. Additionally, it is interesting to study the influence of the unsteady forcing generated by the rotation of the impeller on the stability of a separated flow in the diffuser.

Fig. 4 - Velocity modulus in the pump (relative velocity in the impeller and absolute velocity in the diffuser)

Numerical Procedure Employed for the Simulation

The stator-rotor simulations were performed using the computer program sagarmatha developed within the institute. This program solves the unsteady Reynolds-averaged Navier-Stokes equations for an incompressible fluid on 3D block-structured meshes [4]. The equations are discretized using a cell-centered finite-volume method. The artificial compressibility technique is used for coupling the incompressible velocity field to the pressure field. A high-order upwind spatial discretization scheme based on the approximate Riemann solver of Roe is employed for approximating the advection terms. The diffusion terms are discretized using a centered approximation. A dual time step procedure with the implicit two-stage Runge-Kutta scheme recommended in [5] is used for integrating in time the unsteady Navier-Stokes equations. At each time step, a non-linear system resembling the equations for stationary flow is solved using an ADI method. A detailed description of the numerical techniques employed in the program is given in the sagarmatha user's guide [4].

Steady simulations were conducted using a mixing plane interface condition at the stator/rotor block boundary and unsteady simulations were made using a face sliding block technique. In the latter case, the flow equations are solved in a fixed frame in the diffuser and in a rotating frame in the impeller. The sliding technique consists to move the impeller mesh at each time step and to calculate the cell connections (patches) between the impeller outlet and the diffuser inlet face meshes. The flux at the block interface is then obtained by adding the flux contribution of each patch. This flux is calculated using techniques similar to the one employed for a cell face inside a block mesh. The mixing plane technique was derived such that it has a minimal effect on a usual flux evaluation and any dependence on the relative position between the impeller and the diffuser is suppressed. This is achieved by averaging circumferentially any impeller quantity required in the flux evaluation, at the impeller/diffuser block boundary, for updating the flow in the diffuser. Similarly, diffuser quantities are circumferentially averaged when the impeller flow is updated. For all the simulations, the Baldwin-Lomax turbulence model with wall functions was used to estimate the Reynolds stresses.

Results and Discussions

An unsteady simulation of the fluid flowing in the complete pump (7 impeller blades and 14 diffuser vanes) has been conducted. This simulation was used to verify that the flow in every impeller and every two diffuser channels is the same. Since the computed flow presents effectively a 2p/7 circumferential periodicity (Fig. 5), the remaining sliding simulations were conducted on one impeller and two diffuser channels. For these simulations 100 time steps were used for representing the motion of an impeller blade across two diffuser channels q = 2p/7.

Since only two-dimensional simulations have been performed in this study, using a rather coarse computational mesh (approximately 35,000 grid points for the complete pump), it was possible to perform the unsteady simulations on a workstation within a reasonable amount of time. Using a Hewlett Packard 9000/755 workstation, an unsteady simulation could be completed overnight.

Fig. 5 - Instantaneous pressure contours obtained from an unsteady simulation of the complete pump

Animations of the impeller-diffuser interaction have been made, using the run-time visualization tool TPview [7] developed at the EPFL. This tool enables the transfer of data produced by the simulation program to the commercial Tecplot rendering package. All of the unsteady flow images reproduced in this paper have been produced using TPview in combination with Tecplot. Some of the animations can be viewed on WWW at the address http://imhefwww.epfl.ch/lmf/animation/pump. These include the evolution of the pressure field, the evolution of the absolute and relative velocity norms and the variation of unsteady velocity (difference between the instantaneous velocity and the time-averaged velocity). A selection of images extracted from the animations are presented here. The evolution of the norm of the flow velocity (measured in the stationary frame) is given in Fig. 6. This figure shows colored maps of the velocity norm and lines of constant pressure. The major features of the interaction are apparent in Fig. 6. Periodically the diffuser leading edge cuts the jet fluid leaving the impeller. (The jet finger grows from Figs 6a to 6c. It is sliced in Fig. 6d. Finally, the flow condition of the Fig. 6a is recovered, on the next diffuser channel, in Fig. 6e.) At the trailing edge of the impeller blade, a small vortex shedding can be observed as well. One can note also that the flow in the diffuser, particularly the back-flow region, is not significantly affected by the interaction.

Fig. 6 - Instantaneous velocity modulus in the pump for different impeller blade positions

Fig. 7 - Instantaneous pressure contours in the pump for different impeller blade positions

The time evolution of the pressure is given in Fig. 7. In the simulation a constant ambient pressure was imposed at the outlet of the diffuser. Therefore, the outlet pressure is steady and variations are seen at the pump inlet. In a small band around the vaneless gap part of the pump, complex pressure structures can be observed. These pressure structures are well correlated with the unsteady part of the velocity norm, measured in the relative frame (Fig. 11). Outside this band, the pressure field is smoother and it can be observed that the pressure unsteadiness in the impeller is well synchronized. These global pressure variations are due to potential effects and it has been verified that they can be reproduced by the prescription of unsteady boundary conditions at the outlet of the impeller. It can also be noted that in the diffuser the pressure is changing with time only in the semi-vaneless space. Inside the diffuser, the pressure field is almost steady.

Fig. 8 - Complete unsteady pump simulation using mixing plane - initial flow field

The time average of the unsteady solution has been calculated. When this time-averaged flow field is compared with the steady flow field obtained from a computation of the pump using a mixing plane condition to couple the rotor to the stator, a surprising result is found. The solution in which both diffuser channels are performing identically is not stable! The stable solution is such that the flow in the diffuser channels is different; in one diffuser channel the flow is almost blocked, and in the other channel it is fully attached. This non-periodic solution was found with steady mixing plane simulation of the pump (1 impeller and 2 diffuser channels), with steady simulation of the diffuser alone, using circumferentially uniform inflow, and with unsteady mixing plane solution of the full pump. In this latter case, visualization of the unsteady flow shows clearly how the periodic solution destabilizes slowly and how the non-periodic solution forms (Figs 8 and 9). On the other hand, when sliding mesh simulation and when diffuser simulation with unsteady inlet flow were performed, the time-averaged solution has always been found to be identical in both diffuser channels.

Fig. 9 - Complete unsteady pump simulation using mixing plane - flow field at a later time (3 impeller revolutions later)

To produce a fair comparison with the time-averaged solution, the remaining steady simulations have been carried out by imposing a 2p/14 periodicity at the lateral boundaries of the diffuser. When this new steady mixing plane solution is compared to the time-averaged unsteady solution, small differences are observed. The largest difference is at the stator-rotor interface and near the diffuser vane leading edge. However, these differences never exceed 10%.

Since the computations are performed in a rotating frame in the impeller and in a fixed frame in the diffuser, it is natural (and easier) to calculate the time-averaged solution in these frames. With this procedure the time-averaged solution is discontinuous across the impeller-diffuser boundary. In order to calculate averaged solutions that are continuous across the sliding boundary, it is necessary to perform two averages; one in the rotating frame and one in the fixed frame. The averages are calculated from

(1)

where

• X is the location of the point (in the fixed or rotating frame),
• H(X,t) is a function having two values; H(X,t) = 1 when the point is in the fluid and H(X,t) = 0 when it is in the blade.

In addition to provide a continuous averaged solution, these averages have the advantage to enable the comparison, in the diffuser, between the solution in a pump with vaned and vaneless diffuser. (Both solutions are given in a frame moving with the impeller.) This comparison shows that the presence of the diffuser vanes affects only slightly the flow evolution in the vaneless gap of the pump [6]. Inside the diffuser, the velocity variations are smaller with vanes than without. This comparison invalidates the assumption that the insensitivity of the diffuser to the pulsating flow leaving the impeller, is due to the rapid mixing of the flow in the vaneless gap in front of the diffuser. The averages allow to quantify also the importance of potential interaction effects in the impeller. If the flow in the impeller is steady in the frame rotating with the impeller, a time average performed in a stationary frame will give a solution that is uniform circumferentially. (The time averaged solution is, in this case, identical to the circumferentially averaged solution.) Therefore, any non-uniformity in the circumferential direction is a measure of unsteadiness. This characteristic of the averaged solution (averaging performed in the stationary frame) of the flow in the impeller, was used to verify that the unsteadiness observed in the impeller are due to potential effects. This was effectively shown in [6] by comparing the averaged solution to an Euler simulation on a segment of disk (r [r₁, r₂] and q [0, 2p/7] with r₁ and r₂ respectively the impeller inlet and outlet radii). The boundary conditions used on the disk simulation were: at r₁ a uniform inlet flow was prescribed with the same mass flow as for the pump, at r₂ the time-averaged solution was imposed, and periodic conditions were specified on the lateral boundaries.

Fig. 10 - Evolution of the unsteady component of the velocity modulus - stationary reference frame

With the averages defined above, it is possible to visualize the evolution of the unsteady component of the flow quantities. Comparing Figs 10 and 11, it is obvious that the plots of the unsteady velocity seen by an observer sitting in the stationary or in the rotating frame are quite different. In the stationary frame (Fig. 10), layers of high and low unsteady velocity are piling in the diffuser. These layers are generated by, respectively, the jet and the wake issued at the trailing edge of the impeller. Examining the time evolution from Fig. 10a to Fig. 10d, it can be observed how these layers are cut by the diffuser vane leading edge. From the animation, it appears also clearly that a significant part of each layer is circling around the pump. An observer attached to the impeller sees a completely different unsteady velocity (Fig.11). The unsteady map is composed of spots of high and low velocities that are moving in phase with the diffuser vanes. The spots are formed behind the impeller blade trailing edge and grow while reaching the next blade. These spots are created by the lateral motion of the jet before and after it is sliced by the diffuser vane. A high unsteady velocity is created when the jet moves in the same direction as the mean flow. The low unsteady velocity is generated when the jet moves back to its initial position. It is interesting to note that the constant pressure lines are well correlated with the unsteady velocity measured in the rotating frame (Fig. 11). From the figure it is visible that non-zero unsteady velocities are also found in the diffuser. These values are due to the circumferential non-uniformity of the solution in the diffuser. (When measured in the rotating frame, these non-uniformities are recorded as unsteady signals.) Comparing the unsteady velocity maps for different blade positions, it can be observed that, in the diffuser, the maps have always the same shape. This is another indication that the flow in the diffuser is almost steady.

Fig. 11 - Evolution of the unsteady component of the velocity modulus - rotating reference frame

The ability of the time-averaged solution to encode an unsteady signal (see above) can be an interesting feature. Indeed, one of the difficulties of unsteady flows is the large amount of data that are produced. For a routine usage, it is not possible to store a complete unsteady solution. Therefore, when unsteady flows are simulated, it is preferable to know in advance what to look for in order to avoid having to perform the simulation several times. If the unsteady part encoded in the special average (Eq. 1) is sufficient, the unsteady solution can be manipulated like a steady state solution.

Unsteady pressure and velocity signals have been recorded at different positions in the pump [6]. These signals give a quantitative image of the unsteadiness generated by the impeller-diffuser interaction. However, without the aide of the unsteady maps, these signals are very difficult to analyze (it is almost impossible to infer any mechanism involved in the interaction solely from unsteady signals). The origin of pressure peaks and valleys could be traced only by analyzing the unsteady signals in parallel to the animations. The comparison of the unsteady signals obtained from the stator-rotor simulation with simulations of the impeller and diffuser coupled with unsteady boundary conditions, showed that in the impeller the two signals agree well when the time-averaged flow is used to prescribe the boundary condition at the outlet of the impeller. In the diffuser the agreement is less satisfactory, unsteady pressure and velocity can be reproduced only approximately by the prescription of unsteady boundary conditions.

Conclusions

Unsteady, sliding block computations in a centrifugal pump have been performed and compared with simplified simulations. From the different simulations conducted the following was found.

• The flow in the diffuser obtained from a sliding block simulation is the same for each channel, whereas from a mixing plane computation it tends to be different.
• When periodicity in the diffuser is controlled, the mixing plane and time-averaged solutions differ by only a few percent.
• The presence of the diffuser enhances only slightly the mixing of the wake leaving the impeller.
• The unsteadiness generated in the impeller is due to potential effects.
• Unsteady signals in the diffuser can be reproduced only approximately using unsteady inlet conditions.

A special time averaging procedure has been introduced. It allows to visualize, in a multiple stages simulation, the evolution of the unsteady part of any flow quantity. This new time-average has also the ability to encode some portion of unsteadiness and therefore could be useful to reduce the amount of data produced by unsteady simulations.

Acknowledgements

This work received financial support from the Commission pour la Technologie et l'Innovation and Sulzer Brothers S.A. under Contract Number 3062.1. The author would also like to thank M. Casey, K. Eisele and F. Muggli from Sulzer Innotec for their kind support during the course of this work.

References

• [1] M.V. Casey, M. Eisele, Z. Zhang, J. Gülich and A. Schachenmann, Flow analysis in a pump diffuser, part 1: LDA and PTV measurements of the unsteady flow, ASME Paper, FED Summer Meeting, Symposium on Laser Anemometry, 1995.
  
• [2] M.V. Casey, M. Eisele, F.A. Muggli, J. Gülich and A. Schachenmann, Flow analysis in a pump diffuser, part 2: Validation of a CFD code for steady flow, ASME Paper, FED Summer Meeting, Symposium on Laser Anemometry, 1995.
  
• [3] F.A. Muggli, D. Wiss, K. Eisele, Z. Zhang, M.A. Casey and P. Galpin, Unsteady flow in the vaned diffuser of a medium specific speed pump, ASME Paper, 96-GT-157, 1996.
  
• [4] Y.P. Marx, sagarmatha User's Guide, version 4, IMHEF Technical Report T-96-34, 1996.
  
• [5] Y.P. Marx,Time integration schemes for the unsteady incompressible Navier-Stokes equations, Journal of Computational Physics, 112, 182-209, 1994.
  
• [6] Y.P. Marx, Investigation of stator-rotor interaction phenomena in a centrifugal pump, In 8th International Symposium on Unsteady Aerodynamics and Aeroelasticity of Turbomachines, Stockholm, 1997.
  
• [7] S. Williams, M.L. Sawley and D. Cobut, On-line visualization for scientific applications on the T3D, EPFL Supercomputing Review, 7, 45-50, 1995.

refer to contents	©EPFL-SCR # 9 - 1997
	your comments