Improved Prediction of Pump Performance Through the Rotation–Curvature Correction—An Experimental and Numerical Study of a Low-Specific-Speed Helico-Axial Compression Cell in Series

Accurate numerical analysis through computational fluid dynamics (CFD) applied to turbomachinery is fraught with challenges. The simulations often involve large variations in spatial and temporal scales, leading to strict discretization requirements. Secondary flows and the inherent unsteadiness related to rotor–stator interactions add layers of complexity to the modeling. Most turbomachinery flows are highly turbulent, and turbulence can play a key role in the performance and stability of the machine.

Evolving simulation strategies and turbulence modeling in turbomachinery CFD was reviewed by Tucker [1] and Tyacke et al. [2]. Eddy-resolving simulations are becoming more customary as both the available computational resources and requirements for high-fidelity results increase. Implementing such techniques for high-Reynolds number flows is, however, costly, and most of the simulations conducted in the turbomachinery industry are still relying on steady or unsteady Reynolds-averaged Navier–Stokes (RANS) modeling involving single or two-equation eddy-viscosity turbulence models. One shortcoming in the most widely used eddy-viscosity turbulence models, relevant to turbomachinery applications, is that they are not affected by system rotation and streamline curvature. Different model extensions have been proposed over the years, in an effort to sensitize the turbulence models to such effects.

Helico-axial rotodynamic pumps are no exception to the rule when it comes to a complex internal flow field. Small clearances, secondary flows, and rotor–stator interactions are all common in these pumps, used to boost the production of unprocessed hydrocarbons in the energy sector [3]. As the pumps are designed to handle any fractions of gas and liquid, it is obvious that the introduction of multiphase flow adds even one more layer of complexity to the necessary performance and stability assessments performed in the pump design process. Recent development toward utilization of subsea boosting in oil and gas production at increasing water depths, and with longer tiebacks, means that the pumps must generate more head to overcome losses and the pressure exerted by the fluid column in the production system [4,5]. This drives the multiphase pump design toward higher numbers of stages, with specific speeds lower than in most earlier applications. During normal operation, the high pressure difference across the pump implies a high compression ratio for the gas phase. Additionally, the outlet pressure often exceeds the production fluid's bubblepoint pressure. Therefore, downstream stages within the pump are in many cases operating with gas volume fractions close to 0.

Computational fluid dynamics studies of helico-axial compression cells have been conducted for more than 30 years [6], but most of the related publications have emerged in more recent years. Several studies have focused mainly on modeling of phase distribution and the performance degradation when multiphase flow is introduced in the pump [7,8]. Other publications investigate the impact of geometric variations on performance and flow field properties; e.g., related to the impeller tip clearance [9–11]. For turbulence modeling, most studies have employed the two-equation shear stress transport (SST) model in the simulations. Shi et al. [12] compared the impact of different turbulence models on head and efficiency through steady simulations involving wall functions. No significant model impact on performance was found, but the SST model exhibited the best agreement with experimental data for the internal flow field. Regarding the effect of turbulence model sensitization to system rotation and streamline curvature, no references were found for helico-axial geometries, and it can be argued that this topic is not well-covered for axial turbomachinery applications in general. Liu et al. [13] investigated the effect of including a rotation–curvature correction in the SST model for an axial compressor, where an impact on the predicted performance was found at part-load operation. At these conditions, however, the simplified steady simulation approach may have been the dominant factor leading to the discrepancy between simulated and experimental performance.

In this paper, we detail an experimental and numerical study of a low-specific-speed helico-axial compression cell in series. The effect of applying a rotation–curvature correction to the turbulence model is investigated, and the model is calibrated to establish a new formulation that improves the simulation results. The modeling technique can form the basis for future applications to other turbomachine designs or operating conditions, including multiphase operation.

An experimental facility with multiphase flow capabilities was used to characterize the hydraulic performance of a helico-axial compression cell in series. Results from single phase testing with liquid fresh water are studied in the present work.

The compression cells were installed in a pump test rig that was incorporated in a flow loop. A simplified process flow diagram can be found in Fig. 1, where instruments marked with p, T, and dp indicate measurements of pressure, temperature, and differential pressure, respectively. Liquid is drawn from a 28-m³ separator and is routed through a V-cone flowmeter before it enters the pump test rig. Two different flowmeter sizes were used for the present test campaign, to ensure adequate measurement accuracy for all tested flow rates. See Table 1 for an overview of the instrumentation.

Downstream of the pump test rig, the pressure was dissipated in a choke valve before the fluid entered the separator again. The choke valve was used to regulate the flow rate in the loop when the pump was in operation. Figure 2(a) shows the pump test rig installed in the flow loop with the 6-in. inlet piping at the left and the outlet piping at the right and upper part of the picture. The flexible hose attached to the pump suction side is a gas supply line, not used in the present paper.

The pump test rig comprised a horizontally oriented pump unit, a gear box, and an electric motor. A dynamic torque transmitter was installed between the pump unit and the gear box to measure the pump's shaft power. The electric motor was connected to a variable-frequency drive to enable variable pump speed throughout the test.

A double ceramic tilting pad thrust bearing provided axial support for the pump unit's rotor, with a design load capacity of 170 kN. Lateral support was provided by two journal bearings. All bearings were lubricated by water through external high-pressure circuits that were interfacing the process fluid through teeth-on-stator labyrinth seals.

Three helico-axial compression cells were installed in the pump unit, with a set of inlet guide vanes upstream of the first impeller. The fluid pressure was measured directly upstream and downstream of each impeller, as well as at the outlet of the last diffuser. Absolute pressure sensors were mounted to 1/4 in. tee fittings on the pump casing, exposing them to the relevant locations through ø3 mm holes across the shroud. The instruments can be seen in a vertical position below the tees that emerge horizontally from the pump unit casing in Fig. 2(b).

The tested helico-axial compression cell is an axially compact design adapted for low-specific-speed applications, which typically involve relatively high pump head and low flow rates. Figure 3 illustrates the design with the characteristic overlapping impeller blades suitable for multiphase flows [6,14], as well as the relatively short diffuser vanes that act to straighten the flow before the downstream impeller. The main geometric properties can be found in Table 2. Note that a cavity is formed between the diffuser and the shaft, which includes a wear ring (interstage seal) with a nominal radial clearance of 0.45 mm. The impellers and diffusers were machined in carbon steel (EN 10025 S355J2), with a specified maximum surface roughness of Ra = 1.6 μm. A downscaled version of the cell was previously tested for flow visualization purposes by Gundersen et al. [15].

An inherent feature of the open impeller design is the small clearance between the blade tip and the stationary shroud formed by the pump casing. All cells have the same nominal clearance. However, variations in impeller and shroud diameters within the manufacturing tolerances can lead to slight differences in the actual radial tip clearance between each compression cell. A larger tip clearance results in increased tip leakage flow (TLF) from the pressure side to the suction side of the blade and affects the performance of the cell [16–18]. Table 3 shows the relative radial tip clearances $s/b1$ found by dimensional inspection of the components prior to assembly. s is the radial tip clearance, and $b1$ is the impeller blade height at the inlet.

The pump test rig was operated with tap water as the process fluid. Here, we present 86 steady pump operating conditions at different pump speeds up to 4600 rpm. Each test point is based on average values from steady operation over a period of 60 s. The pump inlet pressure and temperature were for most of the data maintained near 9 bara and 30 °C. However, the inlet pressure was varied during the test campaign to facilitate proceeding multiphase operation with different liquid/gas density ratios. Additionally, some variations occurred for practical reasons, such as varying available cooling power and increasing pressure loss between the separator and pump at the highest flow rates. The full ranges of inlet pressure and temperature for the data points are 6.8 to 12.4 bara and 21 to 59 °C, respectively.

is $1.0×107$ to $5.5×107$⁠. $Ωrot$ is the shaft angular frequency, $RT$ is the impeller tip radius, $ρ$ is the fluid density, and $μ$ is the fluid dynamic viscosity.

In the present paper, we focus on results for the second compression cell only. The upstream and downstream cells form the appropriate boundary conditions with respect to a cell operating in series. The pressure sensors at the inlet and outlet of the second cell have the same relative position with regard to the adjacent geometry and will therefore represent the pressure difference across the cell properly. For the pressure difference over the individual impeller and diffuser, however, the relative position of the sensors will naturally not be identical, and the static pressure measurements may be affected by the differing local circumferential fluid velocity or other secondary flow phenomena, expected near the shroud [15]. As the measured pressure difference across the diffuser was small (below 0.5 bar for the majority of operating points), the relative uncertainty caused by positioning of the sensors can be significant, and the results are not further discussed here.

where Q is the actual volumetric flow rate, and $A1$ is the cross-sectional area of the impeller inlet. The tip-speed Reynolds number $ReT$ is given for each test point by a grayscale.

for each test point. T is the torque, g is the gravitational constant, and H is the head, $H=Δp/ρg$⁠. Note that the uncertainty of the efficiency is relatively large due to the modeling of bearing losses and subtraction of torque related to the two other compression cells. Thrust-bearing losses were estimated based on a model provided by the bearing manufacturer, accounting for thrust and operating speed. Radial-bearing losses were approximated through a Couette flow assumption, first proposed by Petrov [19]. Torque related to the first and last compression cells are subtracted based on their respective fractions of the pressure difference across the pump unit. Error bars for $ψ$⁠, $ϕ$⁠, and $η$ are included in proceeding figures that compare experimental results with numerical analysis results. The error bars correspond to a 95% confidence interval (CI) found through propagation of systematic error, assuming independent variables. The relative errors of 10% and 4% were used for the bearing losses and compression cell torque fraction, respectively.

The nondimensional test results are well-aligned and exhibit clear performance characteristics. For this geometry, any tip-speed Reynolds number dependence would predominantly be evident for the efficiency and the head-flow characteristic at high relative flow rates [17]. From Figs. 4 and 5, no significant dependence is observed for the present range of $ReT$⁠. This indicates that the magnitude of $ReT$ is sufficiently high such that the impact on performance in this range is negligible compared to other factors such as systematic and random measurement error.

Figure 5 indicates a best efficiency point (BEP) for the compression cell in series at $N≈0.7$⁠, which is significantly lower than the typical design-specific speed for conventional axial flow pumps, $N>3$ [20]. A centrifugal or mixed flow impeller would normally achieve the highest efficiency at the present specific speed of 0.7, but those designs would be less tolerant to any multiphase operating conditions. For an open impeller in general, the tip leakage flow rate increases with head and can, depending on the tip clearance, become significant compared to the net flow Q at these low specific speeds. Consequently, leakage losses within the impeller can become significant. The maximum efficiency found during testing is somewhat lower than what can be expected for an axial flow pump with a high design-specific speed [20]. Both leakage losses related to the tip clearance, and internal losses related to local recirculation zones and narrow flow channels, can contribute to this variation in efficiency.

Numerical simulations were conducted with the commercially available CFD solver cfx (ANSYS, Inc., Canonsburg, PA), release 2021 R1 and 2021 R2. The aim of the numerical study was to reproduce the experimental results for head and efficiency at varying relative flow rates through CFD analysis involving eddy viscosity turbulence models. A curvature-correction is calibrated to achieve a turbulence model formulation that leads to accurate performance results. This is done with a view to later apply the simulation methodology to new operating conditions or in the development of new designs.

Figure 6(a) shows the simulated geometry that comprises the full circumference of a compression cell. Blade root fillets toward the hub were omitted. The relative impeller radial tip clearance $s/b1$ was 1.6%.

The geometry was divided into four domains, as illustrated in Fig. 6(b). The multiple frames of reference approach was used together with general grid interfaces between the domains to model rotation. Frame change models (“frozen rotor” for steady-state and “transient rotor–stator” for transient simulations) were applied at interfaces between rotating and stationary domains. A no-slip condition and the relevant relative velocities were specified at the walls. The tip-speed Reynolds number in the CFD simulations was $ReT=1.3×107$⁠.

The inlet and outlet boundaries of the cell were specified with a translational periodicity condition to model streamwise periodicity [21] and thus the cell's performance in series. Velocity components are then periodic, and the pressure is decomposed into the periodic pressure field and a linear term related to the pressure difference across the boundaries, i.e., $Δp$⁠. The linear term results in a force term added to the momentum equations, effectively driving the flow. For each flow coefficient of interest, a corresponding target mass flow rate was specified across the periodic interface. The solver seeks and achieves the specified mass flow rate by modifying the pressure difference across the interface for each time-step.

A streamwise periodic simulation setup implies “fully developed” flow conditions in the simulations. With regards to comparison with experimental results, an initial steady-state CFD simulation was conducted to assess the inlet conditions of the second impeller in the experimental setup. The simulation geometry comprised three circumferentially complete compression cells, as well as an inlet and outlet domain. The inlet domain included the axial guide vanes upstream of the first impeller. Note that the cavity domain was only included for the second cell. The flow rate corresponded to BEP and the standard SST turbulence model was used. A low turbulence intensity of 1% was specified at the inlet boundary, such that the turbulence kinetic energy was $kin=(3/2)(0.01U)2$⁠. Figure 7 shows the development of k throughout the simulated geometry. Note that the streamwise location is normalized for each component in the figure; the inlet and outlet domains were about 6 and 13 times longer axially than one impeller domain, respectively. We see that turbulence levels in the first impeller are initially lower than in the second impeller, but at the outlet, the level is similar to that of the outlet in the second and third impeller. Turbulence levels within all diffusers are similar, and the first diffuser appears to establish inlet conditions for the second impeller that corresponds well with the conditions for the third impeller. Turbulence levels throughout the second and third impeller are very similar. This suggests that it is reasonable to compare experimental results for the second compression cell with results from the streamwise periodic simulation setup.

The impeller and diffuser passages were meshed in ansysturbogrid (ANSYS, Inc., Canonsburg, PA), while the cavity domain was meshed in ansysmeshing (ANSYS, Inc., Canonsburg, PA). A mesh sensitivity study involving a transient setup operating at about 85% relative flow revealed mesh independence for the head coefficient with an average first-layer $y+$ below $≈4$⁠. The mesh used in the simulations is, however, additionally refined such that the average $y+$ is around 1. This ensures that boundary layers, and the flow within the tip clearance, are resolved, see Fig. 8.

The element size in the bulk of the flow is also based on mesh independence for $ψ$ found through several transient simulations with a fixed first-element height at the walls (average $y+≈4$⁠), see Fig. 8(c). The given number of elements is the total for one compression cell, not including the cavity domain. Table 4 provides details about the mesh used in the numerical study, which in total consisted of 99.7% hexahedrons. The remaining elements were prisms. Illustrations of the mesh can be seen in Fig. 9.

The coupled cfx solver was used, where the steady or unsteady RANS equations were discretized using an element-based finite volume method [22]. Following the implicit discretization of the governing equations, the resulting linear equations were solved using an algebraic multigrid method [23]. The transport equations included source terms to account for Coriolis and centrifugal forces in rotating domains. The fluid was modeled as incompressible and with constant properties.

Steady-state simulations were solved with a timescale (false time-step) of approximately $4.77×10−4$ s. For a sufficiently fine mesh, a steady solution where the rms residuals diminished was not found. Instead, the flow field was locally unsteady, and the solution fluctuated slightly. This was anticipated, considering the unsteady flow field behavior observed by flow visualization of the downscaled compression cell [15]. Consequently, steady-state results for pressure, torque, and flow rate were monitored for each iteration and finally evaluated as a moving average over the most recent iterations. Normally, the steady-state simulations were run for 2000 iterations, and the averaged results were based on the last 1000 iterations.

Transient simulations used the respective steady-state simulation results as initial conditions. A time-step corresponding to 20 iterations per vane pass was used, corresponding to 460 iterations per revolution, or approximately $6.52×10−5$ s. By monitoring $Δp$⁠, mass flow rate, and other variables, it was found that most operating conditions required solving two revolutions before the flow field started to exhibit periodic behavior. The simulations were run for a minimum of five revolutions in total, and the result variables were evaluated as a running average over a minimum of three revolutions of periodic behavior.

To close the RANS equations, the widely used SST turbulence model was employed. The SST model includes a blending function that switches between a k–$ε$ and k–$ω$ turbulence model in the freestream and near-wall region, respectively. A complete formulation of the SST model is given by Menter et al. [24]. The model performs well for flows involving adverse pressure gradients and separation and is often applied in turbomachinery simulations [1]. Nevertheless, it does not account for the effects of streamline curvature or system rotation, both typical features of turbomachinery flows.

Smirnov and Menter [25] proposed a sensitization of the SST model to such features. The model is denoted as the SST-CC model and introduces a rotation–curvature correction that enhances or dampens the turbulence kinetic energy production term $P˜k$⁠. The model is based on a proposed sensitization [26] of the Spalart–Allmaras turbulence model [27].

that is multiplied with the turbulence production terms $P˜k$ in the transport equations for k and $ω$⁠.

Here, $μt$ is the eddy viscosity, and $Cμ$⁠, $σk$⁠, $Cω1$⁠, $Cω2$⁠, and $σω$ are constants that are blended by the function $F1$⁠, which is 1 inside boundary layers and 0 in the freestream. Both the standard SST model and the SST-CC turbulence model with different values of $Cscale$ were used in the simulations. Results are shown together with experimental data in Sec. 4.

Numerical simulations at 11 different flow rates were performed for comparison with the full range of operating conditions from the experimental results. Error bars corresponding to a 95% confidence interval are included for the experimental data. Figure 10 shows the head coefficient at different flow coefficients with the standard SST turbulence model.

Both steady-state and transient results show good agreement with experimental data at the three highest flow coefficients. Near BEP (⁠$ϕ≈0.07$⁠), however, steady-state results yield a deficit in head, while the transient results match the experimental data very well. The steady-state head coefficient recovers at lower flow coefficients, while transient results are too optimistic. Neither steady-state nor transient SST simulations are thus capable of reproducing the head-flow characteristic.

Steady simulations employing the frozen rotor frame change model are sensitive to the relative position of the rotor and stator. The full circumferential geometry in the present setup can help to reduce this sensitivity, but a steady simulation will nevertheless be incapable of modeling the impact of unsteady flow features. Regions of separated flow and vortices, emerging from rotor–stator interactions and the TLF, are expected to be prominent in the present compression cell [15]. Unsteady RANS simulations can, however, resolve such coherent structures with length scales similar to the characteristics of the geometry. Therefore, only the unsteady simulation results are used to investigate whether the curvature correction model can lead to an improved performance prediction, while potentially also exhibiting the dominant dynamics of the flow field.

Figure 11 shows results from transient simulations with the SST and SST-CC turbulence models. We recognize the good match for the SST model near BEP (⁠$ϕ=0.068$⁠) and at higher relative flow rates. For relative flow rates below BEP; i.e., part-load operation, the head coefficient is overpredicted. Indeed, streamline curvature related to secondary flows and rotational effects are expected to increase with decreasing flow coefficients. For the SST-CC model simulations, the value of $Cscale$ was varied in the range from 1 to 8 for the operational point $ϕ=0.043$⁠, where the discrepancy with the experimental results was relatively large for the SST model. Results from simulations with different $Cscale$ are denoted by the respective value after “CC” in the figure.

It is seen that the standard SST-CC model; i.e., CC1, had only an insignificant impact on the head coefficient relative to the SST model. Essentially, the same result was obtained for $Cscale=2$⁠, while CC4 showed a discernable drop in head coefficient. Further increasing $Cscale$ to 8 leads to a head coefficient that matched the experimental results. This scaling coefficient corresponds to a maximum value of 3 for the $P˜k$ multiplier $fr2$ in Eqs. (17) and (18). Employing the SST-CC8 model also at the other flow coefficients resulted in a very good match with experimental results for the full range where the head-flow curve slope is negative. At the three lowest flow coefficients analyzed, the performance results were very similar to the standard SST model results. Relative errors of the head coefficient are given in Table 5, where the experimental results have been evaluated through two best-fit second-order polynomials. For the range from $ϕ/ϕBEP$ = 50% to 126%, the absolute rms error of $ψ$ is 0.020 for SST and 0.003 for SST-CC8.

For completeness, the steady-state results with the SST-CC8 model are also shown in Fig. 12. Contrary to the transient simulations, the SST-CC8 model yielded somewhat higher head coefficients than the SST model at part-load conditions. In total, the agreement with experimental data is similar to that of the SST model.

The efficiency $η$ at different flow coefficients is compared in Fig. 13. Both models exhibit a characteristic that is comparable with experimental data. The SST-CC8 model generally exhibits a slightly lower efficiency than the SST model, resulting in a better match.

Here, we inspect selected details of the simulation results in an effort to give insight into why the different models yield a different performance for the compression cell. Note that color bars in the proceeding figures may not include the maximum and minimum values in the domain, but are rather adjusted to improve interpretation.

Starting with the transient results at part-load conditions, $ϕ=0.043$ or $ϕ/ϕBEP=63%$⁠, the time-and-area-averaged relative static pressure difference across the impeller and diffuser is illustrated for the different models in Fig. 14. The pressure increase through the diffuser is small in all simulations, and it is seen that nearly all the excess $Δp$⁠, relative to SST-CC8, can be attributed to the impeller. Hence, a reduced impeller performance is the main cause that leads to a match with experimental data for SST-CC8.

which is circumferentially averaged based on massflow. It is clear that the overall turbulence level is dampened for SST-CC1, relative to the SST model. As can be expected, the eddy viscosity then increases for increasing values of $Cscale$⁠. Elevated eddy viscosity levels generally imply increased diffusion and exchange of momentum, involving also higher viscous losses. It is noted that, also near BEP and at high relative flow rates, the overall eddy viscosity level was higher in SST-CC8 than in SST.

All models show a maximum level of $μt*$ midstream in the impeller. For SST-CC8, there is a distinct high level also at the interface between impeller inlet and diffuser outlet. A portion of the elevated turbulence level extends axially near the shroud surface as indicated by two instances of A in Fig. 15(a). By comparison with the axial velocity in Fig. 15(b), this extension appears to coincide with the shear layer formed between the jet of negative axial velocity from the TLF, and the bulk of the flow; at this flow coefficient, the momentum of the TLF is sufficiently high to induce significant backflow that penetrates upstream of the impeller, into the diffuser.

Figure 15(b) illustrates the extent of the backflow near the shroud by negative axial velocities w, normalized by the impeller tip speed $UT$⁠. It is evident that the strong jet near the shroud extends significantly shorter upstream for the SST-CC8 model. Indeed, a certain reduction in TLF is expected due to the reduced amount of pressure generated by the impeller, compared to the other models. To assess the impact of the reduced outlet pressure, we plot the amount of backflow versus the impeller pressure difference for the SST and SST-CC8 models in Fig. 16.

Here, $QBF$ is the integral of negative axial velocity at the impeller inlet near the shroud, relative span $(R−RH)/(RS−RH)>0.8$⁠, where 0 and 1 correspond to the hub and shroud, respectively. $ψimp$ is the impeller head coefficient evaluated as in Eq. (2), with $Δp$ as the time-and-area-averaged static pressure difference between impeller outlet and inlet. We observe that the amount of backflow is significant and that it varies approximately linearly with $ψimp$ for both models. The linear relation is analogous to the leakage rate in annular seals with turbulent flow. Linear regression models included in the figure exhibit very similar dependence on $ψimp$ for the two models. For the case of $ϕ/ϕBEP=63%$⁠, the reduction in $QBF$ for SST-CC8 is 9% relative to SST. In Fig. 15(b), the corresponding reduction in axial extent of tip leakage jet flow is around 40%. This suggests that the reduced $Δp$ is not the main cause of the reduced extent of the tip leakage jet flow. The elevated eddy viscosity is thus likely to play a significant role. This leads us to Fig. 17, which shows examples of turbulence production near impeller tip and inlet.

Figure 17 illustrates how the curvature correction model impacts turbulence production related to the TLF. In the SST model, the highest values of turbulence production are concentrated in a relatively narrow region of the shear layer emerging from the impeller tip suction side. The same applies to SST-CC1, although now there are indications of increased production also in the adjacent entrainment region, characterized by strong streamline curvature. Further, for SST-CC8, $fr2$ has become more impactful and induces significant production in the entrainment region. The impact on eddy viscosity is reflected in the aforementioned elevated region indicated in Fig. 15(a). Consequently, the TLF interacts more with the bulk flow through diffusion and redistribution of momentum. The backflow jet near the shroud loses energy at a higher rate and suffers in terms of its upstream extension into the diffuser.

The interaction between the TLF and the bulk flow does not only affect axial velocities. As the TLF comes with a significant circumferential velocity component, in the same direction as $Ωrot$⁠, the impeller inlet flow may also be affected circumferentially. Termed as backflow-induced swirl, or prerotation, a circumferential velocity component in the same direction as $Ωrot$ for the impeller inlet flow will effectively reduce the incidence angle and impair the impeller's ability to generate head. In the present compression cell, the upstream diffuser vanes act to stop the circumferential velocity, but there is still the axial distance from the impeller tip to the diffuser trailing edge. To evaluate the degree of inflicted prerotation, we plot the circumferential velocity component in the impeller inlet plane in Fig. 18.

Similar levels of prerotation related to the backflow jet are identified adjacent to the shroud for all models. A significant difference is visible toward the hub, especially at 65–95% and around 30% relative span. Increased prerotation near the backflow jet is visible for the SST-CC models, especially SST-CC8. The reduced head coefficient relative to the SST model is mainly attributed to these impeller inlet conditions.

The difference in prerotation near 30% relative span may be linked to the elevated eddy viscosity in the diffuser outlet and the area marked by a B in Fig. 15(a). For the SST model, the eddy viscosity increases to a relatively high level within the first half of the diffuser. This is a region characterized by shear between the streamwise flow near the shroud and pressure side of the vanes, and separated flow near the hub and suction side of the vanes. The turbulence level is then fairly unchanged through the rest of the diffuser. For SST-CC8, the turbulence level in the diffuser inlet is higher than for SST, but the increase is relatively small through the first half of the diffuser. The main increase occurs in the downstream part and near the outlet of the diffuser.

Figure 19 shows an example of diffuser and TLF streamlines colored by $μt*$⁠. For SST-CC8, notice that some of the streamwise flow from the impeller outlet follows the pressure side of the vanes, near the shroud, while some is interfering with the TLF and entrained in recirculation zones. This interference can resemble impingement and leads to strong curvature for both streamwise and reversed flow. This region marks a transition in secondary flows within the diffuser, where the upstream clockwise recirculation zone, emerging from corner separation, is adjacent to a downstream counterclockwise recirculation zone near the outlet. This is in line with observations at part-load conditions for the downscaled geometry [15]. Isocontours of $Pk*fr2=10−4$ are included in the figure to indicate regions with elevated production of turbulence energy. Isocontours adjacent to walls have been filtered out for visibility purposes. The isocontours are colored by $fr2$⁠, and it is clear that the curvature correction multiplier acts to increase turbulence production in the downstream part of the diffuser, while it tends to dampen it near the diffuser inlet. The streamlines correspondingly exhibit relatively low levels of eddy viscosity in the diffuser inlet, and those exposed to strong curvature show increased eddy viscosity near the outlet. For the SST model, notice that the TLF appears stronger in the sense that streamwise flow is not able to follow the pressure side of the vane, near the shroud, to the trailing edge. Streamwise flow interacts with the TLF and leads to strong curvature also in this case, but without the same levels of turbulence production and eddy viscosity as in SST-CC8. The high turbulence production may explain the near-zero pressure difference across the diffuser in the SST-CC8 case.

In the first part of the impeller channel, SST-CC8 shows a circumferential pattern of elevated turbulence production. The pattern is related to the periodic variation in incoming swirling flow from each diffuser channel, as the impeller blade passes by the diffuser vane. The incoming flow is changing between being stabilizing (convex curvature) and destabilizing (concave curvature) with regard to turbulence. Downstream in the impeller, the turbulence production is significantly reduced and the turbulence kinetic energy decays. However, the streamwise pattern of stabilizing and destabilizing curvature is sustained through the impeller, with a corresponding variation in $fr2$ from 0 to 3. The SST model shows a similar pattern of turbulence production at the impeller inlet, but generally with less variation and maximum values well below $Pk*=10−4$⁠. Figure 20 illustrates the streamwise development of average turbulence kinetic energy and eddy dissipation in the two simulations.

Finally, we comment on another effect of the low eddy viscosity levels seen for SST-CC1 in Fig. 15(a). Near the impeller outlet, there is an interplay between the impeller outlet flow, the cavity (interstage seal) leakage flow, and the separated flow near the diffuser inlet hub surface. A reduced eddy viscosity implies less mixing in the involved shear layers. Flow exiting the cavity domain, into the impeller domain, reaches further into the bulk of the flow and promotes the radial velocity component of the impeller outlet flow. At the same time, reversed flow near the diffuser hub surface can more easily reach the upstream impeller domain. Both phenomena contribute to a blocking of the impeller outlet and could promote stall in the impeller at lower relative flow rates. The amount of axially reversed flow $QBF, diff$ at the diffuser inlet in the SST-CC1 and SST simulations was 37% and 23% higher than in the SST-CC8 simulation, respectively.

At very low flow coefficients, the experimental data exhibit a break point involving a shift in sign for the slope of the head characteristic. The slope is positive for $ϕ$ less than approximately 0.033. Comparing with numerical results in Fig. 11, we observe a similar transition, but at lower $ϕ$⁠. Additionally, the head coefficient is overpredicted for two operating points below $ϕ=0.033$⁠, suggesting that there are detrimental features of the flow field that are not fully represented or modeled.

A very similar shift in slope of the head characteristic was observed for a downscaled version of the compression cell [15]. By introducing a small amount of gas to the flow, Gundersen et al. [15] observed the appearance of nearly stagnant fluid close to the hub and impeller outlet when $ϕ$ was reduced below the point where the single-phase-head characteristic slope was no longer negative. At low relative flow rates, the streamwise flow is prone to boundary layer separation under the adverse pressure gradient in the impeller channels. Indeed, as outlined by Brennen [28], irregularities in the head characteristic at low relative flow rates are generally indicative of impeller flow separation in axial pumps. Based on the observations by Gundersen et al. [15], the phenomenon can be characterized as a form of part-span stall, where the onset is associated with no sudden drop in head and a negligible hysteresis [29].

Distinct peaks in force amplitude near $f*=0.4$ can be seen for both SST and SST-CC8 results. Parenthetically, we mention that both turbulence models also exhibit very similar force amplitudes for the dominant rotor–stator interaction at $f*=24$⁠. The force amplitude near $f*=0.4$ is reproduced for the different relative flow rates, together with the predicted head coefficient, in Fig. 21(b). Notice that no subsynchronous forces were found at 63% and 50% relative flow. At 38% relative flow, both models yield rotating stall where the resulting excitational force, and thus hydraulic asymmetry, is most severe in the SST model. Note that the head characteristic has now become flat for the SST model and slightly less steep for SST-CC8. At 25% relative flow, the force amplitude is at its peak for SST-CC8, and the slope of the head curve is now positive. For SST, however, the rotating stall is no longer apparent as the excitational forces were no longer periodic, but more random. A similar collapse of the phenomenon is seen for SST-CC8, when lowering the relative flow to 13%.

Comparing with experimental results, the inception of the rotating stall in the simulations coincides well with the shift in slope for the tested head characteristic. However, the consequence in terms of head degradation seems to be underpredicted, and one can argue that the severity seems to be delayed when moving toward lower relative flow for SST-CC8. With the assumption that the rotating stall is initiated by a type of flow separation in the impeller, the delay relative to SST can be attributed to the elevated turbulence level throughout the domain, as illustrated in Fig. 15(a). A high eddy viscosity will also generally suppress the extent of any separated or stagnant fluid regions, possibly explaining the lack of head degradation. A supplemental simulation at 38% relative flow was conducted with the SST-CC1 model, which yields significantly lower eddy viscosity levels. The resulting head coefficient was indeed reduced to 0.420, but still overpredicted relative to experimental results. This shows that the eddy viscosity level itself cannot explain the lack of head degradation. Instead, the deficiency may be linked to the eddy viscosity hypothesis employed by the turbulence models in the present study. The curvature correction model modifies the turbulence levels due to streamline curvature and rotation, but the turbulence is still represented by scalar quantities. Accounting for turbulence anisotropy may be necessary to properly capture the effects on the flow field; streamline curvature and system rotation will affect production and redistribution of energy between the components of the Reynolds stress tensor.

Barri and Andersson [30] investigated the effect of system rotation on the flow over a backward-facing step. The rotation resulted in increased anisotropy and local dampening of turbulence, leading to flow separation along the planar suction side of the channel. It seems evident that turbulence anisotropy; e.g., with a locally dampened wall-normal Reynolds stress or Reynolds shear stress, can promote separation under an adverse pressure gradient, even though the turbulence kinetic energy k is still relatively high. Turbulence models that employ the eddy viscosity hypothesis will be unable to model such effects.

where $A2$ is the cross-sectional area at the outlet of the impeller. The experimental data yield a positive slope for the head characteristic when $Ro>14$⁠. This threshold could be indicative of when the eddy viscosity hypothesis is no longer sufficient to accurately model the flow in this type of geometry and range of Reynolds numbers.

The relative angular frequency of the rotating stall found in the simulations is below the typical rotor rotating stall frequencies found in many pumps at low relative flow rates. This tendency seems to be prevailing for open, axial impellers with few blades. Relevant references are given in Table 6, referencing rotating stall-type phenomena found for inducers operating at part-load conditions, not related to cavitation.

Closer investigation of the transient simulations that include the rotating stall suggests that the stall propagation mechanism is not fully explained in a conventional manner. Pumps and compressors with a higher number of impeller blades experience rotating stall as cells of separated flow at the suction side of the blades, propagating due to diversion of the inlet flow that leads to a higher angle of attack on the next blade. The inlet flow of an impeller with few blades is not easily diverted into adjacent channels, especially when there are several upstream diffuser vanes or inlet guide vanes. For the present helico-axial impeller, the transient simulations show a propagation mechanism related to a circumferential variation in the impeller backflow.

Figure 22 shows an illustration of the impeller in blade-to-blade view with propagating flow features involved in the rotating stall. The hatched areas indicate aggravated part-span stall in the outlet of impeller channel 2, as it is in the process of propagating to channel 3. Arrows shown in the stationary frame of reference illustrate fluid flow at the channel inlet, outlet, and across the blade tip (arrows not to scale). The number of arrows at each location gives a qualitative measure of the flow rate relative to the mean, where two arrows are close to the mean. The observed propagating variation in flow rate for a channel varied according to the severity of the rotating stall. For the case of 38% relative flow, the variation of the channel outlet flow rate was approximately $±19%$ and $±15%$ around its mean for SST and SST-CC8, respectively.

The stalled region in channel 2 entails low fluid velocities relative to the impeller and thereby lower static pressure, leading to a reduced channel $Δp$ and blade loading. Thus, the TLF from channel 2 is reduced due to a lower pressure difference across the tip. Consequently, channel 3 will suffer from a gross inlet flow rate deficit due to less local backflow $QBF$⁠. This will in turn lead to aggravated stall in channel 3. Channel 1 is recovering from the rotating stall and is experiencing elevated turbulence levels, while channel 4 is fully recovered with a relatively high flow rate and improved $Δp$⁠. The high $Δp$ causes high backflow and will lead to a high gross inlet flow rate in channel 1. At the same time, the backflow from channel 3 is reduced, and the high inlet flow rate in channel 4 cannot be sustained. As such, all of the flow features propagate to the next channel.

The periodic multistage simulation setup is also likely to affect the propagation mechanism through interstage influence across the diffuser. The absolute variation in impeller channel outlet flow rate was approximately half of the variation at the inlet. When the rotating stall cell is circumferentially aligned in the impellers, it appears that the upstream impeller's locally reduced outlet flow rate will promote the reduction of channel inlet flow rate and act to propagate stall in the downstream impeller. The alignment of rotating stall in a multistage setup has previously been observed for full-span stall in axial compressors [35,36]. Further work is required to verify the rotating stall-phenomenon in an experimental setup for this geometry. An assessment of the impact of the streamwise periodic boundary condition during impeller rotating stall would also be beneficial. Simulating the full three-stage experimental setup would provide insight into whether the predicted rotating stall-phenomenon and the head coefficient of the second compression cell are influenced by any deviating conditions in the upstream impeller.

An experimental and numerical study of a low-specific-speed helico-axial compression cell in series was conducted. In the experiments, a pump unit comprising three cells was operated at varying speeds and relative flow rates. The process fluid was water. Performance results in terms of head and efficiency were evaluated for the second cell in the series. The numerical study included steady and unsteady simulations in the form of RANS-based CFD, conducted for a complete compression cell in an axially periodic setup. The SST turbulence model was employed, with and without a rotation–curvature correction model. The main results and conclusions are summarized as follows.

Experimental results exhibited a compression cell specific speed of 0.7 in BEP. At approximately 47% relative flow, the slope of the head-flow curve changed from negative to positive when further reducing the flow rate. Comparison with numerical results showed that steady-state CFD simulations with the frozen rotor frame change model predicted the head coefficient accurately for high relative flow rates. Near BEP and at lower relative flow rates, however, there was a varying discrepancy in head. Steady-state simulations were deemed irrelevant for further work on sensitizing the turbulence model to system rotation and streamline curvature. This can be attributed to exaggerated consequences of pressure gradients related to strong rotor–stator interactions. In the steady formulation, the flow field is erroneously allowed to fully adapt to pressure gradients that are inherently unsteady.

Transient simulations with the standard SST turbulence model exhibited a very good match with experimental data near BEP and at high relative flow rates. At part-load operation, however, the predicted head was too high. The rotation–curvature sensitized SST-CC model by Smirnov and Menter [25] was applied at 63% relative flow. The overall eddy viscosity level decreased relative to the SST model, but there was essentially no effect on the head coefficient. A model coefficient was adjusted such that the turbulence production multiplier $fr2$ in the SST-CC model was amplified and the maximum value was increased from 1.25 to 3. This new formulation, termed SST-CC8, resulted in a very good match between experimental and numerical results at 63% relative flow and for all relative flow rates where the slope of the head-flow curve was negative.

The main reason for the SST-CC8 model's reduced head, that matched experimental data, was the increased turbulence production in the entrainment region of the impeller TLF. Consequently, the swirling TLF interacts more with the bulk flow near the inlet of the impeller, which leads to increased prerotation. The impact is highest at part-load conditions; at 75% relative flow rate, the relative error of the head coefficient was reduced from 9.6% (SST) to 0.3% (SST-CC8). The efficiency was predicted well by both turbulence models. Relative to SST, the SST-CC8 model produced a slightly lower efficiency overall, which resulted in the best match with experimental data.

The cell's low specific speed entails that the leakage flow rate across the impeller blade tip can become significant relative to the net flow rate through the cell. CFD results showed that the leakage flow penetrates upstream of the impeller inlet plane, leading to backflow. The backflow magnitude varied linearly with the static pressure difference generated by the impeller and amounts to approximately 20% of the net flow rate near BEP. The upstream axial extension of the backflow decreased with the SST-CC8 model, relative to the SST model.

Below 47% relative flow rate, where the slope of the head-flow curve shifts, a rotating stall-phenomenon appeared in the transient simulations for both turbulence models. The rotating stall propagated at a rate of 0.4 times the impeller angular frequency and induced a significant lateral force on the rotor. The relatively low propagation frequency was in the same range as previous findings for axial inducers. The propagation mechanism was related to a variation in TLF magnitude between the impeller channels.

Both turbulence models overpredicted the head coefficient at 38% and 25% relative flow. A possible explanation is that a high scalar turbulence level erroneously delays or dampens flow separation in the impeller. Simulations that account for turbulence anisotropy could in that case be necessary to recreate the experimental results. At 13% relative flow, the rotating stall-phenomenon had collapsed in the simulations, and the predicted head coefficient matched the experimental data.

The calibrated maximum turbulence production multiplier in SST-CC8 is significantly higher than the original proposal by Smirnov and Menter [25]. The original value was selected as a compromise based on results from simulations of wall-bounded and free shear flows. These references did not, however, include axial impellers. The SST-CC8 formulation presented in this paper can improve performance predictions in turbomachinery applications where leakage flows are significant. It is not necessarily in disagreement with results from the reference cases, as the turbulence dampening function is essentially unmodified and may have been dominant for the outcome in these cases.

• OneSubsea Processing AS and The Research Council of Norway (Project No. 310587; Funder ID: 10.13039/501100005416).

The datasets generated and supporting the findings of this article are obtainable from the corresponding author upon reasonable request.

$A1$ =

impeller inlet cross-sectional area

$A2$ =

impeller outlet cross-sectional area

$b1$ =

impeller blade height at inlet

$ca$ =

compression cell axial length

$cr1, cr2, cr3$ =

rotation–curvature correction empirical constants

$Cscale$ =

rotation–curvature correction scaling coefficient

$Cμ, σk, Cω1,$$Cω2, σω$ =

SST model empirical constants

D =

rotation–curvature correction model term

f =

angular frequency in stationary frame of reference

$f*$ =

angular frequency in stationary frame of reference relative to shaft angular frequency

$fr0$ =

rotation–curvature correction function

$fr1$ =

rotation–curvature correction function with limiters

$fr2$ =

rotation–curvature correction function with limiters and scaling coefficient

$F0$ =

lateral excitational force on impeller/shaft

$F1$ =

SST model blending function

$F0*$ =

nondimensional lateral excitational force on impeller/shaft

g =

gravitational constant

H =

head

k =

turbulence kinetic energy

N =

specific speed (nondimensional)

p =

pressure

$Pk$ =

turbulence kinetic energy production

$P˜k$ =

turbulence kinetic energy production in SST model

$Pk*$ =

nondimensional form of $P˜k$

Q =

volumetric flow rate

$QBEP$ =

volumetric flow rate in BEP from experimental data

$QBF$ =

volumetric flow rate of impeller backflow related to TLF

$QBF, diff$ =

volumetric flow rate of axially reversed flow at diffuser inlet

R =

radius

$r*$⁠, $r˜$ =

criteria of rotation and curvature effects

$RH$ =

hub radius

$RS$ =

shroud radius

$RT$ =

impeller tip radius

$ReT$ =

tip-speed Reynolds number

Ro =

rotation number

s =

impeller tip radial clearance

S =

strain rate magnitude

$Sij$ =

strain rate tensor

T =

torque

U =

velocity (Reynolds averaged)

$ui$ =

Cartesian velocity components (Reynolds averaged)

$uθ1$ =

circumferential velocity (Reynolds averaged) in stationary frame of reference, at impeller inlet

$UT$ =

impeller tip speed

w =

axial velocity (Reynolds averaged)

$xi$ =

Cartesian coordinate components

$y+$ =

mesh nondimensional wall distance

z =

axis of rotation

$Δp$ =

pressure difference

$ε$ =

turbulence eddy dissipation

$εijk$ =

Levi-Civita tensor

$η$ =

efficiency

$μ$ =

fluid dynamic viscosity

$μt$ =

eddy viscosity

$μt*$ =

nondimensional eddy viscosity

$ρ$ =

fluid density

$ϕ$ =

flow coefficient

$ψ$ =

head coefficient

$ψBEP$ =

head coefficient in BEP from experimental data

$ψimp$ =

impeller head coefficient based on static pressure difference

$ω$ =

turbulence eddy frequency

$Ω$ =

vorticity magnitude

$Ωij$ =

vorticity tensor

$Ωrot$ =

shaft angular frequency