Abstract

Computational tools have become increasingly important in design and research applications in recent years due to increasing computational resources. In most cases, model geometry and flow physics are simplified to reduce the complexity of the computational model. While this was necessary historically, modern computational tools are capable of including realistic features such as fillets, surface roughness, and heat transfer. This work presents extensive and systematic numerical results from a simulation of a centrifugal compressor stage for an aero-engine application. Numerical results are compared to detailed experimental data to investigate the effect of various modeling decisions, including turbulence models, on the predicted aerodynamics developing through the diffuser passage. Roughness and the inclusion of fillets significantly impact the flow development, especially with the shear-stress transport (SST) turbulence model. This approach leads to the conclusion that the BSL-EARSM model is best able to predict the experimentally determined diffuser flow profiles and overall performance trends with the inclusion of the previously mentioned model features. Additionally, misleading conclusions can be reached if modeling decisions are based on merely matching overall performance values. Finally, frozen rotor simulations are used to roughly approximate the impact of unsteadiness on the flow field. The results show a significant impact and also that the inclusion of approximate unsteady effects tends to further improve the predictive capability of the computational models that were considered.

Introduction

The design process for gas turbine engines has continuously evolved over the past decades as computational capabilities have improved. Computational fluid dynamics (CFD) is a critical design tool because it allows designers to predict performance without conducting significant experimental test campaigns. Designs will continue to advance beyond the limits of historical correlations, and CFD will become a more critical component of the design process. However, centrifugal compressors are a component of gas turbine engine design that present significant challenges for CFD methods.

Moore and Moore performed the first successful simulation of the flow in an impeller for a centrifugal compressor [1]. This simulation was highly simplified, as centrifugal compressors contain many flow features that present difficulties for computational methods. Compressibility effects, unsteadiness, tip-leakage flows, and the effects of a stationary shroud wall were neglected in this early investigation. It also did not include the diffuser—limiting the simulation to the impeller flow field. In the past several decades, computational capabilities have greatly increased, leading to the ability to incorporate detailed features in simulations.

Modern developments in computational methods allow designers to include engine-representative features that can result in more accurate simulation results. This is critical for the future of compressor design, as simulations must be more accurate and predictive (in new design spaces) to facilitate the design of more efficient machines. A significant improvement in simulations is the ability to include geometry and flow physics that are more physically representative of the actual flow field. Early simulations treated the flow path surfaces as smooth walls, thus inhibiting proper representation of boundary layer growth through the passage. Modeling flow passages with surface roughness values associated with the component material and manufacturing process allows for a better prediction of the boundary layer thickness and core flow through the passage. Additionally, the fillet at the intersection of blades with the hub surface is a feature of physical geometry that presents computational difficulty. Like surface roughness, inclusion of this feature will lead to better prediction of the experimentally observed flow structures [2]. Finally, compressors are often modeled as adiabatic systems, since the work input is much greater than the rate of heat transfer to the surroundings. These features (surface roughness, fillets, and heat transfer effects) are often neglected in computational models to increase computational speed.

The choice of the turbulence model also has a significant effect on the flow prediction. Modern CFD methods for turbomachinery generally rely on the Reynolds-averaged Navier–Stokes (RANS) equations. This set of equations represents a manipulation of the Navier–Stokes equations to include the effects of turbulence in a single term—the Reynolds stress tensor. These equations, with the continuity equation, represent four equations for a system with ten unknowns. Thus, additional model equations relating the elements of the Reynolds stress tensor to fundamental flow properties are required to close the system [3].

Several turbulence closure models, of varying complexity, have been developed that are used in turbomachinery simulations. The simplest turbulence model used in this study is the Spalart–Allmaras model. It is a one-equation model that is typically used for external flows, but it is favored in turbomachinery applications because of its simplicity [3]. Two-equation models have also been developed that have become popular for turbomachinery CFD. Each model has its unique strengths and weaknesses, which are explored in this investigation. The two-equation models investigated are the k–ε, kω, and shear-stress transport (SST) models. In general, the k–ε model poorly predicts the flow close to the walls of the flow path [3,4]. The kω model can better predict the flow near walls, but it is sensitive to the freestream conditions of the simulation [3]. In this work, the ansys implementation of the 2006 Wilcox kω model is denoted as BSL (baseline kω model). The 2006 refinement of the kω model has been upgraded to significantly reduce its sensitivity to freestream conditions [3]. The SST model is a hybrid of the k–ε and kω models. It takes the accuracy of the kω model and blends it into the k–ε model in the freestream flow to reduce the impact of freestream conditions [5]. However, the SST model can have difficulty in predicting scenarios with strong secondary flows and streamline curvature [3]. This presents a problem for centrifugal compressor designers, as both are characteristics of flow within a centrifugal stage. To improve flow predictions in this regime, explicit algebraic Reynolds stress models (EARSM) have been employed. These models allow for anisotropy in the turbulence quantities, thus generalizing the constitutive relation and better capturing the effects of secondary flows and strong streamline curvature [6,7].

Each of the above approaches closes the RANS equations using a differential relation between the Reynolds stress tensor and flow quantities. Reynolds stress (RS) models directly model each of the nine components of the Reynolds stress tensor. This effectively shifts the modeling to higher-order correlations and allows a better characterization of complex flows [7].

Several studies have evaluated the differences between these turbulence models and their abilities to accurately predict the complex flow fields associated with turbomachinery. Computational models of compressor cascades have been used to investigate how different turbulence models predict corner separation flows and turbulence anisotropy [8,9]. In a study simulating a rotor in a high-pressure compressor, it was shown that the choice of turbulence model significantly influences the prediction of corner separation [10]. A simulation of the flow through an impeller at 80% speed was performed to compare the performance of the experimental stage with the performance predicted by Spalart–Allmaras, SST, and RS turbulence models. The SST model accurately predicted compressor performance while requiring a relatively low solution time [11].

The objectives for a CFD simulation vary greatly between design and research applications. Designers must prioritize speed and flexibility in their simulations to allow the rapid iteration of design geometries in optimizing the stage performance. This often means that some geometric features are neglected, and certain physical effects are omitted. This can yield results with less detail but requires considerably less time to complete a simulation, which is extremely valuable to an engine development program. Conversely, when using CFD for research applications, the focus of the investigation should be to accurately predict the flow structure, at the expense of increased computational cost. This requires including relevant geometric details, heat transfer, and higher-resolution meshes, which require longer computation time.

To understand the flow mechanisms of a compressor design, it is important to compare the predicted flow field to experimental data. Typically, a comparison of overall stage performance parameters, such as total pressure ratio (TPR) and efficiency, is made. However, these high-level parameters are the result of many different physical processes in the flow field and matching the overall performance rather than the detailed flow physics can yield misleading conclusions regarding modeling quality. In other words, various combinations of phenomena can yield the same overall performance result, limiting the ability of one-dimensional values to gauge model fidelity. This investigation presents a comparison of experimentally acquired data and computational predictions of the flow structure in the diffuser. Specifically, the total pressure contours at the diffuser exit are used to quantify the flow structure. Each incrementally higher-fidelity model is probed at the same locations where experimental data are acquired to compare the exit profiles. These are used to elucidate details about the structure of the core flow and boundary layer flow, including flow separation, through the diffuser passage and inform decisions about modeling choices.

Experimental Facility

The experimental component of this research was conducted in the Centrifugal Stage for Aerodynamic Research (CSTAR) facility at Purdue University. This facility is designed for studying the complex aerodynamics associated with low-specific speed centrifugal compressors for aero-engine applications. The rotating system is driven by a 1 MW AC-electric motor that is coupled to a speed increasing gearbox with a ratio of 30.46:1. The corrected speed is 22,500 rpm and the TPR is approximately 3 at the design point. The impeller has 15 main and 15 splitter blades, with the splitter blades starting at 34% of the impeller passage. The channel-diffuser consists of 35 vanes located at a radius ratio of 1.08. Air flows through the diffuser to a turn-to-axial deswirl component, which passes into a collector. Air is then exhausted out of the collector to ambient conditions. Additional details on this facility including a normalized compressor map can be found in Ref. [12]. A graphical representation of the research compressor is presented in Fig. 1.

Facility Instrumentation.

The facility is densely instrumented to obtain pressure and temperature data used to characterize the flow. Static pressures are measured along the shroud-side surfaces throughout the flow path. Total temperatures are measured at the impeller inlet, diffuser inlet, and the exit of the deswirl component. Total pressures are measured at the impeller inlet, diffuser inlet, diffuser exit, and within the deswirl component. The diffuser exit total pressure rakes are important to this investigation, as the data acquired at this location are used for comparison with the numerical results. There are eight diffuser exit rakes and each have four spanwise measurement locations. The elements are located at 12.8%, 37.6%, 62.7%, and 87.5% span. There are two rakes each at four pitchwise positions and the rakes are distributed around the circumference in eight distinct diffuser passages. These rakes are located at +36.2%, +11.2, −13.7%, and −38.4% pitch where +50%, 0%, and −50% are the pressure surface (PS), mid-passage (MP), and suction surface (SS) of the passage, as illustrated in Fig. 2.

Performance Calculations.

Performance of the compressor stage is quantified through the calculation of the isentropic efficiency and the TPR. The stage TPR is calculated using the total pressure measurements located just upstream of the impeller and in the deswirl component. Two total pressure rakes with five spanwise elements are located just upstream of the impeller. The stage inlet total pressure is calculated as an area average of the measured total pressure values. In the deswirl component, five total pressure rakes with four spanwise elements are evenly distributed around the stage’s circumference. The stage exit total pressure is calculated using an area average of the measured values. The uncertainties in experimental TPR and efficiency are ±0.003 and ±0.5%, respectively.

The isentropic efficiency of the stage is calculated using the total enthalpies at the impeller inlet and the exit of the deswirl component. Calculating stage efficiency with enthalpies allows for consideration of humidity and real gas effects. Stage inlet total temperatures are measured at the impeller inlet using two rakes with five spanwise elements. A hygrometer is located well upstream of the impeller in the inlet duct to measure the humidity of the inlet air. The moisture content of the air is used to determine the mass fractions of the gas constituents in the inlet air, which are assumed constant through the stage. REFPROP is used to determine the thermodynamic properties of the air, including the inlet entropy and total enthalpy based on the measured total pressure, total temperature, static pressure, and relative humidity. Stage exit total temperature is measured using four rakes distributed circumferentially at the exit of the deswirl component with four spanwise elements. The actual exit total enthalpy and isentropic exit total enthalpy are acquired through REFPROP using the deswirl total temperature and pressure measurements. These values are used to calculate the stage isentropic efficiency, which is a metric for comparing numerical and experimental results.

Numerical Approach

All computations were performed using the commercial ansys CFX code Version 19.1. The pressure-based RANS solver implements an element-based finite volume approach with a nonlinear advection scheme [6]. ansys TurboGrid was used to generate a structured grid in both the impeller and diffuser domain using O, C, and H blocks composed of hexahedra elements. Total temperature and total pressure values were prescribed at the inlet domain. Mass flow exit boundary conditions were implemented near design loading while average static pressure exit boundary conditions were applied near the choke operating condition. Most simulations were conducted with a mixing-plane interface between the impeller and diffuser domains. This treatment allows for flow in both directions across the interface and averages the flow leaving the impeller circumferentially in such a way as to conserve momentum, mass, and energy [13]. A frozen rotor interface was also implemented for some simulations in which local flow conditions are directly transmitted from the impeller exit domain to the diffuser inlet domain. Simulations were conducted with a range of angular offsets between the impeller and diffuser domains to estimate the flow field at various instances in the impeller blade passing period. Various combinations of turbulence models, wall treatment, and thermal boundary conditions were used through the course of this study. A graphical representation of the computational domain is presented in Fig. 3.

Smooth walls were treated with scalable wall functions to overcome problems associated with near-wall meshing. Rough walls were treated using a sand-grain roughness height. The effect of roughness was modeled as a downward shift of the logarithmic near-wall velocity profile [6]. Surface roughness measurements were acquired on multiple surfaces of the experimental compressor to account for changes in roughness arising from different manufacturing processes. Various approaches have been implemented historically for the conversion of an average roughness (which is what is typically measured) to the effective sand-grain roughness implemented numerically. The majority of these have applied a simple scaling factor multiplied by the averaged roughness to produce the effective sand-grain roughness [14]. An average of the scaling factors determined in Refs. [1517] was taken resulting in a scaling factor of 8.4. Consequently, the average roughness values that were measured on each surface (blade, hub, and shroud in the impeller and diffuser) were multiplied by 8.4 to produce an estimation of the effective sand-grain roughness applied to that surface in the CFD models that included roughness effects.

Heat transfer effects were included through the implementation of isothermal walls on the shroud of the computational domain. The exterior surface temperature profile was measured experimentally at 13 locations. The temperatures followed a piece-wise linear relationship with radius. Upstream of the impeller leading edge, the wall temperatures increased only slightly in the streamwise direction due to conduction transferring heat from the downstream components. Through the impeller, the wall temperature increased linearly with radius to a nearly constant value on the walls downstream of the impeller trailing edge. Three linear fits were applied to the experimental data for each operating point, shifted slightly to maintain continuity at the interfaces, and applied to the shroud walls of the computational model.

Isothermal boundary conditions were implemented on the shroud-side walls rather than a prescribed heat flux due to the relative ease in experimentally measuring the wall temperature at multiple locations. The temperature measured on the outer wall was applied to the inner wall (no conjugate heat transfer analysis was conducted). To ensure this assumption was valid, the computed heat flux (with the measured wall temperature) was used to calculate a “corrected” inner wall temperature through radial conduction relationships. The relatively thin walls, low heat flux, and high thermal conductivity of the stainless-steel walls resulted in a negligible difference between the inner and outer wall temperatures. This indicates that the use of the outer wall temperature to drive the numerical heat transfer was sufficient.

Grid Independence.

A grid independence study was conducted with nine distinct grids containing between 430,000 and 39,000,000 (39 M) total nodes. The grid density was approximately scaled proportionally within the impeller and the diffuser domains; however, the grid within the impeller tip gap made it impossible to perfectly scale the grid within both domains proportionally. One impeller passage (including one full blade and one splitter blade) and two diffuser passages were included for all simulations. This combination was selected to maintain the pitch ratio within the stability range required for implementing the time-transformation interface method for future unsteady simulations. The results of the grid independence study, in terms of the stage isentropic efficiency, are presented in Fig. 4. Significant changes in the predicted stage efficiency are present as the grid count is increased to 13M. The efficiency increases by 0.14% between 13M and 21M, 0.04% between 21M and 31M, and 0.01% between 31M and 39M. The Grid Convergence Index (GCI) for each grid and each parameter was computed following the procedure given in Refs. [18,19]. This analysis estimated the discretization error in TPR and efficiency to fall below 0.3% and 0.2%, respectively, with the 13M grid.

Despite the efficiency prediction remaining relatively constant and the GCI decreasing to acceptable levels above the 13M node case, the 31M node case was selected for the subsequent analysis for several reasons. First, the grid independence study was only conducted for a single set of modeling decisions (SST turbulence model, adiabatic walls, and no fillets). Selecting the denser grid will ensure that small variations in the required grid resolution that occur due to modeling changes will not unduly impact the results. The SST turbulence model demonstrated the greatest sensitivity to grid density of the models investigated in Ref. [20], so these variations are expected to be small and sufficiently accounted for by the denser grid. Second, despite the overall performance metrics remaining constant, the increased grid density did result in small shifts in the predicted flow profiles up to the 31M node case. To quantify this, a GCI was calculated for each diffuser exit rake element total pressure values. This analysis estimated the maximum discretization error in individual total pressures values as 1.22% with the 13M node case. This value reduced to only 0.03% with the 31M node case. Since this study is focused on extracting information regarding flow physics—rather than predicting overall performance—the increased grid density was deemed worth the added computational cost.

The finalized grid consisted of 16.1M nodes within the impeller domain (including one full and one splitter blade passage) and 7.4M nodes within each of two included diffuser passages. Within both domains, the y+ of the wall-adjacent nodes was maintained under 10. The average y+ was 6.9, 5.3, and 6.3 on the impeller hub, shroud, and blade surfaces, respectively, and 7.2, 8.9, and 5.7 on the diffuser hub, shroud, and vane surfaces, respectively. The impeller contains approximately 90 nodes in the spanwise direction and 85 in the pitchwise direction (within each passage). The impeller tips were gridded using 31 nodes in the spanwise direction to resolve the tip-leakage flow through the tip gap. The diffuser contains approximately 120 nodes in the spanwise direction and 110 in the pitchwise direction (within each passage).

Results

The experimental results focus on the systematic construction of a “best practice” set of modeling decisions based on an evaluation of the aerodynamic impact of various modeling decisions. As mentioned previously, the approach is not focused on matching overall performance metrics but rather on matching flow profiles and performance trends. To this end, the experimentally determined profile of total pressure at the diffuser exit, normalized by the compressor inlet total pressure, was selected as the primary comparison metric due to the high-fidelity experimental data available. For the subsequent figures, these data will be presented first for the experimental results and then for multiple computational results. Each contour is shifted by the minimum total pressure value on that plane to maintain a consistent color scale between the figures. In all cases, contour lines are separated by 0.02. The perspective is from the diffuser throat, oriented downstream with the vanes bounding the passage illustrated on either side of the figures. The pressure side of the passage is on the left and the suction side is on the right with the spanwise coordinate forming the vertical axis. Computational contours are produced by probing the numerical results at the 16 locations that the experimental measurements are acquired. The contours are produced in an identical process between experimental and all computational data, and no extrapolation is performed. The experimental uncertainty associated with the individual measurements is ±0.0025. The spatial sparsity of the rake elements yields uncertainty in the determination of the location of maximum total pressure. This uncertainty was estimated as ±5% in the pitchwise and spanwise directions using numerical results by comparing the location of the global maximum and the location of the predicted maximum when sampled at the rake locations. These uncertainties are not expected to significantly impact the subsequent conclusions regarding modeling performance.

The experimental results at design conditions are displayed in Fig. 5. The data indicate a central “core” region of high total pressure that decays toward the boundaries of the passage due to losses originating from flow separation and friction. The center of this core region is located at −11% pitch and at 54% span. The larger total pressure decrement that exists in the pressure-side-hub corner of the passage may indicate that flow separation is more pronounced on that side of the passage. The general shape of this distribution, as well as the location of the center of the core region, will be used to compare to numerical results and evaluate modeling decisions.

Effect of Turbulence Model.

In the baseline configuration (no fillets, smooth and adiabatic walls), the ability of various turbulence models to accurately predict the flow structure present at the diffuser exit was evaluated. The resulting contours are presented in Fig. 6, which proceed from less complicated turbulence models (the one-equation Spalart–Allmaras model) to more complicated turbulence models (the two full RS models, SSG-RS and BSL-RS) proceeding down the page.

The Spalart–Allmaras model (Fig. 6(a)) predicts an unrealistically large region of separated flow—with the associated significant total pressure losses—extending from the suction-side-hub corner of the passage. The two-equation models (Figs. 6(b)6(d)) produce more realistic predictions of the extent of separation and frictional losses through the diffuser passage. The SST model predicts the core center to be located at +13% pitch and at 67% span. The k–ε and BSL (k–ω) models predict centers at 11% and 10% pitch, respectively, and both at 60% span. Compared to the experimental data, the k–ε and BSL models show slight improvements in the prediction of the core pressure location relative to the SST model. Additionally, the general shape of the prediction shows a qualitative improvement. However, all three two-equation models predict a larger extent of the pressure deficit adjacent to the suction surface of the vane (compared to that along the pressure surface), which does not align with the experimental data. The source of the deficit along the suction surface in the numerical results is flow separation along the vane. The SST model predicts a much larger separation region, beginning at the throat and growing proceeding downstream. The k–ε and BSL models predict a more gradual loss development along the vane surfaces (compared to the SST model) and more balanced between the suction and pressure surfaces of the vanes. The experimental data suggest that this represents a more accurate reproduction of the flow development; however, other modeling aspects may influence this conclusion.

The improvement of the EARSM models (compared to the two-equation models on which they are based) is to continue to shift the core location toward the center of the passage and the experimental prediction. Both EARSM models predict the location of the peak total pressure at 1% pitch and at 52% span, shifted slightly from the results of the two-equation turbulence models. Proceeding further to the two full RS models, the core location is closer to mid-passage and 57% span (SSG-RS) and 50% span (BSL-RS). The EARSM models both predicted an increased total pressure deficit on the suction side of the passage while the RS models, especially the SSG-RS, display a more balanced prediction, closer to the experimental data.

Overall, the RS models appear to yield slightly improved predictions of the flow development to the diffuser exit, as evidenced by the location of the core total pressure region. However, obtaining convergence was a tedious process due to the stiffness of the numerical system associated with these models. Some oscillatory behavior in key properties was present despite significant efforts to reach convergence. This is typical in simulations of centrifugal compressors and becomes a more significant problem at off-design conditions. The increased numerical uncertainty and decreased reliability of obtaining convergence currently limit the usefulness of applying full RS models systematically in research and design.

Although detailed flow prediction is the primary focus of this work, computational cost and convergence behavior is a practical consideration for CFD application. The computational cost per iteration for each turbulence model, normalized by the SST computational cost, is detailed in Table 1. The Spalart–Allmaras and BSL models had the lowest computational cost while the SST, k–ε, k–ε-EARSM, and BSL-EARSM all fell within a 6% band. As expected, the full Reynolds stress models (SSG-RS and BSL-RS) required significantly more computational effort. In terms of convergence behavior, the models fell into three, approximately equivalent groups. The one- and two-equation models (Spalart–Allmaras, SST, k–ε, and BSL) all reached convergence with roughly the same number of iterations required. The two EARSM models required approximately three times the number of iterations and the full Reynolds stress models required approximately ten times the number of iterations (both relative to the one- and two-equation models). As mentioned previously, even then the full Reynolds stress models showed oscillatory behavior in the prediction of key properties. Based on this information, the EARSM models are not prohibitively expensive computationally and could be implemented in both research and design applications. Additionally, the inclusion of fillets, heat transfer, and wall roughness (discussed subsequently) increased the computational cost of the simulations by less than 5% in all cases.

Effect of Fillets, Heat Transfer, and Rough Walls.

The initial results informed a down-selection of turbulence models for which the effects of including fillets, incorporating non-adiabatic shroud-side walls, and applying realistic roughness to all solid surfaces would be investigated. The two EARSM models were selected due to their close matching of the diffuser exit total pressure profile. Additionally, the SST model was included due to its prevalence in use for turbomachinery applications.

The results for various combinations of modeling inclusions with the SST turbulence model are presented in Fig. 7. The absolute results are presented in the left column (Figs. 7(a), 7(c) and 7(e)) while the right column presents the difference between the result and the baseline configuration result (Figs. 7(b), 7(d) and 7(f)). The inclusion of non-adiabatic walls (Figs. 7(a) and 7(b)) does not have a significant effect on the prediction of the diffuser exit total pressure. From a 1D compressible flow perspective, heat removal from a subsonic flow should result in an increase in the total pressure of the flow proportional to the heat transfer rate and the square of the local Mach number. The relatively low rates of heat transfer (less than 0.5% of the overall work input) combined with the subsonic nature of the flow led to the small influence of heat transfer on the total pressure contour at the diffuser exit. The experimental facility does exhibit heat transfer similar to that which is included in the model and that heat transfer does influence the experimentally determined efficiency value—due to the decrease in the measured total temperature rise. Therefore, heat transfer is included in subsequent simulations because it brings the modeled flow physics closer to the true experimental compressor.

The results, with the addition of rough walls (without heat transfer), are presented in Figs. 7(c) and 7(d). As expected, the inclusion of surface roughness leads to increased viscous losses along solid boundaries. The result is a larger total pressure deficit adjacent to the walls. Additionally, the location of the core flow has shifted (relative to Fig. 6(b)) slightly toward mid-passage due to the rough walls. The shape of the high total pressure core flow region has also shifted slightly—a more oval shape around mid-passage rather than filling the triangular region in the shroud-suction-side corner. The results with the addition of fillets (without wall roughness or heat transfer) are presented in Figs. 7(e) and 7(f). The results indicate that the inclusion of fillets has a similar effect on the diffuser exit flow profile as wall roughness. This similarity is in the profile of the total pressure field, not in the absolute value. The inclusion of wall roughness produces a decrease in the total pressure magnitude, while fillets result in an increase in the magnitude. The effect of fillets on the total pressure profile and magnitude arises due to the reduced flow separation predicted in the rounded corners (as are present in the actual hardware) compared to the unrealistic sharp corners in the model without fillets. Sharp corners lead to the model predicting excessive pressure gradients which lead to an overprediction of flow separation within the diffuser.

Finally, the results with all three of these modeling features (non-adiabatic walls, surface roughness, and fillets) for the three turbulence models implemented are presented in Fig. 8. The inclusion of these three features in the model will be referred to as the “high-fidelity” configuration. The results with the SST model (Fig. 8(a)) illustrate that the modeling features compound each other and cause a significant shift in the location of the core location and the total pressure profile at the diffuser exit. The previously presented results with the SST model (Figs. 6(b) and 7) depict contours of constant total pressure largely being directed diagonally, increasing from the hub-suction-side corner toward the shroud-pressure-side corner of the passage. However, with all three modeling features included, the gradient is largely radial, increasing out from the center of the passage. In the results with the BSL-EARSM and k–ε-EARSM models, the shift between the baseline and the high-fidelity model is less dramatic. The location of the peak total pressure is shifted slightly away from the pressure surface, falling nearly at mid-passage. Additionally, the total pressure deficit near the vane surfaces is more symmetric rather than a significantly larger deficit existing along the suction surface of the vane. However, none of these results produce a core pressure location that is shifted as close to the suction surface nor a total pressure deficit along the pressure surface of the vane that is as large as exhibited in the experimental data. While these additional modeling inclusions do bring the model closer to reality—both in terms of including more realistic flow physics and more accurately matching the experimental diffuser exit total pressure contour—they do not shift the prediction far enough to exactly match the experimental measurements.

Effect on Overall Performance Prediction.

Matching absolute values of performance metrics is not explicitly the goal of this work. The computational model does not include every source of loss that is present in the experimental compressor. Therefore, adjusting the model to match absolute values of performance metrics would simply be unrealistically manipulating the flow drivers that are included to account for aspects that are neglected. While this could allow an accurate match for a single design, it would likely reduce the accuracy of the model’s predictive capability for off-design conditions and for new designs. However, accurate matching of trends in the CFD and the experimental data, in terms of overall performance metrics, can provide another metric of model performance and predictive capability.

First, computations were completed with the three turbulence models using the high-fidelity configuration for two additional points: one each at a higher and a lower corrected mass flowrate than the original computations. The slope of the predicted stage TPR and isentropic efficiency were compared with the experimental data. Models that trended well relative to the experimental data were then used to compute a numerical speedline for a more thorough comparison. Notably, the k–ε-EARSM model, with heat transfer, surface roughness, and fillets included, predicted a sharper slope in the TPR speedline than was measured experimentally. Therefore, it was not used to simulate the entire speedline.

The trends in the overall stage total pressure ratio and isentropic efficiency predicted with various modeling combinations are presented in Fig. 9. TPR (Fig. 9(a)) and efficiency (Fig. 9(b)) are plotted against normalized corrected mass flowrate. The low corrected mass flow ends of the speedlines (both experimentally and numerically) are not indicative of surge. The experimentally determined surge point is indicated on the TPR speedline (Fig. 9(a)) but no attempt was made to computationally predict the stability limit of the stage. The experimental uncertainty is within the symbol size. The color and line-style indicate the turbulence model used while the shape and style of the point markers indicate the fidelity of the model configuration. The results obtained using the baseline configuration, omitting heat transfer, wall roughness, and fillet effects are indicated by a white-filled circle while the results obtained using the high-fidelity configuration, including those effects, are indicated by solid-filled diamonds. The experimental data are presented in black with solid-filled circles as point markers.

The experimental TPR speedline shows a vertical portion indicating the choke limit of the stage. With decreasing corrected mass flow, the TPR curve gradually falls over with an almost linear trend toward low corrected mass flows. In terms of efficiency, the experimental results again present a nearly vertical relationship adjacent to the stage choke point followed by a gradual curve over to the upper portion of the speedline. Once out of choke, the stage produces a nearly constant efficiency for a wide range of corrected mass flowrates, with a slight decrease at the lowest presented corrected mass flows.

The SST model (yellow dotted lines in Fig. 9) does a good job of predicting the trend of TPR versus corrected mass flow. Interestingly, the prediction with the baseline and the high-fidelity configuration show similar results regarding TPR. This occurs due to the opposing effects of the surface roughness and fillets, especially in the diffuser passage. The surface roughness acts to increase the viscous losses along solid boundaries proportionally with the square of the flow velocity. This would also cause an increase in the blockage within the passage and should lead to a decrease in the choke flow capacity of the stage. However, the fillets act to dramatically reduce the size of the region of separated flow along the suction surface of the diffuser vane. This is illustrated in Fig. 10 presenting contours of total pressure at 15% span using the SST (Figs. 10(a) and 10(c)) and BSL-EARSM (Figs. 10(b) and 10(d)) turbulence models in the baseline (Figs. 10(a) and 10(b)) and high-fidelity (Figs. 10(c) and 10(d)). This results in lower total pressure losses, a decrease in the blockage within the passage, and should lead to an increase in the choke flow capacity of the stage. Therefore, when both factors are included in the computational model, they offset each other and lead to the comparable TPR trend and choke mass flow prediction between the baseline SST model and the high-fidelity model.

On the other hand, the efficiency trend does change between the two speedlines using the SST turbulence model. This arises due to the third model improvement included in the high-fidelity configuration—non-adiabatic walls. While the surface roughness and fillets offset each other in terms of their contributions to the total pressure loss and the resulting TPR of the stage, heat transfer effects impact the total temperature rise through the stage. Heat transfer reduces the total temperature rise through the stage and, for the same TPR, leads to an increase in the calculated stage efficiency and a change in the efficiency trend versus corrected mass flow. This is only true when temperatures are directly used to compute the stage efficiency. This was the manner in which the experimental efficiencies were computed and, therefore, were also used for the computational results. If a torque-based efficiency were computed, heat transfer would likely have a less significant impact. This highlights the importance of evaluating parameters in an identical manner when comparing experimental and numerical results. Overall, the SST models do not match the trend in the experimental efficiency well. While the experimental efficiency is nearly constant outside of choke, the baseline SST model predicts a continued increase in efficiency with decreased corrected mass flow. That increase continues to a peak at the second lowest corrected mass flowrate included, decreasing slightly to the lowest corrected mass flowrate. The speedline predicted with the SST turbulence model and the high-fidelity configuration shows an increase in the efficiency until it reaches a maximum at the design point before decreasing with a continued decrease in the corrected mass flowrate.

The trends arising from the BSL-EARSM model (solid blue lines in Fig. 9) are distinct from the SST model results. First, the inclusion of the additional modeling features does result in a discernible shift in both the TPR and efficiency trends and the predicted corrected mass flowrate at choke. Relative to the SST model, this arises because the baseline BSL-EARSM model does not predict a significant region of separated flow along the suction surface of the vane (Fig. 10(b)). The inclusion of fillets cannot significantly impact the size of the predicted region of flow separation because there is no flow separation. Therefore, there is no driver to counteract the increased total pressure loss and the increased throat blockage that results from the surface roughness inclusion. The TPR and efficiency trends with the high-fidelity model show a very close match to the experimentally measured trends. With regards to TPR, the high-fidelity configuration predicts a steeper increase with decreasing corrected mass flow (compared to the baseline configuration) due to the increased viscous losses along the rough walls toward higher corrected mass flows (where flow velocities are higher). The slope is slightly steeper than the experimental results. This could indicate that the scaling factor implemented numerically to convert average roughness to a sand-grain roughness was too large. However, it is not advisable to merely adjust that factor until the trends match. As mentioned previously, this could result in artificially adjusting roughness to account for the various physical mechanisms not included in the model. Additional fundamental research correlating measured roughness to sand-grain roughness in the complex aerodynamic context of centrifugal compressors (swirling flow, adverse pressure gradients, etc.) is needed to offer a better scaling factor. In terms of efficiency, the high-fidelity BSL-EARSM model predicts slightly more variation than the experimental data away from choke. The baseline BSL-EARSM model shows a sharp corner to the speedline in transitioning out of choke, not matching the experimental data well.

Conducting the previous analysis and inspecting the analogues of Figs. 58 at higher-loading and near choke yield the same conclusions regarding model performance. That is, the high-fidelity configuration yielded profiles closer to the experimental results (compared to the baseline configuration) and the BSL-EARSM turbulence model produced results closer to the experimental values than the SST turbulence model (for both configurations).

Modeling Recommendation.

These results inform a recommendation for best practice in CFD modeling for designs similar to the centrifugal compressor considered in this work. The approach implemented here, focusing on flow physics and performance trends, results in a different final model selection than would be reached in attempting to match the prediction of performance parameters. Figure 11 presents the difference in TPR and stage efficiency at the design point between the results of various modeling combinations and the experimental values. The abscissa is the difference from the experimental TPR result, and the ordinate is the difference from the experimental efficiency value. A coordinate of (0,0) would indicate that the computational result exactly matched the experimental values. Based on these data, the result closest to the origin would be the “best practice” if the matching of performance parameters at the design point were the main driver in modeling decisions. Specifically, the Spalart–Allmaras turbulence model (omitting heat transfer, wall roughness, and fillets) and the SST turbulence model including roughness effects would show the best performance. Both of these results predict the design performance within 1% in terms of efficiency and 0.01 in terms of TPR. However, the Spalart–Allmaras model predicted an oversized region of separated flow and total pressure loss within the diffuser passage (see Fig. 6(a) and the corresponding discussion). This overprediction of loss was correcting, in a sense, for the overprediction of TPR and efficiency that occurred with the other baseline models. While this produces a better match of the bulk performance metrics of the experimental data, it does not imply a superior predictive capability of the model.

The same argument holds for the SST model with only roughness included. The baseline SST model tends to overpredict efficiency and TPR. Adding roughness shifts them closer to the experimental values. The inclusion of surface roughness does cause the model to better reflect the flow physics that are present in the experimental stage. However, the near-perfect matching of the computational result and the experimental data is merely coincidental. Shortcomings of the baseline model—namely, the overprediction of TPR and efficiency—are offset by the roughness in a way that happens to produce a result near the experimental values. If the model is further improved in terms of reflecting true flow physics by including heat transfer and fillets, the results again deviate from the experimental values. However, this is not indicative of a lower quality computational configuration.

The procedure implemented in this work leads to the selection of the BSL-EARSM turbulence model in the high-fidelity configuration as the recommended computational model. Heat transfer, surface roughness, and fillets should be included because they lead to a model that is closer to reality in terms of including physical flow drivers. Additionally, these phenomena impact the predicted flow field (Fig. 7) and should be included to improve the predictive capability through design changes. The BSL-EARSM model is recommended (over the SST model) due to its increased matching of the diffuser exit total pressure profile (compare Figs. 8(c) to 5) and the trend in TPR and efficiency across the speedline (Fig. 9). However, the SST model (with the high-fidelity configuration) does show relatively good results and is recommended for use in applications where the BSL-EARSM turbulence model presents convergence issues.

Frozen Rotor Results.

The previous results and discussion have been focused on computational results that utilized a mixing-plane interface between the impeller and the diffuser to conduct a steady-state simulation. Efforts were made to produce a numerical model that accurately matched the flow drivers and physics present in the experimental stage. However, unsteadiness is one such flow driver that can significantly impact the measured flow field. Recent experimental measurements of the unsteady velocity field through the diffuser show that unsteadiness persists further into the diffuser passage than typically assumed [21], suggesting a strong influence of unsteady effects on the flow field. The methodology used for model selection here—always stepping toward a more physically realistic model—was done to minimize the impact of omitted flow drivers. However, to obtain a first-order estimate of the impact of unsteadiness on the computational results, simulations were conducted with a frozen rotor interface connecting the impeller and diffuser domains.

Frozen rotor simulations were conducted with the BSL-EARSM and SST turbulence models, both with the high-fidelity configuration. The impeller domain was offset circumferentially by angles between 0 and 22 deg. Since the impeller has 15 full blades, an offset of 24 deg is equivalent to an offset of 0 deg due to rotational symmetry. Thus, the simulations approximate the rotation of the impeller through a full blade passing event. These results are presented in Fig. 12 showing the stage TPR (Fig. 12(a)) and efficiency (Fig. 12(b)) through an approximated blade passing event. The frozen rotor results are compared to the results for the same turbulence model with the mixing-plane interface and the experimental data.

The BSL-EARSM model predicts a pseudo-unsteady variation of 0.04 in the TPR and 1.3% in the stage efficiency through a full blade passing event. The SST model predicts a pseudo-unsteady variation of 0.08 in the TPR and 1.8% in the stage efficiency through a full blade passing event. Averaging the results from each impeller domain offset level was done to produce a pseudo-time-averaged value of both TPR and efficiency which can be compared to the corresponding value obtained with the mixing-plane interface. The pseudo-time-average TPR decreased by 0.03 and 0.08 and the efficiency decreased by 1.1% and 2.4% relative to the mixing-plane results for the BSL-EARSM and SST turbulence models, respectively. In all cases, the frozen rotor analysis produced results that more closely matched the experimental data. This supports the conclusion that unsteady effects have a large impact on the flow development. However, it is difficult to conclude the extent of these effects with the crude treatment of unsteadiness present in the frozen rotor model. Full transient simulations will be conducted with several of the modeling configurations implemented in this work to better evaluate the impact of unsteadiness on the computational prediction of the flow development.

Conclusions

This work has presented extensive numerical investigations regarding the accurate modeling of the aerodynamics of a centrifugal compressor. In developing a “best practice” methodology for the modeling of this compressor, the accurate matching of flow profiles and performance trends was given the highest priority in guiding this development, rather than the matching of performance parameters. Additionally, the physical drivers of flow development present in the experimental compressor were included in the computational model as accurately as possible. This approach results in the following general conclusions regarding the impact of modeling decisions on the prediction of the flow field within this centrifugal compressor stage:

  • The Spalart–Allmaras turbulence model does not accurately predict the flow development through the diffuser passage despite showing the closest match to experimental performance parameters.

  • For the baseline model, higher-order turbulence models tended to more accurately predict the location of the core total pressure region of the flow at the diffuser exit.

  • The two full Reynolds Stress models implemented in this study (BSL-RS and SSG-RS) showed the most accurate matching of the diffuser exit flow profile in the baseline configuration. However, numerical difficulties prevented their rapid, consistent implementation.

  • The inclusion of shroud-side heat transfer had a small impact on the total pressure field at the diffuser exit but did shift the stage efficiency based on temperature rise.

  • The SST model tended to overpredict the extent of flow separation along the suction surface of the vane in the baseline configuration. The inclusion of fillets in the model suppressed this predicted separation.

  • The BSL-EARSM model in the high-fidelity configuration was the best match to the experimentally measured diffuser exit total pressure profile and trend in stage TPR and efficiency.

  • Pseudo-time-average results from frozen rotor simulations show significantly better comparisons to experimental data relative to mixing-plane-based results, highlighting the significant impact of unsteadiness on flow development.

Future work will include several transient simulations to better evaluate the nature and extent of unsteady impacts on the flow field. These results will also be compared with unsteady laser-Doppler velocimetry data acquired within the experimental stage. Furthermore, the effect of bleed offtake, rake intrusion, and assembly deviations on the flow development will be studied.

Acknowledgment

The authors would like to thank Rolls-Royce Corporation for its funding and permission to publish this work. They would also like to acknowledge Grant Malicoat for his extensive support of the test campaign associated with this work.

Data Availability Statement

The authors attest that all data for this study are included in the paper.

References

1.
Moore
,
J.
, and
Moore
,
J. G.
,
1981
, “
Calculations of Three-Dimensional, Viscous Flow and Wake Development in a Centrifugal Impeller
,”
J. Eng. Power
,
103
(
2
), pp.
367
372
.
2.
Oh
,
J.
,
2016
, “
The Effects of Blade Fillets on Aerodynamic Performance of a High Pressure Ratio Centrifugal Compressor
,”
23rd International Compressor Engineering Conference
,
West Lafayette, IN
,
July 11–14
, pp.
1
9
.
3.
Wilcox
,
D.
,
2006
,
Turbulence Modeling for CFD
, 3rd ed.,
DCW Industries, Inc.
,
La Canada, CA
.
4.
Jones
,
W.
, and
Launder
,
B.
,
1972
, “
The Prediction of Laminarization with a Two-Equation Model of Turbulence
,”
Int. J. Heat Mass Transf.
,
15
(
2
), pp.
301
314
.
5.
Menter
,
F. R.
,
1994
, “
Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications
,”
AIAA J.
,
32
(
8
), pp.
1598
1605
.
6.
ANSYS Inc.
, 2018, “
ANSYS CFX-Solver Theory Guide (v. 19.1)
,” no. April. Canonsburg, PA, p.
370
.
7.
Morsbach
,
C.
,
2016
,
Reynolds Stress Modelling for Turbomachinery Flow Applications
,
Technischen Universität Darmstadt
,
Darmstadt
.
8.
Zhang
,
H.
,
Wu
,
Y.
, and
Li
,
Y.
,
2015
, “
Evaluation of RANS Turbulence Models in Simulating the Corner Separation of a High-Speed Compressor Cascade
,”
Eng. Appl. Comput. Fluid Mech.
,
9
(
1
), pp.
477
489
.
9.
Liu
,
Y.
,
Yan
,
H.
,
Liu
,
Y.
,
Lu
,
L.
, and
Li
,
Q.
,
2016
, “
Numerical Study of Corner Separation in a Linear Compressor Cascade Using Various Turbulence Models
,”
Chin. J. Aeronaut.
,
29
(
3
), pp.
639
652
.
10.
Marty
,
J.
, and
Uribe
,
C.
,
2019
, “
Impact of Underlying RANS Turbulence Models in Zonal Detached Eddy Simulation: Application to a Compressor Rotor
,”
13th European Conference on Turbomachinery on Turbomachinery Fluid Dynamics and Thermodynamics. ETC 2019
,
Lausanne, Switzerland
,
April 8–12
, pp.
1
12
.
11.
Gibson
,
L.
,
Galloway
,
L.
,
Kim
,
S. i.
, and
Spence
,
S.
,
2017
, “
Assessment of turbulence model predictions for a centrifugal compressor simulation
,”
J. Glob. Power Propuls. Soc.
,
1
, pp.
142
156
.
12.
Methel
,
C. J.
,
Gooding
,
W. J.
,
Fabian
,
J. C.
,
Key
,
N. L.
, and
Whitlock
,
M.
,
2016
, “
The Development of a Low Specific Speed Centrifugal Compressor Research Facility
,”
ASME Turbo Expo
,
Seoul, South Korea
,
June 13–17
.
13.
Denton
,
J. D.
,
1990
, “
The Calculation of Three-Dimensional Viscous Flow Through Multistage Turbomachines
,”
Proceedings of the ASME Turbo Expo.
,
Brussels, Belgium
,
June 11–14
, pp.
1
10
.
14.
Bons
,
J. P.
,
2010
, “
A Review of Surface Roughness Effects in Gas Turbines
,”
ASME J. Turbomach.
,
132
(
2
), p.
021004
.
15.
Koch
,
C. C.
, and
Smith
,
L. H.
,
1976
, “
Loss Sources and Magnitudes in Axial-Flow Compressors
,”
J. Eng. Power
98
(
3
), pp.
411
424
.
16.
Shabbir
,
A.
, and
Turner
,
M. G.
,
2004
, “
A Wall Function for Calculating the Skin Friction with Surface Roughness
,”
Proceedings of the ASME Turbo Expo
,
Vienna, Austria
,
June 14–17
, pp.
1
11
.
17.
Bunker
,
R. S.
,
2003
, “
The Effect of Thermal Barrier Coating Roughness Magnitude on Heat Transfer with and Without Flowpath Surface Steps
,”
Proceedings of IMECE2003
,
Washington, DC
,
Nov. 15–21
, pp.
1
10
.
18.
Roache
,
P. J.
,
1994
, “
Perspective: A Method for Uniform Reporting of Grid Refinement Studies
,”
ASME J. Fluids Eng.
,
116
(
3
), pp.
405
413
.
19.
Celik
,
I. B.
,
Ghia
,
U.
,
Roache
,
P. J.
,
Freitas
,
C. J.
,
Coleman
,
H.
, and
Raad
,
P. E.
,
2008
, “
Procedure for Estimation and Reporting of Uncertainty Due to Discretization in CFD Applications
,”
ASME J. Fluids Eng.
,
130
(
7
), p.
078001
.
20.
Bourgeois
,
J. A.
,
Martinuzzi
,
R. J.
,
Savory
,
E.
,
Zhang
,
C.
, and
Roberts
,
D. A.
,
2011
, “
Assessment of Turbulence Model Predictions for an Aero-Engine Centrifugal Compressor
,”
ASME J. Turbomach.
,
133
(
1
), p.
011025
.
21.
Gooding
,
W. J.
,
Fabian
,
J. C.
, and
Key
,
N. L.
,
2020
, “
LDV Characterization of Unsteady Vaned Diffuser Flow in a Centrifugal Compressor
,”
ASME J. Turbomach
,
142
(
4
), p.
041001
.