High Throughflow StreamVane Swirl Distortion Generators: Design and Analysis

This section provides an overview on the background of StreamVane distortion devices and the motivation to pursue and implement high throughflow designs. Results on previous computational analyses are briefly discussed to establish the starting point for a thorough literature review. The primary points and take-aways from the literature review are finally discussed, mainly involving three-dimensional throughflow techniques in turbomachinery applications. The remaining sections of the paper cover the computational analyses performed to quantify performance improvements for vane packs with high throughflow features. This includes the models (Sec. 2.1), methods (Sec. 2.2), results (Sec. 3), and conclusions (Sec. 4) throughout the study.

The StreamVane system was developed at Virginia Tech by Hoopes et al. [1] to efficiently test and evaluate turbofan engine performance when subjected to nonuniform flow ingestion. This system offers a robust methodology for designing vane packs that can generate complex, downstream swirl distortion at the inlet of jet engines and/or fan rigs within ground-testing facilities. The vane packs consist of turning vanes that introduce desired flow angles into the otherwise uniform flow field. The distorted secondary flow propagates downstream to form the desired distortion pattern at the aerodynamic interface plane (AIP), which is defined for the purpose of this paper upstream of any nose cone. For reference, two example vane packs are shown in Fig. 1. Due to the continued advancements of inlet systems for commercial aircraft [2], research in inlet distortion has led to heavy interest and vast improvements for StreamVanes and the underlying design methodology. The improvements include engine testing applications [3–5], prediction capabilities [6–8], complex profile generation [9,10], structural durability [11–13], and vortex structure characterization [14–16]. As shown throughout literature, continued research and development has advanced the technology to become an effective and state-of-the-art method for producing fundamental and complex swirl distortion profiles.

In addition to swirl, the vane packs can be coupled with mesh screens to produce a combined swirl and total pressure distortion profile [17,18]. The complete system, known as the ScreenVane, is unique in that it can produce complex distortion patterns while operating under a wide range of inlet Mach numbers depending on the vane pack and screen geometry. Other combined distortion methods, such as the robust and accurate system developed by Castillo Pardo and Taylor [19], are limited to low subsonic Mach numbers due potential choking within the narrow gauze passages. As mentioned, the vane packs consist of turning vanes that accelerate the flow within its passages similar to inlet guide vanes (IGVs). In the subsonic regime, the local flow acceleration along the suction side of each vane is directly proportional to the freestream velocity at the inlet. Therefore, operating ranges for these devices are limited to the critical inlet Mach number to avoid transonic flow and shock induced unsteadiness within the vane passages. It is desirable to continue to increase this upper limit and broaden the range of transonic turbofan applications in which StreamVanes can operate.

Since the vane packs are most commonly used for turbofan inlet distortion applications, it is relevant to review literature on high throughflow fan designs to determine an upper Mach number bound at the fan interface. As stated by Denton [20], one of the main design requirements for transonic fans subjected to uniform inlet flow is the ability to handle high mass flow per unit frontal area. This means high axial Mach numbers at the fan interface, potentially leading to flow choking if the inlet Mach number exceeds a certain limit. In turn, Denton gives an estimate of the upper limit inlet Mach number for commercial transonic fans (low hub–tip radius ratios) at approximately 0.7 [20]. Other studies by Chima et al. [21] and Kor et al. [22] have stated design inlet Mach numbers of 0.65 for commercial turbofan applications. In the former, a supersonic inlet was coupled with a Rolls-Royce Tay fan rotor which operated at an inlet Mach number ranging from 0.56 near stall to 0.67 at choke.

Considering these references, a reasonable upper limit inlet Mach number range can be approximated at 0.6–0.65. However, it must be noted that these values were reported at the fan face where the duct area is reduced due to a nose cone. If the AIP was located in front of the fan face without nose cone blockage, these values would decrease due to continuity. For example, if a nose cone blocked 10% of the overall duct area at the fan face, then an open duct without a nose cone would reduce the Mach number range to approximately 0.51–0.55 (considering an ideal compressible gas and constant mass flow). The values in this range correspond to the Mach number at the AIP, downstream of the distortion generator. Throughout this paper, the mass-averaged AIP Mach number will be reported considering an open duct without a nose cone. To begin implementing high throughflow techniques to increase critical Mach numbers, the peak Mach number locations within the vane passages must be identified.

The current research effort began by conducting computational analyses on fundamental designs to identify the peak Mach number locations within their vane packs. For reference, the computational tools used for these simulations were similar to those described in Sec. 2.2. The twin and quad swirl distortion generators were selected for this analysis, and the corresponding vane packs are displayed forward-looking-aft (FLA) in Fig. 1. The diameter of both designs was set to 43.18 cm (17 in.), and the defined axial chord length was 7.62 cm (3 in.). For the twin swirl, the vanes contained a 0.476 cm (0.1875 in.) maximum thickness and 0.203 cm (0.08 in.) trailing edge (TE) thickness while the quad swirl vanes contained a 0.318 cm (0.125 in.) maximum thickness and 0.132 (0.052 in.) TE thickness. These dimensions are considered “full-scale” and are representative of realistic vane packs used during ground testing. Each individual vane contained a variation in spanwise turning angle to produce the desired tangential flow angle (swirl) at the AIP. Here, and throughout the remainder of the paper, the AIP will be referred to as one diameter downstream (1.00D) of the vane pack TE's.

The outlet pressure boundaries specified during the computational fluid dynamics (CFD) simulations were set to achieve an inlet Mach number of approximately 0.5 (±0.005) for both models. Since the main objective of these analyses was to locate the peak passage Mach numbers, cut planes at the quarter chord were used to visualize the Mach number distributions. These are provided in Fig. 2, where the view is FLA and both vane packs have been, respectively, labeled. As seen, Mach numbers are clearly higher within the passages of the ring support structures. These vanes had zero turning and are typically implemented to structurally support the surrounding turning vanes. The highest Mach number values were located in certain corners where the turning vanes and ring supports intersected to form vane–vane junctions. Due to the dense vane pack and smaller passages toward the center of the twin swirl geometry, it contained higher passage Mach numbers in comparison to the quad swirl design. The peak domain Mach numbers, located within the junctions, were predicted at $Mmax=0.875$ for the twin swirl and $Mmax=0.814$ for the quad swirl considering an inlet Mach number of $M1=0.5$⁠.

To better understand why these particular junctions produced the highest domain Mach numbers, the CFD predicted streamlines along a quad swirl ring support passage are displayed in Fig. 3. The streamlines are colored by the isentropic Mach number values along the inner and outer surfaces. The inner and outer turning vanes combine to produce one of the four vortices within the AIP distorted profile. Since these vanes turn and accelerate the flow, each turning vane contains a suction and pressure side similar to an IGV or turbine blade. Due to the turning of the outer vanes, the flow along the outer surface of the ring support turns analogously, introducing a spanwise flow structure within the passage. As a result, the flow along the inner surfaces must accelerate to conserve momentum. This mechanism inevitably produces an “induced” suction side at certain locations along the inner surface of the ring support vane. When the suction surfaces of the inner turning vanes intersect with the induced suction surfaces of the support vane, the flow accelerates rapidly and generates the highest flow velocities (and therefore Mach numbers) within the passages. The flow within these suction side junctions corresponds to the peak domain Mach numbers identified in Fig. 2.

These results, obtained through a brief CFD analysis, successfully identified the highest Mach numbers generated by two fundamental distortion generator designs. The geometrical features that produced the highest local velocities were suction side junctions between the inner turning vanes and ring supports. Most complex vane pack configurations that use high aspect ratio vanes to achieve the desired distortion profile contain similar support ring junctions. Therefore, the following literature review was conducted to pinpoint well-documented throughflow techniques that would reduce local Mach numbers and increase critical Mach numbers within geometries related to vane junctions.

The primary literature review for this research effort was split among three different categories: (1) two-dimensional designs, (2) three-dimensional designs, and (3) more advanced designs. Specifically, each design category was investigated to gain insight on throughflow techniques that would decrease peak Mach numbers within high-speed junctions. For brevity, only the three-dimensional techniques will be discussed since the final design methodology was selected from that particular category.

The first pieces of selected literature investigated simple junctions between struts and flat plates. The numerical studies by Kim and Mori [23] and Ungureanu and Lungu [24] computed the aerodynamic and hydrodynamic effects of a strut connected with a flat plate at an incline. In other words, the strut was positioned perpendicular to the flat plate and then angled by 30 deg to create an obtuse (120 deg) and acute (60 deg) angle on either side of the strut and flat plate connection. The computations revealed a shift in the leading-edge stagnation location to the acute angle junction, which created steep pressure gradients along the flat plate connection. In turn, the pressure gradients introduced increased velocity magnitudes along the acute junction and decreased velocity magnitudes along the obtuse junction. Experiments performed by Mehta [25] manipulated airflow along wing–body junctions by changing the geometry of the airfoil leading edge. The measurements showed a reduction in vortex strength and velocity magnitude when implementing a narrow, wedge-elliptic leading edge in comparison to a wide, super-elliptic leading edge. Lakshmanan et al. [26] provided predictions of supersonic corner flows after fillets and sweep were defined within a strut and flat plate connection. The results showed that a strut with sweep and large radii fillets generated the least amount of flow disturbance and pressure gradients along the junction. Regarding StreamVane design, leading edge and fillet sizing is limited to additive manufacturing tolerances and structural durability requirements. Therefore, increasing the angle of vane intersections as well as applying sweep were considered promising techniques to improve throughflow aerodynamics and reduce local velocities.

For turbine blade rows, increasing the blade inclination angle is commonly referred to as blade lean, a resulting feature from airfoil stacking or specific design to reduce losses. A simple diagram depicting leaned blades is provided in the top of Fig. 4. Smith and Yeh [27] describe positive lean as the obtuse-angled connection located on the suction side of the blade. The small magnitude pressure gradients normal to the endwall (or hub) results in a pressure increase at the hub for positive-leaned blades. This increase in pressure reduces local velocities throughout the entire chord length of blade–hub junction. Experimental and numerical studies by Harrison [28] and Gümmer et al. [29] investigated the effects of blade lean for axial turbine and compressor stages, respectively. In both cases, blades with positive lean were measured and predicted to contain a decrease in velocity magnitude and isentropic Mach number along the blade–hub junction. This was a direct result of the increase in static pressure around the base of the blade due to positive lean. Other computational predictions by Denton and Xu [30], Bagshaw et al. [31], and Zeng et al. [32] have recorded similar findings. Denton and Xu displayed a clear decrease in Mach number near the hub of a positive-leaned blade, while the Mach number was slowly increased along the span of the blade toward the tip. Bagshaw et al. demonstrated the adverse effects of negative lean in a turbine cascade, where the loading increased near the hub resulting in overturning. Zeng et al. used compound lean (positive lean at both walls) to reduce Mach numbers and passage shocks for compressor blades at transonic Mach numbers. From literature, positive lean and the resulting flow physics are clearly indicative of a reduction in flow velocities near a blade–endwall connection. It was thus hypothesized that implementing positive lean at the suction side junctions within vane pack designs would decrease passage Mach numbers and increase critical Mach numbers.

where $M$ is the Mach number normal to the leading edges, $M∞$ is the freestream (flight) Mach number, and $ϕ$ is the sweep angle. This formulation suggests that wing sweep could be extrapolated to reduce Mach numbers in more complex geometries such as blades and vanes within turbomachinery components.

Upon review, blade sweep has been thoroughly documented for turbomachinery applications in literature. These applications are more relevant for swirl distortion generator design due to spanwise turning angle variations and secondary passage flows that are commonly found in IGV's and turbine blade rows. As stated by Smith and Yeh [27], blade sweep is a typical result of complex hub and casing geometry to achieve necessary performance, weight, and/or dimension requirements in turbine stages. Smith and Yeh define positive sweep by the blade–hub connection moved toward the approaching flow along the axial direction. This sweep definition is depicted in the bottom image of Fig. 4 and also discussed in the paper by Denton and Xu [30]. For a blade with positive sweep, the small magnitude pressure gradient normal to the hub generates a reduction in blade loading at the leading edge of the blade–hub junction due to the sweep angle of the blade. Since the blade is swept back from the hub connection, the same effect creates an increase in loading at the blade tip and casing. The decrease in blade loading at the blade–hub leading edge has been predicted and measured throughout literature. Lewis and Hill [35] reported a reduction in loading along the chord of a swept blade. In the paper by Pullan and Harvey [36], CFD predictions showed a “loading loss” along the endwall of a swept turbine blade that was validated through pressure tap measurements. The reduction in loading reported by both papers corresponded to a decrease in isentropic Mach numbers along the chord of the turbine blade near the hub connection. Considering its documented effect in literature, sweep was selected as another throughflow technique to decrease Mach numbers within vane passages.

From the combination of literature review and the results obtained from the previous CFD analyses in Sec. 1.2, implementing positive lean or sweep at the suction side junctions of a swirl distortion generator were hypothesized to decrease passage Mach numbers and increase critical Mach numbers. Both throughflow techniques were applied separately to conduct a comparative analysis that will be discussed in Secs. 2–4.

All swirl distortion generator models and geometries designed for the throughflow analysis are provided in this section. The geometries consist of a baseline configuration as well as vane packs incorporating throughflow techniques such as lean and sweep. Additionally, the computational tools used to analyze the performance of each design are described. This includes the cfd software, models, domain, and boundary conditions.

where $Uθ$ is the tangential velocity and $Uax$ is the axial velocity. The goal swirl distribution was set at a constant −20 deg (negative clockwise, FLA) from a normalized radius of $r/R=0.2$ to $r/R=1$ (wall). To achieve this value, a linear increase of swirl was defined from $r/R=0$ to $r/R=0.1$ due to the center of the vortex containing zero tangential velocity (zero swirl). However, to keep the overall profile simple, the region within $0≤r/R≤0.2$ was not considered. This resulted in an “ignored” center region and a profile defined geometrically similar to that experienced by a fan with a nose cone (see Ref. [37]). Note, as stated in Sec. 1.1, mass-averaged quantities reported in this paper at the AIP did not account for additional area blockage due to a nose cone. The goal tangential flow angle (swirl) used to design the vane pack is given in the left image of Fig. 5(a).

With the goal profile defined, the design system generated a vane pack that would produce the necessary flow turning to achieve the desired profile at the AIP. The vane turning angles were computed equivalent to the AIP swirl angles, considering the assumptions within the design code. The turning angles along the normalized radius are plotted in the right image of Fig. 5(a), and the resulting vane pack is displayed in Fig. 5(b). As seen, the bulk swirl design consisted of two circular support rings, six inner turning vanes, and 12 outer turning vanes. The inner support ring was located at $r/R=0.2$ and was used as a cutoff point for all turning vanes within the geometry. The outer support ring was located at $r/R=0.6$ and contained turning vane junctions on both inner and outer surfaces. As described in Sec. 1.2, these junctions produce an intersection between a suction side along the turning vanes and an induced suction side along the support ring. For clarity, these six regions are marked with a black star in Fig. 5(b) and will be referred to as the points of interest (POI).

The vane parameters of the bulk swirl design were defined similar to the full-scale parameters used in the twin swirl design from Sec. 1.2. The vane pack diameter was set to $D=43.18$cm (17 in.) with constant vane dimensions of $b=7.62$cm (3 in.) axial chord length, $tmax=0.476$cm (0.1875 in.) maximum thickness, and $tTE=0.203$cm (0.08 in.) TE thickness. The complete list of dimensions is provided in Table 1. The diameter and vane parameters (except axial chord) were kept consistent for each lean and sweep design in order to isolate the impact of both features.

Using the bulk swirl baseline design from Sec. 2.1.1, positive lean was implemented at each POI. This consisted of shifting the vanes tangentially to increase the angle of the vane intersections containing suction side junctions. In result, four angles at the respective corners of the six outer ring junctions were altered: Two corners increased in angle while two decreased in angle. From the baseline, five increments of 5 deg lean were employed to obtain a lean angle parameter set of $λ=[0 deg,5 deg, 10 deg, 15 deg, 20 deg, 25 deg]$⁠. The lean was specified at finite points along the junction chord in order to achieve a constant lean angle throughout the intersection between the outer support ring and turning vane. In total, five “lean” bulk swirl models were designed and are displayed in Fig. 6. The additional spanwise curvature seen in the inner and outer turning vanes was a product of implementing lean angles at the outer ring while maintaining the baseline junction locations at the inner ring and domain wall. Therefore, the spanwise curvature of these vanes became increasingly significant as the lean angle increased. These designs were used as a parameter study to predict the impact of lean angle on the passage and critical Mach numbers as well as the AIP swirl distortion profile generated by the bulk swirl baseline design.

In this equation, $b=7.62$cm (3 in.) is the design axial chord length from Table 1 that was held constant, $R=21.55$cm (8.5 in.) is the design radius, and $ϕ$ is the desired sweep angle. From the baseline, four increments of 5 deg sweep were implemented to obtain a parameter set of $ϕ=[0 deg, 5 deg, 10 deg, 15 deg, 20 deg]$⁠. The bulk swirl sweep designs are provided in Fig. 7, where the views were angled to better visualize the defined sweep angles. As seen, a linear decrease in axial chord length exists from the outer ring to the inner ring and domain wall. These designs were used in part of the parameter study to predict the impact of sweep angle on the domain Mach numbers and AIP swirl distortion profile generated by the bulk swirl baseline design.

The flow fields were predicted by the commercial software ANSYS 2022R1 cfx [38], which solved the Reynolds Averaged Navier–Stokes (RANS) equations in three dimensions. This solver uses the finite volume method to satisfy the local conservation equations of mass and momentum. For the throughflow comparative analysis, a constant inlet Mach number was set at $M1=0.452$ which resulted in maximum domain Mach numbers in the range $0.78≤Mmax≤0.88$⁠. Therefore, the fluid was modeled as air obeying the ideal gas law to account for compressibility effects, and the total energy equation was included in the governing equations. CFX employs density-weighted averaging, known as Favre averaging, when the RANS equations must account for variations in density. Although RANS equations cannot resolve the smaller turbulence scales and dynamics found within junction flows, it can still accurately predict the mean flow velocities within these regions [39]. In terms of downstream swirl prediction, studies by Sanders et al. [9], Stephens et al. [40], and Frohnapfel et al. [18] have validated similar RANS models for distortion generators. In turn, these equations, with an appropriate selection of the encompassing models, were considered sufficient for the flow fields of interest in this study.

To solve for the advection term in the momentum equations, the high-resolution advection scheme based on Barth and Jesperson [41] was selected. An algorithm similar to Rhie and Chow [42] was used to avoid pressure and velocity decoupling due to the nonstaggered grid layout in CFX. Menter's k– ωshear stress transport turbulence model [43] was chosen for its robust switching method to improve model predictions near and far from wall boundaries. CFX employs an “automatic” near-wall treatment when the k–ω form of the shear stress transport model takes over. This method switches between wall functions and the low-Reynolds number method depending on the normalized grid spacing from the wall. Additionally, CFX iterates in pseudo-time when solving the steady-state RANS equations. The iterations continue until predefined convergence criteria are met. For the current study, all solutions were recorded at a pseudo-time-step of 500, in which the root-mean-square residual values for each transport equation were converged to approximately $1×10−4$⁠. With the above models selected, ansys reports second-order spatial approximations for the cfx solver where possible [44].

The CFD domain was defined as a cylindrical duct to replicate typical inlet ducting for jet engines or fan rig ground-testing facilities. The diameter of the domain was set to match the 43.1 cm (17 in.) diameter of each vane pack design. The inlet of the domain was placed one diameter upstream of the leading edges and contained an inlet total pressure of 101.325 kPa (14.7 psi) with a freestream turbulence intensity of 1%. The outlet of the domain was placed five diameters downstream of the TE's and contained an outlet static pressure value set to achieve an inlet Mach number of 0.452 for each design. The vanes and domain wall were modeled as no slip, adiabatic surfaces to capture the viscous boundary layer effects within both regions. A CAD rendering of the CFD domain and corresponding boundary locations is provided in Fig. 8, and a summary of the boundary conditions is listed in Table 2. A grid convergence study was conducted to establish independence between the discretized domain and variables of interest. A version of Roache's grid convergence index (GCI) described by Celik et al. [45] was used to quantify the uncertainties due to discretization error. The complete information regarding this study is outlined in  Appendix A. In summary, a medium sized grid (grid 2) containing 26.2 × 10⁶ nodes and 64.7 × 10⁶ elements was selected for all analyses, and the uncertainty due to discretization error was estimated at 0.4%. An image of the finalized mesh is provided in Fig. 16.

The presented results focus on the passage Mach numbers, critical Mach numbers, and downstream distortion predictions for each vane pack design. These results are directly compared to the baseline case to quantify performance improvements and/or losses after implementing the selected throughflow techniques. The results were acquired from high fidelity CFD simulations corresponding to the methodology described in Sec. 2.2. For reference, a complete list of key results from all simulations is provided in Table 3.

The passage velocity fields within the bulk swirl baseline design were predicted at an inlet Mach number of $M1=0.452$⁠. A contour of local Mach numbers within a quarter-chord plane perpendicular to the streamwise direction is illustrated in Fig. 9, where the view FLA. As expected, the peak Mach numbers were located within the suction side junctions produced by the inner turning vanes and outer support ring. These align with the POI's described in Sec. 2.1.1 and Fig. 5. The maximum Mach number produced by the baseline vane pack was predicted to be $Mmax=0.866$⁠. At the selected operating condition, the mass-averaged exit Mach number at the AIP was $M2=0.492$⁠. Recall from Sec. 1.1, this value reflects the inlet Mach number at the AIP in front of the nose cone in a turbofan or fan rig ground-test configuration.

Additional CFD simulations were conducted to estimate the critical Mach number for the baseline design. This entailed multiple iterations of adjusting the outlet static pressure to achieve an inlet Mach number in which the peak domain Mach number was approximately 1. As a result, the critical Mach number for the baseline design was predicted at $M1, cr=0.491$⁠, with a critical mass-averaged exit Mach number of $M2,cr=0.541$⁠. In other words, if this vane pack was used for a turbofan inlet distortion ground test, the maximum mass-averaged Mach number experienced at the AIP would be 0.541. This value would be even higher at the fan face, where the nose cone blockage would decrease the duct area and increase the velocities within the annulus.

Using the lean models described in Sec. 2.1.2 and displayed in Fig. 6, five CFD simulations were performed to predict the passage velocity fields within each design. Figure 10 shows contours of Mach number at the quarter-chord plane, FLA, for each lean model. A decrease in maximum Mach number was predicted, quantified at 5.41%, within the POI's as the lean angle increased from $λ=5 deg$ to $λ=20 deg$⁠. This was a direct result of the lean implemented at each outer ring junction, where the angle at the suction side junctions (POI's) increased creating a decrease in axial velocity. However, this trend did not continue for the $λ=25 deg$ design. This was due to the peak Mach number regions extending from the POI's toward the center span of the inner turning vanes, where the local vane curvature was the highest. The switch in peak Mach number is depicted by the black stars in Fig. 10, and ultimately caused the positive lean angles at the POI's to be a nonfactor. At the lean angle of $λ=25 deg$⁠, the steep spanwise curvature induced pressure gradients and additional secondary flows along the span of the inner turning vanes. As a result, the peak Mach numbers switched at some value within $20 deg<λ≤25 deg$⁠.

Similar to the baseline design, multiple CFD iterations were conducted to determine the critical Mach numbers for each lean geometry. Comparing the $λ=0 deg$ case (baseline) to the lean angles $λ=5 deg, 10 deg, 15 deg,$ and $20 deg$⁠, the critical Mach number increased by 2.14%, 3.86%, 5.64%, and 6.61%, respectively. However, from $λ=20 deg$ to $λ=25 deg$⁠, the critical Mach number decreased due to the switch in peak Mach number locations previously discussed. For this parameter set, the best throughflow design contained a lean angle of $λ=20 deg$ with a critical inlet Mach number of 0.524.

Along with the critical inlet Mach numbers, the critical mass averaged exit Mach numbers were computed to determine the maximum AIP Mach numbers for each lean design. An increase in lean angle from $λ=0 deg$ (baseline) to $λ=5 deg, 10 deg, 15 deg,$ and $20 deg$⁠, resulted in a 2.44%, 4.46%, 6.54%, and 7.68% increase in exit Mach number, respectively. As expected, there was a 1.29% decrease in exit Mach number between the lean designs $λ=20 deg$ and $λ=25 deg$⁠. These predictions implied there was some optimal POI lean angle (within the selected parameter space) that would produce the highest mass-averaged exit Mach number (⁠$M2,cr$⁠). This is depicted by the plot in Fig. 11, where a fourth-order polynomial interpolation was performed on the resulting $M2,cr$ values. As indicated, a positive lean angle of $λ=20.52 deg$ resulted in the highest mass-averaged exit Mach number of $M2,cr=0.583$⁠. Again, this value would most likely be increased to above 0.6 at the fan face if blockage due to a nose cone was considered. This would push the exit Mach number produced by the optimal lean design within the desired range from Sec. 1.1, depending on the nose cone diameter.

The same CFD and postprocessing methodology was conducted on the sweep designs to evaluate the Mach number changes from the baseline configuration. The sweep designs can be referenced in Sec. 2.1.3 and Fig. 7. The Mach number contours predicted within each model are given in Fig. 12, where the contour plane is still perpendicular to the streamwise direction, but the axial location of the plane is adjusted to be a quarter of the $b′$ chord (see Eq. (3)). From a sweep angle of $ϕ=5 deg$ to $ϕ=15 deg$⁠, the peak Mach numbers remained at some axial location within the POI regions as indicated by the black stars. Within this range, the maximum domain Mach number decreased by 4.06%, indicating a throughflow improvement up to a sweep angle of $ϕ=15 deg$⁠. However, for the sweep angle of $ϕ=20 deg$⁠, the maximum Mach number significantly increased from $Mmax=0.816$ to $Mmax=0.890$⁠. The overall reasoning behind this behavior is similar to the lean designs in which there was a shift in peak Mach number location away from the POI's.

If we recall the literature review in Sec. 1.3, positive sweep implemented at a blade–hub connection resulted in negative sweep at the casing (for simple blades). Also, recalling how sweep was applied to the baseline vane pack in Sec. 2.1.3, shortening the axial chord length at the domain wall and inner support ring resulted in negative sweep within these regions. Again, negative sweep increases loading and axial flow velocities due to the interaction between the low-pressure gradient, normal to the wall, and the sweep angle of the vane. Therefore, in comparison to the standard baseline design, the domain wall and inner support ring junctions generated higher local Mach numbers. As the positive sweep angle at the outer support ring increased, so did the negative sweep angles at the wall and inner support ring. Eventually, the negative sweep locations produced the highest domain Mach numbers and caused the switch in location shown in Fig. 12.

The critical Mach numbers were computed to predict the operating limit for each sweep model. From the baseline design of $ϕ=0 deg$ sweep, the designs with $ϕ=5 deg, 10 deg,$ and $15 deg$ increased the critical inlet Mach number by 1.31%, 2.60%, and 3.74%, respectively. At the sweep angle of $ϕ=20 deg$⁠, the inlet critical Mach number decreased from the 15$deg$ Sweep design by 3.42%. This resulted in the best throughflow sweep design at $ϕ=15 deg$ with a critical inlet Mach number of 0.510. The critical, mass-averaged exit Mach number was calculated to evaluate the “maximum” AIP Mach number generated by the sweep designs. These data are provided in Fig. 13, where the data points are fitted with fourth-order polynomial to determine the optimal sweep angle that produced the highest exit Mach number. As seen, this occurred at $M2,cr=0.561$ for a sweep angle of $ϕ=14.66 deg$⁠. Since this exit Mach number value was less than the maximum mass-averaged value for the 20$deg$ lean design, the sweep geometries within the specified parameter set and operating conditions performed worse in terms of throughflow than the lean geometries, but still improved the overall Mach numbers in comparison to the baseline design.

Since StreamVanes are designed to generate a desired swirl distortion pattern at the AIP, it is worth briefly investigating the swirl profiles produced by each vane pack. Even though both lean and sweep designs showed an increase in critical Mach numbers, if implementing such techniques results in a significantly worse swirl match, then these techniques are counterproductive to the design goals of the overall system. A “good match” swirl profile can be determined by directly comparing the goal swirl profile, used to design the bulk swirl vane pack (Fig. 5(a)), with the swirl profile predicted by the CFD solver. Comparison plots are provided in Fig. 14 for the baseline (a), 20 deg lean (b), and 15 deg sweep (c) designs. Here, the CFD predicted AIP swirl profiles are shown on the left while the goal-minus-predicted swirl comparisons are shown on the right. The comparison plots were generated by subtracting the predicted swirl values from the goal, directly revealing the differences between the two profiles (at the AIP). In these plots, the dashed circles represent five rings with centers of equal area, and the solid inner (red) circle can be referenced as ring 4 located at $r/R=0.84$⁠. The 20 deg lean and 15 deg sweep designs were selected for the swirl comparisons since they were the best performing throughflow designs.

In this equation, $βgoal$ and $βcfd$ are the swirl values from the goal and CFD profiles, respectively, and the overline represents a spatial average taken at the AIP. The bulk swirl baseline design produced an RMSE of approximately 2.35 deg, which will be considered the baseline swirl error for lean and sweep comparisons.

The 20 deg lean vane pack generated additional swirl error near ring 2, located at approximately $r/R≈0.55$⁠, as identified within Fig. 14(b). This was a result of decreased swirl magnitudes (underturning) at the AIP, primarily due to the geometry changes within the outer ring junctions and inner turning vanes. The swirl RMSE for this lean design was calculated at $RMSE=2.54 deg$⁠, resulting in an 8.1% increase from the baseline RMSE. For the 15 deg sweep vane pack, the same additional swirl errors were generated at ring 2, but there were also secondary errors generated around ring 5 (⁠$r/R≈0.95$⁠) near the domain wall. The secondary error regions are depicted in Fig. 14(c) and were attributed to negative sweep that was consequential of the positive sweep implemented at the outer ring junction. The swirl RMSE for this sweep design was calculated at $RMSE=3.14 deg$ resulting in a 33.4% increase from the baseline RMSE.

From these CFD predictions, the 20 deg lean and 15 deg sweep geometries produced a worse swirl match in comparison to the bulk swirl baseline geometry. This was also true for the other lean and sweep models in which the swirl RMSE increased with the parameter angle. This is shown by the correlations plotted in Fig. 15. However, when comparing both throughflow techniques, the lean designs performed better than the sweep designs regarding swirl generation at the AIP. The 8.1% increase in swirl RMSE from the best throughflow lean design was relatively low compared to the 33.4% increase in error from the best throughflow sweep design. This implies that implementing high sweep angles in order to significantly change the throughflow becomes counterproductive in designing an accurate swirl distortion generator. Even for lean modifications, careful design strategies should be employed to prioritize the need between accurate swirl generation and high throughflow. If both qualities are desired, these predictions reveal that positive lean implemented at turning vane-support ring junctions perform the best in comparison to positive sweep. Experimental validation is required to confirm these predictions.

In summary, this paper provides the key details from an analysis conducted to increase critical Mach numbers for StreamVane swirl distortion generator designs. From previous computational analyses and literature findings, positive lean and sweep were selected as the two throughflow parameters to implement within a bulk swirl vane pack. Five different lean angles and four different sweep angles were iterated from a baseline configuration, and high fidelity CFD simulations were performed to determine the improvements and/or disadvantages of both techniques. The results showed that, within the parameter space considered, a lean angle of 20 deg produced a 6.61% increase in critical inlet Mach number and a 7.68% increase in critical exit Mach number. The increase in both Mach numbers for the sweep designs was not as significant, where a 15 deg sweep angle produced a 3.89% increase in critical inlet Mach number and a 3.72% increase in critical exit Mach number. Additionally, it was predicted that the best performing sweep design increased swirl RMSE at the AIP by 33.4% while the best performing lean design only increased swirl RMSE by 8.1%. It was therefore concluded that implementing positive lean at 20 deg would generate the best throughflow results considering the vane pack geometry, operating conditions, and selected throughflow parameters from the study. Future work could include applying positive lean to more complex designs as well as experimental validation for the presented data.

The authors would like to thank the Air Force Research Lab (AFRL) for their technical support throughout this research effort. The progress made in advancing the ScreenVane distortion generation system could not have been achieved without the continued assistance from Chase Nessler of AFRL's turbomachinery branch (AFRL/RQTT). The authors fully acknowledge Advanced Research Computing (ARC) at Virginia Tech for providing computational resources and technical support that have contributed to the results within this paper.

Distribution Statement A: Approved for Public Release; Distribution is Unlimited. PA# AFRL-2022-5924.

• This work was funded by the Air Force Research Lab (AFRL) to advance the ScreenVane combined total pressure and swirl distortion research under ARCTOS P030-00314; Subcontract Agreement 212014.05.00.2016.00.11-C1 (Funder ID: 10.13039/100006602).

Acronyms

$AIP$ =

aerodynamic interface plane

$CFD$ =

computational fluid dynamics

$FLA$ =

forward looking aft

$GCI$ =

grid convergence index

$POI$ =

points of interest

$RMSE$ =

root-mean-square error

Roman Letters

$b$ =

axial chord length

$b′$ =

adjusted axial chord length

$D$ =

vane pack diameter

$e$ =

relative error

$M$ =

Mach number

$N$ =

total number of grid cells

$p̂$ =

observed order of accuracy

$P$ =

static pressure

$r$ =

radial coordinate

$r̂$ =

grid refinement factor

$R$ =

vane pack radius

$t$ =

thickness

$U$ =

velocity

Greek Symbols

$β$ =

tangential flow (swirl) angle

$λ$ =

lean angle

$ϕ$ =

sweep angle

$Φ$ =

variable value for the grid convergence parameters

Superscripts and Subscripts

$1$ =

mass-averaged inlet value; fine grid value

$2$ =

mass-averaged value at the AIP; medium grid value

$3$ =

coarse grid value

a =

approximate value

avg =

area-averaged value

ax =

axial value

cfd =

CFD predicted value

cr =

critical value

ext =

extrapolated value

goal =

goal value

max =

maximum value

TE =

trailing edge value

$θ$ =

tangential value

A version of Roache's GCI, outlined by Celik et al. [45], was performed to establish grid independence and quantify uncertainties due to discretization error for the presented computational results. The study used the bulk swirl baseline model from Sec. 2.1.1 and CFD methodology from Sec. 2.2 to calculate the errors and compare variables of interest between three different grid sizes. Each grid contained refined elements around the surfaces of the vane pack as well as additional refinement from the trailing edges to a plane one diameter downstream (AIP). This is depicted in Fig. 16 for clarity. The boundary layers generated at the vane surfaces and domain wall were captured by prism layers consisting of first layer cell heights defined to achieve a constant $y+≈1$⁠. The coarsest grid, grid 3, contained 11.4 × 10⁶ nodes and 28.6 × 10⁶ tetrahedral and triangular prism elements. This grid was refined around the vane surfaces and downstream region to obtain a medium sized grid. This refined mesh was labeled grid 2 and contained 26.2 × 10⁶ nodes and 64.7 × 10⁶ elements. The same procedure was applied to reach the finest grid size, grid 1, which contained 52.3 × 10⁶ nodes and 127.1 × 10⁶ elements.

Four variables of interest were selected within the domain to establish grid independence. These variables are listed below:

1. The maximum domain Mach number, $Mmax$

2. The pressure drop across the vane pack, $P2/P1$

3. The average pressure on the vanes' surfaces, $Pavg$

4. The average swirl (tangential flow angle) along a ring at $r/R=0.8$ located on the AIP, $βavg$

The computed variables and GCI parameters for each grid size are provided in Table 4. The observed order of accuracy was computed greater than the estimated formal order of accuracy (2.0, see Sec. 2.2.1) for each variable. Therefore, $p̂$ was limited to 2.0 in each calculation to avoid unrealistic GCI values. Since the extrapolated error was approximately 0.1% or less for each variable during grid refinement from grid 2 to 1, grid 2 was considered converged for this study. Therefore, grid 2 (Fig. 16) was selected as the discretized domain for all CFD simulations presented in Sec. 3. The uncertainty due to discretization error for this particular grid can be reported at $GCI≈0.4%$⁠. Note, this does not account for uncertainties due to modeling errors.