Effects of Total Pressure Distribution on Performance of Small-Size Counter-Rotating Axial-Flow Fan Stage for Electrical Propulsion

Counter-rotating fans are of current interest to the industry as they reduce the swirl in the wake flow as well as achieve higher pressure rise per stage compared to single rotor fans. The second rotor, rotating in the opposite direction of the front rotor, recovers the kinetic energy in the swirl component of the wake generated from the front rotor, which, otherwise, would have been lost to the atmosphere. The phenomenon, in turn, provides improved efficiency to the counter-rotating fan stage. Other significant benefits of the counter-rotating fans include reduced overall weight, more work per unit length, lower centrifugal stress on blade, and so on. Stator vaneless compact design of counter-rotating fan (CRF) makes it suitable for various applications where, due to space or size constraint but high loading requirement, conventional industrial fans cannot be used. One such potential field of application is an unmanned aerial vehicle (UAV) with electrical propulsion.

Few pieces of research are reported in open literature concerning performance study of counter-rotating fan stage. Cho et al. [1] showed that in the case of contra-rotating fan the efficiency is at its peak when the hub-to-tip ratio is 0.4, which is almost the same point for front and rear rotor maximum efficiency. Further, they have also established that the static pressure rise is higher at tip regions of the front rotor and hub regions of the rear-rotor blade considering the variation of the relative velocity. Chen et al. [2] discussed that it is best to have a speed ratio of almost equal to one between both rotors to get the optimum performance. They found, when the speed ratio is precisely one, the maximum pressure rise is obtained for a given mass flowrate. Roy et al. [3] observed that stage performance can be improved by decreasing the axial gap between the two rotors. However, Nouri et al. [4] reported that the change of the axial distance between rotors does not seem to change the overall performances, and thus, it can be accounted for its flexibility. Mistry and Pradeep [5] concluded that counter-rotating fans, designed with higher loading in the front rotor, have a flat performance map and a wider range of stable operations. They have investigated the effect of inflow distortion on the performance of the counter-rotating fan stage and discussed the results in detail [6] They observed that the counter-rotating fan stage is highly tolerant of distortion at the inlet [7]. Nayak and Mistry [8] investigated the optimization of the geometrical parameters of contra-rotating fan stage design focusing on the reduction of a number of the blade to achieve the same performance duty as earlier design, and they found a combination of 18 blades on rotor-1 and 16 blades on rotor-2, with the new chord length combination of 50 mm and 45 mm, respectively, gave a pressure rise by 3.5% improvement compared to baseline design which has 19 and 17 number of blades for rotor-1 and rotor-2, respectively, both having a chord length of 45 mm. Vijayraj and Govardhan [9] have investigated the effects of blade sweep on the performance characteristics of contra-rotating axial-flow fans. There are systematic experimental and computational reported work that discusses the effect of parameters like the effect of change of axial spacing, and the effect of change of different speed combinations [10–15] influence the overall operating range and efficiency of the contra-rotating fan/compressor stage. Mileshin et al. [16] have reported a numerical and experimental study of a contra-rotating fan under different flight conditions. It was reported that no changes in total-pressure ratio at the same rotational speed for uniform and non-uniform flow at the inlet are observed. Interestingly, the study reports an increase in the total-pressure rise and adiabatic efficiency when the fan operates under a non-uniform inflow.

The detailed literature review revealed that there is no systematic design approach available for contra-rotating fan stage. Based on expected performance from the fan stage, design modifications need to be carried out which include the availability of space, speed, overall size of the engine, and mission map. The split of aerodynamic loading or expected pressure rise from the individual rotor is not clearly been discussed in open literature which may be due to the proprietary nature of work. Hence, it becomes essential to explore the detailed investigations to understand the effect of aerodynamic loading split between rotors on expected performance requirements.

The main objective of the present paper is to discuss the design methodology of the contra-rotating fan stage and the effect of aerodynamic load split between two rotors on its aerodynamic performance considering the same geometrical parameters.

Axial-flow contra-rotating ducted fans are designed for application in roadable electric-aircraft “Airavat.” The prototype aircraft’s weight is estimated to be around 8 kg. Hence, our propulsion system is required to provide around 100 N thrust during takeoff. Through power requirement calculation, we found it beneficial to use smaller fans in numbers rather than a big fan to achieve the required thrust. A small diameter fan will also ease its installation on the vehicle and enhance thrust vectoring capability. Each small fan is designed to give a total-pressure rise of 1000 Pa and thus a thrust of 10 N. Such fans, ten in numbers, will be fitted to our prototype aircraft. The maximum diameter of the fan is governed by the design constraints of the vehicle. Hub diameter of the fan stage is determined by the diameter of the contra-rotating motor being used. Parametric constraints and chosen parameters for design are shown in Tables 1 and 2, respectively.

Four loading distribution cases have been considered in our design. The expected total-pressure rise is distributed in the ratio of (1) 50–50%, (2) 55–45%, (3) 60–40%, and (4) 65–35% in front and rear rotor, respectively. Other design parameters are kept identical for all the cases. For the front rotor, formulations given by Cohen and Rodgers [17] are followed to calculate basic parameters like flow angles, absolute and relative velocities, degree of reaction (DOR), and diffusion factor (DF) at meanline. The second rotor is assumed to receive the same absolute velocity coming out from the front rotor. Flow enters and leaves the fan stage purely axially. The second rotor rotates in the opposite direction of the front one with the same rotational speed of 7500 rpm at the design point. Axial velocity is assumed to be constant throughout the stage. For the design purpose, we have considered the flow coefficient to be 1.25 at the mid-span of both the rotors. Flow coefficient is defined as φ = C_a/U in this context. Here, C_a is the axial velocity and U ( = π × d × N/60) is the circumferential velocity. The axial velocity value is determined from the assumed flow coefficient at the mid-span. Meanline design of the second rotor is done following similar formulations as in the front rotor. In order to get flow parameters along the span, 13 radial sections are considered. Work is distributed along the radius using variable work distribution methodology. Tip-loaded design configuration is incorporated in order to perform more work from the tip region of the blade. As a consequence, blade camber increases from hub to tip. Losses due to flow three-dimensionality are not considered explicitly in theoretical design but are accounted for by introducing the work done factor in aerodynamic work calculation. The number of blades is determined by limiting the diffusion factor value to 0.6 in order to avoid flow separation issues in the blade passage. Though an increasing number of blades helps in effective flow diffusion inside blade passage, it is constrained by the hub disk space available and aerodynamic efficiency. Efficiency decreases with an increasing number of blades due to larger skin-friction losses. These factors have also been taken into consideration while selecting the number of blades. The axial spacing between both the rotors is taken to be 50% of the front-rotor chord due to the overall length constraint of the fan duct. Incidence angles for both the rotors are assumed to be varying from + 2 deg at the hub to − 2 deg at the tip with zero at the mean radius [5]. The 2-mm tip clearance is given looking to mechanical consideration.

C4 family airfoil is selected for both rotors. Past literature suggests C4 airfoil profile is suitable for low-speed applications in compressor/fan. In house, matlab code is used to generate airfoil profiles with the calculated Camber and stagger angles at each section of the blade. For the C4 profile, maximum thickness occurs at 30% of the chord and maximum camber at 40% of the chord. For our application, maximum thickness is determined as 8% of the chord using the computational fluid dynamics (CFD) study to optimize the aerodynamic efficiency. Basic design parameters at the hub, mid, and tip for each of the four cases are shown in Tables 3–6. Conventional station numbers are taken for calculation with stations 1 and 2 at the entry and exit of the front rotor and stations 3 and 4 at the entry and exit of the rear rotor.

The computational grid is generated using the commercial grid generator package Turbogrid 15.0 [18]. A fine mesh with a traditional topology with control points is generated. The topology blocks create a framework to position the mesh elements. These represent the different sections of the mesh governed by a regular pattern of hexahedral elements. The topology ensures that the elements are placed adjacent to each other without overlaps or gaps, with shared edges in a manner that the entire computational domain is filled with no negative volumes. The topology blocks govern the placement of mesh elements to fill an arbitrary computational domain with a valid hexahedral mesh. The leading edge and trailing edge of the front-rotor blade are captured with H-grid whereas in the case of the rear rotor the leading edge is placed with a J-grid and the trailing edge is placed with H-grid. The regions beyond trailing edges for both the rotors are made specifically denser to capture the wake. Blade surfaces are surrounded by O-grid with a width factor of 0.08. The inlet and outlet are placed with H-grid. Enough layers (around 30 in both front and rear rotor) are added between the hub and the shroud so that the 3-dimensional mesh is interpolated meticulously. The representative mesh for both the flow domains and for both the rotors are as shown in Fig. 3(b).

The computational study is done for all four loading cases pertaining to different pressure rises. The initial aim is to obtain an independent grid, which implies that the results are not altered with a further increase in the number of nodes in the grid. For the mesh independent study to be done, the loading cases, 55–45% and 60–40%, are considered. Each case is subjected to four different sets of grid sizes in terms of total number of nodes (1) 700,000; (2) 950,000; (3) 1,150,000; and (4) 1,500,000. The number of nodes in the front rotor and the rear rotor are kept approximately equal. The size of the grid is dependent upon several factors including y⁺, number of layers next to blade surface, expansion ratio at both outlet and inlet, and number of elements between blade surface and the walls of the computational domain. The desired y⁺ is set to 1 and the Reynolds number, considering front-rotor chord length as the lengthscale, is 136,430, which gives the first cell thickness of about 7.2 × 10⁻⁰⁶. Total-pressure rise (mass flow circumferential averaged (MCA)) from inlet to outlet obtained from different sets of mesh size for 60–40% loading is plotted in Fig. 1. Pressure rise for Sets 2 and 3 overlaps with each other to a great extent but the result obtained from Set 1 mesh differs significantly from them. However, as the number of mesh elements is further increased (Set 4), the skewness of the mesh becomes more prominent at the leading and trailing edge of the blade. Hence, we did not get the required convergence with Set 4.

As far as the mesh independent study result for 55–45% loading (Fig. 2) case is concerned, it is observed that the results from Set 2, Set 3, and Set 4 are consistent and overlapped with each other. Hence, both 60–40% and 55–45% loading cases yield consistent results from the Set 2 mesh grid onward.

From the mesh independence study, it can be concluded that the optimum mesh size to get the converged valid results should be around 900,000–1,000,000.

The commercial software package ANSYS-CFX 17.0 [18] is used for computational analysis. Simulation is done for a single passage containing one blade from each of the front and rear rotors with an assumption of flow periodicity for other blade passages. The entire computational domain is split into two parts corresponding to the front and the rear rotor. The two domains are connected through a frozen rotor interface. From the data obtained through aerodynamic calculations, boundary conditions for computational analysis are given concerned to the mass flowrate at the outlet (per passage, 0.039 kg s⁻¹), total pressure (0 Pa—gauge) and the total temperature (298 K) at inlet, rotational speed (7500 rpm anticlockwise and clockwise respectively for front and rear rotors) for fan blade and no-slip wall at hub, shroud, and blade surfaces (Fig. 3(a)).

In order to validate the computational code used for the present study, the experimental results available by Chetan et al. [7] are used in terms of spanwise total-pressure-rise coefficient at the exit of rotor-1 and rotor-2. The available experimental results were validated for different speed combinations for design and peak pressure mass flowrates.

Figures 4(a) and 4(b) show validation of total-pressure-rise coefficient variation along the span at design mass flowrate. It is interesting to observe that the total-pressure coefficient of rotor-1 matches fairly well up to 50% span of the rotor. Thereafter, it shows a lower magnitude compared to the experimental results by about 2–4%. This is within the reported experimental uncertainty of 3–5%. Similarly, for rotor-2, there seems to be a variation of the total pressure coefficient along the span. Specifically, near the tip region where it shows lower magnitude compared to the experimental results.

Figures 5(a) and 5(b) show the validation of the total-pressure-rise coefficient along the span at peak pressure mass flowrate. The variation of the total-pressure-rise coefficient shows good agreement with experimental results along the span. It also shows good agreement for the total-pressure-rise coefficient of rotor-2 along the span except near the tip region.

Steady-state (Reynolds-averaged Navier–Stokes (RANS)) computational studies are performed for the four cases to evaluate their aerodynamic performance at the design point. k–ω-based shear stress transport (SST) turbulence model is used for simulations in CFX. Flow physics inside the passage and associated aerodynamic losses vary significantly as the loading distribution changes.

Simulation results are validated with the theoretical calculations to check the consistency. Validation for 60–40% loading case is discussed here. The fan stage is designed for a flow coefficient of 1.25 at the mid-span. Axial velocity remains constant (=34 m/s) in theoretical design. As evident from Fig. 6, at the entry to the first rotor, the axial velocity is consistent with the design. Due to the growth of the boundary layer (BL) at the hub and shroud, the effective flow passage decreases downstream. Hence, flow accelerates. Particularly, due to the presence of tip-leakage vortex near shroud, the effective flow passage is less downstream of the first rotor. As a consequence, axial velocity increases to around 40 m/s. At each streamwise location along the span, axial velocity almost remains constant following the theoretical design. Comparison plots for flow coefficient obtained from theoretical calculation and simulation results are shown in Fig. 7. Flow coefficient at the entry of rear rotor obtained from simulation is not matching with theoretical values due to flow three-dimensionality in terms of tip-leakage flow, flow separation, and boundary layer growth. Rotor blades are designed for tip-loaded configuration, and the same is reflected in simulation results (Fig. 10).

To understand the flow physics inside blade passage, axial velocity contours at three spanwise locations near hub (at 20% of blade height), mid (at 50% of span), and tip (at 85% of span) are observed (Figs. 15–18). For all loading cases, there is a presence of low momentum fluid near the trailing edge of the front-rotor suction surface (regions H1, M1, and S1). We could not achieve completely attached flow even by changing the profile thickness and number of blades in the rotor. Rotors are highly loaded despite their small heights and less mass flowrate intakes. As a consequence, rotors rotate at a very high speed. Thus, the region of low momentum fluid persists near the trailing edge of the front rotor. The wake is comparatively thicker near the hub due to the higher blade turning angle as per design (region H1). The wake thickness decreases as we move toward the tip. Near the tip, momentum deficit flow from the suction surface feeds to the tip-leakage vortex of the front rotor (region S1). Rear rotor, rotating in the opposite direction, sucks the wake coming out from the front rotor in its direction of rotation as evident from the axial velocity contour plot at 93% of span (Fig. 8) for 60–40% loading distribution case (region T1). Thus, it suppresses separation and lowers the deviation angle for the front rotor.

Rear rotor working in the wake region of the first rotor is more susceptible to separation from the suction surface (regions H2, M2, and S2) with the change of flow incident angle. Tip-leakage vortex from the front rotor strikes the rear one at the leading edge (region A1). This affects the flow physics on the rear-rotor suction surface, pushing the maximum acceleration region beyond 50% of the chord (Fig. 12, region V2). Leakage flow through the tip of the rear rotor shoots away from its suction surface (Fig. 12, region V2) unlike the front rotor, where the vortex remains attached on the suction surface (Fig. 12, region V1) at the trailing edge. Near the tip, leakage flow from both the rotors interacts in the blade passage of the rear rotor creating blockage (region A2) and thus flow accelerates.

As the loading increases in the front rotor, the wake from its trailing edge gets thicker. With increasing wake thickness, additional flow blockage is created in the axial gap. Thus, flow accelerates more than desired in the passage and incidents the rear rotor at a positive incidence angle, as for the 65–35% loading distribution case. Hence, with increasing loading in the front rotor, the rear rotor eventually operates at the off-design incidence angle, leading to the increased region of low momentum fluid in the rear-rotor suction surface (Figs. 15–18, regions M1 and M2). This phenomenon puts a severe limitation on the percentage of total-pressure rise that can be attributed to the front rotor. Both rotors lose their effectiveness near the tip due to the presence of a tip-leakage vortex. The effect is evident from the spanwise blade loading distribution plot for the 55–45% loading case (Fig. 9).

We observe a significant contribution of tip-leakage low momentum fluid flow to the overall total-pressure loss from spanwise total-pressure-rise (MCA) plot after the front and rear rotor ((Fig. 10). The loss is more in the rear rotor compared to the front one for all loading cases (Fig. 10). Boundary layer growth at the hub also contributes to the total-pressure loss but to a smaller extent. The effect boundary layer at the hub is independent of the loading distribution and leads to the almost same amount of total-pressure loss (Fig. 10) in all cases, whereas, as the loading increases in the front rotor, the effect of tip-leakage vortex becomes more prominent (Fig. 10). From spanwise total-pressure-rise (MCA) plots after each rotor, we have estimated the location in the percentage of the span (Fig. 11), starting from where the pressure-rise falls abruptly near the tip due to the presence of tip-leakage vortex. It is evident from the comparative chart in Fig. 11 that with increasing loading on the front rotor, tip-leakage low momentum fluid engulfs more portion of the blade height both in front and in the rear rotor. The front rotor loses its effectiveness from 75% of the span near the tip and the rear rotor from 72% of the span in a 50–50% loading distribution case. But the same starts from 66% and 58% of the span in front and rear rotor, respectively, for 65–35% loading case. Again, it is evident from Figs. 11 and 12 that the tip-leakage vortex grows larger as it reaches the rear rotor for all loading distributions.

The evaluation of tip-leakage vortex from the front rotor to the rear rotor is shown in Fig. 12. Tip-leakage flow originates near the leading edge of the front rotor. The vortex eventually grows as it moves downstream (Fig. 12, region V1). Tip-leakage flow begins earlier with increasing loading in the front rotor. As a consequence, the vortex effect becomes more vigorous for 60–40% and 65–35% loading distributions, leading to higher vortex-induced losses. We have tried to estimate quantitatively the streamwise location of the tip-leakage flow initiation on the front-rotor suction surface in terms of the axial chord length (Fig. 13). The figure is representative, and the locations of onset of tip-leakage flow for all loading cases are determined through visual impression from the axial velocity contour plots just above the blade tip.

Change of loading distribution affects the flow physics in the axial spacing between the front and rear rotor significantly. Total-pressure loss (MCA) is observed for all four cases due to the acceleration of flow in the axial gap (Fig. 19). Pressure loss is calculated from the total-pressure (MCA) drop in the axial gap, as shown in Fig. 19. Flow accelerates due to the blockage created in the flow passage mainly by the boundary layer growth, wake from the front rotor, and tip-leakage vortex. Minimum total-pressure loss in the axial gap is obtained for 50–50% loading distribution case, and maximum loss is in 65–35% loading case (Fig. 14). The 60–40% loading is more beneficial in terms of loss in axial spacing than the 55–45% loading distribution (Fig. 14). But total-pressure loss in the axial gap is less compared to that due to tip-leakage flow. Hence, the tip-leakage loss factor should be given more consideration while selecting the best loading distribution for CRF in terms of aerodynamic performance. Aerodynamic performance summary for each loading case is discussed below:

Contra-rotating fan stage with equal loading distribution does not perform as desired. Although the front stage gives the designed total-pressure rise (MCA), the rear stage fails to do so (Fig. 19). The second rotor is designed for a total-pressure rise of 515 Pa while it provides only 361 Pa. We observe from axial velocity contours (Fig. 15) that the flow has a negative angle of incidence (AOI) at the leading edge of the rear rotor (region L2). Hence, flow accelerates a bit even on the pressure surface, leading to decreased overall lift force. Thus, the aerodynamic work done by the rear rotor is lesser than desired. The phenomenon affects the overall total-pressure rise of the fan stage. Equal loading distribution seems to be not suitable for contra-rotating configuration even though it has minimum total-pressure loss in the axial gap between the rotors.

Fan stage with 55–45% loading distribution gives the desired total-pressure rise. The front rotor provides a total-pressure rise of 574 Pa, and the rear rotor gives a total-pressure rise of 510 Pa (Fig. 19). As the loading of the front rotor has increased, the wake from its trailing edge grows thicker compared to 50–50% loading distribution case (Figs. 16 and 15). Near the tip, separated flow from the trailing edge of the front rotor adds to the tip-leakage vortex (Fig. 16(c), region S1). In terms of desired total-pressure rise and aerodynamic performance, 55–45% loading distribution is the most suitable configuration for CRF.

Design with 60–40% loading distribution also provides the desired total-pressure rise (Fig. 19). There is total-pressure loss due to flow acceleration in the axial spacing between the rotors. The loss is comparatively less than that in the 55–45% loading case (Fig. 14). We observe a large amount of low momentum fluid on the suction surface of the rear rotor near the trailing edge (Fig. 17, regions H2, M2, and S2). But significant flow acceleration on the suction surface from the leading edge (region E2) compensates for the work loss at the trailing edge. As a consequence, we get the desired total-pressure rise. Pressure loss due to tip-leakage flow is higher (Fig. 10) in this case, making it less suitable compared to 55–45% loading distribution.

In this case, more than the desired total-pressure rise from the fan stage is obtained. Although the front rotor gives the designed pressure rise, the rear rotor provides almost double that it is designed for (Fig. 19). This seems unusual and requires experimental validation for further consideration. Total-pressure loss (MCA) in the axial gap is highest in this case (Fig. 14). As evident from axial velocity contour plots (Fig. 18), flow in the rear rotor is characterized by steep acceleration on the suction surface up to mid-chord (region R2) followed by a region of low momentum fluid (regions H2, M2, and S2). The low momentum fluid region is more vivid near the hub, starting from the maximum thickness point on the airfoil (region H2). Tip-leakage flow loss is also significant in this case (Fig. 10).

It is evident from the earlier discussion that loading distribution significantly alters the aerodynamic performance of the contra-rotating fan stage. While equal loading distribution does not perform well, tip leakage and flow separation loss put a limitation on maximum achievable loading in the front rotor. From the comparative analysis of the aerodynamic performance of contra-rotating fan stage for different loading distributions, it can be inferred that 55–45% loading in front and rear rotor, respectively, is most suitable in CRF application.

The present paper discusses the aerodynamic design of the contra-rotating fan stage and the effect of loading distribution on its performance. For this purpose, four contra-rotating fan stages with 50–50%, 55–45%, 60–40%, and 65–35% loading on front and rear rotors, respectively, are designed following fundamental design procedure. Subsequently, a detailed computational analysis of the fan stages is carried out using ansys cfx at the design condition.

Some of the important conclusions derived from the present work are summarized below:

• In contra-rotating configuration, overall stage performance is majorly governed by the performance of the rear rotor. Flow in the rear rotor is more susceptible to separation compared to the front one based on load distribution.

• The front rotor needs to be designed for a higher total-pressure rise than the rear rotor to achieve the required performance of the stage. In our study, the fan stage with equal loading in front and rear rotors does not perform as desired.

• Again, with increasing loading in the front rotor, losses in terms of tip-leakage flow and total-pressure loss in axial gap increase. The contribution of tip-leakage loss is more than the total-pressure loss in the axial gap between the front and the rear rotor. Thus, the initiation of tip-leakage flow on the front rotor is a major deciding factor for the aerodynamic performance of CRF.

• The region of low momentum fluid on the rear-rotor suction surface increases as the wake from the front rotor gets thicker with higher loading. There is an optimum distribution of loading for which both the rotors perform with the highest aerodynamic efficiency, which is termed as an aerodynamically well-matched condition.

• In this study, we found, contra-rotating fan stage with 55–45% loading in front and rear rotor respectively, is expected to provide the desired total-pressure rise and is best in terms of aerodynamic performance among the loading distributions selected.

We believe the present findings will provide necessary guidelines for the selection of loading distribution for the design of a small-size axial-flow contra-rotating fan stage. Computational results discussed in this paper require experimental validation which is presently underway at IIT Kharagpur under project “Airavat.”

The work is done as a part of the project “Airavat: the future of transportation” sponsored by SRIC, IIT Kharagpur. We are grateful to “Airavat” propulsion team members in particular to V Sai Subhankar and Amit Kumar for their support in simulations and analysis.

There are no conflicts of interest. This article does not include research in which human participants were involved. Informed consent is not applicable. This article does not include any research in which animal participants were involved.

The data sets generated and supporting the findings of this article are obtainable from the corresponding author upon reasonable request. The authors attest that all data for this study are included in the paper. Data provided by a third party are listed in Acknowledgment. No data, models, or code were generated or used for this paper.

d =

sectional diameter

N =

rotational speed

y⁺ =

dimensionless wall distance

C_p =

pressure coefficient

β =

relative flow angles/blade angles

ψ =

total-pressure-rise coefficient = (P_{0, out}–P_{0, in})/0.5 Ca²