Numerical Investigation on Aerodynamics of a Rectangular Blade Rotor under Mars Air Conditions Using Large Eddy Simulation

Abstract

The study of the aerodynamics of a flight vehicle under Martian air conditions is experimentally difficult due to its characteristics such as low air density and temperature, making the vehicle operate at an ultra-low Reynolds number, which in turn introduces a complex flow field. In this paper, to find a proper computational fluid dynamics (CFD) method with which to better understand the aerodynamics of rotor-type aircraft under Martian air conditions, the aerodynamic performance of a rotor with rectangular blades under ultra-low density Martian air conditions is studied. A simulation scheme using a large eddy simulation solver and sliding meshing technology is established, and the method is verified based on experimental results from a Mars Air Simulator (MAS). In addition, the influence of the test bench and chamber is investigated through flow field analysis. The results show that the established method can predict lift in a very accurate manner, but that the torque prediction is not so promising. The study also determines that the fixture and the chamber wall of an MAS has little influence on the prediction of aerodynamic performance due to the quickly decreasing of flow speed and dissipation of vortexes. The test bench has about 5% influence on lift prediction, possibly due to the ground effect of the bench. In addition, simulation under actual Martian air conditions shows that the results agree well with the MAS experiment’s results, indicating that the temperature difference has little influence on the lift performance, and therefore that the MAS is a good tool for the lift prediction of Martian helicopters.

1. Introduction

In recent years, Martian aerial vehicles have become a hot research topic due to the need for the performance of an aerial survey on Mars [1]. Compared with ground-based Martian rovers, aerial vehicles have unique advantages of denying terrain, fast flying, and large area coverage, making them suitable for tasks that ground rovers cannot accomplish [2]. Various forms of Martian aerial vehicles, such as the micro air vehicle [3,4], flying wing airplane [5], and rotor crafts [6,7], have been designed to achieve various tasks. For example, the National Aeronautics and Space Administration (NASA) Ames Research Center designed a Martian helicopter to study highlands on Mars where the Martian rovers cannot reach [8]. Koji et al. conducted a parametric design of a Mars helicopter for pit crater exploration [9]. The Jet Propulsion Laboratory even designed and fabricated a Mars helicopter to test the feasibility of an actual helicopter flying on Mars [10], called the Ingenuity Helicopter, and it has been successfully flied on the red planet [11,12].

However, designing a Martian aerial vehicle is very challenging since the atmospheric environment of Mars is quite different to Earth’s, such as having very low air density, pressure, and temperature [13]. The Martian air, mostly consisting of carbon dioxide, has a density and pressure as low as about 0.017 kg/m³ and 600 Pa, respectively. The unique atmospheric conditions require Martian aerial vehicles to fly in a compressible flow with a very low Reynolds number, which is not normally seen in Earth aerial vehicle applications [14]. Therefore, an understanding of the aerodynamic performance of airfoils, especially for rotorcraft and propeller-based aircraft, becomes critical. Compared with a conventionally high Reynolds number flow, flow at a low Reynolds number shows unique behavior including separation, transition, and reattachment on the wing surface, which strongly affects the aerodynamic performance of airfoils [15,16].

There are experimental [17,18] and numerical studies [19,20] available for helicopters [21] and fixed-wing aircraft [22,23] used on Mars, and most of them have focused on the aerodynamic performance of airfoils in low-Reynolds-number flows. Hiroki et al. experimentally investigated five thin airfoils at $Re=1.1\times {10}^4$ and with a Mach number of 0.2 in a Mars wind tunnel [15] using the pressure-sensitive paint technique. Takuya et al. in Tokyo University carried out a numerical study on the aerodynamic optimization of airfoils for flying-wing type Martian aircraft [5]. Desert et al. conducted a simulation work on the accuracy of low and high-fidelity numerical approaches in predicting the aerodynamic forces at low Reynolds numbers and moderate subsonic Mach numbers [24]. The results prove that 2D Navier–Stokes computations could be used for airfoil shape optimization in the context of low Reynolds number with reasonable accuracy. Phillip et al. carried out a direct numerical simulation on a triangular airfoil to understand its nonlinear lift at a low-Reynolds-number compressible flow by comparing the results with experimental data from the Mars wind tunnel at Tohoku University [25]. Their results revealed that the nonlinear aerodynamic behavior of the triangular airfoil is brought by the lift enhancement attributed to the large leading-edge vortex generated. However, most of the study focused on the characteristics of 2D airfoils, while the rotor of a Mars helicopter works in a condition with a significant three-dimensional effect; moreover, the flow characteristics are much more complex than a two-dimensional airfoil section. Therefore, further research is needed.

Several universities in China are now undergoing experimental research on this topic. For example, Zhao and Quan et al. from the Harbin Institute of Technology carried out several experimental investigations on the hover performance of a single rotor system for a Mars helicopter in a Martian atmosphere simulator [21]. Especially, Quan’s team has conducted experiments on the lift and drag performance on a series of single rotors with rectangular blades of different configurations, which can be used as a good reference for numerical research [26]. However, these research studies have mainly focused on 2D research or experiment investigations, which are not capable of providing detailed flow information to perform in-depth aerodynamic analysis.

As a mathematically demanding area of fluid dynamics and mechanical engineering, turbulence problems often cannot be simulated without significant computational power. The study of the aerodynamic performance of flight vehicles experimentally on Mars is quite not applicable nowadays; therefore, the accurate prediction of the aerodynamic performance of flight vehicles under Mars’ atmospheric conditions is not an easy task because of the high Mach number phenomena at high rotational speed due to the ultra-low Reynolds number in the environment. Therefore, computational fluid dynamics (CFD) methods are widely used to solve this complication. However, without an experiment for verification, it is not sound to make conclusions based on numerical simulations.

In order to decrease the simulation time for a given level of accuracy or to increase accuracy without increasing the simulation time, CFD simulations usually begin by reducing the mathematical complexity of the problem. One of these important techniques in CFD simulations is the large eddy scale (LES) turbulence model, which is widely used in flow simulations [27]. A large eddy simulation, which can be seen as a compromise between direct numerical simulation (DNS) and Reynolds-averaged Navier–Stokes (RANS), is a popular technique for simulating turbulent flows.

In a CFD simulation, there are some phenomena that only occur on small-length scales and may not dominate over the behavior of the system as a whole. Mathematically, the basis of LES is that the flow is decomposed into small- and large-length scales of eddies. The LES turbulence model is used to ignore the smaller scale phenomena in a CFD simulation while focusing on larger length scales. With sufficiently fine meshing and time resolution, it is possible to produce very accurate results in a simulation that only focuses on spatially larger eddies that dominate turbulent flow. Therefore, meshing and time resolution plays an important role in this study, which will be discussed in detail later. Therefore, in this paper, a simulation scheme based on large eddy simulation (LES) is established and verified by MAS experimental data. Based on the experimental data, the influence of the blade fixture, chamber size, and test bench on lift performance is studied.

2. Solution Method

In this paper, the aerodynamic and flow structure characteristics of rotors in Mars’ atmosphere conditions is studied numerically through CFD solutions and the solution schemes were verified by experiment results conducted in a Mars Air Simulator (MAS).

2.1. Experimental Setup

The MAS, as shown in Figure 1a, was constructed in the Harbin Institute of Technology to explore the aerodynamic characteristics of Mars rotors. The MAS is 3 m in diameter and 3.3 m in height, as shown in Figure 1a. Among the experiments conducted in MAS, the lift and torque of several rotors with different rectangular blades were studied, which can be used as a very good control for CFD analysis. The rotor is 500 mm in diameter and 40 mm in chord length, moving at a rotational speed of 3000 rpm to 5500 rpm, resulting in a corresponding Mach Number of 0.23 to 0.42 at blade tip for a room temperature of 288 k; thus, air compressibility must be considered in the simulations. The angle of attack of the blades is 30 degrees. The test rig is installed on a bench, as shown in Figure 1b. The blade, made of carbon fiber, is 500 mm in diameter, 400 mm in chord length, and 1 mm in thickness, as shown in Figure 1c.

The lift and torque values were recorded multiple times and averaged to obtain a final value to reduce error. In this paper, the rotor with a 4:4 rectangular blade (the top one in Figure 1c is adopted as the research subject for its simplicity.

The test stand, as shown in Figure 1d, is located at the center of the MAS chamber. The rotor is driven using a brush-less DC motor with a rated power of 150 W and a rated torque of 0.165 Nm. The lift force and torque are measured using a MINI 40 six-dimensional force sensor.

Though the diameter of the MAS is six times that of the diameter of the rotor, the chamber wall may still have influence on the aerodynamic performance, which is instigated in the following CFD simulations. As the bench is about 250 mm in width, it has to block about a quarter of the projected area of the rotor. In addition, the rotor is only 200 mm above the bench, which is smaller than the 1D (500 mm) of the rotor for a normal helicopter. Under earth conditions, it would have a serious influence on the aerodynamic performance of the rotor due to ground effect.

2.2. Numerical Method

Commercial CFD software Starccm++ was used to model the experiment due to its merit in the generation of a polyhedron grid and its sliding mesh technology. In order to capture the flow structure in a more accurate manner and study the influence of the bench on the aerodynamic performance, after simplifying the blade mounting device, the test bench that may significantly influence the flow structure, thus affecting lift and torque performance, is modeled, as shown in Figure 2. Sliding mesh technology is used in this study. The rotor blades are enclosed in a movable part called the rotation domain, shown as the yellow part in figure, and the other flow field is set as a static fluid domain, called the static domain, which is shown as the gray part in the figure. Since the operation Mach number exceeds 0.4, the boundary condition of the interface between the static domain and the rotation domain was set as free stream to take the air compressibility into account. Detailed sets of grid and boundary conditions are provided in Section 2.

2.2.1. Governing Equations

For the LES turbulence model, the resolved part of the field represents the “large” eddies that are computed numerically, while the sub grid part of the velocity represents the “small scales” whose effect on the resolved field is included through the subgrid-scale model.

The central idea in LES turbulence, where smaller eddies are ignored in a turbulent flow simulation, is mathematically achieved by applying a filtering procedure to the full Navier–Stokes equations, whose instantaneous continuity equation, momentum equation, and energy equation for a compressible fluid can be written as Equations (1)–(3), respectively:

$$\frac{\partial \rho }{{\partial }_{\mathrm{t}}}+\frac{\partial }{\partial {\mathrm{x}}_{\mathrm{j}}}\left[\rho u_j\right]=0$$

(1)

$$\frac{\partial }{\partial \mathrm{t}}\left(\rho u_i\right)+\frac{\partial }{\partial {\mathrm{x}}_{\mathrm{j}}}\left[\rho u_i{u}_j+{p\mathsf{\delta }}_{\mathrm{ij}}-{\mathsf{\tau }}_{\mathrm{ji}}\right]=0$$

(2)

$$\frac{\partial }{\partial t}\left(\rho e_0\right)+\frac{\partial }{\partial x_j}\left[\rho u_j{e}_0+u_{j}p+q_j-u_i{\tau }_{ij}\right]=0$$

(3)

For a Newtonian fluid, assuming Stokes Law for mono-atomic gases, the viscous stress is given by:

$${\tau }_{ij}=2\mu S_{ij}^{*}$$

(4)

where the trace-less viscous strain-rate is defined by:

$$S_{ij}^{*}\equiv \frac{1}{2}\left(\frac{\partial u_i}{\partial x_j}+\frac{\partial u_j}{\partial x_i}\right)-\frac{1}{3}\frac{\partial u_k}{\partial x_k}{\delta }_{ij}$$

(5)

The heat-flux $q_j$ is given by Fourier’s law:

$$q_j=-\lambda \frac{\partial T}{\partial x_j}\equiv -C_p\frac{\mu }{\mathrm{Pr}}\frac{\partial T}{\partial x_j}$$

(6)

where the laminar Prandtl number Pr is defined by:

$$\mathrm{Pr}\equiv \frac{C_p\mu }{\lambda }$$

(7)

To close these equations, it is also necessary to specify an equation of state. Assuming a calorically perfect gas, the following relations are valid:

$$\gamma \equiv \frac{C_p}{C_v},p=\rho RT,e=C_{v}T,C_p-C_v=R$$

(8)

where $\mathsf{\gamma }$, $C_p$, $C_v$ and R are constant.

The total energy $e_0$ is defined by:

$$e_0\equiv e+\frac{u_k{u}_k}{2}$$

(9)

A closed set of partial differential equations can be formed by supplementing Equations (1)–(9) with the gas data for $\gamma$, P_r, $u$, and perhaps R, as well as complementing with boundary conditions.

As for the filtering operation, it is applied through a convolution operation with a filtering kernel. The general procedure for applying a filtering kernel to any function ϕ is defined as follows:

$$\overline{u(x,t)}={\int }_{-\infty }^{\infty }{\int }_{-\infty }^{\infty }u(r,\tau )G(x-r,t-\tau )d\tau dr$$

(10)

The form of this filter kernel is a box filter, meaning the value of the kernel converges to 0 below the length scale limit L and time scale limit T. This follows the same mathematical definition for a filter circuit, where a convolution operation is used to define the relationship between an unfiltered function, an impulse response function, and the final filtered response.

By applying this convolution operation, the effect is to average out any phenomena that occurs on small-length scales and small time scales, thereby eliminating the influence of fast flow fluctuations (small time scales) and small-length scale flow behavior. The above average is generalized to both space and time; however, the filtering procedure could be applied only in space, or only in time, depending on the needs of the simulation.

As a result, the flow field u is redefined in terms of its filtered average and the unfiltered portion of the flow occurring in the small-length scales and small time scales, called the subgrid scale portion. Mathematically, the total flow is defined as a superposition of the two contributions:

$$u_i={\overline{u}}_i+{u^{\prime }}_i$$

(11)

where $u_i$ is the resolvable scale part and ${u^{\prime }}_i$ is the subgrid-scale part. However, most practical (and commercial) implementations of LES use the grid itself as the filter (the box filter) and perform no explicit filtering.

Applying the kernel filtering operation to the subgrid portion yields a result that is identically zero in the entire solution domain. Furthermore, the two sets of data should not overlap, i.e., the two sets are mutually exclusive. Conceptually, this produces two regions where the system can be described—within the highly sensitive spatially/temporally averaged region and in the subgrid region where flow can be described with a separate model that may be computationally less intensive in a CFD simulation package.

The application of this procedure to the Navier–Stokes equations produces two different results depending on whether we are considering compressible or incompressible flow.

For compressible flow, the filtering procedure must be applied to the Navier–Stokes equation of motion and the continuity equation defining the conservation of mass. The resulting filtered equation of motion is:

$$\frac{\partial \overline{\rho }{\tilde{u}}_i}{\partial t}+\frac{\partial \overline{\rho }\widetilde{u_i}{\tilde{u}}_j}{\partial x_j}+\frac{\partial \overline{p}}{\partial x_i}-\frac{\partial {\tilde{\sigma }}_{ij}}{\partial x_j}=-\frac{\partial \overline{\rho }{\tau }_{ij}^r}{\partial x_j}+\frac{\partial }{\partial x_j}\left({\overline{\sigma }}_{ij}-{\tilde{\sigma }}_{ij}\right)$$

(12)

The filtered equation of motion shown above includes differences in sigma terms, which define the response in the fluid viscosity to compression. This equation is sometimes called the Favre-averaged equation of motion for the fluid.

The LES turbulence model and the Reynolds-averaged Navier–Stokes (RANS) model both use some form of averaging to reduce the fundamental CFD equations into a computationally simpler form. Compared with RANS, the interpretation of LES is deterministic and simply splits turbulent behavior into two different regions, each with a different governing model. There are no statistical fluctuations considered in the large-scale region of the system. Some subgrid region models are statistical [28].

This paper modeled the eddy viscosity using the wall-adapting local eddy-viscosity (WALE) model, which can be given by:

$$u_t=\rho {\Delta }_s^2\frac{{(S_{ij}^d{S}_{ij}^d)}^{3/2}}{{({\overline{S}}_{ij}{\overline{S}}_{ij})}^{5/2}+{(S_{ij}^d{S}_{ij}^d)}^{5/4}}$$

(13)

$${\Delta }_s=C_w{V}^{1/3}$$

(14)

$$S_{ij}^d=\frac{1}{2}({\overline{g}}_{ij}^2+{\overline{g}}_{ji}^2)-\frac{1}{3}{\delta }_{ij}{\overline{g}}_{kk}^2$$

(15)

$${\overline{g}}_{ij}=\frac{\partial \overline{u_i}}{\partial x_j}$$

(16)

$${\overline{g}}_{ij}^2={\overline{g}}_{ik}{\overline{g}}_{kj}$$

(17)

where ${\overline{S}}_{ij}$ is the rate-of-strain tensor for the resolved scale defined by:

$${\overline{S}}_{ij}=\frac{1}{2}(\frac{\partial {\overline{u}}_i}{\partial x_j}+\frac{\partial {\overline{u}}_j}{\partial x_i})$$

(18)

where the constant $C_w=0.325$.

2.2.2. Boundary Conditions

Proper boundary conditions play an important role in obtaining good simulation results. Figure 2 shows the domain and boundary condition settings for the simulations. The flow field is divided into a rotation domain and a static domain. The cylinder with a diameter and height of 3 m is used to simulate the MAS, a smaller cylinder that encloses the rotor is used as the rotational domain, and the intersection interface is used at the intersection of the two cylinders. The rotor is placed at the center of the entire computational domain and the bench is set in the static domain. The rotation domain encloses the rotor. The static domain encloses the bench, which is 1 m, 0.3 m, and 0.03 m in length, width, and height, respectively. The rotor has the same dimensions as the experiment, which is 500 mm, 40 mm, and 1 mm in diameter, chord length, and thickness, respectively. The rotor is 0.2 m above the bench.

To simplify the calculation, the fixture, sleeve, and motor that has little influence on the aerodynamic performance is removed in the model.

There are three cases investigated in this study to verify the method, including an investigation of the influence of the bench and the chamber wall, respectively. Boundary conditions are varied according to the cases as follows.

Case 1: to verify the method by comparing with experiment results, all settings are made the same as experiment conditions. The chamber wall and the bench are set as wall condition. The interface is set as freestream condition, with flow speed set to 0 Mach and temperature set to 288 k.

Case 2: to determine the influence of the test bench on aerodynamic performance, the bench is removed from the static domain. All the other settings are the same as case 1.

Case 3: to determine the influence of the chamber wall and temperature, the chamber wall is set as freestream, whose flow speed is also set to 0 Mach, but the temperature is set to 210 k, which is the same as the average temperature of Martian air.

It is worth highlighting that the interface and chamber wall in case 3 are set to freestream rather than velocity inlet because this is conducive to the compressible flow simulation, according starccm++ help files.

Table 1. Properties of Martian air used for calculation in present study.

Parameter	Value
Pressure (Pa)	640
Density (kg/m3)	0.0167
Temperature (k)	288
Speed of sound (m/s)	227
Dynamic viscosity (kg/(m∙s))	1.289 × 10−5
Molecular weight (kg/kmol)	44.01
Specific heat (J/(kg∙K))	831.0
Thermal conductivity (W/(m∙K))	0.0132

provides the parameters used in the simulation, since the established method is verified based on MAS data; therefore, the air temperature was set to 288 k, which is close to room temperature on earth.

3. Method Verification

Method verification must be performed before further research is carried out on the influence of the test bench and chamber wall. The experimental results of the rectangular blade rotor from MAS are shown in

Table 2. MAS Experimental results of rotor with rectangular blades.

RPM	2900	3313	3713	4096	4486	4873	5259
Lift (N)	0.399	0.506	0.624	0.755	0.891	1.037	1.189
Torque (Nm)	0.038	0.046	0.056	0.065	0.075	0.086	0.097

.

Grid quality is one of the keys for good CFD calculation. Since the research subject is under high-speed rotation, with a tip Mach number that exceeds 0.4 in flow of an extremely low Reynolds number, it is very difficult to predict the viscous field and turbulent flow field. Therefore, important and thorough work is required in meshing. The difficulty of meshing in this paper lies in how to choose the appropriate meshing method for the attached surface layer and external meshing method, to set the flow field boundary conditions correctly, and to control the number of meshes to improve the computational efficiency. In this paper, Starccm++ software was used to generate a grid with polyhedral cells for calculation. Due to the complex flow around the rotor blade, especially the leading edge of the blade, which has a certain abruptness and a high Mach number at the blade tip. Therefore, grid refinement is needed in these parts to ensure the accurate capture of the flow characteristics. In this paper, the leading edge and tip of the blades are refined in meshing, especially at the tip, where more than 100 grid points are arranged along the chord direction.

The boundary layer grid is very important to accurately capture the flow characteristics on the surface of the blades. According to the MAS experimental results, the diameter of the rotor is 500 mm and the chord length is 40 mm. Under the maximum rotational speed of 5259 RPM, based on equation 1.9 and the data in

Table 3. Time-averaged lift and torque of different grid size.

Grid Size	Experiment Result	9.69 m	7.43 m	5.67 m
Lift (N)	1.189	1.20	1.23	1.45
Torque (Nm)	0.097	0.116	0.119	0.143
Lift error	-	0.93%	3.4%	22%
Torque error	-	19.6%	22.7%	47.4%

, we can calculate that the Reynolds number is about 5000 at the tip. According to Equation (19), the height of the first layer of the grid near the wall surface is 1 × 10⁻⁶ m when the Y+ value is 1. Thus, in this paper, the height of the first layer of the attached layer grid is set to 1 × 10⁻⁶ m, and the number of attached layers is set to 20. A polyhedral grid is used for volume mesh generation because it has the characteristics of good grid quality and reduces the number of grids; the grid has a total of 9.69 million cells and is seen in Figure 3.

$$y^{+}=\frac{y\rho u_{*}}{\mu }$$

(19)

The grid irrelevance analysis was carried out by controlling the refinement of blade surfaces and edges, as well as the number of boundary layers. For the solver, large eddy simulation, the wall-adapting local eddy-viscosity (WALE) model, and low Y+ wall treatment was adopted. Specifically, a coupled flow equation is employed to consider the compressible flow due to the high Mach number at high speed. The time step is set to $3\times {10}^{-5}$ (approximately 1° for each time step) and the results are seen in Table 2.

According to the results, when the cell number reaches 9.69 million, the prediction of lift is very accurate, which is less than 1%, and the lift prediction error can still be held within 5% at 7.43 million cells. However, when the cell number reaches 5.67 million, the prediction is deteriorated to 22%. Compared with lift prediction, prediction in torque is not so promising: even with 9.69 million cells, the torque prediction has about 20% prediction error. To further study this, in the case of 9.69 million cells, it is discovered that the pressure-induced torque is 0.1132 Nm and the shear stress-induced torque is 0.0028 Nm, which eliminates the possibility that the shear stress is overpredicted. Therefore, this phenomenon needs to be further discussed.

Overall, it is safe to say that the simulation method established in this paper can be used to accurately predict lift and the performance of rotors in Mars air conditions, and that the torque prediction is at an acceptable accuracy for such conditions.

The following calculations are carried out with a setting of 9.69 million cells and the calculations were performed on a computer with an AMD Ryzen 9 3950X CPU and 64 G memory. Each case consumes about 55 G of memory and runs about 72 h to obtain a result.

4. Results and Discussion

Compared with experimental research, CFD simulation provides much more detailed information about the flow field, which is helpful for understanding the flow characteristics of the research subject. The MAS results only provides us with lift and torque values; however, the simulation method in this paper provides us with means to explore the flow characteristics of Mars helicopters more thoroughly. To explore the aerodynamic characteristics of the airflow under MAS air conditions, the detailed flow field of the rotor with a rectangular blade is investigated, and the influence of a test bench on the flow field and the lift and torque performance is also studied and analyzed. Finally, to determine the difference between MAS and real Martian air conditions, the above-mentioned performance of the rotor under Martian air conditions is also evaluated.

This paper compares results of all three scenarios; however, the analysis mainly focuses on the 5259 RPM case, since it has the most sophisticated flow structure. The data and analysis are as follows.

4.1. Simulation Data Analysis

Figure 4 provides the calculation results compared with experiment results from MAS for the rotor with rectangular blades. The case 1 curves are named as With Bench, case 2 as Without Bench, and case 3 as Mars Air condition. It is clear that, for the lift prediction, the results of case 1 agree well with the experiment results, with an error within 2%. However, the torque prediction is not so promising, as there is an approximately 20% deviation for all cases from the experiment results for all CFD calculations. By comparing case 2 with case 1, it is discovered that there is about a 5% difference between lift data. The results of case 3 are in good agreement with case 2. According to the results, the following conclusions can be made. Firstly, the established method can predict the lift of rotors in ultra-low density Martian air conditions in an accurate way, but the torque prediction is not as promising. Secondly, the test bench in the MAS has a little influence on the test results, with only about 5% of difference between values. Thirdly, the MAS can be used to simulate the aerodynamic performance of rotors under Martian air conditions in a very accurate manner, signifying that MAS is a good tool for a Martian helicopter study.

As for the 20% deviation of torque values between simulation results and experimental data, there may be two explanations for it. Firstly, it can be seen from Figure 1b,d that, in addition to the force sensor, the shaft is also connected to the sleeve by solid contact between the shaft and the sleeve. Therefore, the torque may be transferred to the bench through the sleeve due to the friction between the shaft and the sleeve. Therefore, the torque applied on the force sensor is lowered under this circumstance. Secondly the torque values are very small, only creating a lift value of about 1 N, approximately two eggs. Therefore, a small measurement error will amplify the deviation. Thus, the friction-induced error may be amplified in a proportion indication.

In addition to the data analysis, further study in the flow field needs to be conducted to explore the flow mechanisms.

4.2. Flow Field Analysis of Case 1

Figure 5 shows the Mach number streamline (a) of the whole flow field and the velocity streamline (b) around the rotor. It can be seen from Figure 5a that the whole flow field is very complex and consists of multiple vortex rings. After the downstream airflow passes through the rotor disc, it is divided by the test bench and forms two large vortex rings up and down. The vortex rings shrink into smaller vortex rings and disappear as time passes by. The upper one is stronger because the blades create a low-pressure area over the rotor, drawing more air flows. Small vortexes also generate along the edge of the test bench. Notably, although the rotor only reaches maximum Mach number of 0.42 at 5259 RPM rotational speed, the airspeed within the flow reaches 220.9 m/s (Ma = 0.9847), indicating that the low-density Martian air is highly compressible and may exhibit complex flow characteristics. From Figure 5b, we can see that vortexes generate at the leading edge from the tip side of the blade due to high pressure and move along the blade span-wise fast and chord-wise slowly, creating low pressure zones that generate lift. Airflow from a high-pressure zone below the lower surface passes the leading edge and joins the acceleration of airflow on the upper surface.

As for the influence of the bench, it can be seen from Figure 5a that the maximum Mach number of the flow nearly reaches 1; however, the flow speed quickly decreases along the streamline and becomes close to zero at the far corner below the bench. After passing the rotor disk, the airflow impacts the bench by a Mach number of approximately 0.2. Part of the flow passes the edge of the bench and down, joining into the circulation. The other part bounces back due to the impact and curls between the rotor and the bench, creating a high-pressure zone in between—this is the reason why case 1 has a 5% higher lift. This indicates that the bench does have some influence on the lift performance of the rotor. Further research can be made to reveal how the height and bench width affect the results.

Figure 6 shows the slice contours of the pressure and Mach number on the upper surface of a blade. It can be seen that there is a large low-pressure zone created by vortexes over the outer half of the upper surface of the blade. From the Mach number contours, we can see clearly that the vortex generates at the leading edge close to the blade root, attached on the blade and moves along the blade span-wise. The airspeed within the vortex accelerates to maximally 0.985 Mach during the movement and a large vortex grows and begins to detach at 70% of the blade span-wise from the root. It may also split into some smaller vortexes and move along the blade to the root. This reveals that, under the low-density Martian air conditions, the flow is more complex, and the airflow is much easier to increase to a high Mach number. Therefore, air compressibility must be taken into account during CFD research.

Figure 7 shows the pressure contour of one blade of the rotor. It can be seen that, under such low-density air, even for the air flows at a trans-sonic speed, the difference between maximum and minimum pressure is only about 360 Pascal, which is extremely small compared with the case in Earth’s air conditions. This is the reason why the rotor only generates a lift of less than 2 N. The high-pressure zone mainly lies around the blade tip at the leading edge, while the low-pressure zones cover more of the middle part of the blade. Nearly 30% part of the blade close to the root of the blade contributes hardly any lift, and this reveals that blade topology can be made to reduce rotor weight in the actual design of a Mars helicopter. Furthermore, it also indicates that simplifying the model by removing the fixtures has little influence on the research.

4.3. Flow Field Analysis of Case 2

From Figure 4, it can be seen that the test bench has an influence on the structure of the whole flow field by dividing the airflow that eventually forms into two vortex rings. To know its actual influence on the lift and torque performance of the rotor is important because it may affect the accuracy of the experiment. Therefore, the simulations with the test bench removed were performed to explore its influence on the flow field and the lift and torque performance.

Figure 8 presents the streamline and slice Mach number contours of the flow field of case 2. It can be seen that, without blockage of the test bench, the airflow moves directly down to the bottom of the chamber after passing the rotor disc and then flows around the wall, forming a giant vortex ring. The vortex ring diminishes into a smaller ring within the big ring and then disappears. Some air is drawn by the low-pressure zone created by the rotor disc and participates in the circulation. From the slice Mach number contour, it can be seen that, compared with case 1, case 2 has a larger maximum Mach number but smaller vortex intensity. Therefore, it has a weaker low-pressure zone over the upper surface of the blades.

4.4. Flow Field Analysis of Case 3

Figure 9 shows the streamline of the flow field of the case under actual Martian air conditions. Compared with the former two cases, this case has no vortex ring due to the reason that it is not confined in space. The maximum Mach number is slightly increased due to the lower temperature. It has a simpler vortex structure on the upper surface of the blades. The vortex forms at the tip area and moves to the root area and gradually weakens in intensity. From all streamline figures, it is obvious that the airflow speed reduces rapidly after the vortexes leave the rotor disc; thus, the size of the MAS is large enough to eliminate the influence of the chamber wall on the aerodynamic performance. Although the chamber wall does create vortex rings, the intensity is low.

Figure 10 shows the vorticity magnitude contour of case 3. It can be seen clearly from the contour that the vorticity at the blade tip is much stronger and more complex than that at the root. Obvious vortexes generated from the leading edge and blade tip can be observed. The vortex generated from the leading edge moves along the chord direction and up and then dissipates quickly after shedding from the trailing edge. The vortex generated from the blade tip moves along the chord direction and span-wise direction toward the root. The vorticity structure at the blade tip is much more complex than that at the center part of the blade. The reason for this is that the high-pressure zone is highly centralized at the leading edge of blade tip area, similar to the lower surface of Figure 7. Therefore, the pressure difference between upper surface and lower surface of the blade is relatively significant, especially along the chord for the tip edge. This may cause a vortex with great intensity, up to 1.2 × 10⁷, as shown in the contour. While the low-pressure zone above the upper surface covers a large area, the pressure difference is relatively small along the chord and the span; thus, the vortex generated from the leading edge prolongs the forming of a large and stable vortex with a simpler structure. A complex vortex structure with great intensity may consume more energy to generate the same lift, decreasing aerodynamic efficiency. Therefore, one interesting topic worth further investigation would be the designing of a structure to breakdown the highly centralized high-pressure zone, so as to lower the intensity of the vortex at the blade tip area. This also demonstrates that the established method can predict the small and sophisticated flow structure of the airflow with ultra-low air density and a low Reynolds number.

5. Conclusions

In this paper, the aerodynamic performance of a rotor with rectangular blades under ultra-low density Martian air conditions is studied numerically based on experiment results from a Mars Air Simulator (MAS). A simulation scheme using a large eddy simulation solver is established and the influence of test bench and chamber wall of the MAS is investigated. From this, the following conclusions can be made.

1. The established method can be used to accurately predict the lift performance of the helicopter rotor with about 1% error; however, the torque prediction is not so promising, possibly due to a friction-induced error in the experimental results;

2. The Mars Air Simulator can be used to simulate Martian air conditions in an accurate manner, the fixture and chamber wall has little influence on the lift performance prediction, while the test bench has about 5% influence. Topology design can be made to reduce blade weight by removing some of the blade area close to the root;

3. The rotor, with a maximum Mach number of 0.42, creates a maximum Mach number up to nearly 1 in the airflow; therefore, compressibility must be taken into account in CFD simulations of low-density Martian air conditions to improve accuracy, and airfoil optimization needs to be performed to mitigate this phenomenon.

This paper may provide some guidance for future experimental and CFD studies on Martian helicopters. For example, the influence of the test bench can be further studied to eliminate its influence with a new design set. A new blade topology can be designed after analyzing the flow field and pressure distribution to improve efficiency.