1.

INTRODUCTION

The Solar Array Drive Assembly, internationally known as SADA. As the main driving mechanism of the solar cell array, its functions include supporting the solar wing, rotating the solar cell array towards the sun to obtain maximum illumination, transmitting electrical power and signals between the solar cell array and satellite bodies, and minimizing the volume and mass of the solar cell array as much as possible [1]. The harmonic reducer is an important component in the SADA device, mainly completing the transmission of motion and power, as well as the task of mechanism connection. It is the key to ensuring the accuracy, load-bearing capacity, motion safety, and motion stability of aerospace machinery during the motion process. Compared to ground environments, space environments experience significant temperature variations and torque fluctuations, often in low-speed and light-load conditions. Therefore, studying the mechanics and fatigue of harmonic reducers in space can guide the analysis of failure mechanisms, performance evaluation, and lifetime prediction of active components in various propulsion systems.

In terms of the dynamic and fatigue analysis of harmonic reducers, in 2013, Yan Feng et al. established a fatigue model based on transient analysis results to predict the fatigue life of flexible gears [2]. In 2016, Li Shuting conducted a study on the stress and fatigue strength calculation of the bottom plate of a flexible gear by establishing a mechanical model for contact analysis of harmonic reducers, proposing a method to evaluate the fatigue failure strength of the bottom plate [3]. In 2017, Xia Tian et al. performed fatigue analysis on flexible gears using finite element analysis software and compared the results with actual fatigue failure cases, identifying the gear ring and flange at the bottom of the disc as the most susceptible locations for fatigue failure [4]. In 2018, Ye Nanhai et al. investigated the influence of structural parameters of the flexible gear on fatigue life [5]. In 2021, Huang Qingwen et al. considered the influence of small stress and predicted the service life of flexible wheels based on the modified P-S-N curve [6].

Currently, when analyzing harmonic reducers, researchers often simplify the tooth profile to facilitate calculations and improve convergence. This paper focuses on studying the stress and deformation of harmonic reducers used in space environments under low-speed light-load conditions. Based on this, fatigue analysis is conducted, and a comparison is made between the results of simplified tooth profile analysis and refined full-tooth modeling.

2.

SPATIAL HARMONIC TOOTH PROFILE ANALYSIS

In the process of harmonic gear transmission, the engagement between the flexible gear and the rigid gear is very complex due to the presence of elastic deformation in the flexible gear, which is influenced by the deformation of the neutral layer in the flexible gear and the tooth profile equations of the flexible gear and the rigid gear. Regarding the tooth profile equations of the rigid gear and flexible gear in harmonic reducers, numerous different tooth profiles have been proposed by scholars both domestically and internationally, including the involute tooth profile proposed by the Soviet Union, the S-shaped tooth profile proposed by Ishikawa of Japan [7], the double circular arc tooth profile [8], as well as the CTC tooth profile and P-shaped tooth profile derived from the double circular arc tooth profile. The double circular arc tooth profile is less likely to generate sharp points and tooth interference, and it has high transmission efficiency, making it widely used in space harmonic reducers. In this paper, a three-dimensional model is established based on the double circular arc tooth profile, and the full-tooth model is used for finite element analysis.

The double circular arc tooth profile consists of two circular arcs and a tangent line. To address the interference issue during engagement, a commonly adopted approach in modeling is to specify the tooth profile equation for either the flexible gear or the rigid gear and solve for the other segment’s tooth profile equation through conjugate calculations. The tooth profile of the flexible gear in this paper is given in the following figure 1:

Figure. 1

Flexible gear Tooth Profile

Where segments AB and CD are circular arcs, and segments EA and BC are straight lines. The tooth profile equation for segment AB is as follows:

where δ represents the angle between the common tangent line and the y-axis.

The tooth profile equation for segment BC is as follows:

The tooth profile equation for segment CD is as follows:

Referring to the XBS-50 harmonic reducer, solving the tooth profile equation for the flexible gear yields the parameter values shown in the following table 1:

Table 1.

Flexible gear tooth parameters

During the harmonic transmission process, it is necessary to consider the influence of the elastic deformation of the flexible gear on the rigid gear. Therefore, the envelope method is chosen to solve the tooth profile of the rigid gear, transforming the elastic deformation of the flexible gear into a part of the conjugate motion between the rigid gear and the flexible gear. Ultimately, the conjugate tooth profile is obtained using the envelope theory [9]. Based on the engagement theory, the following assumptions are made: the shape of the flexible gear’s median line changes while the perimeter remains constant; the shape of the teeth on the rigid gear and the flexible gear does not change during the engagement process; the wave generator is completely rigid, with the flexible gear as the input and the rigid gear as the output. The motion of each point on the flexible gear can be decomposed into translation along the deformation curve and rotation around a point. By applying a transformation matrix, the coordinate system of the flexible gear can be transformed into the coordinate system of the rigid gear [10]. Therefore, the tooth profile of the flexible gear in the coordinate system of the rigid gear can be represented by the following equation:

Where x_g, y_g represent the positions in the coordinate system of the rigid gear, x_r, y_r represent the positions in the coordinate system of the flexible gear, ρ is the polar radius of the original curve, γ is the angular difference between the two wheels when the flexible gear drives the rigid gear to rotate, and φ₁₂ is the angle between the normal of the point before and after the deformation of the flexible gear(the angle between φ₁ and φ₂). When the flexible gear rotates at an angle of φ₁, it drives the rigid gear to rotate φ₂. The meshing principle is shown in the following figure 2.

Figure. 2

The meshing principle of harmonic drive

According to the envelope method, the tooth profile of the rigid gear must be completely enveloped by the curve family of the flexible gear’s teeth. Therefore, the points on the rigid gear satisfy the following equation:

Using an iterative method in MATLAB to solve the partial differential equation, the discrete points on the curve of the rigid gear are obtained, select 12 points shown in the following table 2:

Table 2.

Fitting points of rigid gear tooth profile

The discrete points are fitted to obtain the tooth profile equation for the rigid gear as follows:

convex arc segment:(x + 0.247)² + (y − 40.4261)² = 0.2701²

concave arc segment: (x − 0.926)² + (y − 40.396)² = 0.5145²

The key component parameters for the flexible gear are in the following figure 3 and table 3:

Figure. 3

Flexible gear plane figure

Table 3.

Flexible gear parameters

The number of teeth on the flexible gear is 200, and the number of teeth on the rigid gear is 202. The wave generator, flexible bearing, flexible gear, and rigid gear are assembled to form a three-dimensional model as shown in the figure 4:

Figure. 4

Harmonic reducer assembly

For comparison, a simplified model of the tooth section is created as shown in the upper part of the following figure, while the rest of the model remains the same as the original model. The refined tooth models is shown in the lower half of the figure 5.

Figure. 5

Simplified tooth profile models (up) and refined tooth models (down)

3.

REFINED MODEL FINITE ELEMENT ANALYSIS

The current finite element analysis research on the refined model of harmonic drives is not sufficiently comprehensive, especially regarding the dynamics and fatigue analysis of spatial harmonic drives operating at low speeds and light loads. This paper will evaluate the motion state of spatial harmonic drives based on the results of finite element mechanical analysis and study their potential failure modes.

The wave generator and rigid gear, excluding the gear teeth, are set as rigid bodies, while the flexible gear, flexible bearings, and gear teeth of the rigid gear are set as flexible bodies. The material parameters for each component are listed in the table 4:

Table 4.

Material parameters of harmonic reducer

3.1

Static Analysis

3.1.1

Contact Connection Settings

Based on the actual motion and contact conditions of the harmonic drive, five pairs of contact pairs are set as shown in the table 5, all of which are face-to-face contacts. The most influential factor in the contact problem is the normal stiffness value, which can be taken between 0.1 and 1. A smaller value leads to better convergence but may result in contact penetration issues. Due to the complex structure of the harmonic drive and the involvement of a large number of meshing teeth, a stiffness value of 0.1 is chosen to ensure convergence, and contact penetration is observed in the results. Additionally, the small sliding option is disabled, and stiffness is updated at each iteration with automatic time step control during time integration. The connecting member is set as the rotation of the wave generator with respect to the ground.

Table 5.

Contact Region Settings

Contact Region	Type	Formulation	Frictional Coefficient	Normal stiffness
Wave generator & Flexible bearings inner ring surface	Frictional	Augmented Lagrange	0.12	0.1
Flexible bearings inner ring & Flexible bearing rollers	Bonded	MPC	/	/
Flexible bearing rollers & Flexible bearings outer ring	Frictional	Augmented Lagrange	0.08	0.1
Flexible bearings outer ring & Flexible gear inwall	Frictional	Augmented Lagrange	0.08	0.1
Teeth of the rigid gear & Teeth of the flexible gear	Frictional	Augmented Lagrange	0.12	0.1

3.1.1

Meshing

The flexible bearings are assigned a tetrahedral mesh, while the remaining parts are assigned triangular meshes. Key components are subjected to mesh refinement. The mesh size for the contact surfaces between the rigid gear and flexible gear teeth is set to 0.3mm. The mesh size for the contact between flexible bearing rollers and flexible bearings outer/inner ring is set to 1mm. The size for the remaining contact areas is set to 2mm, while non-contact areas use the default size.

3.1.2

Boundary Conditions

To simulate the real environment of a spatial harmonic drive application, the outer ring of the rigid gear is fixed, and the remote displacement of the flexible gear is fixed axially. The wave generator is constrained by its connecting member. A light load condition is simulated by applying a moment of 100N∙mm to the bottom flange of the flexible gear.

3.1.3

Analysis Settings

The load is set to two steps, with the first step simulating the assembly process of the wave generator for 0.1 seconds without applying any load. The second step takes 1 second and applies the load. Automatic step on, with a maximum of 100 sub-steps. Enabling weak springs can eliminate rigid body deformations. Since the flexible gear undergoes significant deformation, the large deformation option is turned on. To improve convergence speed, the line search option is enabled, and the Newton-Raphson option is set to “full”. The convergence criteria can be relaxed appropriately, with deformation convergence and rotation convergence turned off, while force convergence and torque convergence tolerances are adjusted to 1.5%.

3.1.4

Static Analysis Results

The deformation nephogram is shown in the figure 6 left. Due to the assembly of the wave generator, the flexible gear and flexible bearings experience deformation at the long axis, with a maximum deformation of 0.61226mm occurring at the front end of the flexible gear teeth. At the short axis, there is a gap between the outer ring of the flexible bearing and the inner ring of the flexible gear, indicating frictional wear.

Figure. 6

Deformation nephogram (left) and stress nephogram (right) of static

The stress nephogram is shown in the figure 6 right, with the maximum stress of 495.25 MPa occurring on the inner ring of the flexible bearing. The maximum stress on the flexible gear occurs at the root of the flexible gear teeth that mesh with the rigid gear teeth, with a stress value of 459.69 MPa. It can be observed that, under light load conditions, compared to harmonic drives used in robots, the flexible gear teeth of spatial harmonic drives experience lower stresses at the root. The most probable failure location is in the flexible bearings, including damage to the inner ring of the flexible bearing and lubrication failure, and fatigue failure at the root of the flexible gear teeth.

The stress nephogram at the meshing point of the gear teeth is shown in the following figure 7, indicating no contact penetration, thus validating the reasonable setting of the contact normal stiffness.

Figure. 7

The stress nephogram of teeth mesh

In the results of Statics analysis, the stress at the flexible bearing and the flexible gear tooth reached more than 400 MPa. In order to better identify the failure position of the harmonic reducer, transient dynamic analysis was carried out to simulate the movement process of SADA mechanism in space.

3.2

Transient dynamic analysis

3.2.1

Contact Connection Settings

The contact pairs are set up similarly to the static analysis. The connecting member is set as a rotational connection between the wave generator and the ground, a fixed connection between the outer ring of the rigid gear and the ground, and a rotational connection between the inner ring of the flexible gear and the ground.

3.2.2

Meshing

Tetrahedral meshes are used for the bearings and the outer ring of the wave generator, while triangular meshes are used for the remaining parts. The mesh size for the contact surfaces between the rigid gear and flexible gear teeth is 0.3mm. The mesh size for the outer ring of the wave generator and the inner ring of the flexible gear is 3mm. The contact areas have a mesh size of 1mm, while non-contact areas use the default size.

3.2.3

Boundary Conditions and Analysis Settings

Two load steps are defined: the first load step, from 0s to 0.5s, represents the assembly process of the wave generator, and the second load step, from 0.5s to 2s, represents the rotation of the wave generator. The initial time step and minimum time step are set to 10, while the maximum time step is set to 250. To simulate a low-speed condition, a rotational speed of 0.2 rad/s is applied to the wave generator in the second load step. The maximum iteration steps are adjusted to 1000 through a command stream to improve convergence. The remaining settings are the same as in the static analysis.

3.2.4

Transient dynamic Analysis Results

The wave generator starts rotating from the first load step, and the deformation and stress are analyzed at the second, where the maximum values occur, the deformation nephogram is shown in the figure 8 left. The maximum deformation during the rotational motion is 0.64632mm, appearing on the front end of flexible gear teeth with the long axis of the wave generator. The deformation exhibits periodic variations as the wave generator rotates. Additionally, there is slight deformation between the wave generator and the inner ring of the flexible bearing during the motion, indicating the presence of frictional wear.

Figure. 8

Deformation nephogram (left) and stress nephogram (right) of transient dynamic

The stress nephogram is shown in the figure 8 right, with the maximum stress of 606.46 MPa occurring at the inner side of the flexible gear corresponding to the long axis of the wave generator. The maximum stress at the root of the flexible gear teeth is 584.49 MPa. The stress at the meshing point between the rigid gear and flexible gear teeth is approximately 404 MPa. This indicates that under low-speed conditions, during the movement of the flexible gear, it bears alternating loads, resulting in high stress. The root of the teeth at the meshing point is prone to damage, and the inner side of the flexible gear and the outer ring of the flexible bearing are prone to wear. The stress nephogram at the meshing point of the gear teeth is shown in the following figure 9.

Figure. 9

The stress nephogram of teeth mesh

4.

COMPARISON OF SIMPLIFIED MODEL FINITE ELEMENT ANALYSIS

To compare the influence of simplified tooth profiles on the analysis results, a simplified model is subjected to static analysis. The preprocessing steps are identical to thefine-grained model, and the static analysis results are obtained as follows in the figure 10 and 11.

Figure. 10

Deformation nephogram of Simplified Model

Figure. 11

The stress nephogram of Simplified Model

The maximum deformation is 0.38462mm, occurring at the inner ring of flexible bearing. The maximum stress is 409.11 MPa, occurring at a location similar to that in the fine-grained model. Comparing with the fine-grained model, it can be observed that the deformation and stress distribution in the deformation and stress nephograms are relatively similar, but there are significant differences in numerical values. The maximum stress value differs by 86.14 MPa, with an average stress difference of 52.48 MPa. This indicates that the simplification of the tooth profiles has a certain impact on the analysis and calculation results. The simplified model shows lower deformation and stress values compared to the finegrained model, which in turn affects fatigue analysis and life prediction.

5.

FATIGUE ANALYSIS

Based on the mechanical analysis results, the results are imported into nCode. The SN Constant module in nCode is used for analysis, to simulate the actual working condition of the solar panel deployment, a load type selected with “Constant Amplitude” cycling between -1 and +1, simulating the reciprocating motion of the solar panel deployment at 72°and folding up. The stress fatigue calculation method is set to Standard, which utilizes the standard S-N curve to calculate damage.

5.1.1

Material Settings

Edit the “Material Map” option to define the materials and obtain the S-N curve based on the material’s tensile strength. To obtain a more accurate material S-N curve, it is necessary to correct for the yield strength limit. The S-N curves of the material before and after the correction are shown in the figure 12.

Figure. 12

S-N curve of 30CrMnSiA (left) and 45 # steel (right) material

5.1.2

Solver Settings

The stress combination is used to apply the results of finite element analysis to the material’s S-N curve. The stress combination method is set to “Critical Plane”, which uses rainflow counting on multiple planes. The formula is as follows:

Due to the fact that the S-N curve used for fatigue calculations is based on the condition of zero mean stress, while in actual calculations there are situations where the mean stress is not zero, and within a certain stress range, a positive mean stress will reduce the fatigue limit, while a negative mean stress will increase the fatigue limit. Therefore, it is necessary to make corrections for non-zero mean stress conditions in order to convert the actual stress state of the material to the stress ratio state during testing based on the S-N curve [11]. This process requires the use of the Goodman theory. In order to handle the data using statistical analysis methods and express the fatigue performance of the material more accurately, a survival rate of 50% is set.

5.2

Fine-Grained Model and Simplified Model Fatigue Analysis Results

5.2.1

Fine-Grained Model Fatigue Analysis Results

The fatigue analysis results are as follows in the figure 13: Under low-speed light-load conditions, the weak point of fatigue life in the harmonic reducer primarily occurs in the flexible gear teeth with a fatigue cycle count of 15300 cycles. That means the harmonic reducer unfolds and folds the solar panel 15300 times, and the material survival rate reaches below 50%. The weak points of fatigue life are shown in figure 16, with a total of 9 points distributed at the root of the flexible gear teeth (MAT-2) and one point distributed on the inner ring of the flexible bearing (MAT-26), with a fatigue cycle count of 2.068×104 cycles, and there is a certain risk of fatigue damage at the bottom of the flexible gear barrel, while the remaining parts are relatively safe.

Figure. 13

Fatigue Analysis Results of Harmonic Reducer

Figure. 14

Weak points in fatigue life of harmonic reducers

5.2.2

Simplified Model Fatigue Analysis Results

Based on the results of static analysis, the results were imported into nCode. The SN Constant module in nCode was used for analysis, with the same pre-processing as the fine-grained model.

The fatigue analysis results obtained are as follows in the figure 15: The weak point locations in terms of fatigue life are similar to those of the fine-grained model. The lowest fatigue life occurs at the root of the gear teeth in the meshing area of the flexible wheel, with a fatigue cycle count of 16,170 cycles. Among the ten positions with the lowest fatigue life, nine are located at the root of the flexible wheel teeth (MAT-2), and one is located in the inner ring of the flexible bearing (MAT-4), with a fatigue life of 21,190 cycles, all greater than the fatigue life values obtained from the refined modeling of gear teeth. And there is a certain risk of fatigue damage at the bottom of the flexible gear barrel.

Figure. 15

Simplified model fatigue analysis results

Figure. 16

Weak points in fatigue life of simplified model

5.3

Comparison of fatigue analysis results between the two

For a better comparison of the fatigue life of key components in the harmonic reducer, ten minimum life points were selected for comparison in the tooth root of the flexible wheel and the inner ring of the flexible bearing for both models, as shown in Figure 17. In comparison, there is a small difference in the minimum fatigue life values, but the simplified tooth profile and the overall fatigue life analysis of the flexible bearing in the simplified model are significantly greater than those in the refined model, making fatigue failure less likely to occur. The life at the bottom of the flexible wheel cylinder is compared as shown in Figure 18, and the life in the simplified model is much smaller than that in the refined model, with a more concentrated fatigue location. This indicates that the simplification of the tooth profile has had a certain impact on the fatigue analysis of the harmonic reducer, thereby affecting the determination of fatigue failure locations and life prediction.

Figure. 17

Comparison of weak points of Fine-Grained and simplified model

Figure. 18

The fine-grained model (left) and simplified model flexible gear barrel bottom (right)

6.

SUMMARY

In this paper, a comprehensive tooth-level fine-grained modeling was conducted on the harmonic reducer used in space applications. The fine-grained model was subjected to static and transient dynamic analyses using ANSYS Workbench. The simulation results were then imported into ANSYS nCode for fatigue analysis, taking into account the material’s S-N curve. The following conclusions were drawn: