This paper represents the application of finite element analysis for the strain wave gear with modified conjugate tooth surfaces. The unmodified tooth profile is designed at a cross section derived from the fundamental kinematic model of the strain wave gear. The conjugation of the tooth profiles has been verified by the plane stress finite element model. Under nominal load condition, the flexspline has elastic deformation compared with its unloaded shape. The flexspline tooth surface is longitudinally crowned to have a localized contact pattern. Such longitudinal crowning amounts are determined from the deformation of the flexspline in order to avoid assembling interference under no load condition. To analyze the contact pattern under nominal load condition, the finite element model of manufactured tooth surfaces with modification is established. The simulation results show that no severe stress edge contact exists for the modified strain wave gear. And the simulation results are compared with experiments of contact pattern for verification.
Strain Wave Gear is a special type of mechanical gearing system that has unique characteristics compared with cycloidal drives or planetary gears. It has three basic components with advantages of compactness, zero backlash, high precision, and high gear ratio from 30:1 to 320:1. It’s the key component for a robotic arm joint. In recent years, the availability of a robotic arm increases substantially due to its important role in automation, so the high-performance strain wave gear is also needed. The gear industry has a well-established gearing theory [1, 2], design code [3, 4], and design simulation software [5, 6] to improve gear-transmission performance. However, the lack of similar tools restrains the development of the strain wave gear. The objectives of this research are as follows:
- Build a finite element model of the strain wave gear assembly with crowned tooth profile.
- Use a plane stress finite element model to verify conjugation of the designed tooth profile.
- Study the deformation of the flexspline compliant cup by finite element analysis, which is used to calculate the lengthwise crowning amount for the hobbing process.
- Study the contact pattern of the finite element model and verify the result by using contact pattern experiment.
The three main components of a strain wave gear are the wave generator, flexspline, and circular spline as shown in Figure 1. The wave generator inserts into the open end of the flexspline cup. The flexspline will deform into an elliptical shape at the open end and keep a circular shape at the other end. The open end of the flexspline cup has teeth on the external surface, and the circular spline is a rigid ring gear. The teeth will mesh between the circular spline and flexspline along the major axis of the ellipse, shown as the roller bearings in Figure 1. The strain wave gear has two degrees of freedom, which is analogous to a planetary gear train. The gear ratio can be calculated from
Subscript F, W, and C refer to the flexspline, circular spline, and the wave generator, ω, is the angular velocity of the component, and N is the number of teeth. For a robot arm joint, the wave generator is driven by the servo motor, and the flexspline and circular spline are connected to the fixed link and moving link. The wave generator and fixed link are two inputs, and the output moving link velocity can be calculated from the above equation.
Unlike a planetary gear train, the flexspline is not a rigid body but a compliant cup with elastic deformation [7, 8]. Teeth on the flexspline have variant instantaneous velocities, which are governed by the shape of the wave generator. The motion of a tooth on the flexspline has a radial displacement, u, circumferential displacement, v, and oscillating angle, φ . The theoretical conjugate tooth profiles for the flexspline and circular spline are derived from the following procedure as in reference . Design data for the gear is in Table 1.
Selecting a wave generator shape solves the motion of a tooth on the flexspline with respect to the circular spline.
Select a double circular tooth profile  for the flexspline and calculate coordinates of points on the profile in the flexspline coordinate. Double circular profile will increase the contact ratio under the motion shown in Figure 2.
Calculate trajectory of the points under the relative motion between the flexspline and circular spline by coordinate transformation.
Find the envelope of the trajectory point cloud by using the analytical method  or graphical method .
The conjugate profiles are assigned to a cross section along the longitudinal direction of the teeth.
Figure 2 shows the motion of one tooth on the flexspline with respect to the circular spline. The conjugate designed cross section will have theoretical conjugation between the circular spline and flexspline. In other words, the two profiles will be perfectly tangential to each other during the meshing process.
Plane Stress Simulation
To verify the conjugation, a plane stress finite element model is developed by the following procedure:
At the conjugate designed cross section, the teeth are modeled and further discretized into sub regions for brick mesh as shown in Figure 3. Finer meshes are used at the contact region and root fillet in order to calculate contact stress and bending stress. Coarser meshes are used at the rest regions to reduce calculation time . A mesh size convergence study has been done for the criteria of deformation.
Contact pairs are defined between the wave generator and flexspline inner surface with initial penetration at the major axis as shown in Figure 3(a), gap at the minor axis. The initial penetration will be ramped during the first load step. Correct contact between the wave generator and flexspline inner surface will be established at the end of the first load step. The contact condition is an augmented Lagrange method with no friction.
Contact pairs are defined between the teeth of the flexspline and circular spline. The contact elements are deactivated at the first load step and then reactivated at the second load step after the contact between the wave generator and flexspline are established. This element-birth-and-death technique is employed in simulating the addition of layers for additive manufacturing in reference . The contact condition is an augmented Lagrange method with no friction.
Figure 4 is the plane stress model results for the first load step. The initial penetration between the wave generator and flexspline are solved by the contact pair. Though no torque load is added, the stress in the flexspline is caused by its shape change. Its bending stress is only decided by the wave generator shape. The contact between teeth happens at both right and left sides of the flexspline. Furthermore, the teeth in the first quadrant has a right side tooth profile in contact as in Figure 4(a). The teeth in the second quadrant in Figure 4(b) has a left side tooth profile due to the symmetry under no load condition. For each pair of teeth, there is clearance like a rigid gear. However, the strain wave gear will have zero backlash due to the double side contact.
As shown in Figure 4, the profile is tangent to each other at every contact point. Although the plane stress simulation is static with no component moving, the instant shown in Figure 4 represents the input periodic motion of wave generation since the meshing between teeth happens along the entire circumference. The contact ratio of the strain wave gear is as high as 24. If the wave generator rotates clockwise by angle 2π/n, in which n is an integer from -12 to 12, it’s equivalent to rotate the whole assembly by the same angle. The static model shows 24 contact positions of a pair of teeth to verify the conjugation. If the tooth profiles don’t have conjugation, the same 24 pairs of teeth will have extra clearance or interference instead of tangency. Since the contact ratio of the strain wave gear is high, the static plane stress results show enough contact positions to verify the kinematic conjugation between the tooth profiles.
Figure 5 shows the contact status between teeth when a counterclockwise torque load is applied to the flexspline. In the second quadrant of the flexspline, 15 pair of teeth are in near contact status  compared with eight pair of teeth at the opposite side due to the deformation of the flexspline under torque. For the assembly, the deformation will be contributed by the teeth deformation and the compliant cup deformation.
Compliant Cup Deformation
The deformation of the flexspline compliant cup is three dimensional, which will affect the teeth meshing at other cross sections other than the designed cross section. In reference , a fully conjugate tooth surface is found from the kinematic model under no load condition. However, this paper will use a different approach to design the modified tooth surface with consideration of lengthwise crowning for the hobbing process.
A cylindrical coordinate is shown in Figure 6(a). The origin of the coordinate is at the center of the rigid end of the compliant cup. The Z-axis is along the longitudinal direction of the cup. The X-axis points to the major axis of the elliptical wave generator. The Y-axis is the angular coordinate. According to the coordinate defined, the deformation of the compliant cup can be broken down into three components. Radial deformation u along the X direction, circumferential deformation v along the Y direction, and oscillating angular deformation φ measured from the X-positive direction. Components u, v, φ are the same as the displacement mentioned in session 2. The deformation can be solved analytically by the given wave generator shape for the points at each cross section’s neutral layer as in reference . They are functions of the cross section’s longitudinal position. In other words, a different cross section along the longitudinal direction has a different deformation. The assumption of the analytical method is that the deformation is totally governed by the wave generator geometry under no load condition. In this paper, finite element model is used to analyze the deformation under any load condition, and teeth meshing will be considered for the next chapter.
As shown in Figure 6(b), the compliant cup will deform into a three-dimensional shape. Figure 6(c) shows the contact pressure between the inner surface of the compliant cup and outside surface of the wave generator. The contact happens at two places: one is toward the rigid end of the cup along the major axis, and the other one is toward the open end of the cup along the minor axis. So, the deformation of the cup is found to be not totally governed by the wave generator shape, but also affected by the contact status between the wave generator and flexspline compliant cup inner surface .
Figure 7 shows the major and minor axis’s radial deformation for the compliant cup’s different cross section along longitudinal direction Z. The wave generator has an elliptical shape with a circumference the same as the inner surface of the cup before deformation. The major and minor axis of the wave generator has the designed values comparing with the actual deformed values shown in Figure 7.
Since the contact between the wave generator and the compliant cup is not uniform, the open end of the cup doesn’t have the same shape as the wave generator. Three critical cross sections are defined along the tooth lengthwise direction. At the designed cross section, the deviation between the actual major axis radial deformation and designed value is um. At the heel cross section, the deviation between actual minor axis radial deformation and designed value is uh. At the toe cross section, the deviation between actual major axis radial deformation and designed value is ut. Deviation um, uh, and ut will cause interference between the flexspline tooth surface and circular spline tooth surface. So, longitudinal modification is added to the flexspline tooth surface. The crowned amount can be calculated from the compliant cup radial deformation for the three critical cross sections as in Figure 8. The profile has crowned amount um, uh, and ut at the three critical cross sections by the plunging motion of the hobbing cutter. The finite element model’s deformation result solves um = 19 µm, uh = 64 µm, and ut = 62 µm for the given strain wave gear.
Loaded Tooth Contact Pattern
The strain wave gear has conjugate tooth profiles at a designed cross section and is further longitudinally crowned. It will be free from interference for assembly. Due to the high contact ratio, periodic motion and the ring shape of the components , all the teeth with different polar angle at one given wave generator position will represent one tooth’s motion when the wave generator rotates. In other words, one tooth at the given wave generator position will have one contact ellipse. Instead of simulating the rotation of the wave generator, one can overlay the contact ellipse of all the teeth at the instant to have the contact pattern and path of contact for one tooth.
The crowned tooth surface will have a localized contact pattern under no load condition. Under a load condition, the loaded tooth contact pattern is needed to simulate the final contact pattern result, especially due to the flexibility of the compliant cup. The criteria of the contact pattern include the following:
- No high stress edge contact under any load condition.
- The contact pattern spans at least two thirds of the face width.
- Under no load condition, the contact pattern is toward the toe of the tooth surface.
- Under nominal load condition, the contact pattern is shifting to the center of the tooth surface.
Due to the strain wave gear’s kinematics, the tooth profile is not involute or cycloid. The relative motion between the flexspline and circular spline as shown in Figure 2 is different from the relative hypocycloid motion of a pair of rigid internal meshing gears. Involute or cycloid profiles cannot have conjugation under such motion. Instead, in Figure 9, the definition of the tooth profile’s three main segments includes the tip circular arc radii rt, root circular arc radii rr, and common tangent straight line, l. The tip fillet rtf, and root fillet rrf, will not engage in meshing. The selection of such a profile for the flexspline will lead to a high contact ratio under the relative motion between the flexspline and circular spline. High quality brick meshes as in reference  are used for the crowned tooth surfaces. The total nodes number of the model is 1.35 million.
Comparing the radial deformation of the flexspline in Figure 6(b) with Figure 10(a) for no load condition, the max radial deformation is at the major axis of the wave generator with 0.3 percent difference, which verifies the crowned tooth surfaces have no interference between the flexspline and circular spline. Under 20 N*m load condition, the radial deformation is shown in Figure 10(b). The max deformation reduces 11 percent, and the max deformation location shifts from the major axis to the second quadrant as shown in Figure 10(c).
Torsional deformation causes the flexspline to be detached from the wave generator as mentioned in reference [13, 14].
Figure 11 shows the loaded tooth contact pattern result under a 20 N*m torque load. Unlike the rigid gear’s single oval shape contact pattern, the strain wave gear’s contact pattern can be divided into three regions as in Figure 11 and Figure 12. Region I has the highest contact pressure of 94 MPa. The mean point location is at the designed cross section longitudinally. As shown in Figure 12(a), region I has no edge contact. Region II has a max contact pressure of 39 MPa, and it is at the edge of the wave generator as shown in Figure 6(c)’s high contact pressure area. The contact boundary between the wave generator and inner surface of the flexspline causes the shape change of the flexspline teeth, which leads to the higher contact pressure at region II. Region III has a max contact pressure of 77 MPa. Due to the detachment between the flexspline and wave generator, the toe of the flexspline will be in contact with the circular spline. Region III has an edge contact.
However, the max contact pressure is lower than region I. The contact pressure result is for the purpose of comparison of contact pattern marks with experiments, and the contact pressure has not been compared with Hertzian contact stress.
Prototyping and Testing
Since the strain wave gear has an enclosed ring shape, a gear-marking compound cannot be used to test the contact pattern. The contact pattern mark will be smooshed during disassembling. The contact pattern is tested by running the strain wave gear under a nominal load for 12 hours on the test rig, then the surface topology can be observed under a microscope.
Figure 13(a), 13(b), and 13(c) show the three components of the given strain wave gear. Figure 13(d) shows the test rig with motor input on the right, torque load on the left, and the simulated strain wave gear in the middle. Figure 14(a) shows the tooth surface before running the experiment; the machining marks are along the longitudinal direction. After running for 12 hours, Figure 14(b) shows the contact pattern with darker contact marks with an angle toward the profile direction. Figure 14(c) shows the three contact regions, which verify the simulation results in Figure 11 and Figure 12.
Conclusions and Future Work
Based on the performed research and results, the following conclusions can be drawn:
A finite element model is established for the strain wave gear assembly with a longitudinal crowned tooth surface. The simulation result for the contact pattern has been verified by experiments. The model can be used for future design to shorten the design period.
The shape of the flexspline is thoroughly studied. The deformation results can be used for calculating the longitudinal crowning amounts.
The contact pressure between the wave generator and inner surface of the flexspline is found to be not evenly distributed along the longitudinal direction. The deformed shape of the flexspline compliant cup open end is governed by the wave generator shape and also the contact status.
Under the torsional load, the teeth meshing and the shape of the flexspline are a coupled problem. The loaded tooth contact pattern analysis for the strain wave gear has solved the problem.
Plan for future work is as follows:
- Design the wave generator with a compatible shape with the deformed compliant cup inner surface to lower the contact pressure.
- The shape of the wave generator can be optimized similar to the cam profile. The optimal shape might not be an ellipse for the strain wave gear’s dynamic performance.
- Conduct a mesh convergence study with criteria of stress and compare contact pressure results with Hertzian contact stress.
- Study how profile crowning will affect transmission error.
- Study how different load and load direction will affect the contact pattern and stiffness of the strain wave gear.
The authors express deep gratitude to Shenzhen Tongchuan Technology Company Co.,Ltd. for prototyping and experimenting to verify the simulation results.
- Litvin, F. L., and Fuentes, A., 2004, Gear Geometry and Applied Theory, Cambridge University Press, Cambridge, UK.
- Stadtfeld, H. J., 2014, Gleason Bevel Gear Technology, the Gleason Works, Rochester, USA.
- ANSI/AGMA, 2001, Fundamental Rating Factors and Calculation Methods for Involute Spur and Helical Gear Teeth, 2001-D04.
- ANSI/AGMA, 2003, Rating the Pitting Resistance and Bending Strength of Generated Straight Bevel, Zerol Bevel, and Spiral Bevel Gear Teeth, 2003-B97.
- IGD Academic Research, Release 3.5.4, IDG User’s Guide, Rochester Institute of Technology.
- KISSsoft Academic Research, Release 03.2017, KISSSoft User’s Guide, KISSsoft AG.
- Dong, H., Ting, K., Wang, D., 2011, “Kinematic Fundamentals of Planar Harmonic Drives,” ASME. J. Mech. Des.,133(1).
- Dong, H., Wang, D., Ting, K., 2011, “Kinematic Effect of the Compliant Cup in Harmonic Drives,” ASME. J. Mech. Des., 133(5).
- Musser, C. W., 1955, “Strain Wave Gearing,” U.S. Patent No. 2,906,143.
- Gonzalez, I, Fuentes, A., 2017, “Implementation of a Finite Element Model for Gear Stress Analysis Based on Tie-Surface Constraints and Its Validation Through the Hertz’s Theory,” ASME. J. Mech. Des., 140(2).
- ANSYS® Academic Research Mechanical, Release 19.0, Help System, Contact Technology Guide, ANSYS, Inc.
- Roberts, I., Wang, C., Stanford, M., Mynors, D., Esterlein, R., 2009, “A three-dimensional finite element analysis of the temperature field during laser melting of metal powders in additive layer manufacturing,” International Journal of Machine Tools and Manufacture, 49(12-13), Pages 916-923.
- Kayabasi, O., Erzincanli, F., 2007, “Shape Optimization of Tooth Profile of a Flexspline for a Harmonic Drive by Finite Element Modelling,” Materials & Design, 28(2), Pages 441-447.
- Hofmann, D.C., Polit-Casillas, R., Roberts, S.N., Borgonia, J.-P., Dillon, R.P., Hilgemann, E., Kolodziejska, J., Montemayor, L., Suh, J.-O., Hoff, A., Carpenter, K., Parness, A., Johnson, W.L., Kennett, A., Wilcox, B., 2016, “Castable Bulk Metallic Glass Strain Wave Gears Towards Decreasing the Cost of High-Performance Robotics,” Nature, Article no. 37773.
Printed with permission of the copyright holder, the American Gear Manufacturers Association, 1001 N. Fairfax Street, Suite 500, Alexandria, Virginia 22314. Statements presented in this paper are those of the authors and may not represent the position or opinion of the American Gear Manufacturers Association. (AGMA) This paper was presented September 2018 at the AGMA Fall Technical Meeting in Oakbrook, Illinois. 18FTM09