Determination of Transmission Error and Mesh Stiffness in Spur Gear Pair using CAD-FEM Integration Approach

Unwanted sound and sensations are key sources of excitations in gear drives. They developed because of Transmission Error (TE). TE is a consequence of geometric or engineering flaws like profile/pitch error etc. or distortions like spall, indentation, crack, rubs etc. arising due to the diverse load conditions. These distortions and various gear parameters like number of teeth, contact ratio, module, pressure angle etc. have huge effects on TE and produce changes in mesh stiffness. This demands to investigate the effects of these parameters on TE and mesh stiffness for the avoidance or early finding of causes of malfunctions in the transmission system using computer models using CAD-CAE (FEM) software. In this paper the TE and mesh stiffness is determined using CAD-FEM integration approach and the impact of some of the gear parameters, tooth tip radius and geometric flaw-pitch error is analyzed. The modeling of spur gears & assembly to form gear pair is done in CAD software SOLIDWORKS. The gear pair formed is then introduced into FEM software Ansys for simulation using transient structural analysis method to find angular deformations and then TE and mesh stiffness. Several charts are drawn amongst rotation angle of one of the gears (driver gear) and TE/mesh stiffness for different gear parameters. The work demonstrated the use of CAD-CAE integration approach and point out that all these parameters affect TE and mesh stiffness in a meaningful way.


Introduction
Gears are the backbone of the transmission system, and spur gears are the most frequently used elements in it.They are also exposed to distortions because of various engineering/geometric flaws or altering load situations.These distortions are responsible for the development of unsolicited sound and excitations resulting in power or torque loss.To explore the effects of these on power transmission systems such as gear drives, several methods ranging from theoretical or mathematical to experimental or computer simulations are frequently applied successfully.The work presented here shows the use of a CAD and FEM software integration approach developed by [1] for the calculation of mesh stiffness to find the TE and mesh stiffness to analyse the effects of various gear parameters, tooth tip radius and pitch error on TE and mesh stiffness.Pitch error is the difference in theoretically correct pitch and 3 [20] presented a revolutionary high-order phasing gear to lessen mesh stiffness variation.The gear pair is used to study the contact line, and the phasing parameters are optimised to provide almost no mesh stiffness fluctuation.To reconcile the kinematics and centrifugal fields of spur gears, Zheng et al. [21] created an analytical mesh stiffness model that included tooth contact and centrifugal expansions.In comparison to previous models, FEM, and experiments, quasi-static and dynamic solutions exhibit acceptable accuracy and discernible centrifugal stiffening at high-speed conditions.Gear wear increases vibration and noise level and has an impact on meshing excitations like mesh stiffness and gearbox error.Shen et al. [22] suggested a geometric model to assess how gear wear affects mesh stiffness and USTE.According to experimental findings, gear wear only modifies the amplitude of the meshing frequencies and their sidebands rather than the spectrum's overall structure.He and Yang [23] offer a unique gear thermal stiffness model to investigate the static and dynamic properties of gear system vibration.For time-varying thermal mesh stiffness and gear thermal mesh stiffness, it derives general analytical formulations.A new nonlinear dynamic model for a spur gear system that takes into account dynamic force increment and velocity-dependent mesh stiffness was proposed by Liu et al. [24].The effect of velocity-dependent mesh stiffness and dynamic force increment on the dynamic properties of the spur gear system is depicted and quantified using numerical data.
It has been learned from the literature that the researchers are using an analytical, experimental, or numerical methods to measure or forecast the effects of different displacements on TE and mesh stiffness.To calculate/predict TE and mesh stiffness in gears, numerous CAD/CAE software for modelling, analysis, and simulation are utilised on a regular basis.For these computations, several researchers use an individual methodology or a mix of methodologies.But still, there is a lot of scope for the use of simple and easy to understand procedures to find the TE and mesh stiffness by considering deformations due to geometric/manufacturing/loading conditions using CAD and CAE (FEM) software to benefit numerous researchers.Also, a very few of the researchers attempted pitch error, gear parameters and tooth tip radius together effects on TE and mesh stiffness.
The 3D modelling and assembly of different spur gears are done in SOLIDWORK's software, and these gear pairs of various parameters are then introduced into CAE/FEM software Ansys for the analysis purpose.From these analysis results numerous graphs are drawn amongst TE/mesh stiffness and rotation angle or mesh angle of driver/driven gear.

Gear Input Parameters
The main gear parameters required for gears are module, number of teeth and pressure angle.Other gear parameters such as addendum circle, dedendum circle, base circle, pitch circle diameter, tooth thickness etc. are calculated from these parameters based on the type of tooth proportion system.The tooth form is involute curve and is drawn using equation driven curve option.These relations are represented in table 1 [25][26].

Gear Modeling
The healthy (correct) and faulty (defective) gears of various parameters are modelled based on the procedure explained in [25][26].Fig. 1 shows the various curves of the gear and modelled gear respectively.

Gear Assembly (Gear Pair Formation)
After completion of geometric modelling of different gears, now the various combinations (pairs) of gears are formed.The assembly module of SOLIDWORKS software is open and gear 1 is inserted and then gear 2 is inserted.To make the assembly different mate (positions two components relative to one another) options coincident, distance and mechanical gear mate etc. are used to form the pairs.Fig. 2 show assembly of one of the pairs and various mates used.

Determination of TE and Mesh Stiffness using Ansys Workbench
In an uncorrected drive, TE is the consequence of the output gear departing from its theoretical position and the actual position held by it.Geometric imperfections, manufacturing flaws, tooth deformations, lubrication, and other factors can all contribute to TE in gear drives.The presence of TE in gear drives results in a grating point in the noise and vibration waves.Pitch Error (PE) is a type of geometric inaccuracy in teeth.It's the distinction between real and theoretically precise pitch.PE is created in this study by boosting the tooth thickness to 1% and 2% of the theoretically correct thickness.Fig. 2. Spur Gear pair and different mate options.
The angular and linear representations of TE are given by ( 1) and (2), which are evaluated at the base circle or pitch circle.In the current work TE is calculated at the base circle.The mesh stiffness is then represented in torsional and linear way as given by ( 3) and (4).
where θgear1 & θgear2 are the angle of rotations, Rbgear1 & Rbgear2 are base circle radius of driver gear 1 & driven gear 2, respectively.T represent resistive or braking torque and KTorsional and KLinear represent torsional mesh stiffness (Nm/radian) & time varying mesh stiffness (N/m) respectively [1,[3][4].The most convenient representation of mesh stiffness in literature is the time varying mesh stiffness (TVMS) representation, so in this work it is used for analysis.The technique provided by [1] is utilised for calculating TE and mesh stiffness.All the spur gears necessary for the investigation are parametrically designed in the CAD software SOLIDWORKS.
By modifying various gear properties, parametric modelling allows for the creation of many gears.After that, the modelled gears are put together to make different gear pairs.The distinct gear pairs are healthy gear pairs, which contain both healthy gears, and faulty gear pairs, which contain one healthy gear and another defective gear (1% & 2% PE).This is already explained in section 2. The specifications for these gears and gear pairs are shown in table 2. There are 24 gears total, and 24 gear pairs (assemblies) are created.
Ansys workbench is chosen owing to its wide ability to solve any complicated linked physics computations in a simplified way in a single environment.Any finite element analysis/method involves three major processes, known as preprocessing, processing, and postprocessing.Poisson's ratio, ν 0.3 Tooth tip radius (mm) 0.5, 1.0, 1.5

Preprocessing
In this step, the type of analysis system, geometry, material properties, surface contact definition, mesh generation, boundary conditions, and different analysis settings are performed.These are explained as below.

1) Analysis System
There are different analysis modules/systems for solving various applications in Ansys Workbench.Here, a transient structural analysis is used for the analysis work.Fig. 3 show the Workbench containing various analysis systems and a user interface for transient structural analysis.

2) Geometry and Material Properties
Ansys has an interlinked user interface for SOLIDWORKS.Any file containing 3D models can be directly opened in the Ansys mechanical environment while maintaining all design details.The gear pair is imported into the Ansys Workbench environment and material is assigned to each of the gears in the gear pair (See Fig. 3).The material assigned is structural steel, whose modulus of elasticity is listed in table 1.

3) Defining Contact Regions
The contact zone between gear is chosen as frictionless with 0.1 mm penetration tolerance value and normal stiffness factor as 1.To achieve convergence, initial contact is established using "Adjust to Touch" interface treatment.Contact stiffness sensitivity is reduced by applying "Augmented Lagrange formulation".This is represented in Fig. 4.

4) Mesh Generation
Once the contact region is defined then element formation is done.The SOLID185 and CONTA170 element types are used.Because FEM takes a long time to compute, so few pairs of teeth are fine meshed to speed up the process.The meshed gears and tiny meshed teeth are shown in Fig. 3.

5) Defining Boundary Conditions
Body ground revolute joints are attached at the hub of the driver and driven gears.All other degrees of freedom are fixed, and the gear pair is allowed to rotate along its axis of rotation only.The driver gear is given a constant very low rotational velocity equivalent to 1 mesh cycle angle and the driven gear is given a braking torque.(Fig. 5

.). 6) Analysis Setting
To disable the inertial effects, the time integration feature is switched off.However, the large deflection should be on.For quasi-static analysis, a system damping value of 0.1 is utilised.Auto Time Stepping can be used to speed up the computing process if necessary and the sub-steps are selected in such a way that 1 sub-step equals 1° rotation angle.Fig. 6 show the analysis settings.

Processing (Analysis)
After completing pre-processing stage, the non-linear loaded tooth contact analysis is performed.

Post Processing (Result Solutions)
The relative rotation of the driver gear and driven gear is measured with the help of joint probes attached to the two gears of the pair.Fig. 7 shows the joint probes.The Quasi-static Algorithm is 8 utilised to compute the TE and TVMS [1].The simulation data produced is entered into (1), ( 3) and (4) to get the TE and TVMS corresponding to the rotational angle.

Numerical Illustration and Discussion
The gears used in the work are listed in table 2. Now to use FEM to find the TE and mesh stiffness, import one of the healthy gear pairs, say module 3 mm, number of teeth 18, pressure angle 18°, into Ansys workbench first.The method employed is transient structural analysis.The SOLID185 and CONTA170 finite elements are then used to mesh this pair, resulting in 339308 elements and 682373 nodes.The contact pair is frictionless, with 0.1 mm of penetration tolerance and a touch interface treatment.Because FEM takes a long time to compute, 4 pairs of teeth are fine meshed to speed up the process.The meshed gear pair and tiny meshed teeth are shown in Fig 3 .All other degrees of freedom are fixed, and the gear pair is allowed to rotate along its axis of rotation.The driver gear is one, while the driven gear is the other.The driver gear is given a constant rotational velocity of 0.5254 rad/sec, which is equivalent to 1 mesh cycle angle and the sub-steps are selected in such a way that 1 sub-step equals 1° rotation angle, while the driven gear is given a braking torque of 200 Nm.To obtain relative angular positions, the flexible rotation probes are connected to both the driver and driven gear.After a successful simulation/analysis, the varied angular locations acquired using probes on the driver and driven gear are input into (1) -( 4) to provide TE and mesh stiffness.Following that, the analysis is carried out in the same manner for all other gear pairs as listed in table 2 and various plots of the TE and mesh stiffness curves for pressure angle, number of teeth, module, pitch error and tooth tip radius variations as a function of driver gear rotations are obtained (Figs.8-15).The maximum and minimum values of TE and mesh stiffness i.e., TVMS are represented in table 3 and 4 respectively.The minimum value of TE occurs when double tooth contact takes place, and the maximum value occurs when single tooth contact takes place during the meshing of gear pairs while maximum value of mesh stiffness occurs in double tooth contact zone and minimum value occurs in single tooth contact zone.Figs.9a-9c and 13a-13c depict graphs related to the variation of module effect on TE and mesh stiffness, respectively.Tables 3 and 4 represent the maximum and minimum values of TE and mesh stiffness, respectively, for different parameters.When the module changes from 3 mm to 5 mm, there is a little variation in TE in the case of a healthy gear pair.TE increases for gear pairs with pitch errors.It shows some variation in mesh stiffness in the case of a healthy gear pair as well as a gear pair with pitch errors.This can be seen from the maximum and minimum values given in tables 3 and 4 respectively.

Influence of number of teeth on TE and Mesh Stiffness
In case of number of teeth variation, it is observed from Figs. 10a-10c, 14a-14c and Tables 3-4, there is some variation observed in TE and mesh stiffness.There is some decrease in TE and mesh stiffness observe when number of teeth varied from 18 to 30.This observation is noted for both healthy and faulty gear pairs.

Influence of pressure angle on TE and Mesh Stiffness
The pressure angle variation effect on TE and mesh stiffness is depicted in Figs.8a-8c and 12a-12c, while the maximum and minimum values are shown in Tables 3-4, respectively.From this information, it is seen that as the pressure angle increases from 18° to 25°, there is a decrement in TE, but the variation is very small or negligible in both healthy and faulty gear pairs.The mesh stiffness shows an increasing trend.As the pressure angle increases, it causes tooth to become thin at the tip and thick at the bottom portion, making the gear strong at the lower portion.

Influence of pitch error on TE and Mesh Stiffness
Due to pitch error variation, it is noted that there is an increase in TE values and an increase in mesh stiffness.
Since the pitch error is created by increasing the tooth thickness by 1% and 2% of the original value, the tooth becomes thick at the lower portion and increase the single tooth contact zone.(Figs.8d, 12d and Tables 3-4).

Influence of tooth tip radius on TE and Mesh Stiffness
The tip radius is created by removing a little quantity of material around the tip of the gear tooth.Because tip relief is commonly utilized to minimize transmission errors, dynamic loads, vibration, and noise, it's crucial to look at how tip radius affects the TE and TVMS.The effect of tip radius on the TE and TVMS is seen in Figs.
11a-11c and Figs.15a-15c respectively.In general, changing the tooth tip radius has only a little impact on the TE and TVMS's maximum and lowest values.However, due to the larger tooth tip radius, the two-tooth contact zone is enlarged while the one tooth contact region is reduced.

Conclusions
By adapting and using the CAD and FEM integrated approach for analysing the TE and mesh stiffness, the presented work investigated the impacts of the gear parameters module, teeth number, pressure angle, tooth tip radius, and geometric precision pitch error on TE and mesh stiffness.SOLIDWORKS is used to create the 3D models of gear pairs, which are then seamlessly loaded into the finite element system as the ANSYS workbench platform offers direct, associative, bidirectional interfaces with all major CAD packages.Figs. 8 to 15 show the results of Ansys simulations for various gear specifications plotted against the driver gear's rotation angle on the horizontal axis and the TE/mesh stiffness on the vertical axis.The observations from the work are as follows.
• The adapted method for determining the TE and mesh stiffness using the CAD-FEM integration approach is successfully applied in the case of gears with pitch error, tooth tip radius variation, and other gear parameter variations.
• Gear parameters module, pressure angle, and teeth quantity affects TE and mesh stiffness.Pressure angle variation has a very little impact on TE, but it increases the mesh stiffness.Number of teeth affects TE mesh stiffness.Lower teeth gear pair have more value of TE and mesh stiffness.Module variation in case of faulty gears has some impact on TE and reduction in mesh stiffness while healthy gear pair saw very less or negligible impact on TE, but mesh stiffness variation observed.
• In case of geometry flaw -pitch error impact on TE and mesh stiffness, pitch error variation causes TE fluctuations.There is some increase in mesh stiffness noted.
• There is some reduction in TE and mesh stiffness observed when tooth tip radius changes from 0 to 0.5 mm and after that its impact is negligible.

Table 2 .
Gear parameters used in presented work.

Table 3 .
Maximum and minimum values of TE (μm).

Table 4 .
Maximum and minimum values of mesh stiffness (N/m).