uation of the effect of misalignment and profile (1).docx

Sandro BaroneLeonardo Borgianni Paola Fortee-mail: p.forteing.unipi.itDipartimento di Ingegneria Meccanica,Nucleare e della Produzione,University of Pisa, Italy, Via Diotisalvi 2, 56126 Pisa, ItalyEvaluation of the Effect ofMisalignment and Profile Modification in Face Gear Drive by a Finite Element Meshing SimulationFace gear drives have many advantages over other cross axis transmissions especially in high performance applications. The lack of published design experience and design standards make their design difficult. This is mainly due to the complex geometries and to the lack of practical experience. For these reasons face gears have not been used for long. This work is aimed at investigating the behavior of a face gear transmission considering contact path under load, load sharing and stresses, for an unmodified gear set including shaft misalignment and modification on pinion profile. The investigation is carried out by integrating a 3D CAD system and a FEA code, and by simulating the meshing of pinion and gear sectors with three teeth, using contact elements and an automated contact algorithm. The procedures followed to create the 3D models of teeth in mesh are described and finite element analysis results discussed showing the differences between unmodified, modified and misaligned teeth. Results show the influence of load on theoretically calculated contact paths, contact areas, arc of action and load sharing. The differences with respect to the ideal case are sometimes remarkable. Further developments are discussed. DOI: 10.1115/1.1767818#Journal of Mechanical DesignSEPTEMBER 2004, Vol. 126 935Downloaded 01 Jun 2010 to 6. Redistribution subject to ASME license or copyright; see /terms/Terms_Use.cfmIntroductionFace gear drives are a particular kind of cross axis transmission made of a pinion with involute teeth meshing with a face gear.Face gears have historically been used for applications with low torque and low to moderate speed. Lack of experience and published research in high power, high velocity usage, have hindered their application in these fields for a long time. In the last decade, the aerospace industry has turned its attention to face gear drives, with private and government sponsored research 14#. In layouts employing torque split, due to the high transmission ratio, face gears allow reductions in the number of transmission stages that, in turn, can lead to sensible mass reductions and to an increase in reliability and maintainability, which are directly connected to life cycle costs. This is particularly true if the transmission includes a spur pinion: lack of axial forces permits a layout without axial bearings, which are unavoidable in the case of spiral bevel gearing. Moreover some studies showed, for this kind of transmission, a very low sensitivity to misalignment in terms of transmission errors, leading to low vibration levels and low noise in operating conditions.Experience with highly loaded light gears in high velocity usage shows the need of taking into account reductions in rim and tooth stiffness for the evaluation of transmission behavior. In fact, gear teeth are not directly loaded and tooth and rim deformation, by coupling hertzian deformation with structure deflections, will affect location and shape of the contact zone, local sharing and contact stress distribution. Considering fatigue, the most loaded critical sections can change passing from the tooth to the rim 5#. All these factors affect fatigue life, noise and vibrations, thermal degradation and action of lubricants.Design methods for the evaluation of face gear stresses are derived from spur gears standards with suitable modificationsContributed by the Power Transmission and Gearing Committee for publication in the JOURNAL OF MECHANICAL DESIGN. Manuscript received May 2003; revised Feb. 2004. Associate Editor: A. Kahraman.3,4#. The soundness of these methods is hard to assess without experimental tests. To evaluate face gear behavior in a high performance field of usage, without a commonly approved design experience and standard, the meshing problem must be dealt with in its complexity.The finite element method for the analysis of stresses in gears is widely accepted. Much work has been done assuming a hertzian contact pressure distribution 6#. However, when the loading conditions are severe and the gear geometry is complex, contact constraints should be modeled more realistically and this can be accomplished in various ways simulating the meshing process of deformable pinion and gear teeth with 2D and 3D models 713#. Contact between elastic bodies can be faced with different FEM techniques, otherwise the elastic structural problem can be separated from the contact problem, and the latter can be solved with numerical approaches 1215#.Most of the work reported in the technical literature regards spur, helical and bevel or spiral bevel gears. As regards face gear drives some results have been reported concerning the analysis of a single tooth with a load distribution on an ideal contact line 16#, the meshing simulation between single teeth 17#, the analysis of the meshing of pinion and gear sectors to evaluate optimal modifications to the pinion profile 18#, and the evaluation of the load split for a complete face gear drive in this case the meshing was simulated with the aid of suitable elements! 19#. Recent papers 20,21# present numerical approaches based on combination of finite element and analytical methods. The contact analysis is carried out analytically assuming a load distribution due to an initial mismatch between pinion and face gear tooth flanks, while the tooth stress distribution away from the contact area is calculated by a classical FEA.Copyright 2004 by ASMEIn previous works, the authors compared face gear drives with bevel ones by FEA assuming a hertzian contact pressure distribution 22#, investigated a single pair of deformable teeth in contact, by the contact algorithm of a commercially available FE code 23#, and analyzed the possibility of studying the behavior of a spur pinion engaging with a face gear by integrating FEM and CAD tools 24#. In this work the authors extended the study considering the effects of the applied torque, pinion profile modifications and misalignments of gears, so as to evaluate the transmission behavior for a wide range of situations.Geometries Generation by EnvelopesFace gear modeling involves the description of surface geometry. While the pinion has a simple involute profile, the face gear has a surface of high complexity.Only in the last decade the geometry of face gear drives, especially for high power transmissions, have been defined analytically 25# and modern methods based on computerization of design and meshing of gears have been applied to this type of gears. Face gear generation is only one particular case of the more general theory of envelopes to families of surfaces. For cams or gears, generating families are defined considering the subsequent positions assumed by the shaper in the generating process. For this reason, surfaces of the family are consistent they do not modify during the motion! and the family is defined with only one motion parameter which relates the movements of the tool to the movements of the generated gear. A consistent family of surfaces can be parametrically described as by Eq. 1!, where r is the position vector of the generic point belonging to the family in a particular reference system.rI5rIu,u,f!(1)Parameter fis the parameter of motion, which uniquely defines the meshing position and the corresponding surface of the family while u e uare surface coordinates.The envelope to a family of surfaces can be calculated finding points for which relation 2 is verified this relation is called equation of meshing 2527#!.rI SrI rIDrI8,f,rI8,u ,rI8,u#5f u u5fu,u,f!50(2)Equation 2! imposes the geometrical condition for which if a point belongs to the envelope, in that position the three vectors obtained by the derivation of the position vector in f, u, ubelong to the same plane. These vectors have a simple geometrical meaning:rI/frepresents the vector tangent to the trajectory of the enveloping surface, while rI/u and rI/uare the tangential vectors to the surface in two independent directions, and their vectorial cross product defines the normal to the surface in the examined point. Following this interpretation, it is possible to express Eq. 2! in a kinematic way:fu,u,f!5nIu,u,f!vIu,u,f!50(3)Solution of Eq. 3! gives, for each value of the motion parameter f, points on the enveloping surface that belong to the envelope. These points generally belong to curves that represent contact lines between the shaper and the generated flank. The gear fillet is modeled in a similar manner, as produced by the movement of the tip edge of the shaper or as a result of the envelope of the subsequent positions of the tip fillet of the tool. At the Department of Mechanical, Nuclear and Production Engineering of the University of Pisa a software was developed 28# for the generation and tooth contact analysis of face gears with a cylindrical involute pinion, with straight or helical teeth, with a variable angle between shafts and in presence of misalignments.This code produces, as output, ASCII files containing points which discretize each contact line on the shaper and gear flank and fillet Fig. 1!. These data can be used for the generation of a finite element model of the face gear tooth.Fig. 1Theoretical surfaces of face gear tooth fillet and flankSolid Modeling and FEM ModelsThe approach adopted in various works reported in the technical literature for 3D finite element model generation, includes the use of a specifically developed geometric modeling program, which gives an output compatible with the FEA code.In this work, in order to obtain a better control at low cost on mesh generation and on geometrical features of gears not directly related to the generation process itself profile and/or gear teeth modifications, creation of fillets, etc.!, solid modeling of gear flank surfaces was preferred. The models were obtained interpolating data obtained from the enveloping generation code.The face gear and the mating spur pinion were both modeled with the commercially available solid modeler Pro/Engineer. Points from the generation code were imported in an ASCII file as a set of ordered points belonging to contact lines of the shaper and the face gear. These points were interpolated with NURBS surfaces approximating the flank and the fillet of the face gear Fig.2!.Interpolating surfaces show a resulting error in the distance from the original points about 5 orders of magnitude lower than the characteristic tooth dimensions lower than 1 micron!. The solid model was obtained by geometry reflection, taking advantage of symmetry, and by the boundary definition at the outer and inner diameter, taking into account the pointing and undercuttingFig. 2 NURBS surfaces approximating the face gear tooth surfacesFig. 3Face gear solid modelconditions, which define the longitudinal dimension of the teeth. The solid was then generated joining the surfaces bounding the tooth volume Fig. 3!.The pinion has straight teeth with an involute profile that can be directly implemented in the software, so it was modeled using the parametric equations of the involute flank. The solid model was controlled by some parameters such as the pinion number of teeth, the module and the pressure angle. The surface was described analytically in the CAD environment, consequently no error was introduced in the CAD model.The solid models were then exported into the FEA environment, Ansys. Data exchange was accomplished by the IGES standard with a good final accuracy of the models, due to the common geometrical database between the source and the destination code, and to the simplicity of the exported model.Mesh generation, preprocessing, FEM analysis and postprocessing of results were accomplished by the same code. Following a previous experience on contact analysis applied to gears 23,24#, it was assessed that meshing simulation improves considerably if a regular mesh is used on contact surfaces, and if the mesh is realized with elements that can model in an affordable way not only the global stiffness, but even stress gradients. Isoparametric brick elements with 8 nodes were chosen, to obtain a good accuracy in stress gradients and to keep a reduced dimension of the numerical problem low number of degrees of freedom!.The geometrical characteristics of the original surfaces can be better maintained by a surface discretization with hexaedral elements. This is because hex elements permit to maintain generatrices in cylinders and the quasi prismatic shapes of gears. This is not true for tetrahedral meshes, which produce very irregular surfaces with poor results from the meshing simulation point of view. In some way, hex meshes are a more natural way of discretizing gears. Starting from a surface mapped mesh on the lateral boundaries of the bodies, a volume solid mesh was generated by sweeping the elements created on a source surface the front surface of tooth!. In this way, a quite regular mesh was obtained.The detection of the contact area was another problem to face in the process of mesh generation. While the contact between the shaper and the face gear develops along a curve line contact!, the contact between the face gear and an engaging pinion different from the shaper is theoretically a point point contact!. This means that the contact will develop over an almost elliptical area, where the major semiaxis can be 2 orders of magnitude greater than the minor one. An accurate detection of the contact area without using particular techniques needs a really fine mesh on a surface of a 3D body. In this case it was impossible to handle the model dimension with the available hardware. Postprocessing was done on results that show a reduced sensitivity to this kind of problem load sharing, movements of contact area, pinion stress during meshing!. A mesh which could produce a small error in the longitudinal definition of the contact area and a much greater error inFig. 4FEM constrained model of face gear sectorthe transversal direction was accepted. Once the tooth volume was meshed, contact and target elements necessary to simulate meshing were defined, as described above.This procedure brought to the FEM model of a single contacting pair; the two sectors were finally obtained by copying the single tooth nodes and elements around the gear axes. Fem models of gear and pinion sectors were generated in separate working sessions, and then assembled in a common space with the aid of suitable reference systems to obtain the desired alignment.The face gear sector was constrained fixing the lateral and the bottom surfaces of the rim, while the nodes attached to the lateral surfaces of the pinion sector were constrained to rotate rigidly around the axis of the pinion. The loading condition consisted of a torque applied to a node defined on the pinion axis Figs. 4, 5!.Fig. 5 FEM constrained and loaded model of engaging spur pinion sectorAssuming a particular meshing position as a reference, each other position could be reached by rotating the models with an appropriate macro developed in APDL a special programming language in Ansys!. This macro copied nodes and elements in the desired position and applied the pre-existing boundary conditions on the models. This procedure was efficient as it permitted to use the same mesh for different analyses, and results were not affected by the mesh variability.Meshing Simulation by FEMNowadays, it is certainly easier to analyze gear contact stresses thanks to the development of contact algorithms and their implementation in commercial finite element codes occurred in the last years and great number of references can be found in the technical literature on a variety of approaches 2934#.In the FEA code Ansys chosen for this study different techniques are implemented for surface to surface contact analysis: penalty function methods and augmented Lagrangian methods. Penalty methods are more efficient from the computational point of view, but they are very sensitive to the assumed contact stiffness, bringing to potentially ill-conditioned problems for high stiffness values. Moreover penalty methods always produce final penetration between bodies, the amount of which is strictly related to the assumed contact stiffness: the higher is the stiffness value, the lower is the resulting penetration. Purely Lagrangian multiplier approaches bring to expensive computational problems, even if numerically more stable. Augmented Lagrangian methods try to reduce problems, increasing the time required to reach convergence. An augmented Lagrangian method was chosen for this study.For detection of contact between surfaces, the FEA code has search algorithms based on a hierarchical classification of potentially contacting surfaces; these are divided in target or slave! and contact or master! surfaces. More than one target surface can be related to the same contact surface. Penetration between nodes on the contact surface and elements of the target surface is controlled introducing reaction forces on contact surfaces nodes when penetration is detected.Contact and target surfaces are defined by creating surface meshes on the underlying solid mesh, with special contact and target elements. To completely define a contact pair, contact and target elements have to be referred to the same set of characteristic parameters such as contact stiffness, allowed penetration tolerance, friction coefficient, and so o