NASA/CR--2002-211277 of Procedure for Tooth Contact Analysis a Face Gear Meshing With a Spur Gear Using Finite Element Analysis George Bibel University of North Dakota, Grand Forks, North Dakota January 2002 The NASA STI Program Office... in Profile Since its founding, NASA has been dedicated to CONFERENCE PUBLICATION. Collected the advancement of aeronautics and space papers from scientific and technical science. The NASA Scientific and Technical conferences, symposia, seminars, or other Information (STI) Program Office plays a key part meetings sponsored or cosponsored by in helping NASA maintain this important role. NASA. The NASA STI Program Office is operated by SPECIAL PUBLICATION. Scientific, Langley Research Center, the Lead Center for technical, or historical information from NASA's scientific and technical information. The NASA programs, projects, and missions, NASA STI Program Office provides access to the often concerned with subjects having NASA STI Database, the largest collection of substantial public interest. aeronautical and space science STI in the world. The Program Office is also NASA's institutional TECHNICAL TRANSLATION. English- mechanism for disseminating the results of its language translations of foreign scientific research and development activities. These results and technical material pertinent to NASA's are published by NASA in the NASA STI Report mission. Series, which includes the following report types: Specialized services that complement the STI TECHNICAL PUBLICATION. Reports of Program Office's diverse offerings include completed research or a major significant creating custom thesauri, building customized phase of research that present the results of data bases, organizing and publishing research NASA programs and include extensive data results.., even providing videos. or theoretical analysis. Includes compilations of significant scientific and technical data and For more information about the NASA STI information deemed to be of continuing Program Office, see the following: reference value. NASA's counterpart of peer- reviewed formal professional papers but • Access the NASA STI Program Home Page has less stringent limitations on manuscript at http'llwww.sti.nasa.gov length and extent of graphic presentations. • E-mail your question via the Internet to TECHNICAL MEMORANDUM. Scientific [email protected] and technical findings that are preliminary or of specialized interest, e.g., quick release • Fax your question to the NASA Access reports, working papers, and bibliographies Help Desk at 301q521-0134 that contain minimal annotation. Does not contain extensive analysis. • Telephone the NASA Access Help Desk at 301q521-0390 CONTRACTOR REPORT. Scientific and technical findings by NASA-sponsored Write to: contractors and grantees. NASA Access Help Desk NASA Center for AeroSpace Information 7121 Standard Drive Hanover, MD 21076 NASA/CR--2002-211277 of Procedure for Tooth Contact Analysis a Face Gear Meshing With a Spur Gear Using Finite Element Analysis George Bibel University of North Dakota, Grand Forks, North Dakota Prepared under Cooperative Agreement NCC3-904 National Aeronautics and Space Administration Glenn Research Center January 2002 Available from NASA Center for Aerospace Information National Technical Information Service 7121 Standard Drive 5285 Port Royal Road Hanover, MD 21076 Springfield, VA 22100 Available electronically at http: //gltrs.grc.nasa.gov/GLTRS PROCEDURE FOR TOOTH CONTACT ANALYSIS OF A FACE GEAR MESHING WITH A SPUR GEAR USING FINITE ELEMENT ANALYSIS George Bibel Department of Mechanical Engineering University of North Dakota Grand Forks, North Dakota 50202 SUMMARY A procedure was developed to perform tooth contact analysis between a face gear meshing with a spur pinion using finite element analysis. The face gear surface points from a previous analysis were used to create a connected tooth solid model without gaps or overlaps. The face gear surface points were used to create a five tooth face gear Patran model (with rim) using Patran PCL commands. These commands were saved in a series of session files suit- able for Patran input. A four tooth spur gear that meshes with the face gear was designed and constructed with Patran PCL commands. These commands were also saved in asession files suitable for Patran input. The orientation of the spur gear required for meshing with the face gear was determined. The required rotations and translations are described and built into the session file for the spur gear. The Abaqus commands for three-dimensional meshing were determined and verified for a simplified model containing one spur tooth and one face gear tooth. The bound- ary conditions, loads, and weak spring constraints were determined to make the simplified model work. The load steps and load increments to establish contact and obtain arealistic load was determined for the simplified two tooth model. Contact patterns give some insight into required mesh density. Building the two gears in two different local coordinate systems and rotating the local coordinate systems was verified as an easy way to roll the gearset through mesh. Due to limitation of swap space, disk space and time constraints of the summer period, the larger model was not completed. INTRODUCTION Face gears for use in helicopter transmissions were studied. The face gear has several advantages over the tradi- tional spiral bevel gear. Two advantages are reduced sensitivity to nfisalignment and reduced noise from low trans- mission error (ref. 1). The face gear tooth surface geometry isbased on the kinematics of the generating action of the pinion shaper. The instantaneous line of contact on the pinion tooth is defined by the development of the equation of meshing. The face gear tooth surface is derived by coordinate transformation of its contraform on the pinion surface (refs. 1and 2). The existing design methods for face gear tooth stresses are simple modifications of spur gear stress analysis programs. It is difficult to validate these design procedures with strain gages because face gear teeth are very small. Therefore it is desirable to develop finite element techniques to validate the existing face gear design technology. The work reported here describes a process for doing three-dimensional contact analysis using the finite element method of a face gear contacting a mating spur gear. Described are the problems associated with geometry, meshing and convergence of the contact analysis. ANALYSIS PROCEDURE Face Gear Surface Points The description of the face gear surface, as given by the analysis from reference 1,consists of 30 points on ten different sections (corresponding to ten different Z values). NASA/CR 2002-211277 1 The input to this analysis was as follows: Input TNIP, TN2 and TNI, where TNIP is the pinion number of teeth, TN2 is the gear number of teeth, TNI is the number of teeth of the shaper: 17,69,18 Input diametral pitch: i0 Input the shaft angle (degrees): 9O Input the pressure angle (degrees): 27.5 Input : e(mm), g(minutes), and q(mm), where e is the misalignment in the direction mutually perpendicular to the plane formed by the axes of the gear and pinion, g is the error of the shaft angle, q is the misalignment along the gear axis: O.001 ,0.001,0.001 Points 1 to 20 define the tooth face. Points 21 to 30 define the tooth fillet. Points 20 and 21 coincide. A surface made of all points from the analysis is seen in figure 1. Figure 2 shows the points on the inner most section and the points on the outer most section. In figures 1 and 2, it is seen that some points on the fillet wrap around onto the fil- let of the adjacent tooth. The axis of rotation of the face gear as defined by the analysis is the Y axis (see fig. 3). The first point of each tooth sections always starts at Y = 0. All subsequent points have increasing negative Y values. The largest negative Y value corresponds to the bottom of the fillet. When the negative Y value starts to increase from the bottom of the fillet, the points are wrapping around onto the fillet of the next tooth. The points on the fillet of the adjacent tooth are discarded from the model. The points used on each section are 1to 20 to define the tooth face and points 22 through the largest negative Y value to define the fillet. The number of points used to identify the fillet varies from six to zero. The first 20 points on each of ten sections (200 points total) was used to define the tooth face. Points 21 to 30 on each section are not used initially. These 200 points were input with Patran PCL in the session file LTooth. ses. The session file LTooth2. ses creates curves through the 200 points on the tooth face. Points 22 to 30 on each section are used to identify the fillet. Not all of the eight points are used to identify the fillet. Only those points up to the highest negative Y value. The points used to identify the fillet are given in the Patran session file LF i 11 et. s es. This file also creates curves through the points on the fillet. LSurface. ses makes all of the surfaces on the tooth face and fillet. Solids. ses mirrors all of the sur- faces about the minus YZ plane (0.1 plane in Patran notation) and makes the solids for the tooth and fillet. When this tooth is rotated to create an adjacent tooth, the points do not line up in the fillet region. This can be understood by looking at the spacing of the points in the fillet region in figure 2. The spacing is uniform and not designed to identify the true bottom of the fillet. The actual spacing for the first section fillet points is about 0.010 in. The "true" bottom of the fillet is not accurately defined. The maximum gap and overlap is about 0.0035 in. or about athird of the spacing used. By adjusting the points on the bottom of the fillet to lie on the same radial line (0 = (0.5)360/(69 teeth)), the gaps and overlaps can be eliminated. Two points were adjusted about 0.003 in. and two points were adjusted 0.002 in. The remaining six points were adjusted 0.001 in or less. The following sessions files are played in the order listed: gearA, ses, gearBl, ses, gearB2, ses, gearCl, ses, gearC2, ses, and gearC3, ses. All ofthese files have been combined into FaceGear. ses. The face gear consists of the first tooth plus two teeth rotated clockwise and two teeth rotated counterclockwise for a total of five teeth. Spur Gear Geometry The following data was used as input to the NASA Glenn computer program Gpat2 a. exe, which was used to define the spur gear geometry (ref. 3): NASA/C_2002-211277 2 17 Number of teeth on gear N N=External gear I000 Number of teeth on cutter 27.5 Pitch line pressure angle, deg I0 Diametral pitch, teeth/in Y Y=Standard teeth 0.65 Radius for 0.2 backup ratio, in 0.5475 Slot outer radius, in 0.35 Hub outer radius, in 0.26 Hub inner radius, in The spur gear consists of the first tooth plus one tooth rotated clockwise and two teeth rotated counterclockwise for a total of four teeth. The file used to create the spur gear and rotate and translate into mesh are given in the Patran session file Spur. se s. Running Spur. se s after Face Gear. ses will generate the complete model. Because of limitation of time, disk space, and swap file errors, the "big" model was not used. Verification of three- dimensional contact with Abaqus was done on a simpler model consisting of one face gear tooth and one spur gear tooth. The files used to create this smaller model are Faces. ses and sSpur, ses. When generating the spur gear, answer yes to all questioned asked by Patran. Orientation of the Two Gears in Mesh Figure 4 shows the orientation of the face gear and spur gear. The face gear is centered at the global origin with the Y axis being the axis of rotation. The two-dimensional profile of the spur gear, as generated by the program, lies in the YX plane. The Z axis is the axis of rotation of the spur gear. As shown in figure 4, the spur gear profile is extruded 1.285 in. in the Z direction to establish the depth of the spur gear. The center of the face-gear tooth face is at Z = 3.501427 in., the spur gear must be translated Z = +2.858927 in. to center on the face gear (2.858927 = 3.501427 1.285/2). Since the face gear is in the ZX plane, and the spur gear profile is in the XYplane, with equal parts above and below the X axis, the spur gear must be translated in +Ydirection to be in mesh. This translation equals the spur gear radius nfinus the face gear tooth height plus a clearance of 0.030 in. or g = +0.7552 in. (g = 0.95 0.2248 + 0.03). In addition to the above translations, the tooth must be rotated into mesh. The above translations result in a tooth on top of the spur gear. A tooth on the bottom of the spur gear is needed for mesh. Rotating a spur gear tooth 180°results in a tooth that is one half tooth out of sequence for meshing. One half tooth rotation corresponds to one half of 360/(17 teeth) = 10.588235 °. Therefore, the total rotation to obtain mesh is 190.588235 °. The actual values of the Y translation and the Z axis rotation required for mesh are somewhat arbitrary. Final mesh is verified by viewing the mesh in Patran (see fig. 5). Zooming on figure 5 verifies no interference between the spur and face gear. A summary of the translations and rotations to obtain the spur gear and face in mesh are as follows: 1. Translate the spur gear in the +Z direction 2.858927 in. to center on face gear tooth. 2. Translate the spur gear in the +Ydirection 0.7552 in. 3. Rotate the spur gear 190.588235 ° to engage it in mesh. The translations for the spur gear were obtained by defining an appropriate local coordinate system. Local coor- dinate systems were also defined as an easier way to rotate the gear through mesh and will be discussed later. Boundary Conditions Since the face gear is centered at the reference global system, it is easier to fix the spur gear and constrain the face gear with a rigid link to rotate about its axis of rotation, the Y axis. This was done with rigid beams between the inner diameter of the face gear and the axis of rotation for the face gear. The load was applied as point loads to the face gear. A weak spring was used to constrain the rotation of the face gear (and oppose the point loads applied to the face gear). NASA/C_2002-211277 3 Because the face gear was modeled almost to its inner diameter, the pie sector of the face gear narrows as the inner diameter approaches Y = 0. There is concern this narrow sector is flexing. It may be more appropriate to fix the edge surfaces of the face gear and constrain the spur gear to rotate about its axis of rotation. The simplified two tooth model that successfully ran did not use rigid beams to force rotation of the face gear about it is axis of rotation. Two nodes on the inner diameter of the face gear were fixed with zero translation in all directions. These two points defined an axis of rotation for the single tooth face gear model. Those two points are about 0.25 in. from the true axis of rotation. Using *MPC (inulfipoint constraint) to make arigid link may be a better way to constrain one of the gears to rotate about its axis of rotation. Three-Dimensional Contact With Abaqus The following steps are required to do three-dimensional contact with Abaqus. 1. Identify the surfaces that contact. *SURFACE DEFINITION, NAME=FACETOOTH FI, FACETOOTHONE is auser designated name. FI is the set of elements on (i.e., ELSET), for example, the face gear tooth 1 contact region. The ELSET of elements involved in contact must be identified. This was done by applying a nfinor pressure load within Patran to the tooth face. The Abaqus input deck will then have an ELSET identified and available for surface definition. On the large nine tooth model the pressure loads were designated f/to f5 on the five face gear teeth and sl to s4 on the four spur gear teeth. When a load is applied on the face gear in the positive X direction, surface sl contacts with f/, s2 with f2, etc. Surface definition must always occur in pairs. At least one surface must be identified on the face gear and one surface identified on the spur gear. If two pairs of teeth are to contact, then there will be four surface definition conmmnds. The surface definition for the spur tooth might look as follows. *SURFACE DEFINITION, NAME=SPURTOOTH SI, 2. Identify a contact pair. This comlnand is used to identify pairs of surfaces that interact with each other. *CONTACT PAIR, SMALL SLIDING, INTERACTION=MYANALYSIS FACETOOTH, SPURTOOTH MYANALYSIS is auser given nalne. FACETOOTH and SPURTOOTH are the user given nalnes given in the sur- face definition commands. When a contact pair contains two defornmble surfaces, the user must choose which surface will be the slave sur- face and which will be the master. The master surface is the stiffer structure or structure with coarser mesh if the two bodies are of the same stiffness. The name of the slave surface is the first data item on the *CONTACT PAIR colnnmnd. *CONTACT PAIR, INTERACTION=NAME SLAVE SURFACE NAME, MASTER SURFACE NAME With the spur gear fully constrained, it was designated the master surface. After an unsuccessful initial try, additional optional parameters were added to the *CONTACT PAIR coin- mand. These parameters were HCRIT=. 01 and ADJUST= 0.0 01. These parameters did not help the analysis NASA/C_2002-211277 4 converge. They were left in the input deck and described here in an attempt to thoroughly describe the input deck that did run. 3. Defne surface interaction properties. *SURFACE INTERACTION, NAME=MYANALYSIS Where MYANALYSIS is the nalne given by the user in the *CONTACT PAIR colnlnand. 4. All of the above colnlnands nmst be entered into the input deck above the *STEP colnlnand. 5. The *STEP colnlnand created by Patran must be inodified to the following: *STEP, NLGEOM, INC=50 NLGEO is short for nonlinear geolnetry. This indicates alarge deforlnation probleln. The deforlnation of con- tact is large colnpared to an elastic deforlnation of steel. INC= 50 ineans the load step is broken up into 50 substeps or increlnents to help the solution converge. It is difficult to get acontact probleln to converge on the first loadstep. This is because the inodel is floating and free to accelerate until contact is established. When the problem was not converging the following error and warning messages occurred in Abaqus. ***WARNING: OVERCLOSURE OF CONTACT SURFACES FACE and SPUR IS TOO SEVERE -- CUTBACK WILL RESULT. YOU MAY WANT TO CHANGE THE VALUE OF HCRIT ON THE *CONTACT PAIR OPTION. The above warning occurred inany tilnes and ultilnately resulted in the following error inessage indicating non-convergence in the ten increlnents initially used (i.e., INC = 10) ***ERROR: TOO MANY INCREMENTS NEEDED TO COMPLETE THE STEP To overcolne these error inessages, a very slnall load and a high value for INC was used. The analysis finally ran with a 5 lb load and INC = 50. INC = 50inakes the probleln iterate and run longer. A slnaller value will speed up the analysis, but the solution inay not converge. The 5 lb force was applied in Patran and ap- peared in the Abaqus input deck. . Apply a realistic load with a second load step. Once contact is successfully established, the model is now stiffer and can withstand arealistic load. This was done by copying everything that appeared between the *STEP command and the *END STEP command and pasting it after the existing *END STEP command. Several NSET and *END STEP commands are contained between the *STEP and *END STEP command. These sets of nodes and elements were deleted. Presumably it would not hurt to leave it in. Also the load on the nodes was changed from 1lb per node to 50 lb. Sulnlnary Of Procedure Required To Duplicate Successful Three-Dilnensional Analysis (The Two Tooth Model) 1.Enter Patran and run FaceS. ses to inake face tooth. 2. Run sSpur, ses to make spur tooth and answer yes to all questions. 3. Create the Abaqus input deck and edit as follows: A. Add the contact conmmnds as explained above. B. Modify the *STEP conmmnd as explained above. C. Add a second load step as explained above. The load must be increased as explained above. The following changes were inade to the input deck for the inodel with one tooth on each gear: (For one load step with 5lb load on face gear). NASA/C_2002-211277 5 *SURFACE DEFINITION, NAME=FACE FI, *SURFACE DEFINITION, NAME=SPUR SI, *CONTACT PAIR, SMALL SLIDING, INTERACTION=_, HCRIT=.01, ADJUST=0.001 FACE, SPUR *SURFACE INTERACTION, NAME=AAA ** STEP I, DEFAULT STATIC STEP ** LOADCASE, DEFAULT ** *STEP, NLGEOM, INC=50 NOTE: The existing *STEP conunand nmst be removed and replaced with the one shown above. HCRIT and ADJUST options were added when it was not converging. These options may not be needed. The two tooth Inodelinput deck is Pair2. inp.This Inodelwas inadefrolnFace. ses and sSpur, ses. The *. inp file was Inodified by adding the contact colnlnands above and by changing the *STEP colnlnand as shown. The first attempt on this model was a 1-1b force applied to five nodes (five lb. total force) with INC= 10 on the *STEP colnmand. This attempt resulted in the warnings and error messages described above. When INC was changed to 50, the problem did run to completion. The resulting nlaxinmm stress was 2600 psi with contact at one node in the upper corner of the face gear. After contact is established, more load can be applied in a second load step. To apply the second load step, everything between *STEP and *END STEP was copied and pasted into the input deck. The ELSET and NSET definitions were deleted as redundant. The force on the five nodes were increased from 1to 50 lbs. Contact in- creased to three nodes. The two load step input deck is Pair2a. inp. RESULTS AND DISCUSSION Results For Two Tooth Model (Using C3D8, Eight-Node Linear Brick Element) The first successful run had one load step with 5 lb of force applied. Contact was at one node. The contact stresses were about 2600 psi. Since the actual load should be about 194 times larger and the load should be shared with two pairs of teeth, this stress appears realistic. The second run had a second load step with 250 lb applied. This is about 1/4 of the design load. Contact spread to 3 nodes. The contact pattern at first appears to skip nodes especially when viewing the stress contours on the spur gear. However when looking at the contact pattern on the face gear it can be seen that the pattern actually cuts across a diagonal of a single row of four elements as illustrated in figure 6. This indicates the mesh is too coarse and the contact pattern is fiat. For the case with 250 lb applied force, the contact stresses increased to 46,000 psi. This is considered realistic for such a coarse model. The contact stress pattern is shown in figure 7for the spur gear and figure 8for the face gear. The contact pattern of two nodes contacting across the diagonal of arow of four elements renmined. This implies a4 by 2increase in mesh density should give adequate results. (i.e., four times the number of elements along the height of the teeth and two times the number of elements along the length of the tooth.) This recommendation is based on the results of FEA modeling and favorable strain gage comparison done on spiral bevel gears (ref. 4). A 4by 2increase in mesh density should give about twice as ninny contacting nodes as in the spiral bevel study. In- creasing the mesh density and using the nine tooth model (instead two teeth) will result in models 4by 2by 9/2 = 36 times bigger. Figures 9 to 11 show the Patran "seeds" used to create the mesh in the face gear and spur gear. Meshing Action Obtained With Rotation Of Local Coordinate Systems One method of rotating the gears through mesh is to build each gear in its own local coordinate system. The local coordinate systems are then rotated, as required for meshing, in the Patran session file. This results in the rota- tion of the two gears in the global coordinate system, the system in which the analysis occurs. This is far easier than rotating the gears in Patran and redoing all contact surface definitions and boundary conditions. NASA/C_2002-211277 6