Bevel Gear Tooth Bending Stress Evaluation Using Finite Element Analysis

Prepared by Emre Turkoz, BSME | [email protected] Can Ozcan, MSME | [email protected]

AKRO R&D Ltd. Phone: +90 (262) 678-7215 KEMAL NEHROZOGLU CAD. GOSB TEKNOPARK HIGH TECH BINA 3.KAT B5 GEBZE/KOCAELI/TURKEY - 41480

1

1. Introduction Bevel gears are used widely at different applications in Industrial Machinery, especially in the automotive industry. Since bevel gears have such a great range of applications, it’s crucial to be able to analyze their deformation under an applied load. In this work, our aim is to investigate the behavior of a bevel gear set under a given moment using Finite Element Analysis. The results are evaluated both numerically and analytically. For the analytic solution, formulas from Norton [1] is used. Finite element analysis is used as the numerical method. Autodesk Simulation Mechanical 2012 is used to perform finite element analysis.

2. Properties of the Bevel Gear Set The bevel gear set consists of two helical gears. In gear terminology, the smaller one is called pinion, and the larger one is called gear. The properties of the gear and the pinion are as follows:

# of tooth in Gear: Ng = 29 # of tooth in Pinion: Np = 17 Facewidth: F = 62.354 mm Gear pitch diameter: dg = 220 mm Pinion pitch diameter: dp = 130 mm Pressure angle: Θ = 20o Spiral angle: ϕ = 35o Module: m = d/N = 7.58 mm

3. Description of the Problem The problem solved is the static application of a moment of 600000 Nmm on the pinion, which tries to rotate but is hindered by the grounded gear. The torque is transferred to the gear through contact faces on tooth pairs. The moment causes on these pairs a contact force to be generated. Apart from the contact stress this force forms, roots of the contact teeth also suffer from tooth root bending stress. The aim of this work is the evaluation of this root bending stress generated during the static application of the moment. The numerical and the analytical solutions are compared to validate the model used for the finite element analysis.

4. Analytical Solution of the Problem The methodology for the analytical solution is obtained from Norton [1], as stated before. The formula for the tooth root bending stress, for the gear or for the pinion, is given below:

2

: Tooth root bending stress [Mpa] T : Torque applied or transformed to the gear/pinion [Nmm] d : Diameter of the gear/pinion [mm] F : Facewidth [mm] J : Geometry factor of the gear/pinion m: Module [mm] Ka: Application factor Km: Load distribution factor Ks: Size factor Kv: Dynamic factor Kx: Gear geometry factor (spiral/straight)

Gear Ratio

0.586207

Tp [Nmm] d [mm]

600000 220

F [mm]

62.354

J

0.21

m [mm]

7.58

Ka

1

Km Ks Kv Kx

1.6 1 1 1.15

[MPa]

44.82072

The analytical calculation is performed for the gear in our problem. The parameters and the result are given in the table at right above.

5. Modeling of the Problem Using the Finite Element Analysis

Figure 5.1: Top and Right views of the meshed bevel gear set

As stated above, Autodesk Simulation Mechanical 2012 is used to perform the finite element analysis. As the Analysis Type, “Static Stress with Linear Material Models” is chosen, since the model doesn’t include any nonlinearity. As Mesh settings, an absolute surface mesh size of 6 mm is imposed. Solid mesh is set to the option “All tetrahedral”. Contact setting is left as the default setting, bonded. To get more accurate results, mesh of the contact region is refined. The vertices in the contact zone are selected as refinement points and they are forced to have the mesh size of 1.25 mm and the radius of 7 mm.

3

The boundary conditions and moment applied should be specified in the Load and Constraint Groups section. Since the tetrahedron element doesn’t possess rotational degree of freedoms, separate beam joint elements should be defined, on which rotational degree of freedoms can be imposed. Two surfaces encapsulating the inner cylindrical area of the gear and the two surfaces encapsulating the cylindrical surface of the shaft connected to the pinion are selected and joints are added to these surface pairs. The two joint vertices of the gear are selected and fixed boundary conditions are imposed, whereas the two joint vertices of the pinion are imposed only one rotational degree of freedom, which is y direction in our model. The two vertices in the pinion joint are selected and imposed a moment of -300000 Nmm in y direction, which add up to -600000 Nmm, the desired amount for our model. For shorter solution times, contact region surfaces can be separated from their corresponding parts by assigning a new surface attribute to the participating line elements of each part. Then these contact surfaces should be selected and specified as in surface contact.

6. Numerical Solution of the Problem Using the Finite Element Analysis The finite element analysis results are pretty much close to the analytically evaluated results. The mean tooth root bending stress, evaluated by selecting the nodes at the root of the contact teeth, has the value of 37,016 MPa, which corresponds to the 17% difference with the analytical result.

Figure 6.1: The gear mesh. The contact region has the finest elements

4

Figure 6.2: A closer look at the contact region. Pay attention to the contact pattern where the stresses are high

To calculate the tooth root bending stress, the vertices in the root region are selected and the mean stress is calculated. The mean, as it can be seen from the figure below, is 37,016 MPa.

Figure 6.3. Calculating the root tooth bending stress

5

To see the big picture more clearly, stress distribution plot of the root vertices are generated as can be seen below. It is to be observed that the stress values in general lie between 20-50 MPa. The values are concentrated between 35 and 40 MPa. 160 140

von Mises Stress [MPa]

120 100 80 60 40 20 0 -72

-67

-62

-57

-52

Position in z Direction [mm]

Figure 6.4. Stress distribution of the root vertices.

7. Discussion We see a great similarity between the numerical and the analytical results. From the results evaluated, it can be said that the FEA Analysis is validated. The difference in between is caused by many factors. The accuracy of the FEA results may be increased by using more mesh elements, which encapsulate contact regions more densely. Also a smaller tolerance for the solution of the stiffness matrix can be imposed.

8. References [1] Norton, Robert L., “Machine Design: An Integrated Approach”, Third Edition, 2006, Pearson Prentice Hall .

6