Residual Stresses in Passenger Car Wheels

Knowledge of the residual stress state in wheels resulting from manufacturing and subsequent service loading is useful for several practical reasons. The ability to estimate residual stress levels permits the tuning of manufacturing processes to control the magnitude and distribution of these stresses in new wheels in order to achieve safe performance in service. Similarly, understanding the redistribution of residual stresses following application of service loads (wheel/rail contact and thermal stresses) is crucial to avoid operating conditions which may lead to premature wheel failure. Axisymmetric (2-dimensional) analyses are typically performed in order to conduct manufacturing process simulations since these processes affect the entire wheel in a circumferentially uniform sense. Generally, analyses involving service loading have sought to identify the “shakedown state” at which the residual stress distribution stabilizes after some number of loading cycles. In order to properly account for service loads, 3-dimensional models are required since contact and brake shoe thermal loading are not axisymmetric. Since the as-manufactured residual stress distribution must be considered in a service loading simulation, 3-dimensional modeling of this process is required. This paper presents a preliminary comparison of 2and 3-dimensional modeling of the wheel heat treatment process. Except for the increased computational time required for the 3-dimensional analysis, the results agree favorably. The 3-dimensional model is used to simulate service loads involving wheel-rail contact loading representative of a typical passenger car. The model is exercised with a variety of material models for comparison with previous work. Results are presented for multiple loading scenarios and shakedown stress states are established for a range of applied loads. INTRODUCTION Residual stresses are important to understand in order to avoid operating conditions which may lead to development of adverse stresses which can cause premature wheel failure. Residual stresses in wheels originate during the manufacturing process and are subsequently modified when wheels are placed in service and subjected to repeated wheel/rail contact and thermal loading during on-tread friction braking. The manufacturing process generally leaves the wheel rim in a state of residual compression. This compression helps to resist wheel tread crack formation. Thermal loading from ontread friction braking has been demonstrated to cause rim stress reversal from compression to tension, leading to the development of wheel tread thermal cracking. Early attempts to estimate residual stresses in wheels considered a combination analysis. Standard finite element techniques were applied to estimate the residual stresses due to the quenching and annealing portions of the manufacturing process [1, 2]. These stresses were then used as an initial condition for subsequent consideration of mechanical (wheel/rail contact) and thermal (from friction braking) stresses that were analyzed using a “shakedown” approach [1, 3]. The shakedown method purports to provide efficiency in that the stabilized residual stress distribution is achieved in a single step, without the need to consider the loading history cycle-by-cycle. The method, however, comprises several limitations, the most important of which is the elasticperfectly plastic material characterization. More recent research has focused on the effect of brake shoe heating and the potential for rim stress reversal [4, 5]. This work was accomplished using an axisymmetric (2dimensional) representation of the wheel. This modeling assumption precludes realistic application of wheel/rail 1 Copyright © 2006 by ASME contact loads, since the earlier research demonstrated that thermal loading is the dominant service load. A secondary goal of this work is to begin to formalize the procedures to be specified in a developing American Public Transit Association (APTA) wheel design standard. The new standard is under consideration as a replacement for the current Association of American Railroads (AAR) Standard S660. The S-660 standard specifies the conduct of specific finite element analyses using prescribed loading conditions. However, the loading specified in the S-660 standard is more relevant to freight than passenger applications. Specifically, the thermal loading requirement represents a drag-braking scenario, more common in freight than passenger operations. Further, the current S-660 has several shortcomings: 1. The analysis assumes fully elastic conditions. 2. There is no allowance for the existence of beneficial compressive residual stress that is imparted during manufacture. 3. The basis for approval is an empirical comparison. Approval for use of the wheel in service is granted following favorable comparison (by an independent third party) of results of this analysis with those in a database of previous analysis results for other wheels. In order to develop a revised wheel qualification procedure, a methodology must be developed to overcome these limitations. As described above, the bulk of previous work has focused on application of axisymmetric models to estimate residual stresses due to heat treatment and thermal loading from braking. Contact loads were not considered. To properly account for wheel/rail contact effects and represent braking more realistically, a three-dimensional model is necessary. Furthermore, in the spirit of developing a useful alternative wheel design standard, an integrated modeling approach is desired. An integrated model will overcome the first two limitations noted above. The remainder of this paper seeks to address these issues. The revised wheel design standard is envisioned to be self-qualifying in that independent review of the results will not be required. Instead, application of a fatigue criterion is being considered whereby the adequacy of the wheel design can be demonstrated using the results of the prescribed analysis. This effort is described in a companion paper in these proceedings [6]. The context for the work reported here is an assessment of the importance of contact load effects to the design standard. Previous work, based on axisymmetric models, inherently limits such an examination [1,2]. Restrictions on the analysis technique imposed simplified representations of several important features. To account for the lateral movement of the wheel on the rail, equivalent Hertz contact loads were applied to a rectangular patch for only one (static) wheel load. In addition, the inelastic effects had to be represented as an Elastic, perfectly plastic material with carefully chosen flow stress levels. For regions away from the tread surface, neglect of contact effects is well justified. In regions close to the surface, a more accurate representation of the influence of wheel-rail interaction could adjust or tune calculations based on braking loads alone. This paper starts with a model of wheel manufacturing to establish the credibility of a three-dimensional model of a wheel. The same mesh is used to examine the influence of load and material parameters on the nature of the residual stress field in the wheel. These effects are examined as service conditions without pre-stress from manufacturing to ensure that the contact field is the sole influence. The depth of the compressive zone near the tread surface is the focus of the calculation. HEAT TREATMENT SIMULATION: COMPARISON OF 2D AND 3D MODEL RESULTS A 32-inch (81 cm) reverse dish passenger car wheel is chosen for the prototype analysis to allow comparison with previous results obtained using an axisymmetric model. The wheel is quenched from a uniform temperature of 1550 °F (843 °C). The wheel is then annealed at 925 °F (496 °C) for approximately 4 hours. After annealing, the wheel is allowed to cool to room temperature. The analysis procedure follows that described in [1]. A complete description of the development of the three-dimensional heat treatment model presented here is described in [7]. Temperature-dependent thermomechanical material properties are used. The room temperature yield strength is 45 ksi (310 MPa). Viscoelastic creep is accounted for using a user subroutine in ABAQUS [8]. Convective and radiative boundary conditions are applied to permit surface cooling during the simulations. Two and three-dimensional models were constructed to compare results of the heat treatment simulation. The 2-D model is similar to that presented in [1-5] and comprises 1362 elements, as shown in Figure 1. Special care is taken in the construction of the three-dimensional model so that sufficient element density exists in the vicinity of the point of application of the contact loading. Figure 1. 2D axisymmetric model. 2 Copyright © 2006 by ASME The three-dimensional model is shown in Figure 2. It consists of approximately 53,000 8-node brick elements. The mesh is graded in the circumferential direction for computational efficiency. Figure 2. 3D heat treatment/contact model. Figure 3 shows the refined mesh in the vicinity of the contact load application point. The dense mesh is needed to capture the contact region details accurately. Figure 3. Mesh refinement in wheel rim (detail from Figure 2). The residual circumferential (hoop) stress is the result of most interest from this analysis. Contours are shown in Figure 4 (for the 2D mesh) and Figure 5 (for the 3D mesh). Contours are in MPa (1 ksi = 6.895 MPa). The 3-dimensional model requires substantially more computational time. However, both the qualitative distribution and quantitative magnitudes are in excellent agreement. Results for transient temperature and other stress components are in comparable agreement between the two models. These checks were used to assess the acceptability of the tied constraint used to connect the regions of dissimilar mesh. Figure 4. 2D model: hoop stress in wheel rim after simulated manufacturing process. Contours in MPa. Figure 5. 3D model: hoop stress in wheel rim after simulated manufacturing process. Contours in MPa. CONTACT SIMULATION: MODELS AND RESULTS Contact loading was considered in two ways. First, a rigid “rail” was developed whose geometry approximated that of a 132RE rail crown. Initial results using a rigid representation of the rail resulted in extremely high contact pressure at the wheel/rail interface due to the small size of the of the wheel/rail contact patch. In order to achieve the proper contact pressure distribution and patch size, a deformable rail 3 Copyright © 2006 by ASME model was required. To minimize model complexity, a “hybrid” deformable rail was created using a small number of deformable 3D elements to represent the rail head coupled to a rigid body which could be used to control the position and displacement of the rail. Symmetry boundary conditions are applied to the wheel/rail model shown in Figure 6. Figure 6. 3D wheel model with deformable rail. Figure 7 shows the construction of the parts for the deformable rail that loads the wheel. Only the portion of the rail that contacts the wheel is needed to represent an indenter that applied the load. Figure 7. Deformable rail model consists of two parts: deformable tip (left) and rigid support (right). Reference values and validation for the model were established by considering the classic Hertz elastic contact solution for a static wheel load (P = 17,500 lb or 77.843 kN) applied by a 32 in. wheel on a 10 in. rail crown. In the analytical solution, the major axis of the contact ellipse is 0.64cm; the minor axis is 0.468cm; and the maximum stress is 1243 MPa. For the finite element model, the major axis is 0.65cm; the minor axis is 0.56cm; and the maximum stress is 1227 MPa. Several material characterizations were investigated. Table 1 lists the five that were compared. A linear, elastic material is included as a reference. Young’s modulus is 30,000 ksi (213,331MPa); the kinematic hardening modulus (if active) is 4,282 ksi (29,526 MPa). Table 1. Material definitions. Materia l model Description Yield strength