Subject to Dynamic Cornering Fatigue
CAE/FEA Engineer at Aventec
Introduction
As a critical component of the vehicle, automotive wheels must meet strict safety requirements. The dynamic cornering fatigue test is a required standard by SAE. The test simulates cornering induced loads to the wheel, and it is commonly known to be the most severe test to pass in the industry.
Meeting the requirements of this test requires an extensive amount of resources, especially at the development stage where design iterations and field measurements are combined to come up with a reliable design. Furthermore, the complex shape and geometry of wheel designs make it hard to rely fully on an analytical solution for fatigue analysis.
In this work, I performed a numerical simulation of the dynamic cornering fatigue test using Abaqus/CAE and Fe-Safe. Three different methodologies were presented to model the wheel bending moment. Shape optimization using Tosca was also performed to optimize the fatigue life of the wheel design.
To push the complexity of the study furthermore, I performed a fatigue-based shaped optimization combining outputs from Fe-Safe with Tosca and Abaqus/CAE. The results showed that a reliable optimization solution should consider the fatigue induced damage rather than the static solution.
The dynamic cornering fatigue test is a standard SAE test (SAE J328). If the wheel design passes this test, it has good chances of passing all other required durability tests which usually include radial fatigue tests and impact tests.
During the cornering fatigue test setup, as illustrated in Figure 1, the downside outboard flange of the wheel rim is clamped firmly to the test frame, then a loading shaft is attached to the mounting surface of the wheel through bolts while it is connected to a load cell at the other end.
In a typical qualification testing program, the wheel design should withstand +150,000 fatigue cycles to pass the test. For demonstration purposes, the typical load has been raised to 6,125 N in this study to cause premature failure. I used the aluminum A356T6, having a Young’s modulus of 69,000 MPa and a Poisson’s ratio of 0.33.
For the first part of this project, I wanted to compare different ways from a more complete and complex simulation to a simpler abstraction while comparing the final results. Therefore, I proposed three different ways of performing the bending test on the same rim design (Figure 2), which the static loading component that precedes the fatigue cyclic loading.
Figure 2: Aluminum Wheel Rim Design
First, the experimental setup is fully modeled including the aluminum rim, the bolts, and the bending arm. In the second simulation, I removed the bolts and used a tie constraint to model the connection between the rim internal loading surface and the bending arm. In the third model, I removed the bending arm and used a coupling constraint to connect the aluminum rim internal loading surface to a loading reference point placed at a distance equivalent to the bending arm length.
Once the results were compared, I used the last simulation results (model #3) to perform the rest of the modeling including fatigue simulation and shape optimization.
Figure 3: Modeling Approach
Static Loading
Three separate models need to be prepared in Abaqus (Figure 4). In all three models, the rim’s downside outboard flange was clamped, and the rim was meshed with 143,444 C3D10 elements (Figure 5). In the first model (model #1), the bending arm is connected to the rim with five bolts. A tightening bolt torque of 100N is applied to each bolt. A static load of 6,125 N is applied at the bending arm’s free end’s reference point in the downward direction the bending arm was modeled with rigid body elements.
For the second model (model #2), the bolts are removed from the model and the bending arm is connected to the wheel using a tie constraint. Similarly, to the previous model, the bending arm is modeled using rigid body elements, and the bending load is applied at the free end’s reference point.
For the third model (model #3), the bending arm is removed from the model, and is replaced by a reference point connected to the internal loading rim surface via a kinematic coupling constraint.
Figure 5: Meshed Wheel Rim
The obtained results show very similar values of contour plots for Mises stresses and for Principal stresses for all the three models as show in Figure 6 and Figure 7. While the runtime was considerably faster; 1,049 s, 164 s, and 50 s for Model #1, model #2 and Model #3 respectively. The very comparable results prove that the simpler abstraction (Model #3) is a valid approach to model the static bending test, which will be used for subsequent fatigue and shape optimization with way faster turnarounds.
Fatigue Analysis
I used the obtained static results from Model #3 analysis above to perform the fatigue analysis using Fe-Safe. A scale and combined approach was used to apply to the cyclic loading by using the generated stresses from the static analysis as amplitude. A loading ratio of R=-1 was considered, meaning that the same cyclic amplitude was applied in the downward and upward directions. The normal strain algorithm with Marrow stress correction was used. I relied on Fe-Safe External Database for fatigue material parameters as shown in Table 1:
Table 1: Fatigue Material Parameters
As expected, fatigue life results show that damage will initiate at the spokes level with an estimate of 20,714 cycle as illustrated in Figure 8. The obtained life cycle is way below the required standard (+150,000 cycle), therefore the proposed design fails to qualify; this was done on purpose in order to show case how we can use shape optimization to improve the design. The next section will discuss the how.
Shape Optimization
Shape optimization is mostly used at the end of the design process when the general layout of a component is more or less fixed and only minor changes and improvements are allowed (Figure 9). As an initiative to maximize the fatigue life of the rim’s proposed design, I performed a shape optimization analysis using TOSCA.
In the shape optimisation simulation, the objective function was to minimize Mises stresses with a constant volume constraint. I added some other restrictions that respect the geometry and the manufacturability of the rim. Restrictions include fixed outside perimeter of the rim, rotational symmetry, stamping constraint in the small spoke holes, demolding constraint, sliding control for the outer and the inner rim surface.
Figure 10 and Figure 11 show an apparent smoothing of the stress contours around the spokes area, this smoothing corresponds to a 5.60% stress reduction for Von Mises stresses, and 7.19% reduction of principal stresses.
Figure 11: Shape optimization results – Max Principal Stress contours: Left-original design, Right-optimized design
Fatigue Analysis after Shape Optimization
I reran the fatigue analysis on the optimized rim design. The goal was to investigate the optimized design performed under cyclic loading to see whether the shape optimization procedure would help improve its performance as it did for static loading.
For the new optimized design, the minimum fatigue life is observed around the spoke area with an estimate of 20,007 cycles, which corresponds to a 3.41 % reduction in life compare to the original design.
Figure 12: Shape optimization results – Max Principal Stress contours: Left-original design, Right-optimized design
Often stress reduction already leads to a significant increase in durability. Nevertheless, for realistic models, stress peaks are identified through static analysis which may differ largely from areas of maximum damage. In these cases, stress based shape optimization may even worsen the design performance, which suggest that the fatigue life simulation should always be included in the optimization loop.
References
X. Wang, X. Zhang, Simulation of dynamic cornering fatigue test of a steel passenger car wheel, International Journal of Fatigue 32 (2010) 434–442
U. Kocabicak, M. Firat, Numerical analysis of wheel cornering fatigue tests, Engineering Failure Analysis 8 (2001) 339-354
Abaqus 2020 Documentation.