Using Finite Element Models to Predict Suspension Member Loads and Compliance in a Formula SAE Vehicle
A racing vehicle suspension system is an elastic structural linkage that defines the many of the handling characteristics of the racecar while supporting it under complex loading scenarios. The Formula SAE team at Virginia Tech uses Abaqus to determine suspension member loads and compliance to design a safe and effective suspension system.
An Abaqus finite element model was developed for the right front suspension corner, shown in Figure 1, to determine member loads and suspension compliance. The finite element model was initially developed with beam elements, allowing axial, bending and torsional loads, and connector elements to represent kinematic degrees-of-freedom of the joints. Welded control-arm members on the upright, simplified pull-rod (PR) mounting brackets on the upper control arm (UCA) and the toe-rod (TR) were also represented. The pull-rod member actuates the spring and damper through the bell crank to the wheel assembly, previously mounted on the upright, Figure 2. The front-corner model used several design load cases, revealing reduced axial loads and increased bending moments reducing the critical buckling load of the compressive members.
Figure 1. Corner suspension assembly with components labeled, beam/connector FE model.
Figure 2. Detailed representation of the upper control arm and pull-rod connection to upright.
The Abaqus front-corner suspension model incorporates steering loads from the driver, input as prescribed displacements at the toe-rod (TR). The steering linkage displacement changes the upright orientation angles and wheel load directions applied to the suspension. Including steering inputs in the FE model result in significant changes in member loads for load cases involving slip-angle effects used to determine the effective steer angles during cornering. Quasi-static design loads are used to predict the vertical movement at the wheel center and associated member loads. The suspension designer uses these results to determine if changes to spring rate or anti-roll bar stiffness will result in a more desirable wheel movement for a given loading condition.
Determining which suspension components contribute most to camber and toe compliance in the suspension system requires a more refined finite element model. The purpose of the suspension compliance model was to match camber and toe stiffness goals and breakdown stiffness on a component level. A three-dimensional finite element model of the suspension linkage parts was developed from a full-car solid model, importing the front suspension corner parts into Abaqus. A discrete rigid tire model was used to avoid confounding the suspension compliance with the tire elastic response. Assembly constraints were used to locate the suspension parts, defining sets and contact surfaces in the part models. The model makes extensive use of partitioning and sets to parameterize part meshing using C3D10M elements. Contact-pair modeling between joint components was as realistic as practical, using shear and frictional forces between contact pairs to mimic bearing and clamp loads. Driving condition load cases were applied at the tire contact patch with boundary conditions applied at the inboard suspension points on the chassis. Two load cases were studied for suspension compliance, the 5g bump and pure lateral load under acceleration cases. Figure 3 shows the displacement magnitude for the lateral load under acceleration load case and the stresses in the rod-end connections. The compliance at the wheel center was used to estimate the overall corner compliance. The displacements at the joints were queried to determine the load distribution and relative displacement in the rod-ends, including whether or not the joints reached the hard stops in the spherical bearing.
Figure 3. Right front corner compliance model, (a) displacement magnitude for the lateral load under acceleration load case, (b) von Mises stress in the rod-end connections.
Virginia Tech FSAE uses Abaqus extensively for design, analysis and simulation for chassis, suspension and driveline subsystems. Previous modeling emphasis was associated with load transfer through contact modeling in assemblies and subsystems, suspension, chassis mounts, bell-crank design and integrated composite structure. The immediate future design and modeling efforts are to support dynamic load simulation and model correlation with vehicle system test. The Abaqus simulation environment allows Virginia Tech FSAE to evaluate integrated vehicle subsystem and systems design, in addition to component level analysis. Effective use of integrated multi-step simulation is key to making better design trade-offs and optimizing vehicle performance.
Lane Borg, Associate Engineer, Performance Test Driver
Johnson Miles, Associate Engineer Crane and Large Derrick Product Development
Bob West, Associate Professor Mechanical Engineering Department Virginia Tech
