Finite Element Analysis of a Space-Frame Chassis

This project aims to analyze a simplified space-frame chassis of a Formula SAE racecar. The finite element analysis will look at the maximum stress and displacement of the chassis with the mounted engine load and suspension pickup. Matlab and Abaqus were both used for the FEM solutions and the results from the two were compared. Results were very similar for displacement but some differences exist for the stress values as different ways of intepretations are used.

I. Introduction

Space frame chassis are commonly used in race cars. The goal of race car chassis is to be lightweight and rigid. As a space frame chassis utilizes a tubular design, it is convenient for prototyping and the suspension, engine, and body panels are directly attached to the chassis. The space frame is an idealized model of the structure built from rigid linked connected to freely rotating nodes and it tries to achieve a perfectly rigid frame.  This project analyzes the maximum stress and displacement of the Formula SAE racecar chassis under specific loads. Through finite element analysis, each node will be calculated for three displacements and three rotations with respect to the global Cartesian axes. The specific loads from engine and suspension are incorporated into the final calculation.

II. Finite Element Formulation

For each node of a spatial beam element, there are 6 degrees of freedom: the displacement in x, y, z direction and the angular displacement about the x, y and z axes. A two-node spatial beam element will have altogether 12 degrees of freedom. The local stiffness matrix (in the local coordinate) can be derived by a linear supposition of the stiffness matrices of (a) bar in axial tension; (b) bar in torsion; (c) Euler-Bernoulli beam in bending (x-y plane) and (d) Euler-Bernoulli beam in bending (x-z plane). The details of the derivation are left out but the matrix supposition is explained with the figure below:

Figure 1: Stiffness Matrix Supposition

After some coordinate transformation, the local stiffness matrix can be expressed in the global coordinate.

III. Validation and Benchmark with Cantilever Beam

Before using the stiffness matrix and coordinate transformation on the entire chassis structure, this finite element formulation was tested on a single cantilever beam with a concentrated force applied to its end in Matlab and Abaqus. The results were plotted as shown in Fig. 2 and Fig 3. Four different element sizes were checked. As the element size reached about 20 elements, the solution converged. As shown in all four plots, the displacement solutions from Matlab and Abaqus matched with the analytical solution with less than 1% error. The stress solution from ABAQUS shows a slightly larger error.

Figure 2: Displacement plots of cantilever beam comparing analytical, Matlab, and Abaqus solutions

Figure 3: Stress plots of cantilever beam comparing analytical, Matlab, and Abaqus solutions

IV. Geometry and Boundary Conditions

The space-frame structure’s geometry is shown in Figure 4. The chassis members are structural steel tube with 3 different specifications: D33t2, D25.4t1.5, D14t1 where D and t denotes the outer diameter and wall thickness respectively.  The engine block can be considered as a rigid body compared to the stiffness of the chassis. But since the behavior and properties of rigid elements in ABAQUS is not clear, a different approach is taken for better comparison. In this project, the engine block is modeled with a set of members connecting the 6 engine mounting points, with a Young’s modulus 10 times that of structural steel. A uniform mesh size of 25mm is used to generate the FEA grid for this analysis. 

Figure 4: Space-frame chassis geometry

As shown in Fig. 5, the boundary conditions for the chassis are fixed supports at the front suspension pickup points, constraining the nodal displacement in the x,y,z direction. The rear suspension pick-up points are loaded with concentrated forces in the opposite direction on each side to simulate the chassis twist during vehicle cornering. The forces are both in the z direction with a magnitude of 2kN.

Figure 5: Finite Element Analysis Set-up

V. Results

1. Deformation

The torsional stiffness results from MATLAB and ABAQUS are 3266 Nm/deg and 3264 Nm/deg, which are very close.

To quantify the difference in deformation between the Matlab and Abaqus solutions, the structural nodes’ displacements are extracted and compared as shown in Fig. 6. The maximum different is at the order of 1e-3 mm, which is negligible. Many of the points with larger differences correspond to short chassis members. Since a uniform size of 25mm is used, some of these members may not have enough resolution to resolve the curvature in geometry.

Figure 6: Displacement difference between Abaqus and Matlab at chassis structural nodes

2. Stress

Although the solution from MATLAB and ABAQUS are very close in terms of deformation, the solutions for maximum principal stress show have more differences, as shown in Fig 7. The maximum principal stress across a given section is exported, i.e. the outer most position. The overall pattern and distribution of stress are similar between the two solutions. But in terms of the maximum value of the maximum principal stress and where it occurs. The two solutions differ. In MATLAB, it occurs at one of the engine mounts with a magnitude of 111.6 MPa. In ABAQUS, it occurs at the junction of the front roll-hoop and the side impact structure, with a smaller magnitude of 96.5 MPa. At the front suspension pick-up points and the top of the roll-hoop, there is also a higher level of stress compared to ABAQUS’s prediction.

Figure 7: Maximum principal stress of the chassis frame from (a) Matlab solution and (b) Abaqus solution

3. Discussion

The MATLAB code and ABAQUS implicit give similar results in terms of total deformation and hence the chassis torsional stiffness, which is the main target for a chassis frame design. The code is successful in this sense. However, the solution for stress is less satisfactory. This is partly due to the nature of stress field being a first-order derivative of deformation. Since the mesh is generated almost uniformly across the whole structure, the stress values accuracy is limited by the mesh resolution around areas with large gradient. This is reflected in some of the areas with high stress values in Fig 7.a.

Since the displacement fields are very close between MATLAB and ABAQUS, and that the stress predictions for a cantilever beam are also similar, it is possible that the difference in stress post-processing is related to a different algorithm. The MATLAB code calculates the principal stress taking into account of the nodal displacement due to axial tension and the bending in two planes.

The question then becomes: whether ABAQUS uses the same way of calculation. Since the angular displacement at each node cannot be extracted from ABAQUS, the same code to calculate stress from nodal displacement cannot be applied to ABAQUS data to confirm this.

However, it is confirmed by changing the cantilever benchmark model into a spatially loaded case where Fy = Fz = \sqrt(2)/2 P, P is the concentrated load in the previous cases. It can be seen that the stress output from ABAQUS is lower than MATLAB. This shows that ABAQUS only takes into account the bending in one of the planes instead of both.

Figure 8: Stress output of cantilever loaded in both x-z and x-y planes from MATLAB and ABAQUS

VI. Conclusion

The MATLAB code and ABAQUS have both successfully predicted the chassis total deformation and hence the torsional stiffness with a negligible difference. However, the Stress predictions have much more differences. This is partly due to limited meshing resolution around areas with stress concentration but could also be related to a different post-processing algorithm used by ABAQUS. It stressed the point that FEA post-processing results from commercial software should be treated cautiously.

Nevertheless, the MATLAB code is believed to be accurate enough for solving the deformation and torsional stiffness. It could therefore be used for automated design optimization by assigning different tubing profile to different members to achieve the best stiffness-to-mass ratio.

VII. References

1. Ferreira A.J.M., MATLAB Codes for Finite Element Analysis, Springer Science+Business Media, Ontario, 2009, Chaps. 8.