Finite Element Analysis of Hyperloop Chassis

Goal: Mechanical simulation of a chassis body in a non-inertial reference frame undergoing rapid deceleration from its brakes

 

Loading and Analysis Conditions

For the boundary conditions of the chassis frame element model, the initial velocity of the system will be the theoretical maximum velocity of 120 m/s. The maximum braking force is 351.5N per brake. Each brake will have a 2 point connection to the chassis, resulting in a load of 175.75N being applied to each of the brake connection points. Overall there are a total of 12 brakes, resulting in a total braking force of 4128N. This total braking force results in an approximate 5g deceleration since the chassis is 82.4 kg.

Reducing Complexity Pt. 1

Beginning with determining the structural stability and general stress distribution, a solid model of the chassis base frame will be simplified. These simplifications can be seen in the image to the right, which includes the removal of non-essential bolt holes and hardware. Ultimately, the splitting of this frame along its symmetric axis decreases the time to compile, mesh and solve the model.

Mesh with tetrahedron elements

Finite Element Analysis Implementation

Starting with solving for the stresses and strains of the chassis frame, a transient structural model in ANSYS is produced, applying forces that lead to a constant 5g deceleration over the braking period. This constant deceleration means that the analysis needs to be done in a non-inertial reference frame to account for the additional inertial forces [1].

Since the brakes are bolted on the chassis, the forces are assigned to the bolt holes. Each bolt hole is applied 175.75N with the assumption that the forces from each brake, 351.5N, are split evenly. A distributed mass of 80.2 kg along with the standard earth gravity is applied on this chassis to include weight other subsystems that would be mounted on this chassis, such as propulsion and electronics.

Tetrahedron elements were selected for the mesh to avoid the time-consuming hex dominant element shaping. Given that quadratic elements generally produce more accurate results than their linear counterparts, using these second-order tetrahedron elements, will help produce accurate results at larger element sizes, decreasing the necessary computation time.

Convergence Study

The initial element size used in analyzing the chassis is 160 mm. Using the element size of 160 mm results in a max Von Mises stress of 101.65 MPa. The deformation in the X and Y direction are also tabulated in Figure 16 and they are 0.085 and 0.74 mm respectively. Max X and Y deformation were chosen to be analyzed over general deformation because the movement of the body resulted in ANSYS undesirably including the displacement of the body in the deformation calculation. Further convergence studies were performed over a range of element sizes from 160mm to 5mm. Images from the right show data and graphs of the convergence studies. From these plots, it can be seen that the stress converges at around 20mm.

 

Finite Element Analysis Results

Applying the convergence element size of 20 mm, the Von Mises maximum stress is 112.1 MPa, which is under the tensile yield strength of 241 MPa. The safety factor for this design is thus 2.15, representing an acceptable factor of safety (fos) for high-speed aerostructures. At regions without stress concentrations, the stresses in the frame members range from 10 MPa to 50 MPa. The deceleration in ANSYS is scaled in a manner that fits in the screen.

 

Reducing Complexity Pt. 2

The previous chassis was weight was negligible at roughly 2% of the weight of the whole vehicle. As a result, the new design is heavier and retains more material, but trades off for reducing complexity and adding another symmetry axis for future FEA. Moreover, the manufacturing process is much simpler.

References

[1] R. Martin, “5.6: Non-inertial frames of reference and inertial forces,” Physics LibreTexts, 05-Nov-2020. [Online].

 

Next
Next

Brake Pad Thermal FEA