Bicycle Crank Arm — Static Structural FEA

Problem setup

Before touching ANSYS, the expected stress and deflection were calculated by hand using beam bending theory — treating the crank as a cantilever. This gave ~15,400 psi and 0.067 in. These benchmarks were used later to confirm the simulation was in the right ballpark.

Geometry and material

The 3D CAD model was imported into ANSYS. Non-essential parts (pedal, spindle) were suppressed. Aluminum 6061-T6 was assigned manually (E = 10 Mpsi, ν = 0.33) — replacing ANSYS's default steel, which would give completely wrong results.

Mesh — hexahedral elements

The part was meshed with 20-node hexahedral elements (SOLID186) using the MultiZone method — more accurate than the default tetrahedral mesh for the same number of elements. Finer elements (0.1 in) were applied at the spindle holes where stress concentrations were expected. Result: 8,845 nodes, 1,626 elements, 26,535 equations solved.

Boundary conditions

The three spindle holes were fixed (zero displacement in all directions), replicating the bolt-to-bottom-bracket interface. A 100 lbf upward force was distributed over the pedal bore surface — ANSYS converted this to 509.34 psi of surface traction automatically. All other surfaces were left free (zero traction by default).

Solving

ANSYS assembled and inverted a 26,535-equation system using a Preconditioned Conjugate Gradient (PCG) solver across 4 parallel CPU cores. Convergence was reached in 175 iterations with a residual of 9.3×10⁻⁹ — well below the 1×10⁻⁸ tolerance. Total wall time: 17 seconds.