Context
Individual first-year master's (MESI) lab project (Finite Elements module) at the Faculty of Physics & Engineering, University of Strasbourg, supervised by Dr Salah Elbarnaty and Prof. J.P.M. Correia. The case study: a 2 m cantilever beam (200 mm section, 1 mm thick, steel) under a 250 N load, in a plane-stress assumption. The goal: validate a linear elastic model by comparing the ABAQUS simulation against the analytical strength-of-materials solution, and understand how mesh density and element formulation drive accuracy.
Approach / Solution
I first set the analytical reference (Euler-Bernoulli): second moment of area, maximum normal stress (±75 MPa, well below the 400 MPa yield limit) and tip deflection (4.762 mm). This solution is the yardstick for every numerical configuration. In ABAQUS I built the model carefully: geometry, steel material (E = 210,000 MPa), consistent units (mm / MPa / N), the clamp defined from the initial step, and Sets to apply boundary conditions and loading once before duplicating the model across the eight configurations. I used plane-stress elements CPS4 (linear quads) and CPS8 (quadratic). I then crossed two factors: mesh density (1×6, 2×12, 4×12, 8×24) and interpolation order (CPS4 vs CPS8). For each case I extracted the S11 stress map, the U2 deformed shape, the nodal reactions RF2 and the relative error on deflection, gathered in a comparison table.
Results
The standout result: with just 6 quadratic CPS8 elements I get a 0.33% error on deflection, better than 192 linear CPS4 elements (0.94%). With CPS4 the convergence is monotonic but slow (40.7% error at 1×6, down to 0.9% at 8×24); with CPS8 it is essentially reached at the coarsest mesh. I also exposed and understood shear locking: on a coarse CPS4 mesh the linear elements are too stiff to capture the bending curvature, underestimating the deflection by 40%. On the validation side, the support reaction is always exactly 250 N (global equilibrium), and the S11 distribution stays symmetric about the neutral axis, two sanity checks I verified every time. My takeaway: choosing an element formulation suited to the physics beats blindly refining the mesh, a valuable mindset in an industrial setting where compute time matters. This lab was also my first hands-on with ABAQUS, and made me understand why such a solver becomes essential once you leave the linear case (nonlinearities, contact, crash), where CAD tools like Inventor Nastran hit their limits. Avenues I could still explore: push into nonlinear (large displacements, plasticity, contact), compare with beam or shell elements, study reduced integration and its hourglassing modes, and benchmark ABAQUS against another solver on the same case.