Intro to FEA

Why it matters

Hand calculations work for shafts, beams and bolts with simple shapes. Real parts have holes, fillets, ribs and odd loads. Finite element analysis (FEA) estimates the stresses and deflections in such parts by splitting the geometry into many small, simple pieces (elements) joined at nodes, writing the stiffness equations for each piece, assembling them into one large system of equations (K·u = F), and solving for the node displacements u. Stresses come from those displacements.

FEA is powerful and easy to misuse. A colourful stress plot looks convincing whether the model is right or wildly wrong. The most important skill in this lesson is sanity-checking.

The workflow

1. Define the question. What do you need: peak stress, deflection, stiffness, a natural frequency? This decides the type of study (linear static, modal, thermal...).
2. Prepare the geometry. Remove details that do not affect the answer (small cosmetic fillets, text, threads) but keep details near the region of interest.
3. Assign materials. Young's modulus E and Poisson's ratio for stiffness; yield strength for comparison. For structural steel, E is about 200 GPa and Poisson's ratio about 0.3.
4. Apply boundary conditions. Fixtures (where the part is held) and loads (forces, pressures, bolt preload). This is where most errors come from: a real bolted face is not perfectly rigid.
5. Mesh. Choose element type and size. Finer meshes are more accurate and slower.
6. Solve, then check before you believe it.

Worked example: a cantilever you can check by hand

A steel bar is fixed at one end and loaded at the other. Length L = 200 mm, rectangular section b = 20 mm wide by h = 10 mm deep (load acting across the 10 mm depth), tip load F = 100 N, E = 200,000 MPa.

second moment   I = b * h^3 / 12 = 20 * 10^3 / 12   = 1,666.7 mm^4
tip deflection  d = F * L^3 / (3 * E * I)
                  = 100 * 200^3 / (3 * 200,000 * 1,666.7) = 0.80 mm
root stress     s = M * c / I = (100 * 200) * 5 / 1,666.7 = 60 MPa

An FEA of this bar should give a tip deflection very close to 0.80 mm (slightly more if the model includes shear deformation and the real fixed-end behaviour). The stress at the top surface near the fixed end, away from the corner, should be close to 60 MPa.

How to sanity-check any FEA result

• Compare with a hand calculation of a simplified version, as above. If FEA and the hand calculation differ by a factor of 2 or 10, find out why before going further.
• Check reaction forces. The solver reports the forces at fixtures. They must balance the applied loads (here, 100 N and a 20 N·m moment at the fixed end).
• Look at the deformed shape (with exaggerated scale). Does it bend the way you expect? Parts flying off or bending the wrong way mean missing or wrong constraints.
• Check units. A mm model with loads entered as if in metres gives results off by factors of 1,000 or more.
• Run a mesh convergence study. Refine the mesh in the region of interest and re-solve. Displacement should settle quickly; stress should settle to within a few percent. If it keeps rising with every refinement, you are probably looking at a singularity.

Singularities

At a perfectly sharp re-entrant corner, or at a point load or a point fixture, the theoretical stress is infinite. FEA shows a "hot spot" there that grows every time you refine the mesh. That number is not real. In the cantilever, the corners where the bar meets the fixed support do this. Real parts have fillet radii and real supports are not perfectly rigid, so the fix is to model the real fillet, read stress a small distance away, or treat the support more realistically, not to report the peak.

Free tools

• FreeCAD FEM workbench with the CalculiX solver is free and handles linear static and modal studies. Meshing uses Gmsh or Netgen, bundled with FreeCAD.
• Several commercial packages offer free student or limited editions; check their current terms. Checked on 2026-10-23.

Common mistakes

• Over-constraining. Fixing every face of a bolt hole makes the part far too stiff.
• Reading peak stress at a singularity.
• Using linear analysis beyond yield. Linear static FEA assumes stress is proportional to strain. Once the result is above yield, the answer is no longer valid (non-linear analysis is a separate topic).
• Trusting defaults. Default mesh sizes and contact settings are not chosen for your problem.

A note on real design

FEA supports engineering judgement; it does not replace it. Results for real products are checked by experienced engineers, validated by testing where it matters, and, for designs that affect public safety, reviewed and signed by a licensed professional engineer.

Recap

• FEA solves K·u = F on a mesh of elements; stresses come from displacements.
• Most errors come from boundary conditions, units and meshing.
• Always compare with a hand calculation, check reactions and deformed shape, and run a mesh convergence study.
• Hot spots at sharp corners and point loads are singularities, not real stresses.

Try it

On the Do tab, model the cantilever in FreeCAD, run it, and compare the result with the hand calculation.