[Advanced] — How the PDEs actually get solved, and the failure modes that make a plausible-looking result wrong.

Why numerical methods

Navier’s equations and Navier–Stokes have closed-form solutions only for simple geometries and simple loads. Real parts have holes, fillets, contacts, and mixed materials.

So you discretise: replace a continuous field with a finite set of unknowns, and the PDE with a large algebraic system.

The finite element method

The idea in three steps:

1. Weak form. Multiply the governing equation by a test function and integrate by parts. This lowers the required continuity — the strong form needs second derivatives, the weak form needs only first — so you can use simple piecewise-polynomial approximations.

For elasticity, the weak form is the principle of virtual work:

Internal virtual work = external virtual work, for any admissible virtual displacement.

2. Discretise. Divide the domain into elements. Within each, approximate displacement by shape functions interpolating nodal values:

3. Assemble and solve. Substituting gives the element stiffness matrix, assembled into a global system:

A note that connects this to kinematics: because you assume a continuous displacement field, compatibility is satisfied automatically. That’s the main reason displacement-based elements are the default.

And the variational view: the FE solution minimises total potential energy over the space of possible nodal displacements. It’s the principle of minimum potential energy restricted to a finite-dimensional space — which is why the method converges to the true solution as elements shrink.

Elements

Character
Linear tet (TET4)fills any geometry automatically; overly stiff in bending
Quadratic tet (TET10)mid-side nodes; much better, and the practical default for complex geometry
Linear hex (HEX8)superior accuracy per DOF; hard to mesh automatically
Quadratic hex (HEX20)best accuracy; expensive to generate
Shellthin structures — bending without meshing through thickness
Beam1D members → Beams

Linear tetrahedra are too stiff in bending, and it’s a real error, not a subtlety. A cantilever meshed with TET4 can be 50% too stiff even with a fine mesh, because a constant-strain element cannot represent the linear strain variation bending requires. Use TET10 or hexahedra for anything where bending matters. This is one of the most common sources of wrong FE answers, and it’s silent.

Integration is done numerically at Gauss points. Full integration is exact for the polynomial order and can lock. Reduced integration is cheaper and fixes locking, at the risk of hourglassing — spurious zero-energy deformation modes that look like a wavy mesh pattern in the results. If you see an hourglass pattern, the answer is meaningless.

The locking family

Three related failures, all producing an artificially stiff result:

Volumetric locking — nearly incompressible materials (: rubber, plastic metal flow). Elements cannot deform without changing volume, so they lock up. Fix: mixed u–p formulations, selective reduced integration, F-bar. → Finite Deformation

Shear locking — thin elements in bending develop spurious shear strain. Fix: reduced integration, incompatible modes, or use shell elements.

Membrane locking — curved shells, similar mechanism.

The symptom is always the same: results far stiffer than reality. If your rubber seal model is inexplicably rigid, or your thin plate deflects a tenth of what hand calculation says, suspect locking before suspecting the physics.

Verification and validation

The distinction that matters, and the one most often skipped.

Verification — “am I solving the equations right?”

  • Mesh convergence. Refine and re-solve. If the answer changes significantly, you haven’t converged. This is non-negotiable and routinely skipped. A single-mesh result is an opinion
  • Check against analytical solutions for simplified cases
  • Check equilibrium: do reaction forces sum to the applied load?
  • Check energy balance

Validation — “am I solving the right equations?”

  • Compare against experiment
  • Is the constitutive model valid in the regime you reached?
  • Are the boundary conditions physically real?

A converged solution to the wrong problem is still wrong, and it will have smooth, professional-looking contours.

The mesh convergence pattern

displacement
    │            ╭──────────  ← converged
    │        ╭───╯
    │    ╭───╯
    │ ╭──╯
    └─────────────────────→  elements

Refine until the quantity you care about changes by less than a few percent. Note that displacement converges much faster than stress — a mesh that gives good deflection can still be badly wrong on peak stress, because stress is a derivative of the displacement field and derivatives converge more slowly.

Stress singularities never converge. At a re-entrant corner or a point load, refining the mesh makes the peak stress climb indefinitely — the continuum solution genuinely is infinite there. Reporting “maximum stress” from such a location is meaningless. Either model the real fillet radius, or use fracture mechanics, or evaluate stress away from the singularity per Saint-Venant.

The other methods

Finite difference (FDM) — approximate derivatives on a structured grid. Simple, fast, and poor with complex geometry. Common in wave propagation and some CFD.

Finite volume (FVM) — integrate over control volumes, enforcing conservation cell by cell. Conservative by construction, which is why it dominates CFD.

Boundary element (BEM) — discretise only the boundary. Excellent for infinite domains (acoustics, soil–structure interaction), and it produces dense matrices, so it scales badly.

Meshfree / SPH — no mesh, just particles. Suited to extreme deformation, free surfaces, fragmentation. Less accurate, harder to impose boundary conditions.

Isogeometric analysis — use the CAD NURBS basis directly as shape functions. Removes the meshing step and the geometry approximation error. Promising, not yet mainstream.

The split worth remembering: FEM for solids, FVM for fluids. Both solve continuum equations; the difference is that conservation is structurally guaranteed in FVM, which matters more when the equations are conservation laws in the first place.

Nonlinear and dynamic solution

Nonlinear — Newton–Raphson with load increments, as in Finite Deformation. The tangent stiffness is reformed each iteration.

Dynamics splits into two very different worlds:

Implicit (Newmark, HHT) — solve a system each step. Unconditionally stable, so large time steps are allowed; each step is expensive. Use for structural dynamics, earthquake response, anything where the response is smooth and the duration is long.

Explicit (central difference) — no system solve; each step is cheap. Conditionally stable — the step must satisfy the CFL condition:

the time for a wave to cross the smallest element. That’s typically microseconds, so it’s only viable for short events.

Use explicit for: impact, crash, blast, explosive forming, high-rate metal forming.
Use implicit for: everything slower.

The practical consequence of CFL: one tiny element anywhere in your mesh sets the global time step and can make an explicit analysis a hundred times more expensive. Mesh quality isn’t just about accuracy — in explicit dynamics, one bad element is a runtime cost. Mass scaling is the usual (and slightly dishonest) workaround.

Where results go wrong

In rough order of frequency:

  1. Wrong boundary conditions. Over-constraining creates artificial stiffness and phantom reaction forces; under-constraining gives a singular stiffness matrix. The most common error by a wide margin
  2. No mesh convergence study. A single mesh is an opinion
  3. Reading stress at a singularity. Point loads, sharp corners, and constraint edges — all meaningless
  4. Wrong element type. TET4 in bending
  5. Locking, unrecognised
  6. Material model outside its valid range. Linear elastic run predicting stress above yield, reported as though it means something
  7. Units. Especially the mm–N–MPa vs m–N–Pa mix, and mass density in consistent units. A factor of is entirely achievable
  8. Ignoring geometric nonlinearity where rotations exceed a few degrees → note 10

The habit that catches most of these: do a hand calculation first. Estimate the deflection with and the stress with . If FE disagrees by a factor of ten, one of you is wrong — and it’s usually the model. The hand calculation is not obsolete; it’s your only independent check. → Beams and Structures

Tools

Commercial: Abaqus (nonlinear, research-grade), ANSYS (broad), LS-DYNA (explicit/crash), COMSOL (multiphysics), Nastran (aerospace heritage).

Open source: CalculiX (Abaqus-compatible input syntax), Code_Aster, FEniCS and deal.II (write the weak form directly — excellent for learning), Elmer, OpenFOAM (the CFD standard).

Learning recommendation: FEniCS lets you write the weak form in near-mathematical notation and get a solution, which makes the connection between the theory and the code unusually direct. Or write a small 2D linear-elastic FE solver yourself — element stiffness, assembly, boundary conditions, solve. It’s a few hundred lines and it removes the black box permanently.

That project would fit the build-your-own-shit format well, and it’s a genuine gap in this vault.

The honest note

Modern FE software will produce a smooth, colourful, professional-looking result for almost any input, including nonsense. There is no warning for a wrong material model, an unconverged mesh, or a boundary condition that doesn’t exist in reality.

The software solves the equations. Deciding whether they were the right equations remains yours, and it’s the part that requires the rest of this track. → the domain note


↑ Back to Continuum Mechanics