Material Definition Error Resolution — FEA

210 is correct in GPa — but what units is the rest of your model in? If you're using meters and Newtons (SI), you need 210×10⁹ Pa. If you're in the common Abaqus convention of millimeters, Newtons, and MPa, then 210,000 MPa is correct. "210" in an SI-meters model gives a modulus roughly 10⁶ times too small — the solver won't always error out, it'll just give enormous deformations.

Thermodynamically, ν = 0.5 exactly means the bulk modulus becomes infinite — \( K = E / 3(1-2\nu) \) blows up. The stiffness matrix becomes singular, which is why it fails. In practice you use ν = 0.499 or 0.4999 to approximate incompressibility — but you also must switch to hybrid (mixed) elements like C3D8H in Abaqus. Standard displacement elements with near-ν = 0.5 lock and give completely wrong results even without crashing.

Auxetic materials — like certain foams and lattice structures — actually expand laterally when you pull them. ν can legitimately be negative for those. The thermodynamic constraint is that the strain energy must be positive definite, which gives \( -1 < \nu < 0.5 \). Anything outside that range means the material would spontaneously release energy from a stressed state, which is physically impossible.

In a static analysis, \( [K]\{u\} = \{F\} \) — mass doesn't appear anywhere, so density is optional. The moment you go dynamic — modal, harmonic, transient — the equation of motion is \( [M]\{\ddot{u}\} + [C]\{\dot{u}\} + [K]\{u\} = \{F\} \). Without density, \( [M] \) is a zero matrix, and natural frequencies \( \omega = \sqrt{k/m} \) all go to infinity. That's why the solver rejects it.

Yes — if you apply a body force via gravity (Abaqus: *DLOAD, GRAV), the solver multiplies density by gravitational acceleration to get the body force. Without density, the gravity load is zero. Surprisingly common mistake when copying models from a benchmark that had no gravity.

Yes, that's a problem. Most solvers linearly extrapolate beyond the last data point. If your yield strength goes from 400 MPa at 20°C down to 50 MPa at 600°C, and the solver extrapolates to 900°C, it will predict −100 MPa yield strength — which is physically nonsense and will produce completely wrong plastic strains. Some solvers clamp at the last value, others extrapolate, and few give you a clear warning. You need to extend your data table to cover the full expected temperature range.

A few options. First, if those high-temperature regions are not structurally critical (e.g., a weld pool that will re-solidify), you can add a small near-zero yield strength entry at the max temperature with an anneal flag to reset plastic strain. Second, consult elevated-temperature material databases — NIMS (Japan), ASME Sec. II, or vendor data sheets often go higher. Third, at least add a "floor" entry at your max expected temperature so the solver doesn't extrapolate into negative territory.

Plasticity in FEA is solved by a "return mapping" algorithm. At each increment, the solver makes a trial elastic stress step, checks if the stress is outside the yield surface, and if so, "returns" it back to the yield surface by computing the correct plastic strain. If the time increment is too large, the trial stress lands so far outside the yield surface that the return mapping iteration can't converge — it's like trying to Newton-iterate from a starting point that's way off in the distance. The fix is to take smaller time increments so the stress stays close to the yield surface.

Yes — adaptive time stepping is your friend here. In Abaqus, use *CONTROLS, ANALYSIS=DISCONTINUOUS for highly localized plasticity, or add viscoplastic regularization via *RATE DEPENDENT even with a very small viscosity parameter. Regularization smooths the stress return without changing the physics significantly. Also check your hardening curve — if it has a sharp kink or goes perfectly flat (ideal plasticity), the return mapping has to travel farther at each step.

This is a Mooney-Rivlin limitation. The 2-parameter Mooney-Rivlin model — \( W = C_{10}(I_1-3) + C_{01}(I_2-3) \) — fits well at moderate strains but its predicted stress can actually decrease with increasing strain at large deformations depending on the C₁₀/C₀₁ ratio. That violates the Drucker stability criterion (stress must increase monotonically with stretch), and Abaqus detects this and aborts. Real rubber stiffens significantly at large strains due to chain alignment — you need a model that captures this.

Neo-Hookean is actually simpler and can have similar issues at extreme strains. For large-strain rubber (above 100% engineering strain), the Yeoh model or Ogden model are better choices — they fit the characteristic S-shaped stress-stretch curve of rubber accurately. The key is to fit your model parameters to test data that spans the full strain range you expect in the simulation — uniaxial, biaxial, and planar tension if possible. Abaqus lets you input test data directly with *HYPERELASTIC, TEST DATA and will fit the parameters for you.