3. CAE model fundamentals for crashworthiness

Crashworthiness simulation rests on a specific numerical foundation: explicit finite element analysis. Unlike implicit solvers used for static stiffness or modal analysis, the explicit method advances the solution through a large number of very small time increments without assembling or inverting a global stiffness matrix. This distinction shapes every modeling decision that follows — element size, mass scaling, contact treatment, and material definition all interact with the stability limit of the explicit scheme.

3.1 Why Explicit Formulation Dominates Crash Analysis

The semi-discrete equation of motion for a nonlinear dynamic system is:

M·a(t) + C·v(t) + F_int(u,t) = F_ext(t)

where M is the mass matrix, C the damping matrix, F_int the internal nodal force vector (a nonlinear function of displacement u), and F_ext the applied external load. In an explicit solver, the mass matrix is lumped (diagonal), so the acceleration at each node is obtained directly:

a_n = M⁻¹ · (F_ext,n − F_int,n − C·v_n)

Velocities and displacements are then updated with a central-difference time integration scheme. No matrix inversion and no Newton–Raphson iteration are required. The trade-off is conditional stability: the time step must satisfy the Courant–Friedrichs–Lewy condition, approximately

Δt ≤ 2 / ω_max ≈ L_min / c

where L_min is the smallest element characteristic length and c is the wave speed in the material. For steel, c ≈ 5000 m/s; a 5 mm element therefore yields a stable step around 1 μs. A 100 ms crash event thus requires roughly 100,000 increments — computationally feasible precisely because each increment is cheap.

3.2 LS-DYNA and PAM-CRASH Workflows

Both LS-DYNA and PAM-CRASH are explicit solvers widely used in the automotive industry. Their input decks share the same conceptual structure even though keyword syntax differs. A typical workflow proceeds through preprocessing, solving, and postprocessing, with the solver input file as the central artifact.

In LS-DYNA, the deck is organized into keyword blocks. A minimal crash model includes:

*KEYWORD
*CONTROL_TERMINATION
$  endtim    endcyc    dtmin
   0.120              1.0e-7
*CONTROL_TIMESTEP
$  dtinit    tssfac    isdo
             0.90
*DATABASE_BINARY_D3PLOT
$     dt
   0.002
*PART, *SECTION_SHELL, *MAT_*, *CONTACT_*, *BOUNDARY_*, *INITIAL_VELOCITY_*

PAM-CRASH uses a comparable but differently named structure: /RUN, /TITLE, /MAT, /PART, /SHELL, /CONTACT, and /TIME. The mapping between the two is not one-to-one, but the modeling intent is identical. When transferring a model between solvers, verify that shell formulation, hourglass control, and contact penalty stiffness are re-specified rather than assumed.

A practical checkpoint list before submission:

• Confirm endtim covers the full physical event plus a margin for rebound.
• Set dtmin small enough to avoid premature termination but large enough to catch genuine instability.
• Verify initial velocity is applied to the correct node set or rigid body, with direction consistent with the global coordinate system.
• Check that the d3plot output interval resolves the peak crush phase — typically 1–2 ms for a full frontal impact.

3.3 Material Models for Crash

Material selection determines whether the simulation captures the energy absorption mechanisms that govern real crash behavior. The most common families are:

For *MAT_024, the plastic hardening curve is entered as pairs of effective plastic stress and plastic strain. A common error is to supply engineering stress–strain data directly; the solver expects true stress and true plastic strain. Convert using σ_true = σ_eng(1 + ε_eng) and ε_pl = ln(1 + ε_eng) − σ_true/E. Failure is often triggered by a plastic strain limit or by *MAT_ADD_EROSION, though erosion must be used cautiously because deleting elements removes mass and can artificially reduce energy absorption.

3.4 Contact Definitions

Contact in explicit crash models is typically penalty-based: the solver detects penetration and applies a restoring force proportional to the penetration depth and a penalty stiffness. The two dominant formulations are single surface and surface-to-surface.

*CONTACT_AUTOMATIC_SINGLE_SURFACE is the workhorse for self-contact within a deforming structure — for example, a folding rail contacting itself. *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE is used when two distinct parts interact, such as the barrier against the vehicle front. Key parameters include:

• FS and FD: static and dynamic friction coefficients. For steel-on-steel, FS ≈ 0.1–0.15 is a common starting point; for rubber or coated surfaces, higher values apply.
• SFS and SFM: scale factors on the slave and master sides, used to tune penalty stiffness when excessive penetration or contact instability appears.
• SOFT: soft constraint option, often set to 1 or 2 for contacts involving foam or very soft materials to avoid overly stiff penalty forces.
• DEPTH: search depth for initial penetration. A value of 0 disables the initial penetration check; a small positive value is safer for models with slight initial overlaps.

Contact energy is reported in the glstat file. If contact energy exceeds roughly 5–10% of total internal energy, the contact definition or mesh is likely too coarse, and the result should be treated with caution. Similarly, a negative sliding energy or a sudden spike in contact energy usually indicates a penetration or a penalty stiffness problem.

3.5 Reading the Energy Balance

The single most informative diagnostic in an explicit crash run is the energy summary in glstat. Total energy should remain approximately constant. Internal energy rises as the structure deforms; kinetic energy falls correspondingly. Hourglass energy should stay below 5% of internal energy — if it exceeds this, refine the mesh or switch to a fully integrated shell formulation. Contact energy, as noted, should remain a small fraction of internal energy. A sudden jump in either hourglass or contact energy is a reliable indicator that the model has developed a numerical problem rather than a physical one.

These fundamentals — explicit time integration, solver-specific keyword structure, rate-dependent material definitions, penalty contact, and energy-based verification — form the modeling vocabulary that the subsequent discrepancy analysis will rely on. Every comparison between physical test and CAE result is ultimately a comparison between two realizations of this same numerical framework, and understanding where the framework can diverge from reality is the first step toward quantifying that divergence.