Structural
Use structural FEA to answer questions about deformation, stress, reactions, natural frequencies, forced vibration, shock response, buckling, and nonlinear load paths. RunMat keeps the physical model independent from meshing and execution: geometry defines regions, the mesh discretizes them, the model assigns materials, sections, supports, and loads, and the study chooses a procedure graph.
The typed .fea language covers the complete structural procedure set described on this page, and
the native .fea execution path runs it. Each result records the actual formulation, operator
identities, backend, convergence, residual, and recovery evidence.
What equations does RunMat solve for structural FEA?
For small-strain linear elasticity, RunMat uses displacement as the primary unknown:
with essential displacement constraints on and traction on . Tetrahedral finite elements and the declared constitutive capabilities produce the canonical semidiscrete system
The selected procedure determines which terms and states are active:
.fea procedure | Discrete problem |
|---|---|
structural static | |
structural preload | Static equilibrium plus retained prestress/geometric state |
structural modal | |
structural transient | Direct integration of |
structural modal_transient | The same dynamics projected into a retained modal basis |
structural harmonic | |
structural modal_harmonic | Harmonic dynamic stiffness projected into modal coordinates |
structural prestressed_modal | |
structural buckling | Generalized eigenproblem using elastic and prestress-derived geometric stiffness |
structural prestressed_harmonic | Harmonic response about an explicit prestressed state |
structural modal_response_spectrum | Modal peak response followed by the declared modal combination rule |
structural random_response | Modal transfer functions applied to input CPSD/PSD and integrated statistics |
structural nonlinear | Incremental equilibrium |
RunMat does not silently add weak springs, mass, damping, a reference constraint, or a load case to make these systems solvable.
How do I run a linear static stress analysis?
This complete model assigns steel to both solids in a STEP assembly, fixes one face on each disconnected occurrence, applies a resultant force to the left part, and requests displacement and von Mises stress:
The included STEP file carries the authored body and end-face names the study selects; select name resolves only names authored in the CAD file. The study stays in one readable source file; exporting the project preserves its CAD names.
geometry bracket {
file = "./geometry/two-box-assembly.step"
units = m
region left_body : solid { select name "left_body"; expect exactly_one }
region right_body : solid { select name "right_body"; expect exactly_one }
region left_support : face { select name "left_support"; expect exactly_one }
region left_load_face : face { select name "left_load_face"; expect exactly_one }
region right_support : face { select name "right_support"; expect exactly_one }
}
mesh bracket on geometry.bracket {
tetrahedra {
order = linear
target_size = 1.5 m
maximum_deviation = 0.05 m
}
}
material steel {
mass_density = 7850 kg/m^3
elastic {
youngs_modulus = 200 GPa
poisson_ratio = 0.3
}
}
model loaded_bracket {
assign material.steel to geometry.bracket.region.left_body
assign material.steel to geometry.bracket.region.right_body
constraint left_support {
structural.fixed { target = geometry.bracket.region.left_support }
}
constraint right_support {
structural.fixed { target = geometry.bracket.region.right_support }
}
load service_traction {
traction on geometry.bracket.region.left_load_face = [166.6666666667, 0, 0] Pa
}
load_case service { include load.service_traction }
}
study bracket_static {
geometry = geometry.bracket
mesh = mesh.bracket
model = model.loaded_bracket
analysis static { structural static {} }
output displacement = analysis.static.field.node.displacement
output stress = analysis.static.field.element.von_mises_stress
}The traction tuple is a global XYZ intensity. In this fixture the selected end face is ,
so [166.6666666667, 0, 0] Pa integrates to a resultant in +X while boundary
quadrature distributes it consistently over the face mesh. A face target alone does not rotate an
arbitrary traction vector onto that face normal.
runmat check bracket.fea
runmat plan bracket.fea
runmat run bracket.feaFor isotropic linear elasticity, is assembled from youngs_modulus
and poisson_ratio. Dynamics also requires mass_density. A face never owns the solid material
behind it: material coverage must be assigned to the participating solid or cell regions.
Why is my structural stiffness matrix singular?
A singular or non-coercive stiffness operator usually means one of the following:
- rigid-body translation or rotation remains unconstrained;
- a part or included model is disconnected;
- a tie, connector, or contact does not cover the intended regions;
- a beam/shell region lacks its required section or orientation;
- a material/property assignment misses participating elements;
- constraints conflict or collapse the admissible subspace.
RunMat reports the typed target and source span for constraints and preserves constrained-space operator evidence. Fix the physical model. Do not add arbitrary supports merely to make factorization succeed; that changes reactions, modes, and load paths.
How do I run a modal analysis and check natural frequencies?
study bracket_modes {
geometry = geometry.bracket
mesh = mesh.bracket
model = model.loaded_bracket
analysis modes {
structural modal { modes = 30 }
retain basis
}
}The eigensolve operates on the constrained and . Each mode records angular frequency , frequency , the mode shape, modal mass/stiffness, residual, and normalization identity. Check that:
- the first modes are physically plausible and not unconstrained rigid modes;
- cumulative participating mass is sufficient in every excited direction;
- repeated or closely spaced modes are treated as a subspace rather than compared vector-by-vector;
- frequency and mode shapes converge under mesh refinement;
- the basis was produced by the exact operator and mesh used downstream.
How do I run transient structural dynamics with a pulse or time history?
Direct transient dynamics uses the canonical mass, damping, and stiffness operators and advances the physical state over the declared time samples. RunMat's direct structural path uses Newmark-family effective equilibrium; accepted steps retain balance and reaction evidence.
signal impact_history : force over time {
samples = [
{ at = 0 ms, value = 0 N },
{ at = 2 ms, value = 1 kN },
{ at = 8 ms, value = 0 N },
]
interpolation = linear
extrapolation = reject
}
model impacted_bracket {
assign material.steel to geometry.bracket.region.body
constraint support {
structural.fixed { target = geometry.bracket.region.fixed_face }
}
excitation impact {
force {
target = geometry.bracket.region.loaded_face
signal = signal.impact_history
direction = global([0, -1, 0])
kinematics = fixed_frame
}
}
}
study transient_response {
geometry = geometry.bracket
mesh = mesh.bracket
model = model.impacted_bracket
analysis response {
structural transient {
start_time = 0 s
end_time = 50 ms
time_step = 0.1 ms
}
}
}The time step must resolve load breakpoints and the highest response frequencies of interest. Initial displacement, velocity, and acceleration are typed initial conditions; they are not inferred from the first signal sample. Restart state must match the operator and topology identity of the continuing analysis.
How do I run harmonic or frequency-response analysis?
Direct harmonic response solves a complex dynamic-stiffness system at each declared frequency. Modal harmonic response first projects the operators and forcing through a retained basis:
analysis modes {
structural modal { modes = 40 }
retain basis
}
analysis response after analysis.modes {
structural modal_harmonic {
basis = analysis.modes.state.basis
frequencies = [20, 50, 100, 200] Hz
}
}Use direct response when modal truncation is unacceptable; use modal response when the retained basis
captures the excited band and participation. Check damping, frequency spacing around resonances,
complex equilibrium residual, and modal truncation. A frequency list is part of study identity.
A modal-reduced sweep is accepted on its reduced-space residual and publishes its full-order
imbalance as the modal truncation measure; static_correction = applied_loads and modal
residual_vectors reduce it (see modal truncation and residual vectors).
The solid harmonic qualification case checks physical Tet4/Tet10 direct and modal response against independent element integrals and oscillator amplitude, phase, and power references. Its one-DOF scope and remaining promotion gates are documented with the runnable test.
How do preload, prestressed modes, and buckling connect?
A preload step retains a prestress state. Prestressed modal, buckling, or harmonic steps must name that exact state and declare their dependency:
analysis preload {
structural preload {}
}
analysis buckling after analysis.preload {
structural buckling {
prestress = analysis.preload.state.geometric_stiffness
modes = 10
}
}A preload publishes several states, so it has no single state to rename with retain; the
consumer names the one it needs, here geometric_stiffness.
The geometric stiffness is derived from the retained equilibrium state. RunMat rejects topology/operator mismatches rather than applying prestress from a different model. Linear buckling factors are bifurcation indicators for the linearized problem; they do not include imperfections, post-buckling response, plasticity, or contact changes unless a separately qualified nonlinear formulation explicitly models them.
How do I run response-spectrum or random-vibration analysis?
Response-spectrum analysis evaluates each retained mode against a named spectrum, then combines modal peaks using the declared combination method. It does not reconstruct a unique time history. Closely spaced modes require a correlation-aware rule such as CQC rather than unconditional SRSS.
Random response operates on power or cross-spectral density. In modal coordinates,
and variance follows from integration over angular frequency. Input PSD/CPSD units therefore carry the inverse-domain unit and cannot be substituted by an amplitude spectrum.
The checked runnable examples
modal-response-spectrum.fea
and modal-random-response.fea
show the complete spectrum declarations, modal state flow, and outputs.
How do I run nonlinear structural analysis?
structural nonlinear declares an explicit load-factor domain. The nonlinear solver advances bounded
increments, forms the current residual and tangent, iterates to the requested equilibrium target,
and records accepted or rejected increment evidence. Contact and follower loading change the
residual/tangent and must be declared as such.
analysis load_path {
structural nonlinear {
start_load_factor = 0
end_load_factor = 1
}
}Convergence of Newton iterations is not validation of the constitutive model. Check increment size, residual and energy norms, contact penetration, load/reaction balance, path dependence, and whether the implemented material/contact formulation is qualified for the intended use.
Structural constraints, loads, materials, and outputs
- Structural constraints documents every support, prescribed-motion, coupling, tie, periodic, and equation kind.
- Structural loads documents force, moment, traction, pressure, body force, signals, directions, distribution, follower kinematics, and load cases.
- Models covers material, beam/shell/solid property ownership and composition.
- Outputs covers typed fields, projections, spatial reductions, probes, histories, sampling, retention, and partial access.
How do I inspect Tet10 stress without hiding its within-element variation?
Quadratic tetrahedra recover strain and stress at the same four physical integration points used by stiffness assembly. Each point is a first-class result entity with a stable identity and physical position. Element strain, stress, von Mises stress, and strain-energy density remain available as Jacobian-weighted projections for summaries and element plots; use the integration-point field when within-element variation or recovery error is the engineering question.
Retain both views in the study when you need to compare them:
study bracket_check {
analyze static using model.loaded_bracket
output stress_at_quadrature = analysis.static.field.integration_point.stress
output element_stress = analysis.static.field.element.stress
}The corresponding RunMat selectors are typed:
pointStress = stepResult.field(fea.StructuralField.integrationPointStress());
elementStress = stepResult.field(fea.StructuralField.stress());Tet4 publishes the same four-entity layout with its constant tensor repeated. That keeps mixed-order partitioning and paging uniform without implying four independent Tet4 stress states. Recovery smoothing is region-side aware: integration points extrapolate to element nodes, but nodes shared by different material regions do not erase a legitimate stress jump.
How do I know a structural FEA result is credible?
At minimum, review geometry and units, material and section coverage, load resultants, support reactions, mesh quality, discretization convergence, equation residuals, energy balance, formulation identity, backend identity, and recovery evidence. Dynamics additionally needs time/frequency convergence, damping justification, mass participation, and basis truncation evidence. Buckling and nonlinear work needs imperfection and path-sensitivity studies appropriate to the engineering decision.
Continue with meshing, study contracts, verification and validation, and result evidence.