Linear Static Analysis
Complete Reference Guide

What is Linear Static Analysis?

Linear static analysis is the most fundamental — and most commonly performed — type of structural finite element analysis. It predicts the deformation of a structure under applied loads, assuming three conditions are all simultaneously satisfied:

1. Material linearity — stress is proportional to strain: \(\boldsymbol{\sigma} = \mathbf{C}\,\boldsymbol{\varepsilon}\) (Hooke's Law holds throughout)
2. Geometric linearity — deformations are small enough that the original geometry can be used to write equilibrium equations (the structure's shape does not change appreciably under load)
3. Static loading — loads are applied slowly (quasi-statically), so inertia forces and damping are negligible; the structure is in static equilibrium at all times

When all three conditions hold, the structural problem reduces to solving a single linear system of algebraic equations — which modern solvers handle with remarkable efficiency, enabling models with tens of millions of degrees of freedom to solve in minutes on workstations.

Linear static analysis is the correct tool for a vast range of engineering problems: structural frames under service loads, pressure vessels at operating conditions, machine components under steady forces, and electronic enclosures subject to gravity and thermal expansion in the linear regime. It is the indispensable first step that every structural simulation engineer must master before advancing to nonlinear or dynamic analysis.

The Governing Equation: [K]{u} = {F}

The central equation of linear static FEM is deceptively simple in appearance:

Where:

• \([\mathbf{K}]\) is the global stiffness matrix [N/m] — assembled from element stiffness matrices; symmetric, positive semi-definite. Its size is \(n_{\text{DOF}} \times n_{\text{DOF}}\) where \(n_{\text{DOF}}\) is the total number of degrees of freedom.
• \(\{\mathbf{u}\}\) is the global displacement vector [m] — the unknowns we solve for (translations and rotations at each node).
• \(\{\mathbf{F}\}\) is the global force vector [N] — assembled from nodal forces, pressure loads, body forces, and prescribed thermal loads converted to equivalent nodal forces.

How the Stiffness Matrix is Built

Each element has a local stiffness matrix \([\mathbf{k}^e]\), computed by integrating the material stiffness through the element volume:

Where \([\mathbf{B}]\) is the strain-displacement matrix (derivatives of shape functions with respect to spatial coordinates) and \([\mathbf{C}]\) is the material constitutive matrix (encodes Young's modulus, Poisson's ratio, and material symmetry). The integral is evaluated numerically using Gaussian quadrature. Element matrices are then assembled into the global \([\mathbf{K}]\) by the direct stiffness method — each element's contribution is added to the rows and columns corresponding to its node global DOF numbers.

Solving the System

After applying displacement boundary conditions (which eliminate the rows and columns corresponding to constrained DOFs, or equivalently introduce penalty terms), the resulting reduced system \([\mathbf{K}_r]\{\mathbf{u}_r\} = \{\mathbf{F}_r\}\) is solved by a direct sparse solver (LU factorization, often using algorithms like PARDISO, MUMPS, or SuperLU) or an iterative preconditioned conjugate gradient solver. For large models, iterative solvers with AMG (algebraic multigrid) preconditioners scale more favourably.

Post-Processing: From Displacements to Stresses

Displacements are the primary unknowns. Strains are recovered by differentiation of the displacement field:

Stresses are then computed from the constitutive law: \(\{\boldsymbol{\sigma}\} = [\mathbf{C}]\{\boldsymbol{\varepsilon}\}\). Because stresses are derived by differentiating the displacement field (one order lower in polynomial), they are less accurate than displacements — this is why stress convergence studies require finer meshes than displacement convergence studies.

Assumptions and Limitations

The Superposition Principle — A Unique Advantage

One profound consequence of linearity is the principle of superposition: the response to multiple simultaneous load cases equals the sum of responses to each load case applied separately. This means you can run a single stiffness matrix factorization and solve for dozens of different right-hand side load vectors at negligible additional cost — a major efficiency advantage for design studies and load combinations. Nonlinear solvers cannot exploit this because the stiffness matrix changes with every load step.

Key Element Types in Linear Static Analysis

1D Elements

Euler-Bernoulli Beam

The classical beam element assumes that plane sections remain plane and perpendicular to the neutral axis after bending — the Euler-Bernoulli (EB) hypothesis. This gives a 2-node element with 3 DOFs per node in 3D (two bending slopes and one torsion, plus axial). Accurate for slender beams where the span-to-depth ratio exceeds roughly 10. The transverse shear deformation is neglected, which means EB beams are overly stiff for short, deep beams — they lock.

Timoshenko Beam

Extends Euler-Bernoulli by allowing the cross-section to rotate independently of the neutral axis slope — adding a shear angle as an independent kinematic variable. This correctly captures transverse shear deformation and avoids locking for short/deep beams. In Abaqus: B21 (Euler-Bernoulli-like, 2D), B31 (Timoshenko, 3D). In ANSYS: BEAM188 uses Timoshenko theory by default.

2D Elements

Plane Stress

For thin in-plane structures where the out-of-plane stress \(\sigma_z = 0\): thin sheets, plates loaded in their own plane. The out-of-plane strain \(\varepsilon_z\) is non-zero (the thickness changes freely). Implemented with 2D elements in the x-y plane. Typical use: sheet metal stampings, thin mounting flanges, 2D frame cross-sections.

Plane Strain

For very long structures where the out-of-plane strain \(\varepsilon_z = 0\): the structure cannot expand in the z direction because it is constrained by adjacent material (long dams, tunnels, pressure vessels in the mid-section far from end caps). The out-of-plane stress \(\sigma_z\) is non-zero and computed from the in-plane strains. In Abaqus: CPE4R (quad, reduced integration, plane strain).

Axisymmetric Analysis

For structures with a rotational axis of symmetry (cylinders, pressure vessel heads, discs, O-rings, bolts), the 3D problem collapses to a 2D cross-section in the r-z meridional plane. The full 3D stress state is recovered using the axisymmetric strain-displacement relationship that includes the circumferential (hoop) strain \(\varepsilon_{\theta\theta} = u_r/r\). In Abaqus: CAX4R; in ANSYS: PLANE183 with axisymmetric keyoption. Efficiency gain: reduces a 3D model with millions of cells to a 2D model with thousands.

Shell Elements

Kirchhoff-Love Shell

Thin shell theory based on the Kirchhoff hypothesis (normals remain normal to the mid-surface after deformation; no transverse shear). Accurate for thin structures where thickness/span < 1/20. Requires C1 continuity of shape functions, which limits element choices. Not suitable for thick shells.

Mindlin-Reissner (Thick) Shell

Adds transverse shear degrees of freedom — the normal is allowed to rotate independently of the mid-surface slope. This avoids the C1 requirement and handles both thin and moderately thick shells. The dominant shell element in commercial codes: S4R in Abaqus (4-node quad, reduced integration), SHELL181 in ANSYS. Reduced integration (1 in-plane integration point for S4R) prevents shear locking and is generally recommended unless you have hourglassing concerns.

3D Solid Elements

Special Elements

• RBE2 (rigid body element) — distributes force/moment from one node (independent) to many nodes (dependent) with rigid kinematic constraint. Used for bolted connections, load application points. In Abaqus: *RIGID BODY or MPC type BEAM/TIE.
• RBE3 (interpolation constraint) — distributes load from one reference node to many dependent nodes weighted by distance, without adding artificial stiffness. Preferred for load application where stiffening the joint is undesirable. Abaqus: *MPC type RBE3.
• Spring element — models connectors with specified axial or lateral stiffness [N/m]. Useful for foundations, bushings, mounting brackets, and simplified joint behavior.
• Gap/contact element (linear regime) — in the linear regime, gaps can be pre-opened or pre-closed; linear gap elements model one-way stiffness (compression only, no tension).

Convergence and Mesh Refinement for Static Problems

The finite element solution converges to the exact solution of the boundary value problem as the mesh is refined — provided the elements satisfy the completeness and compatibility requirements (the patch test). In practice, "convergence" means that refining the mesh further does not change your quantity of interest (displacement, maximum stress, reaction force) by more than an acceptable tolerance.

What Converges Faster: Displacements or Stresses?

Displacements converge faster than stresses — typically one polynomial order faster. For linear elements (complete first-order polynomial basis), displacements converge at \(O(h^2)\) (second order in element size h) while stresses converge at \(O(h^1)\) (first order). For quadratic elements, displacements converge at \(O(h^3)\) and stresses at \(O(h^2)\). This is why stress-critical analyses should use quadratic elements (TET10, HEX20, S8R) and require finer meshes than displacement-dominated problems.

Stress Concentrations and Singularities

At sharp re-entrant corners (90° notches in CAD geometry), the exact elasticity solution is a stress singularity — stress theoretically approaches infinity as mesh is refined. A linear static FEM model will faithfully reproduce this: the peak stress at the corner will keep increasing with mesh refinement without bound. The correct response is:

1. Add a fillet radius to represent the actual manufactured geometry (no real corner is perfectly sharp)
2. Use submodeling (cut-boundary method): run a coarse global model first, then apply the global displacements as boundary conditions to a refined local model of the stress concentration region
3. Use stress intensity factors or J-integral if the sharp notch is intentional (fracture mechanics approach)

Articles in This Section (30+ topics)

Organized by element type and analysis technique:

Beam Elements

2D Formulations

Shell Elements

3D Solid Elements

Special Elements & Techniques

Thermal Stress (Linear Regime)

Verification: Patch Test and Convergence Study

The Patch Test

The patch test is the fundamental check that a finite element formulation is correct. It verifies that a patch of elements — with arbitrary node positions and a distorted mesh — can exactly reproduce a constant strain state when the correct displacements are applied. Any element that passes the patch test will converge to the correct solution as the mesh is refined. If an element fails the patch test, no amount of refinement will give the right answer.

In practice, you apply a uniform constant-stress analytical solution (e.g. pure tension, pure shear) as displacement boundary conditions on the outer nodes of a small distorted mesh patch. The interior node stresses should exactly reproduce the applied stress state. This is the first thing researchers do when implementing a new element formulation.

Mesh Convergence Study Protocol

1. Define your quantity of interest (QOI) — usually the maximum von Mises stress in a critical region, or a peak displacement
2. Run at least three mesh densities: coarse, medium (half element size), fine (quarter element size)
3. Plot QOI vs. element size or number of DOFs. A monotonically converging sequence confirms correct formulation.
4. Apply Richardson extrapolation to estimate the exact solution: \(Q_{\text{exact}} \approx Q_h + \frac{Q_h - Q_{2h}}{2^p - 1}\) where \(p\) is the convergence order (2 for linear elements on displacements)
5. Report the solution only when QOI changes < 2–5% between the two finest meshes

When to Go Nonlinear

Linear static analysis is not always appropriate. Here are the clear indicators that a nonlinear analysis is required:

Author: サイトマップ