Wing Structural Analysis in Simcenter
Put a wing box through its paces with industrial FEA before it ever flies.
Last reviewed: March 2026Overview
The wing box — the load-carrying structure running spanwise through the wing — is one of the most structurally critical and carefully analysed components on any aircraft. It must withstand limit loads (the most severe loads expected in service) with no permanent deformation, and ultimate loads (1.5× limit) without catastrophic failure, in accordance with FAR/CS-25 airworthiness regulations. Finite element analysis using Nastran is the primary analytical method for this substantiation, and Simcenter (the commercial pre/post-processor built around Nastran) is the dominant industrial tool for this work.
In this project you will model a simplified wing box (two spars, upper and lower skins, ribs at defined stations) using shell (QUAD4) elements in Simcenter. The aerodynamic loads — chordwise pressure distributions and spanwise load distributions — are derived from a VLM analysis (either XFLR5 from the wing optimisation project or a simple analytical lift distribution) and applied as surface pressures. You will run three analysis types: a static stress analysis for the 2.5g manoeuvre load case, a linear buckling analysis to check panel stability, and a fatigue life estimate using the FEMFAT or Simcenter Durability module.
Structural analysis certification skills are in high demand across aerospace OEMs, Tier 1 suppliers, and certification consultancies. A demonstrable Nastran/Simcenter project — particularly one that includes buckling and fatigue — substantially differentiates a candidate from peers who have only used general-purpose FEA tools like ANSYS Mechanical for academic assignments.
What You'll Learn
- ✓ Build a wing box shell-element FE model in Simcenter with correct property and material card assignments
- ✓ Convert aerodynamic lift distributions into equivalent nodal and pressure loads in Nastran format
- ✓ Interpret static stress analysis results including reserve factors and identify critical load paths
- ✓ Perform and interpret a linear buckling analysis to assess panel stability margins
- ✓ Estimate fatigue life using a stress-life (S-N) approach and identify the life-limiting structural detail
Step-by-Step Guide
Define the wing box geometry and create the mesh
Define a rectangular wing box (span 6 m, chord 1.2 m, depth 15% chord) with two spars at 15% and 65% chord, skins on upper and lower surfaces, and ribs at 10 equally spaced spanwise stations. Build the surface geometry in Simcenter and mesh with QUAD4 shell elements at approximately 50 mm element size. Assign aluminium 2024-T3 shell properties (thickness 3 mm spar web, 4 mm skin, 5 mm spar caps modelled as CBAR elements).
Define load cases from VLM results
Import or manually enter the spanwise lift distribution for a 2.5g pull-up manoeuvre from your XFLR5 or Schrenk's approximation. Convert the distributed lift to equivalent nodal forces on the upper and lower skin nodes at each rib station using the panel area weighting method. Apply a root fixity constraint (clamped at the wing root spar-to-fuselage interface). Verify equilibrium: the sum of applied nodal forces should equal the total wing lift force.
Run the static analysis and assess reserve factors
Run the Nastran SOL 101 static solution. Post-process the results in Simcenter: plot von Mises stress, principal stresses, and displacement contours. Compute the reserve factor (RF = allowable stress / applied stress) for each major structural region. Identify any regions with RF < 1.5 (the FAR/CS-25 ultimate load factor) and document which load path is critical. Increase spar cap area or skin thickness as needed to achieve RF ≥ 1.5 everywhere.
Perform linear buckling analysis
Run Nastran SOL 105 linear buckling analysis on the same model. Extract the first five buckling eigenvalues and mode shapes. The first eigenvalue represents the ratio of applied load to buckling load: a value above 1.5 means the skin panels will not buckle at limit load. Identify the panel with the lowest buckling eigenvalue and add longitudinal stiffeners (modelled as CBAR elements) to raise its buckling resistance above the required margin.
Estimate fatigue life with the stress-life method
Define a simplified load spectrum: 50,000 cycles at the 1g level, 5,000 cycles at 2.5g, and 500 cycles at the gust design load (typically 3.5g for a CS-25 aircraft). Extract the peak stress at the most critical joint (spar cap-to-root fitting) for each load level. Use the aluminium 2024-T3 S-N curve (from MIL-HDBK-5 or Metallic Materials Properties Development) and Miner's cumulative damage rule to estimate the fatigue life in flight hours. Compare against the typical 40,000 flight hour design life requirement.
Produce a certification-style stress report
Structure a stress report following the format of a real Aircraft Structural Analysis Report: title page, scope, reference documents (FAR/CS-25 paragraphs), geometry and material description, load derivation, FE model description (element types, mesh statistics, boundary conditions), analysis results with figures, reserve factor summary table, buckling margin table, fatigue life summary, and a conclusions/disposition section. This document format is what certification authority DERs and DEs review for structural substantiation approval.
Career Connection
See how this project connects to real aerospace careers.
Aerospace Engineer →
Structural engineers at OEMs and Tier 1 suppliers use Simcenter/Nastran daily for airframe substantiation; this project provides direct preparation for those roles.
Aerospace Manufacturing →
Manufacturing engineers assess tooling loads and assembly-induced stresses using the same Nastran shell-element methodology demonstrated here.
Aviation Maintenance →
Maintenance engineers reviewing structural repair schemes use FEA results to assess whether a repair restores original strength margins — understanding those results is essential.
Avionics Technician →
Technicians performing structural modifications for avionics installations need to understand what stress reports say about load path disruption and allowable hole sizes.
Go Further
- Add a composite laminate skin model (PCOMP card) and compare the structural weight savings against the aluminium baseline at equivalent strength.
- Perform a flutter analysis (SOL 145) to check aeroelastic stability of the wing and compare the flutter speed against the design dive speed requirement.
- Implement a sizing optimisation loop in Python that drives the Nastran batch solver, extracts reserve factors, and automatically adjusts skin thickness and spar cap area until minimum weight is achieved with all margins positive.
- Correlate the FE model against a simple beam bending test (3-point bend of a model wing box fabricated from balsa or aluminium sheet) to validate the FE predictions.