Simulate Landing Gear Impact
Discover how much force hits the landing gear at touchdown—before building anything.
Last reviewed: March 2026Overview
Every aircraft landing gear must pass a drop test before the aircraft is certified to fly. The FAA and EASA require that landing gear withstand at least 2.0 g of vertical acceleration during a hard landing without permanent deformation. Testing real hardware is expensive and time-consuming; finite element simulation lets engineers perform hundreds of virtual drop tests in days, iterating on geometry and material before a single prototype is built.
Siemens Simcenter (formerly Nastran/NX) is one of the two dominant structural simulation platforms in aerospace—the other is ANSYS. In this project you will use Simcenter's student tools to model a simplified nose landing gear oleo strut as a cylindrical column, apply a dynamic impact load representing a hard landing, and view the resulting stress distribution to determine whether the design is safe. You will also vary the wall thickness to see how structure weight and safety factor trade off against each other.
The workflow you practice—geometry → mesh → boundary conditions → solve → post-process → iterate—is identical whether you are analyzing a model rocket fin or a Boeing 777 main landing gear. The physics and the software philosophy are the same; only the scale and complexity change. Structural simulation is a core skill for every mechanical or aerospace engineering job, and Simcenter experience on a portfolio stands out strongly to university admissions teams.
What You'll Learn
- ✓ Explain the finite element method (FEM) in plain terms: what nodes, elements, and stiffness matrices represent.
- ✓ Import or create a simplified 3D landing gear geometry in Simcenter.
- ✓ Apply fixed constraints and dynamic impact loads to a finite element model.
- ✓ Run a linear static analysis and interpret von Mises stress and displacement results.
- ✓ Calculate the safety factor for a given material and load, and determine whether redesign is required.
Step-by-Step Guide
Access Simcenter student tools
Siemens offers free access to Simcenter Nastran and NX for students through the Siemens Academic Program. Register with your school email and download the student license. Alternatively, your school's engineering department may have a lab license—ask your physics or engineering teacher. Install NX and verify you can open it by creating a new Part file. If neither option is available, Simcenter Femap with Nastran has a free trial that works for this project.
Create the landing gear geometry
In NX, create a new Part. Model a simplified oleo strut as a hollow cylinder: outer diameter 80 mm, inner diameter 68 mm (wall thickness 6 mm), length 400 mm. This represents the main structural tube of a small aircraft nose gear. Add a flat circular plate 150 mm diameter × 10 mm thick at the bottom to represent the axle housing. Use the Unite command to merge both bodies into a single solid. This simplified geometry captures the key structural behavior without requiring the full complexity of a real gear design.
Assign material and generate the mesh
In the Simulation Navigator, right-click the geometry and select "Assign Material." Choose Aluminum 7075-T6 from the material library—yield strength 503 MPa, density 2810 kg/m³. Create a new FEM file (right-click → New FEM and Simulation). Use the 3D Tetrahedral mesh tool with element size 5 mm. Run the mesh check—you should see no failed elements. View the mesh to confirm the cylinder walls are meshed through-thickness with at least 2 element layers; if not, reduce element size to 3 mm.
Apply boundary conditions and impact load
Simulate the gear attached to the aircraft structure at the top: select the top circular face and apply a Fixed constraint (zero displacement in all directions). This represents the gear pivot attachment to the airframe. Apply the drop-test load to the bottom axle plate: a vertical force representing 2.5 g times the aircraft nose gear share of maximum landing weight. For a 1,200 kg aircraft with 30% load on the nose gear, nose gear load = 0.30 × 1200 × 9.81 × 2.5 = 8,829 N—apply this upward on the axle plate face. Also apply a 25% side load (2,207 N horizontal) to simulate cross-wind landings.
Run the analysis and view results
Right-click the Simulation in the Navigator and select Solve. The Nastran solver runs in seconds for this small model. When complete, open the Results navigator and plot "Von Mises Stress" on the deformed shape. The color contour will range from blue (low stress) to red (high stress). Identify the location of maximum stress—it will typically be at the transition between the tube and the axle plate. Also plot "Nodal Displacement" to see how much the gear deflects under load. Record the maximum stress value in MPa.
Evaluate safety and iterate on wall thickness
Calculate the safety factor: SF = yield strength / maximum von Mises stress = 503 / σ_max. Regulatory requirements typically demand SF ≥ 1.5 for limit load (which we have already scaled to 2.5 g). If your SF is below 1.5, increase wall thickness to 8 mm, remesh, and re-solve. If SF is comfortably above 2.0, try reducing wall thickness to 5 mm to save weight. Create a table with three rows (wall 5, 6, 8 mm) showing mass, maximum stress, and SF. Plot mass vs. SF to illustrate the weight-safety tradeoff. Write a brief recommendation for the optimal wall thickness.
Career Connection
See how this project connects to real aerospace careers.
Aerospace Engineer →
Structural engineers at every aerospace company run FEM simulations daily to certify components; Nastran and Simcenter are the industry-standard tools and proficiency with them is explicitly listed in job postings.
Aerospace Manufacturing →
Manufacturing process engineers use simulation to verify that forging, machining, and joining operations do not introduce residual stresses that could cause in-service fatigue failures.
Aviation Maintenance →
When inspectors find cracks or corrosion in landing gear, structural engineers run FEM crack propagation analyses to determine safe inspection intervals—understanding the simulation process helps maintenance professionals communicate requirements clearly.
Avionics Technician →
Vibration and shock loads that affect avionics boxes are analyzed using the same FEM methods; technicians who understand structural simulation can better specify installation requirements for sensitive electronics.
Go Further
- Replace the linear static analysis with a transient dynamic simulation using a time-varying impact force profile (a half-sine pulse over 0.1 seconds) and compare peak stress to the static result.
- Add a fatigue analysis using Simcenter's fatigue module and compute how many landing cycles the gear can withstand before crack initiation—compare to the FAA minimum of 20,000 landings.
- Export the FEM mesh as a Nastran BDF file and solve it with the free pyNastran Python library, comparing results to the Simcenter solution.
- Research a real landing gear failure incident (e.g., the 2005 Air France A340 runway overrun in Toronto or the 2020 Air India Express runway exceedance) and discuss what structural simulation role played in the accident investigation.