Finite element analysis (FEA), explained
Finite element analysis helps predict how a part or structure will respond to loads, vibration and heat before physical prototypes are built. This guide explains how the finite element method turns a design into a mesh of small elements, which type of analysis answers which question, how to check that the answer can be trusted, and which Simcenter tools do the work.
What is finite element analysis?
Finite element analysis (FEA) is the simulation of how a product or an assembly performs structurally, acoustically, thermally or electromagnetically. It is the practical use of the finite element method (FEM), which divides the design into many small, simple pieces, approximates the physics on each and solves them together as one system of equations.
FEA helps engineers predict whether a part will bend, break, vibrate, overheat or fail under real conditions, before physical prototypes are built. Typical results are stresses, displacements, temperatures inside solids and natural frequencies. It is used to replace or supplement physical tests and hand calculations.
FEA and FEM are often used as synonyms, and so are “FEA simulation” and “FEM simulation”. Strictly, FEM is the mathematical method and FEA its use on an engineering problem; engineers also say “the FEM” for the meshed model itself.
FEA and CFD
FEA predicts how solid structures respond to loads, vibration, heat and pressure. Computational fluid dynamics (CFD) simulates how liquids and gases flow and carry heat; the CFD basics are in our handbook. Many real problems need both, for example when the pressure of a flow bends a flexible part: that is fluid–structure interaction. FEA and CFD are two of the main branches of CAE simulation.
FEA is used most in aerospace, automotive, electronics, industrial machinery, marine and consumer products, and widely in energy, turbomachinery, life sciences and building services.
How the finite element method works
The finite element method turns a continuous part into a finite set of unknowns, in six steps:
- Divide the geometry into elements
The part is split into many small, simple elements that meet at points called nodes. Together they form the mesh, and each element carries the material and structural properties of the part.
- Interpolate inside each element
The displacement at any point in an element is interpolated from its nodes with simple shape functions: each one equals one at its own node and zero at the others.
- Assemble the stiffness matrix
Each element has its own stiffness matrix, which links the forces at its nodes to their displacements. The software adds them into one global stiffness matrix for the whole model. This assembly step is the heart of the method.
- Apply loads and constraints
At every node, either the force or the displacement is known in each direction: the loads and constraints are the boundary conditions of the analysis. The constraints must also stop the model moving as a rigid body, or the system of equations cannot be solved.
- Solve K·u = F
For a linear static case the equations read K·u = F: K is the global stiffness matrix, u the unknown nodal displacements and F the nodal loads. Solving gives u.
- Calculate strains and stresses
Strains follow from the displacements, and stresses from the strains through the material’s stress–strain relation. These are what the contour plots show.
Element types: 1D, 2D and 3D
1D beam elements
Two-node line elements for frames, beams and early concept models
2D shell elements
Quadrilaterals and triangles for thin walls; thickness is a property
3D solid elements
Hexahedra, tetrahedra and pyramids for bulky parts
Beam elements suit long, slender members and early design studies, for example of a car body or an airframe before the detailed geometry exists. Thin-walled parts such as sheet metal are meshed with shells; bulky parts such as an engine block with solids.
Elements also differ in order, shown here for 2D elements. Linear (first-order) elements have nodes only at their corners. The three-node triangle has constant strain and stress inside the element, hence its name, the constant strain triangle; the four-node quadrilateral has a bilinear displacement field. Quadratic (second-order) elements add mid-side nodes and let strain and stress vary linearly. Quadratic elements are therefore usually preferred for stress results and curved geometry, while linear elements are often adequate for deformation. Constant strain triangles are best kept away from stress concentrations such as the edges of holes and corners.
Types of FEA
Which analysis you run depends on the question. Simcenter Nastran names its analyses by solution sequence (SOL) numbers, which the table gives where they apply.
| Analysis | The question it answers | In Simcenter |
|---|---|---|
| Linear static | Stress and deflection under steady loads, with small deformation and linear material. Results scale with the load. | Simcenter Nastran SOL 101, Simcenter OptiStruct |
| Nonlinear static | Large deformation, plasticity or contact, where doubling the load need not double the response. | Simcenter Nastran SOL 401 and 402 |
| Modal analysis (normal modes) | The natural frequencies and mode shapes of the structure. | Simcenter Nastran SOL 103 |
| Linear buckling | The load at which a slender or thin-walled part becomes unstable. | Simcenter Nastran SOL 105 |
| Frequency response and random vibration | The response to harmonic or random (PSD) excitation. | Simcenter Nastran SOL 108 and 111; Simcenter OptiStruct (the random vibration example below) |
| Transient dynamics | The response to loads that change over time. | Simcenter Nastran SOL 109 and 112 |
| Crash and impact (explicit dynamics) | Short, highly nonlinear events such as crashes, impacts and drop tests. | Simcenter Radioss |
| Thermal and thermo-mechanical | Temperatures in solids, and the expansion and stress they cause. | Simcenter 3D; Simcenter SimLab with Simcenter OptiStruct |
| Fatigue and durability | How long a part lasts under realistic, repeated load histories. | Simcenter 3D |
| Acoustics and NVH | Noise, vibration and harshness (NVH): noise and vibration performance, and how to reduce noise. | Simcenter 3D |
Modern FEA often couples several physics: thermal and mechanical loads together, flexible bodies in a multibody (motion) model, or a flow that loads a structure in fluid–structure interaction.
Implicit or explicit solvers
Implicit solvers suit static problems and longer, low-speed events. Explicit solvers such as Simcenter Radioss suit short, highly nonlinear events such as crashes, impacts and drop tests. Simcenter OptiStruct covers both.
Worked example · Viktor Hultgren, Volupe
When does a column buckle?
In one of our blog posts, Viktor Hultgren compares three ways to find when a 1 m tall UPE100 column under compression buckles: Euler’s hand formula and two analyses in Simcenter 3D. A linear buckling analysis (SOL 105) solves an eigenvalue problem: each eigenvalue is a load multiplier, and with a 1 kN reference load the lowest eigenvalue gave the buckling load directly. As a rule of thumb, it is valid while the loads cause no visible deformation and the stresses stay below yield.
| Method | Buckling load | What it assumes |
|---|---|---|
| Euler’s formula (hand calculation) | about 210 kN | A perfectly straight column. A design version with an effective-length factor of 2.1 allows for imperfections and gives a lower value. |
| Linear buckling, SOL 105 | about 201 kN | The meshed column as an eigenvalue problem: small deformation, elastic material |
| Nonlinear buckling with an imperfection, SOL 401 | about 191 kN, onset | Elastic material, with the first buckling mode as an initial imperfection; large displacements, and an arc-length method follows the load path through the collapse |
The linear result lies between the two Euler values in the post. With the imperfection included, the nonlinear run showed buckling starting at about 95% of the maximum load, about 191 kN, which the post finds strikingly similar to the hand calculation with an effective-length factor of 2.1, the value recommended for design. Plasticity was not switched on, so with the high stresses in the flanges the real column would probably collapse slightly earlier. Read the full buckling example.
Worked example · Johan Dahlberg, Volupe
Random vibration
Random vibration is usually described by a power spectral density (PSD). In Johan Dahlberg’s Simcenter OptiStruct example, the analysis runs in three steps: a modal analysis with modes up to about 1.5 times the highest PSD frequency, a frequency response, often to a unit load such as a unit acceleration, and a PSD step that combines that frequency response with the input PSD curve.
The RMS (root mean square) value is the square root of the area under a PSD curve: in the post’s illustration, a PSD with an area of 184 g² (g is the acceleration due to gravity) has an RMS value of 13.6 g. The demo model is a single flexible plastic part, clamped at one end and excited in one direction with a generic PSD; the RMS displacement at its tip came out at about 46 mm. Read the random vibration example.
The FEA workflow: pre-processing, solving and post-processing
Most FEA follows three steps: pre-processing, solving and post-processing. Steps 1 to 3 below are pre-processing.
- Idealise the geometry
Remove details away from the areas you assess. A fillet removed where stress is high leaves a sharp corner.
- Mesh
Choose 1D, 2D or 3D elements and refine where stress changes fast. Thin walls get shells on a midsurface.
- Materials, loads, constraints
Assign material properties, apply loads and constraints, and choose the analysis type.
- Solve
The solver solves the equations. Large models can take significant time and computing power, and more companies run them in the cloud.
- Post-process and decide
Review contours, animations and reports, and define derived results.
Change the model and run again (back to step 2, pre-processing)
Shells on a midsurface. Thin-walled parts are usually better modelled with shell elements than with solids. A shell mesh sits on a midsurface halfway between the inner and outer faces, and the wall thickness becomes a shell property. Simcenter 3D can create midsurfaces and carry the thickness across.
Mesh density. Fillets, corners and other details with steep stress gradients usually need smaller elements than regions where stress changes little. For buckling, our buckling post cites a Simcenter Nastran recommendation of five grid points (nodes) per half-wave of the buckled shape; in the same post, a 4 m column meshed with 250 mm and with 1,250 mm elements gave a similar first buckled shape but significantly different load multipliers.
Can you trust an FEA result? Mesh convergence and validation
A finite element model gives an approximate answer to an idealised problem. Two kinds of check decide whether it can be used: verification (is the model solved correctly, for example by a mesh convergence study) and validation (is it the right model).
Mesh convergence
In a mesh convergence study the mesh is refined step by step, with smaller elements or higher-order elements, until the result of interest stops changing. The converged value approaches the exact answer to the mathematical model, which is not necessarily how the real part behaves.
A classic check is a plate with a hole under tension. For a small hole in a very large plate, theory gives a peak stress of three times the far-field stress, at the edge of the hole across the load. In a University of Cincinnati teaching example, a 10 × 10 in plate with a hole of 1 in radius under 100 psi, three element types converged to about 322 psi:
| Element type | Coarsest mesh | Finest mesh |
|---|---|---|
| Linear quadrilaterals (Q4) | 312.4 psi, 506 elements | 322.4 psi, 31,349 elements |
| Quadratic triangles (T6) | 320.2 psi, 1,518 elements | 322.2 psi, 24,516 elements |
| Quadratic quadrilaterals (Q8) | 320.6 psi, 501 elements | 322.2 psi, 14,333 elements |
The coarsest meshes were 0.5–3% low, and the quadratic elements converged faster: for 1% accuracy, 501 quadratic quadrilaterals were enough. The converged value is about 7% above 300 psi, the exact solution for an infinitely large plate; this plate is 10 in wide. Our grid convergence index (GCI) calculator applies the same idea to a study on three grids.
Check the model before the numbers
Three simple checks come before the stress values. Look at the deformed shape to make sure the boundary conditions are applied correctly, check that the model is in equilibrium (the reaction forces balance the applied loads), and check symmetry and antisymmetry where they should apply.
Sharp corners and stress singularities
At a sharp inside (re-entrant) corner, linear elasticity predicts stresses that are, in theory, unbounded. Ordinary finite elements cannot reproduce this. As the mesh is refined, the solution approaches an exact answer that is unbounded at the corner, so the peak stress there does not converge. A peak stress reported exactly at a sharp corner should therefore be treated with caution. Removing an inside fillet during idealisation creates such a corner.
Verification and validation
Verification asks whether the model is solved correctly: is the computational model mathematically right, and is the numerical error small enough? Validation asks whether it is the right model, by comparing results with measurements. Our guide to CAE simulation covers both in more detail.
Validation compares a simulation with a real test of the same event, as in this crash model next to the physical test.
Reading FEA results: stresses and the safety factor
In a 3D solid model, the stress at a point has six components. Two derived values do most of the work in design checks.
- Principal stresses are the normal stresses on the planes where shear stress is zero: the highest and lowest normal stress at a point. A brittle material cracks along a principal plane when the largest principal stress exceeds its tensile strength, so for brittle materials that is the value to check.
- Von Mises stress (equivalent stress) combines all the components into one value, based on the energy of distortion. For ductile materials, yield is predicted when the von Mises stress reaches the yield stress from a tensile test, and most FEA codes calculate it.
Safety factor against yield = yield stress ÷ von Mises stress
Structures are usually sized so that stresses stay below yield by a suitable safety factor. In Simcenter 3D a result probe can calculate it element by element. Brittle materials such as ceramics fracture before they yield, so for them a yield check is not enough.
Read the contour plot with care
A contour plot is not the raw element result. The post-processor first extrapolates the stresses from the integration points to the nodes: in an MIT teaching example of a plate with a hole, this raised the peak from 3.26 to 3.59 times the far-field stress. It then usually averages the values at each node, which is meant to give more accurate stresses but also smooths out real jumps, so switch the averaging off at nodes between two materials or at other geometric discontinuities.
To check a single stress state by hand, use our von Mises stress calculator: it also gives the principal stresses and the safety factor against yield.
Simcenter tools for FEA
Simcenter has several tools for structural analysis. Some share a solver: Simcenter 3D and Simcenter Femap both run Simcenter Nastran. Simcenter OptiStruct and Simcenter Radioss are solvers in their own right, and Simcenter SimSolid works without a mesh. Simcenter 3D can also build and run models for third-party solvers such as Abaqus, Ansys and LS-DYNA, and Simcenter HyperMesh can export models to the formats of other solvers.
Model, mesh and solve
- Structures, dynamics, acoustics and thermal in one environmentSimcenter 3D
- Finite element solver for linear and nonlinear structures, dynamics and acoustics, inside Simcenter 3D or standaloneSimcenter Nastran
- Pre- and post-processing, from beams to solid meshesSimcenter Femap
- Meshing and assembly of large modelsSimcenter HyperMesh
Femap or Simcenter 3D? Both run Simcenter Nastran: Simcenter Femap as a standalone pre- and post-processor, Simcenter 3D as one environment for several physics.
Specialised solvers and design
- Structural analysis with built-in topology optimisationSimcenter OptiStruct
- Explicit dynamics: crash, impact, drop testsSimcenter Radioss
- Analysis on full CAD assemblies without a meshSimcenter SimSolid
- Simulation and generative design for designersSimcenter Inspire
Mesh or no mesh? Simcenter SimSolid works on the CAD geometry without simplifying or meshing it; classic FEA builds a mesh first, so the analyst chooses the element types.
Apart from Simcenter Nastran, which runs inside Simcenter 3D or on its own, all these tools are listed on our Simcenter FEA software page. Volupe runs Simcenter 3D and Simcenter HyperMesh training and supports users across the Nordic countries and Europe; find your regional contact.
Not sure which tool fits your analysis?
Tell us what you need to predict, and a Volupe engineer will suggest where to start.
A short history of the finite element method
- 1943
Mathematician Richard Courant approximates a solution with functions that are linear over each triangle of a triangular net, an early form of the method.
- 1956
Turner, Clough, Martin and Topp publish “Stiffness and deflection analysis of complex structures”, work from Boeing on aircraft structures.
- 1960
Ray Clough of the University of California, Berkeley, names the “finite element method” in a paper on plane stress analysis.
- 1965
By the end of the year the new name has replaced the older “direct stiffness method”.
- 1966
NASA contracts the development of NASTRAN, a general-purpose finite element program; the first operational version is delivered in 1969.
- 1967
O. C. Zienkiewicz, with Y. K. Cheung, publishes The finite element method in structural and continuum mechanics, which the US National Academy of Engineering calls the first book devoted to the method.
Sources and changelog
Sources
Siemens, Finite element analysis (FEA), FEA vs CFD, Structural dynamics simulation, Durability and fatigue, midsurfaces for shell meshing and meshless simulation (webinar).
Siemens product pages: Simcenter 3D, Simcenter Nastran, Simcenter Femap, Simcenter HyperMesh, Simcenter OptiStruct, Simcenter Radioss, Simcenter SimSolid and Simcenter Inspire.
D. Roylance, MIT, Finite element analysis, Transformation of stresses and strains and Yield and plastic flow (PDF); Y. Liu, University of Cincinnati, Lecture notes: an introduction to the finite element method (PDF, source of the plate-with-a-hole convergence study).
J. L. Swedlow, Singularity computations (NASA NTRS, PDF); ASME, Simulation credibility assessment: introduction to verification, validation and uncertainty quantification (PDF).
History: R. Courant, Variational methods for the solution of problems of equilibrium and vibrations (1943); M. J. Turner et al., Stiffness and deflection analysis of complex structures (1956); R. W. Clough and E. L. Wilson, Early finite element research at Berkeley (PDF); W. K. Liu, S. Li and H. S. Park, Eighty years of the finite element method (arXiv, 2021); National Academy of Engineering, memorial tribute to O. C. Zienkiewicz; NASA, Computerized Engineering (Spinoff 1998).
Worked examples, Volupe blog: Setting up buckling solutions in Simcenter 3D and Time step control in Simcenter Nastran (Viktor Hultgren); Random vibrations and PSDs in Simcenter OptiStruct and Simcenter SimLab thermal and structural simulations (Johan Dahlberg); Using Guyan reduction to create superelements (Viktor Hultgren, the source of the SOL numbers); and the posts linked in the text.
Images: Siemens Simcenter image library. The plate with a hole and the element illustrations are drawn by Volupe.
Changelog
October 2026: first version, written from Siemens web pages, published course notes and papers, and Volupe’s own worked examples.
FEA in practice: articles by Volupe engineers
All articlesBuckling
linear and nonlinear, step by step
Simcenter 3D
Setting up buckling solutions in Simcenter 3D
Viktor Hultgren, Volupe · 2025
Read the article →
Random vibration
from PSD input to RMS response
Simcenter OptiStruct
Random vibrations and PSDs in Simcenter OptiStruct
Johan Dahlberg, Volupe · 2026
Read the article →
Nonlinear
restart from a converged preload
Simcenter 3D
Saving time starting over: nonlinear restarts
Viktor Hultgren, Volupe · 2025
Read the article →
Superelements
reduce a large assembly
Simcenter 3D
Using Guyan reduction to create superelements
Viktor Hultgren, Volupe · 2025
Read the article →
Result probes
safety factor per element
Explicit dynamics
contact, friction and impact
Simcenter Radioss
Bouncing ball paradox, solved with Simcenter Radioss
Johan Dahlberg, Volupe · 2026
Read the article →
Questions about finite element analysis
Questions about your analysis?
Volupe’s structures engineers
Simcenter 3D, Femap and Nastran, and Simcenter HyperMesh, OptiStruct and Radioss
Choose “Technical question” in the form below and describe your case.
Ask a technical question →
What is the difference between FEA and FEM?
FEM, the finite element method, is the mathematical method. FEA, finite element analysis, is its use on an engineering problem. The two are often used as synonyms, and engineers also call the meshed model “the FEM”.
What is FEA used for?
To predict whether a part or structure will bend, break, vibrate, overheat or fail before physical prototypes are built: stresses, displacements, natural frequencies, buckling loads, temperatures and fatigue life. It is used most in aerospace, automotive, electronics, industrial machinery, marine and consumer products.
What is the difference between FEA and CFD?
FEA simulates solids: how structures respond to loads, vibration, heat and pressure. CFD simulates liquids and gases: flow, pressure, turbulence and heat transfer. When a flow deforms a structure, the two are coupled in fluid–structure interaction.
How accurate is FEA?
It is an approximation, and its error can be estimated. A mesh convergence study shows how much the answer still depends on the mesh, and validation against tests shows whether the model represents the real part. In a classic plate-with-a-hole teaching example, the coarsest meshes were 0.5–3% below the converged peak stress, and the finest meshes of three element types agreed within 0.05%.
How fine should the mesh be?
Fine enough that refining it further no longer changes the result you care about. Use smaller or higher-order elements where stress changes quickly, such as fillets and holes. For buckling, our buckling post cites a Simcenter Nastran recommendation of five grid points per half-wave of the buckled shape.
What is modal analysis in FEA?
A modal, or normal modes, analysis calculates the natural frequencies and mode shapes of a structure. In Simcenter Nastran it is solution sequence SOL 103. In our Simcenter OptiStruct random vibration example, it is the first of three steps, before the frequency response and the PSD step.
When do I need a nonlinear analysis?
When deformation is large, when the material yields, or when parts come into contact: then the response no longer scales with the load. Linear static analysis is quick and robust when strains and displacements are small and the material stays elastic.
When do I use an implicit or an explicit solver?
Implicit solvers suit static problems and longer, low-speed events. Explicit solvers, such as Simcenter Radioss, suit short, highly nonlinear events such as crashes, impacts and drop tests. Simcenter OptiStruct covers both.
Which Simcenter tool should I use for FEA?
It depends on the job: Simcenter 3D or Simcenter Femap with the Simcenter Nastran solver for general structural work, Simcenter HyperMesh for large models, Simcenter OptiStruct for analysis with optimisation, Simcenter Radioss for crash and impact, and Simcenter SimSolid for analysis on full CAD assemblies without a mesh. Apart from the Simcenter Nastran solver, all of them are listed on our Simcenter FEA software page, and you can book a demo.
Talk to an engineer in your region
Every Volupe business developer holds an engineering degree. Find your regional contact below, or send us a message.
Ask us about FEA (finite element analysis)
Use this form for licence quotes, demos, training and technical questions.
What happens next
- A reply within one day.
- A scoping call with one of our engineers.
- A quote, demo or other next step that fits your enquiry.
After purchase: support from Volupe simulation engineers.