How to Validate a Finite Element Model Before Trusting the Results
An FE solver returns a stress field for any model it is given. Wrong boundary conditions, a fixed support where the real joint rotates, stiffeners never connected to the plating: none of it stops the run. The output looks equally finished either way, with a color scale and peak values at named nodes. Nothing in the postprocessor flags the model as wrong. Below we go through the checks that separate a physically sound model from one that merely finished solving, before any of those numbers reach a code check.
What the Sleipner A Investigation Found
On 23 August 1991, the concrete base of the Sleipner A platform sank in Gandsfjord during a controlled ballasting test. A tricell wall failed, the structure took on water, and it went to the bottom. The loss came to roughly USD 700 million.
The SINTEF investigation ruled out material defects and workmanship. It found that the linear elastic analysis run in NASTRAN had understated shear stresses in the tricell walls by about 47%. The source was element shape: distorted elements in the global mesh. Working from those low values, the designers neither increased the wall thickness nor detailed shear reinforcement.
A re-analysis after the loss predicted failure at a submersion depth of 62 meters. The wall had actually failed at about 65 meters, a difference under 5%. A properly verified model would have exposed the capacity shortfall at the design stage.
Verification and Validation Answer Different Questions
ASME V&V 10 draws the line between the two terms. Verification assesses whether the mathematical model and numerical solution have been implemented and solved correctly. Validation assesses how well the model represents the physical system, typically through comparison with experimental or field data. A model can be verified without fault and still be invalid if its restraints do not behave the way the real connections do.
FEM analysis rests on discretization of a continuum. The structure is divided into elements, and within each element the displacement field is approximated by polynomials of a given order. The solution is therefore approximate by construction. How approximate is something that can be quantified rather than assumed.
Codes have started treating this as a subject in its own right. The second generation of Eurocode 3 adds EN 1993-1-14 (2025), Design assisted by finite element analysis. Annex C of EN 1993-1-5 already sets requirements for the material properties a model may use and for explicit input of initial imperfections, geometric and structural alike, in plated elements. An idealized linear elastic model with no imperfections does not by itself constitute a limit state verification.
Checks That Come Before Reading Stresses
Start with force balance. The sum of support reactions equals the sum of applied loads, and that trivial statement works as a first filter: an imbalance above roughly 1% of the total load points to an error in the boundary conditions, the load vectors, or mesh connectivity. Element stiffness and material properties have no bearing on global equilibrium, which is what makes the check useful for narrowing the cause.
Mass properties come next. The solver computes mass from assigned densities and element volumes, so a mismatch between the computed mass and center of gravity and an independently maintained weight report points to duplicated elements, a wrong density, or a component lost during assembly. The NASTRAN model verification procedure NASA published in 1995 calls for exactly this comparison against expected values.
Connectivity is tested by a free-free modal run. Strip out every restraint and extract natural frequencies. A free body in space has six rigid body degrees of freedom, so the first six frequencies should come back at zero. A seventh zero frequency, or one that is suspiciously low, means part of the model is attached to nothing: coincident nodes left unmerged, or a local mechanism nobody intended.
Mesh Convergence Can Be Calculated
Two runs at different mesh densities indicate a trend. Quantifying the discretization error takes three refinement levels at a constant scaling ratio r, which yields the actual order of convergence p = ln|(f₃ – f₂)/(f₂ – f₁)| / ln r. Richardson extrapolation applied to those same three solutions estimates the asymptotic value at zero element size. The Grid Convergence Index, or GCI, converts the differences between meshes into an error bound. The recommended safety factor for GCI is 1.25 when three meshes are available and 3.0 when only two are.
The method came out of computational fluid dynamics, and it transfers to solid mechanics. In a cantilever beam study published in the Bulletin of the Polish Academy of Sciences, the order of convergence ranged from 1.43 to 3.66 depending on element formulation, and GCI stayed under 2%. The extrapolated deflection of 5.107 mm matched the closed-form Timoshenko solution of 5.156 mm to better than 1%.
In a published convergence study, the residual change in peak equivalent stress between the last two refinement steps came to 3.2%. Nodal displacements converge faster than stresses, since displacements are the primary solution of [K]{u}={F} while stresses follow from derivatives of that field. A mesh that has converged on deflection can still be too coarse to resolve peak stress.
Nonlinear work complicates the idea. Element size couples to strain gradients and to the criteria that delete failed elements, and DNV-RP-C208 treats the choice of material failure model together with the mesh parameters as a single problem statement.
Locations Where Nothing Converges
Re-entrant corners with no fillet radius, concentrated nodal forces, point restraints: in a linear elastic formulation, the stress tensor at these locations grows without bound as element size approaches zero. There is no limit to converge to.
Separating a physical stress concentration from a singularity comes down to watching the sequence. Under refinement, a concentration approaches a finite maximum asymptotically. At a singularity, the value keeps climbing. Refining the mesh at a singular node has no analytical meaning. The stress state is assessed another way: read results at a distance from the feature where elements converge normally, model the actual fillet radius from the drawing, or extrapolate to the weld toe by the hot spot method when the detail is checked for fatigue.
Over-Restrained Models Are Stiffer Than the Structure
Too few restraints announce themselves. The stiffness matrix turns singular and the run aborts. Too many restraints stay quiet. Idealizing a flexible connection as a rigid fixity introduces stiffness the structure does not have, which understates deflections and shifts the stress maxima away from the regions where they genuinely concentrate. A symmetry condition imposed where the model is symmetric in geometry but not in loading or supports produces the same distortion.
Error from unrealistic boundary conditions runs many times larger than the discretization error that mesh refinement removes.
This is where the split between verification and validation becomes practical. Mesh convergence bounds discretization error for the equations as posed. It says nothing about whether those equations describe the real structure. An accurately solved model of the wrong idealization carries no engineering value.
Cross-Checking Against an Independent Solution
An ASCE study from 2021, built on interviews with 35 practicing engineers, documented 145 cases of analysis error. The method used most widely to catch them was comparison: verification by hand calculation, a parallel run in a second program, or independent review by another engineer. Thirteen errors in the sample surfaced only during construction, which is the argument for doing this work upstream.
Comparison works on decomposed sub-problems: a cantilever, a plate with a hole, and a simply supported beam. Closed-form solutions and handbook stress concentration factors exist for these, so the difference can be expressed as a percentage. A discrepancy of orders of magnitude points to an error in the problem statement, in boundary conditions, loads, or units, and no amount of mesh density will remove it.
Documenting the validation is what gives an independent reviewer something to audit. The report carries results at three refinement levels, the justification for each boundary condition, evidence of convergence in the quantity the code check consumes, and the solver version. Any change in geometry or topology voids the convergence study, which was tied to a mesh that no longer exists. That is why the checklist and the acceptance criteria belong inside the project’s calculation documentation.



Leave a Reply
Want to join the discussion?Feel free to contribute!