2D Finite Element Analysis - Stress Field & Frames

What it solves

This is a 2D finite element stress calculator for a thin plate in plane stress. It meshes the geometry with constant-strain triangles, solves the displacement field, and plots the resulting stress field as a colour contour - von Mises stress, the principal stresses, or the individual components. It runs entirely in your browser with no install and no login.

Plane stress is the right idealisation when the plate is thin compared with its other two dimensions and loaded in its own plane, so the out-of-plane stress is effectively zero. That covers gusset plates, brackets, webs, cleats, lifting lugs and most flat plate details in steelwork.

Von Mises stress in the contour

The von Mises stress combines the in-plane stress components into a single equivalent value that can be compared directly against the yield strength - which is what makes it the default contour for checking whether a plate detail is overstressed. It is a scalar, so it has no direction and is never negative; a region at 250 N/mm2 von Mises in S275 is at yield regardless of whether the underlying state is tension, compression or shear.

Because it discards sign, the von Mises plot alone will not tell you whether a region is in tension or compression. Switch to the principal stress view for that. This matters for a plate in compression, where a low von Mises value can still be a buckling problem that a plane-stress analysis does not model at all.

Reading the stress concentration

The peak value in the contour is what governs a plate detail, and it is almost always at a geometric discontinuity - a hole, a re-entrant corner, a notch or a sudden change of width. The plate-with-hole preset exists to show this: the stress at the edge of the hole is several times the average stress across the section.

A mesh that is too coarse under-reports the peak, because a constant-strain triangle cannot represent a steep gradient inside a single element. If refining the mesh keeps raising the peak value, the mesh is not yet converged. At a genuinely sharp re-entrant corner the theoretical stress is infinite and the value will keep climbing forever - that is a real property of the idealisation, not a solver bug, and it is why fillet radii exist.

Worked example - cantilever plate, verified against beam theory

The cantilever-plate preset is a 2.0 m by 0.4 m plate, 10 mm thick, in steel at E = 210 GPa, fixed along the left edge and carrying a 10 kN shear at the free end. These are the tool defaults, so you can reproduce this without entering anything.

Because the plate is a deep cantilever, elementary beam theory gives an independent check on the FEM result:

Second moment of area, t H^3 / 12

5.333e-5 m4

Root bending moment, P L

10 x 2.0 = 20.0 kNm

Root bending stress, M c / I

75.0 N/mm2

Tip deflection, P L^3 / 3EI

2.38 mm

Span-to-depth ratio

5.0

The FEM contour should show a bending-stress distribution at the fixed edge peaking near 75 N/mm2 at the top and bottom fibres and passing through zero at mid-depth. Expect the FEM value to differ by several per cent, and to be the more accurate of the two: at a span-to-depth ratio of only 5 this is a deep cantilever, so shear deformation is significant and beam theory - which ignores it - understates the deflection. Agreement to within a few per cent is the expected outcome; a wildly different answer means a boundary condition is wrong.

Running that comparison on a case you can solve by hand is the single most useful habit with any FEM tool. It catches the errors that matter - wrong units, wrong restraint, load applied in the wrong direction - which produce plausible-looking contours rather than obvious failures.

Worked example - plate with a hole

The second preset is a 1.0 m square plate, 10 mm thick, with a 0.15 m radius central hole, carrying 50 kN of uniaxial tension. The hand check here is the stress concentration factor:

Hole diameter to plate width, 2r / W

0.30

Gross-section stress, P / (W t)

5.00 N/mm2

Net-section stress, P / ((W - 2r) t)

7.14 N/mm2

Kt on net section (Peterson, finite width)

2.35

Expected peak stress at the hole edge

16.8 N/mm2

The classical Kt = 3.0 applies to a circular hole in an infinite plate referred to the gross stress. This plate is not infinite - the hole takes up 30 per cent of the width - so the finite-width factor referred to the net section is about 2.35, which corresponds to roughly 3.4 on the gross stress. The peak von Mises value in the contour should land near 17 N/mm2 at the sides of the hole, on the axis perpendicular to the load, with the stress at the top and bottom of the hole going slightly compressive.

Formula reference

Von Mises, plane stress

$\sigma_{vm} = \sqrt{\sigma_x^{2} - \sigma_x\sigma_y + \sigma_y^{2} + 3\tau_{xy}^{2}}$

Principal stresses

$\sigma_{1,2} = \dfrac{\sigma_x + \sigma_y}{2} \pm \sqrt{\left(\dfrac{\sigma_x - \sigma_y}{2}\right)^2 + \tau_{xy}^{2}}$

Maximum shear stress

$\tau_{\max} = \dfrac{\sigma_1 - \sigma_2}{2}$

Plane-stress constitutive law

$\sigma = \dfrac{E}{1-\nu^{2}}\,\bigl[\varepsilon\bigr]$

Stress concentration

$\sigma_{\max} = K_t\,\sigma_{nom}$

The theory page derives the constant-strain triangle formulation and shows where each of these comes from.

Assumptions and limits

The analysis is linear-elastic plane stress: material stays on the elastic line with no yielding or redistribution, displacements are small, and the out-of-plane stress is zero. A von Mises peak above yield tells you the plate would yield locally - it does not tell you the plate has failed, because a ductile steel plate redistributes around a local peak, which this analysis cannot represent.

Buckling is not modelled. A plate in compression can be perfectly safe on stress and still fail by buckling out of plane, which a plane-stress analysis cannot see by construction. Nor is anything out of plane represented: bending across the thickness, plate-bending stiffness and any three-dimensional effect are outside the scope.

Results depend on the mesh. Peaks at discontinuities are mesh-sensitive and always under-reported by a coarse mesh, and at a mathematically sharp corner they do not converge at all. Fatigue, fracture and residual stresses from welding or cutting are not included.

FAQ