Finite Element Method (FEM) Calculator — CST Plane Solver
Solve 2D plane-stress and plane-strain problems with constant-strain-triangle finite elements: displacement, von Mises stress, and mesh convergence.
Finite Element Method Mesh Solver
- |u|
- u_x
- u_y
- max |u|
| e | σvM | εxx | εyy | min angle |
|---|---|---|---|---|
| 0 | 17.518 MPa | -2.48e-4 | 8.70e-5 | 26.57° |
| 121 | 17.518 MPa | 2.48e-4 | -8.70e-5 | 26.57° |
| 2 | 16.275 MPa | -2.25e-4 | 8.70e-5 | 26.57° |
| 123 | 16.275 MPa | 2.25e-4 | -8.70e-5 | 26.57° |
| 4 | 14.485 MPa | -2.04e-4 | 7.34e-5 | 26.57° |
| 125 | 14.485 MPa | 2.04e-4 | -7.34e-5 | 26.57° |
A clear path from inputs to results.
Solve a 2D linear-elastic structural problem with the finite element method. The tool builds a triangular mesh over a rectangular panel, assembles the global stiffness matrix from constant-strain triangle (CST) elements, applies supports and a distributed edge traction, and solves for the displacement of every node — then recovers strain, stress, and von Mises fields and runs a mesh-refinement study.
How to use
- Pick a preset problem (cantilever bend, uniaxial tension, shear panel, or compressive plate); each sets the geometry, support edge, and loaded edge.
- Choose plane stress (thin part) or plane strain (thick/constrained part) as the 2D idealisation.
- Set the mesh density in X and Y; more cells give a finer mesh and more accurate, less blocky stress.
- Set the material: Young’s modulus, Poisson’s ratio, thickness, and density.
- Set the surface traction on the loaded edge in kPa, and optionally enable self-weight as a body force.
- Read the peak displacement, peak von Mises stress, strain energy, and reaction-balance residual, and inspect the deformed mesh, von Mises contour, and convergence plot.
The formula
Reference: Constant-strain triangle (CST) plane-elasticity formulation and global assembly K_e = t A Bᵀ D B, K U = F; Zienkiewicz, Taylor & Zhu, The Finite Element Method; Cook, Malkus, Plesha & Witt, Concepts and Applications of Finite Element Analysis; Logan, A First Course in the Finite Element Method.
Worked example
Uniaxial tension of a steel panel
- Uniaxial tension preset: panel 1.8 m × 0.7 m, thickness 15 mm, E = 210 GPa, ν = 0.30, plane stress, left edge fully fixed, right edge pulled by a 650 kPa traction in +x, self-weight off, 12 × 6 mesh (182 DOF, 168 free).
- 1
The tool meshes the panel into 144 CST triangles, assembles each element stiffness K_e = t·A·BᵀDB with the plane-stress constitutive matrix D = E/(1−ν²)·[[1,ν,0],[ν,1,0],[0,0,(1−ν)/2]], and lumps the edge traction into equivalent nodal forces. The total applied horizontal force is traction × thickness × height = 650,000 × 0.015 × 0.7 = 6825 N. After fixing the left edge it solves KU = F by Cholesky factorisation. The reaction at the support sums to −6825 N, so the global force balance residual is ~1×10⁻¹¹ (machine zero) — equilibrium is satisfied. Recovering stresses per element gives σ_xx clustered around the far-field value σ = traction = 0.650 MPa (0.619–0.706 MPa across elements), with the peak von Mises stress 0.697 MPa. The largest nodal displacement is |u| = 5.545 × 10⁻⁶ m, within 0.5% of the textbook uniaxial value u = (σ/E)·L = (0.650 MPa / 210 GPa) × 1.8 m = 5.571 × 10⁻⁶ m; the small shortfall is the Poisson contraction suppressed at the fully fixed edge.
Peak displacement ≈ 5.55 µm, far-field axial stress ≈ 0.650 MPa (matching the applied traction), peak von Mises 0.697 MPa, and a force-balance residual at machine precision — the FEM result reproduces uniaxial-tension theory to sub-percent accuracy.
Interpreting the result
The displacement field shows how the part deforms under load, and the von Mises contour shows where it is closest to yielding — compare the peak von Mises against the material’s yield strength to judge safety. Because CST elements carry constant strain and stress within each triangle, the stress field looks blocky on a coarse mesh; the convergence study shows the peak displacement settling toward a mesh-independent value as you refine, which is how you know the answer can be trusted. The reaction-balance residual is a correctness check: a value near machine zero confirms the assembled system is in global equilibrium.
Assumptions & limitations
- The material is linear elastic, homogeneous, and isotropic, defined entirely by Young’s modulus and Poisson’s ratio; no plasticity, damage, or large-deformation effects are modelled.
- The analysis is 2D: plane stress assumes a thin part free to contract through thickness, while plane strain assumes thickness is fully constrained; the choice changes the constitutive matrix D.
- Constant-strain triangles interpolate displacement linearly, so strain and stress are uniform within each element — accuracy therefore depends on mesh density, which the refinement study makes explicit.
- Supports are ideal: a fixed edge sets both displacement components to zero at every node on it, which locally restrains Poisson contraction and perturbs the stress near the support.
- Edge tractions are converted to statically equivalent nodal forces (half the edge force to each end node of a segment), and self-weight, when enabled, is a consistent body force b = [0, −ρg].
- Deformations shown in the viewport are exaggerated by a labelled factor for visibility; the reported displacement magnitudes are the true solved values.
Frequently asked questions
What is a constant-strain triangle (CST)?
A CST is the simplest 2D solid element: a triangle with three corner nodes and linear displacement interpolation. Because displacement varies linearly, its derivatives — the strains — are constant over the element, hence the name. CSTs are robust and easy to assemble but need a fairly fine mesh to capture stress gradients, which is why mesh refinement matters so much.
Why does the stress look blocky and change with mesh density?
Each CST holds a single constant stress value, so a coarse mesh shows large uniform patches. Refining the mesh gives more elements and a smoother, more accurate field. The convergence study solves coarse, current, and fine meshes and reports how the peak displacement changes, so you can confirm the solution is approaching a mesh-independent answer.
How is the von Mises stress computed and why use it?
From the element stresses it is σ_vM = √(σx² − σxσy + σy² + 3τxy²). Von Mises combines the stress components into a single equivalent value that predicts the onset of yielding in ductile metals: when it reaches the material’s yield strength, the part begins to yield. It is the standard scalar for strength checks of metal structures.
When should I use plane stress versus plane strain?
Use plane stress for thin parts loaded in their plane (plates, membranes, brackets) where the through-thickness stress is essentially zero. Use plane strain for long or thick bodies constrained from deforming along their length (dams, tunnel linings, a slice of a long shaft) where the through-thickness strain is essentially zero. The two use different constitutive matrices and give different stiffness.
What does the reaction-balance residual tell me?
After solving, the tool sums the external applied forces and the support reactions. For a correct, in-equilibrium solution they must cancel, so the residual ‖R + F‖ should be essentially zero (around 10⁻¹¹ for the tension example). A large residual would indicate a modelling or solver problem, so it serves as a built-in sanity check.
Does fixing the whole edge affect the result?
Yes, slightly. Fixing both displacement components along the left edge prevents the panel from contracting sideways there (the Poisson effect), which stiffens the region near the support and makes the stress non-uniform close to it. Away from the support the field recovers the clean uniaxial state, which is why the computed peak displacement is within about 0.5% of the simple σL/E estimate.
Methodology last reviewed 2026-10-06. Results are informational and not financial or engineering advice — see our disclaimer.