cFEA

Finite element analysis in your browser: check one solid part for stress and movement, natural frequencies or temperatures. Bring in a STEP or STL file or a simple shape, mesh it, set the supports and loads, solve, and read the results in 3D and in a report.

cFEA overview: a part meshed and solved, with the stress shown in colour

Overview

A cFEA document is a finite element analysis of one solid part. It is solved on our servers with the open-source code_aster solver and the Gmsh mesher, and checked against hand calculations.

  • Linear static: movement and stress under forces, pressures, gravity and prescribed movements.
  • Modal: natural frequencies and mode shapes, held or free.
  • Steady-state thermal: temperatures and heat flow.

cFEA gives results and a record of how they were made. It does not check the part against a design code. The full guide is in the User Manual chapter.

Access and Limits

  • Open to every signed-in user except client users, on every plan.
  • Free plan: 1 cFEA document a month, like every other document type, and 1 solve a month. Showing the model and making the mesh are not counted, and a failed solve does not use the month's solve. Paid plans: no limit.
  • A model has a limit on its number of elements. An uploaded file may be up to 50 MB. A run that takes too long (2 minutes for the model, 10 for the mesh, 30 for the solve) is stopped and says so.

Getting Started

  1. On the project page click the + next to cFEA and give it a file number, a name, a description and a revision description.
  2. Click its name. Work down the steps on the left, 1 Geometry to 7 Report; the 3D view on the right shows what each one has made. The page saves by itself.
  3. For a first try use or use a simple shape in step 1: a box, a cylinder or a plate with a hole.

The Seven Steps

  1. Geometry. Choose the length unit, then upload a STEP (.step, .stp) or an STL file, or use a simple shape. A STEP file must hold a solid and an STL file must be closed. Read the warnings under the model.
  2. Material. Pick one from the library at your temperature, or type your own values (marked unverified). Guided mode warns about unchecked values; Professional mode refuses them.
  3. Mesh. Set the element size and choose quadratic (accurate) or linear (fast, stiffer) elements. Refine locally on faces, inside a box or inside a sphere. Press Generate mesh, look at it on the Mesh tab, then Approve mesh: you cannot solve before.
  4. Analysis and conditions. Choose static, modal or thermal, then Add supports and loads and click the faces they act on (fixed support, prescribed displacement, pressure, force, gravity; fixed temperature, heat flux, convection). The supports and loads are drawn on the model as symbols, so the set-up can be read at a glance: a green pin for a fixed support, cyan double-headed arrows along each direction held at zero for a prescribed movement (and an arrow along a movement you type), red arrows pressing on a face for a pressure, an orange arrow for a force, dots for a fixed temperature, orange arrows into the part for a heat flux, blue arrows for convection and one purple arrow beside the part for gravity. The arrows follow the signs and directions you type; their size follows the model, not the value. The Loads button above the view hides them.
  5. Run. Press Solve. The page shows the step and the time. Any change afterwards marks the results out of date.
  6. Results. Look at them in 3D (below).
  7. Report. Write your purpose, sources, assumptions and acceptance criteria, then open the report as a page, a PDF or a Word file.

Shell Elements (Thin Plates and Shells)

For a thin part (a plate, a tank wall, a chute) a shell model needs far fewer elements than a solid one. At the top of step 3 (Mesh) set Element type to Shell and give the thickness; the analysis is linear static.

  • Geometry: a STEP file of surfaces, or of a solid (its faces then make one closed shell; the inside is not meshed). Or use Flat plate under or use a simple shape.
  • Supports and line loads go on edges (Pick edges: click a line of the model), pressures on faces. A fixed edge is clamped or simply supported (movements held, rotations free).
  • Moment: Add → Moment (total on the edges) applies a bending or twisting moment (N·m, about the global X, Y, Z axes, right-hand rule) along the picked edges; it is spread over the edge nodes. It is drawn as a curved arrow about each axis (a negative value turns the other way). A moment about the edge's own direction twists the plate, one about an axis across it bends it. To hold a rotation instead, use Prescribed displacement (rotations) or a Fixed support (clamped).
  • Pressure direction: a positive pressure acts against the face normal; the arrows show it, and Push the other way flips it.
  • Results: the stress is given for the top face (the side the normal points to) and the bottom face, and as the worse of the two. The element is a three-node triangle (code_aster DKT, Kirchhoff theory): good for parts much thinner than their other dimensions, not for thick ones, and transverse shear is not included.
  • Checked against plate theory: a clamped square plate under pressure gives the centre deflection to 0.5 % and the edge stress to 0.6 %.

Reading the Results

  • Show picks the result: displacement, von Mises or principal stress, temperature, heat flux, or a mode shape (tick Animate).
  • Deformation shown magnifies the movement; the factor is written beside the slider.
  • Edges and Mesh draw the part's edges and the mesh over the colours.
  • Values: Nodal is smoothed over the neighbouring elements; Elemental shows each element on its own.
  • Hover over the part to read the value under the pointer. The tooltip says if it is an element's own value or interpolated.
  • Slices (button under the view) has one slider for each axis (X, Y, Z). A slider puts a cutting plane through the model and removes the part beyond it; tick Flip to keep the other side. You can also type the position in the box beside the slider. A part that is cut is closed with a face where the plane passes through the metal, on the Geometry and Mesh views too. On the results the cut face shows the stress, displacement or temperature inside the part. A mode shape has no values inside, so its cut faces stay open.
  • Downloads: the solver's result file (MED), the solver log and input, and a picture of the view.
  • While a mesh or a solve runs, a console under the progress line shows what the program prints (and a line every 30 seconds while it is busy). Afterwards, Show the mesh output (Mesh panel) and Show the solver output (Run panel) open the same text again, also for a run that was refused or failed.
  • Quality graph: click a bar to see the elements of that quality (in red, inside the see-through mesh) in the 3D view; click it again to clear. The side panel's right edge can be dragged to make the panel wider.
  • Results colours: choose the colour scheme (rainbow, viridis, plasma, magma, cool-warm, greyscale), type two values in Colour from / to to colour only between them (the rest takes the end colours, or grey with Grey outside these values), and choose smooth or banded contours. Show max and min labels the largest (red) and smallest (blue) value on the model with a leader line and lists them with their position; Make the rest transparent leaves only the elements at those values solid. The results table gives the largest von Mises stress as a nodal (smoothed) and as a per-element value, and Smoothing difference in the Show list maps where they disagree (a mesh too coarse there).

Reading Stresses with Care

  • Stress at the edge of a support or at a sharp corner is a singularity: it keeps growing as the mesh is refined. When the largest stress is at a support edge, the results and the report say so and give the largest value away from the support edges.
  • Make the mesh finer and solve again. A number that no longer changes is a result.
  • Displacements settle much sooner than stresses: compare them, and the reaction forces, with a hand calculation first.
  • Linear elements smooth the stress; quadratic ones are more accurate but their nodal values can overshoot at sharp corners, so look at the Elemental values too.

The Report

  • Press Open the report in step 7. It takes pictures of the geometry, mesh and results, then opens in a new tab with a summary, the model, the results, the limits and a sign-off block.
  • Download it as PDF or Word, or print it. It is stamped DRAFT: not checked and says so when the mesh or the results are out of date.
  • What you write in step 7 is printed as yours; the software does not check it.

Troubleshooting

  • No solid / STL not closed: export a solid body from your CAD program, or repair the STL.
  • Inverted elements: use a smaller element size, or refine round the thin feature.
  • Mesh too big: use a larger size, or refine only where it matters.
  • Solver stopped: the part is probably not held. Add or correct a support.
  • Free tier limit: the month's free solve is used; it returns at the next monthly reset, or upgrade.

FAQ

Why does the largest stress keep growing when I refine the mesh?

It is at a support edge or a sharp corner, where the stress is a singularity. Judge the stress away from those places.

Is the result checked against a code?

No. cFEA gives stresses and displacements; checking them against a code is for you and your checker.

Can I analyse an assembly?

Not yet: one solid part, linear and elastic, with no contact between parts.