FEMcell: how to use it

1. the screen
2. load an example
3. import CAD or a mesh, or build a body
4. thickness and material
5. meshing
6. element type and integration
7. picking where things go
8. supports, springs, enforced displacement
9. links and MPCs
10. contact
11. large deflection
12. loads
13. reading results
14. modal and buckling
15. limits

01the screen

Toolbar: examples, import, open json, save json, then mesh, solve and results. Models save and open as JSON files.

Left list: mesh settings, then bodies, points, sets, links (rbe2 / rbe3), mpcs (tie / equation), supports, loads, load cases, combinations, contact and analysis. Each group has a + add button. Pick an item to edit it.

Right panel: edits whatever is selected.

Show and hide: ctrl+b hides the selection, ctrl+shift+b shows only the selection and ctrl+shift+u shows everything. This works on bodies, elements and markers. Each body in the tree has an eye toggle, and mesh lines have their own toggle. Drag panel edges to resize them; the legend can be dragged too.

View: the mouse works as in NX. Middle-drag rotates freely, with no stop at the poles. Press and hold the middle button on the model for a moment to rotate about that point (a small cyan marker shows it); otherwise the view rotates about its centre. shift+middle-drag or middle+right drag pans. ctrl+middle-drag or left+middle drag zooms; scroll zooms toward the cursor. Left click picks and left-drag box-picks. A right click opens a small view menu: fit, iso, top, front, side, reset. f or ctrl+f fits the view and home resets to iso. On a trackpad, alt+drag rotates and alt+shift+drag pans. Two-finger pinch zooms and pans on touch. Over the view, scroll and pinch move the model only, not the page. On screens wider than 900 px the page itself doesn't scroll: each panel scrolls on its own. The iso, top, front and side buttons snap the camera, and fit brings the whole model back. bg sets a background image, GIF or video from a file or link, with opacity and speed sliders. It can also put one GIF on every element, tinted with the contour colour and playing faster at higher stress.

Units: set per model by units in the model file: N-mm-MPa (default, also written SI or mm), N-m-Pa, lbf-in-psi or consistent (no unit labels). Every length, force, stress, stiffness and density in the file is read in that system. Imports and the examples use N-mm-MPa.

On a phone the three panels become tabs: model (the list), view (3D) and edit (properties).

02load an example

Press examples, pick one and press solve. Each one shows its hand-calc values under reference values.

• l-bracket: 2 mm 6061-T6 angle bracket bolted at two M5 holes (RBE2), 50 N down on the free flange. Bending stress at the end of the bend: 93.8 MPa by hand.
• pressure vessel: 2 mm steel tube with hemispherical end caps, 1 MPa inside. Mid-length hoop stress pr/t = 50 MPa, axial stress 25 MPa.
• chassis panel: 3 mm aluminum robot base plate, motor weight and torque spread into four bolt holes with RBE3, on springs at the wheel mounts. Sum of vertical spring reactions 29.02 N.
• mpc tie: a cantilever plate built from two separately meshed halves joined with an equal-dof tie. mpc tie reference is the same plate in one piece. Tip deflection PL³/3EI = 4.30 mm for both.
• load cases: a 1.6 mm 2024-T3 sheet cantilever with two load cases, a 1.5 x combination and the envelope.
• wing box, full semi-span: 6 m swept, tapered two-spar box with 10 ribs (Ti-6Al-4V pylon and gear ribs), 12 Z-stringers per cover, thickness zones, and an access-panel row with doublers. 7075-T6 upper cover and spars, 2024-T3 lower cover and ribs. Engine and gear loads enter through RBE3 fittings. Five load cases plus four 1.5 x ultimate combinations, about 263k DOF, roughly 90 s to solve.
• modal: simply supported square plate and modal: cantilever plate: natural frequencies against closed-form values.
• buckling: simply supported plate, uniaxial compression (k = 4) and buckling: Euler column, pinned-pinned: buckling loads against closed-form values.
• wing box, ribs + stringers: 1200 mm span, 400 x 120 mm box clamped at the root. 2024-T3 skins, 7075-T6 spars and stringers, three ribs with lightening holes and a 100 mm access hole in the lower skin, joined by welds. Three load cases plus a 1.5 x ultimate combination, about 96k equations.
• honeycomb sandwich panel: 303.1 x 200 mm, 12 mm core of 10 mm hex cells, every cell wall a shell between 0.8 mm 2024-T3 skins, with a potted insert. Three cases: pressure, 3-point bend and insert pull. 3-point bend face stress is within 5% of sandwich theory.

03import CAD or a mesh, or build a body

Press import (STEP, IGES, STL or OBJ) or drop the file on the page. A dropped .json opens as a model.

STEP and IGES

Import report, shown before anything is added:

Imported CAD bodies are 6061-T6 with Q4 elements, quad shape and element size = bounding-box diagonal / 40. Curved edges get at least one division per 18° of turn. Four-sided CAD faces get a structured all-quad mesh. To size CAD edges, pick edges, a chain or a loop and choose edge sizing on the selection bar: set an element size (a maximum: the count rounds up) or a number of elements (1 to 2000 per edge; closed edges such as a hole need 3 or more), with an optional bias ratio (largest / smallest element, 1 to 1000; small at the start, the end, the middle or both ends). On a chain or loop, the start follows the chain from the first picked edge, and an arrow beside each edge points from the small elements to the large ones; the flip boxes turn single edges round. An edge split by a weld keeps its count and bias, with a node moved onto the split. If an edge is in two edge sizings, a number of elements beats a size, the smaller size wins, the later number wins, and the winner's bias is used. Edge sizing is saved by edge name, so it holds through a remesh, and the seed marks show where the mesh nodes will go. Selectors: body/face:Fn, body/edge:En and body/boundary. Edge seeds use the key edge:En. If a free edge lies on another CAD body with no weld between them, solving gives a heads-up naming the edge.

STL and OBJ

A surface mesh comes in as the mid-surface of a shell body named part, 2 mm thick, 6061-T6, T3 elements. Nodes closer than the merge tolerance are joined. Units are read as mm, so a part 25.4× too small was exported in inches. Limit: 60k nodes per import. A closed solid STL comes in as its outer skin.

Build: flat plate, bent plate (bracket), cylinder or tube, cone, curved roof, box with any faces open, hemisphere (dome) or sphere. Built bodies have named edges and holes, so supports, loads and refinements can snap to them. Holes are available on plate and bent plate bodies.

04thickness and material

Set thickness per body. It's the full wall thickness, centred on the mid-surface. Pick a material from the list. The list gives typical E, Poisson's ratio and density with a source for each. Allowables come from public-domain MIL-HDBK-5J where we have them.

For your own material, right-click Materials in the tree (or press +) and enter E, Poisson's ratio, density and, optionally, Fty and Ftu. duplicate as custom copies a built-in so you can edit it. Custom materials are saved in the model and in a library in this browser, which you can import and export as a file. The allowable check uses a custom material's Fty and Ftu when they're given. Density is in kg/m³; E, Fty and Ftu follow the model's units. A copy of a built-in keeps "user, copied from" and the original citation in its source. Built-in ids (for example the 5J fem- ids) can't be reused: a custom material or library entry with one is given a new custom- id. E must be between 0.0001 and 2,000,000 MPa, Fty can't be more than Ftu, and names must differ. The stress check also gives max von Mises / Ftu for a custom material with Ftu.

Rigid parts: set stiffness behavior to rigid in a part's details. The part moves as one piece tied to its centroid, or to a reference point you pick; supports, loads, gravity, contact and welds still act on it. Its mass, centroid and inertia show under resolved. Results show its displacement and no stress (blank in the csv). Rigid parts welded together move as one about one reference point; giving them different points is an error. In buckling, the part adds no stiffness of its own; the loads it carries turn with it. With large deflection on, it turns with its reference point at any angle; supports, links and welds on it stay small-rotation.

05meshing

Open the mesh panel with mesh on the toolbar or mesh settings at the top of the left list. Each body also has a mesh block in its own properties. Geometry and mesh edits remesh automatically. Any edit marks the last results out of date.

mesh panel

Which size wins: a refinement, then the body size, then the global size, then auto. Auto is 1/20 of the longest side of the body's flat (u, v) layout. An imported body keeps its own triangles unless remesh at this size is ticked.

body mesh block

refinement targets

The refine button on the selection bar does the same as + refine: a named hole, edge, bend or line is used as-is, anything else becomes a box around the picked nodes padded by 0.25 x the body size. Refining something already refined keeps the smaller size. On a mapped mesh the refined size fills the rows and columns that cross the target. On a free mesh the size grows away from the target by 0.3 x the distance until it reaches the body size.

method, seeds (model file only)

merging

Nodes closer than the merge tolerance are joined into one. Set it on the model row, under advanced (mesh.tol); default 1e-6 x the model size. To keep bodies apart so an MPC can join them, tick keep bodies unmerged on a tie, or set "merge_coincident": false under mesh in the model file. Nodes still merge inside each body.

mesh quality

After a mesh the panel lists mesh quality with the quad and tri counts, then metric, worst, limit and count over. show highlights the elements over a limit.

An inverted or zero-area element is an error and names the element. plot mesh quality (or mesh quality under show) colours each element by its worst metric over its limit, 1 = at the limit. The same check is in results > diagnostics.

Size limits: 1,500,000 elements and 4,000,000 degrees of freedom, or less if the browser runs out of memory. Meshing stops with an error above either. Models over 120,000 degrees of freedom use a multithreaded iterative solver; smaller models, contact, modal and buckling use the direct solver. Chrome runs it on several threads, Safari on one.

06element type and integration

Each body has its own element type, integration scheme and drilling factor, under the body's advanced settings.

integration (Q4)

T3 always uses exact integration. Selective is not offered; files that ask for it run as mitc with a heads-up.

drilling factor: in-plane twist stiffness as a fraction of G·t·A. Default 0.03, range 0.01 to 1.

07picking where things go

Supports, loads, links, MPCs, refinements and sets act on a set of nodes or faces. Pick in the 3D view, type the set, or pick a name from the dropdown, which lists the edges, holes and faces your bodies have.

• Pick mode: node, edge, face, body or vertex (keys 1 to 5). Click the active mode again to turn picking off. vertex picks only the corners of imported CAD (its B-rep vertices), for point loads and supports that follow the model through a remesh.
• Edge chains and loops: in edge mode, double-click an edge to pick its tangent chain, or hover an edge and press L to pick the boundary loop of the face under the cursor (shift+L adds, ctrl+L toggles). On imported CAD, chains and loops are saved as their CAD edge names, so loads, supports and edge sizing on them follow a remesh.
• Imported CAD: in the geometry view, edge and face picks select the CAD's own edges and faces, not mesh lines, so edges that meet in a line but are separate in the STEP or IGES file stay separate. These picks are saved by name and follow the model through a remesh.
• Click picks what's under the cursor, ctrl-click (cmd on a Mac) toggles an item in or out of the selection, shift-click adds and ctrl+shift-click removes. Hovering highlights the edge, face or body that a click would pick. Double-click picks the whole named edge, hole or face it belongs to.
• Left-drag from empty space for a box pick. A box pick replaces the selection; use shift-click to add. visible only (on by default) limits the box to what you can see.
• angle tol, deg (default 30): faces grow across neighbours whose normals turn less than this, and edges follow the loop while it turns less than this.
• The selection bar turns the pick into a support, load, rbe2, rbe3, mpc, refine or save set. pick next to a field fills that field: pick, then done, Enter or right-click. Esc cancels.
• In node mode, clicking a node after a solve shows its displacement and stress.
• Picking in the view needs a mouse. On touch, type the set or use the dropdown; tapping a node shows its values.

A set saved from named geometry follows the model through a remesh. A set saved as raw node or face ids stops matching when the mesh changes; re-pick it.

coordinate systems

The coordinate systems folder under geometry holds global and any local systems. + adds one, from the current pick if there is one. Each system is cartesian or cylindrical (r, θ, z about its z axis).

• origin: typed, or from a pick: a vertex, an edge midpoint, a circle centre, a face centroid or a cylinder axis.
• z axis and x axis: typed, or from an edge direction, a face normal or a cylinder axis. reverse flips a picked axis. x is squared to z.
• Selecting a system's row shows its triad in the view. Picked systems follow a remesh.
• Results: the coordinate system dropdown in a result's details turns displacement components and stress components into that system. The legend, the probe, the through-thickness view and the reaction probe name the system.

08supports, springs, enforced displacement

Pick where the support goes, then the kind. Directions 1-3 are moves along x, y, z; 4-6 are rotations about x, y, z.

• fixed (all 6)
• pinned (moves only): 1-3 locked.
• pick directions: lock the ticked directions.
• symmetry plane: locks the move normal to the plane and the two in-plane rotations.
• antisymmetry plane: locks the two in-plane moves and the rotation about the normal.
• enforced displacement: set moves (length unit) and rotations (rad) per direction; blank leaves it free. The reaction is reported.
• spring to ground: kx, ky, kz (force / length) and krx, kry, krz (moment / rad).

coordinate system turns the directions of pick directions, symmetry, antisymmetry and enforced displacement into a local system: 1-3 are its x, y, z (r, θ, z when cylindrical). Springs take their k along the local directions too.

If something can still slide or spin, the solve stops and names the node and direction that's free.

09links and MPCs

Ties, equations and couplings are solved by elimination (default, exact) or penalty (penalty factor default 1e5 x the largest diagonal it touches; 1e3 to 1e7). They are under mpcs in the left list and under mpcs in the model file. The mpc tie example shows the layout. After a solve each MPC lists its equation count, max violation and max force.

10contact

A pair has a surface it lands on (faces) and a pushing side (nodes), and a type: bonded, frictionless, frictional (set μ) or none (kept in the file, off). Advanced: method (penalty default, or augmented lagrange), penalty scale (default 1), search distance (default auto) and initial gap (default from geometry). Contact load steps (default 1), max iterations per step (default 30) and convergence tol (default 1e-4) are under analysis.

• Node-to-surface, small sliding. Each pushing-side node is paired with the nearest face on the undeformed mesh, again after every remesh.
• The gap is skin to skin: mid-surface distance minus half of each thickness. Face normal direction does not matter. Sliding and friction act at the skin, so bending moves the contact point; bonded also ties in-plane rotations through the offset. Search distance auto is 2 x the larger half-thickness.
• Frictionless or frictional skins overlapping by more than 1% of the thinner sheet stop with an error; set an initial gap to override. Pairing two faces of the same shell is an error. Thinning under load is not tracked.
• Penalty stiffness is 100 x the stiffer side's diagonal x penalty scale. Augmented lagrange repeats the solve until the overlap is under 1e-3 x the thinner wall (or max_overlap).
• A step that does not converge is cut in half, up to 5 times.
• Results: contact pressure and contact status (0 open, 1 slip, 2 stick) plots, a contact line in the summary and the contact convergence table.
• With contact on, each combination is solved as its own nonlinear case from the factored loads, not added up. Contact models use the direct solver.

10blarge deflection

static structural → analysis settings → large deflection ("analysis": { "large_deflection": true }) makes the static solve geometrically nonlinear: large rotations, small strains.

• Corotational T3 and Q4 shells. Full Newton with 10 load steps by default (number of load steps; max iterations and convergence tol under advanced). A step that does not converge is cut in half, up to 10 times, unless auto cut-back is off ("auto_cutback": false).
• Pressure follows the deformed faces, and its load stiffness is in the Newton tangent. Forces and moments keep their direction.
• A follower pressure on a free end (a pad on a cantilever tip) is not conservative, so it gets no buckling or snap-through heads-up. Neither do moments.
• Links, MPCs, springs and supports in a coordinate system stay linear (small rotation at the control point). Contact pairs come from the undeformed mesh. Each combination is solved as its own case.
• Load control only: a snap-through or buckling point gets a heads-up, and the path through it is not traced. Modal and buckling analyses use the linear static state.
• The deformed shape is drawn at true scale. The summary and status bar give steps and iterations. Click a row in the step table to see that step's displacement; stresses are for the last step.
• Up to 60,000 elements, direct solver.

11loads

• force on a set or control point. spread: total (default) splits the value along the set by edge length; each puts the full value on every node. An optional moment can go with it.
• moment on a set or control point.
• pressure on faces. direction: along face normal (default), outward or inward from the middle of the picked faces.
• gravity: an acceleration vector, default -z, applied with each material's density. 1 g = 9810 mm/s² in N-mm-MPa.

Force, moment and gravity take a coordinate system; the components are turned at each node, so in a cylindrical system fθ is tangential everywhere.

Each load and support can belong to one or more load cases. Combinations are factored sums of cases.

12reading results

• deformed shape is drawn at the scale factor shown. Displacements are in the model length unit.
• surfaces: top (z = +t/2), mid (z = 0) and bottom (z = −t/2), linear through the thickness.
• what you can plot: von Mises, signed von Mises (the sign of the larger in-plane principal), principal s1 and s2, Tresca and max shear, membrane von Mises (mid) and bending von Mises ((top − bottom) / 2), σxx, σyy, σzz and τxy in global axes, σxx, σyy and τxy in surface-local axes, displacement, contact pressure and status, thickness, material, mesh quality and the error estimate. The legend names the field, the surface, the averaging and the units. Show top, mid, bottom or worst of the three.
• local axes: z is the averaged element normal, x is global X projected onto the surface (global Y where the normal is within 17° of X), and y = z × x.
• through thickness: local stresses at one node at bottom, mid and top, with membrane and bending parts, as a table and a plot. Stress is linear through the thickness.
• error estimate: the raw element stress minus the smoothed nodal stress, in stress units.
• averaging: nodal averaging in the shared surface axes at each node, so curved shells average correctly, with a least-squares fit of the element-centre values at clamped and free edges.
• allowable check compares the max von Mises stress to the material's yield and also gives the peak away from links and supports. A MIL-HDBK-5J entry is used only when its thickness range covers the body thickness, in the body's grain direction (L, LT or ST) if you set one, and the check names the entry, range and direction. If no entry covers the thickness it says "no 5J allowable for this thickness" and gives no ratio. It never borrows the nearest range.
• reactions: the summary under Solution lists each support's force and moment (about the origin), the sum, the applied load and their balance, plus the force carried by each link and MPC. copy copies it as a table and export csv writes every case.
• insert reaction on a support, link or MPC (right-click it, or drag it onto Solution) adds its own reaction probe. Pick moments about the centroid, the origin, a node or a point, in global or local axes, for one case or the envelope max or min.
• free-body cut: pick faces or a body for the part, and edges for the cut line, then right-click in the view and choose insert reaction. It gives the internal force and moment across the cut. Picks on CAD faces and edges survive a remesh.
• result: with load cases, pick a case, a combination or the envelope. download csv exports one case or combination. With a results coordinate system picked, its u, rotation and stress columns are in that system (ur, uθ, σθθ, ...) and the first line names it.

12bmodal and buckling

• add one from the + on static structural: modal analysis or eigenvalue buckling. Each gets its own branch and its own solution.
• modal settings: number of modes (default 6), an optional range min / max in Hz, consistent or lumped mass, and supports the same as static structural or none (free-free; the 6 rigid modes come out at 0 Hz). Every material needs a density. In the results, download csv gives the mode table and download mode shape csv the shown mode (buckling too).
• point masses go under connections: a mass (and optional ixx, iyy, izz) spread over the picked nodes. They also add weight under gravity.
• buckling runs on the static loads (or the load case you pick) and reports load multipliers λ: buckling load = λ × applied load. Linear (bifurcation) only.
• results: the solution table lists mode, freq in Hz and effective mass in x, y and z as a % of the total, or mode and λ for buckling. Click a row, or pick a mode under total deformation, to plot it. Mode shapes are normalized to max |u| = 1, so the legend has no units. Play animates the shape.
• solve runs static structural first when there are loads, then every modal and buckling analysis. With no loads it runs only the modal analyses.

13limits

• Small displacements unless large deflection is on (large rotation, small strain). Static, modal and linear (eigenvalue) buckling; contact and large deflection are the only nonlinearities. Linear elastic isotropic materials only (E and Poisson's ratio). No orthotropic or laminate shells, plasticity, arc-length post-buckling, fatigue or transient dynamics.
• Contact is node-to-surface with small sliding. No self-contact or surface-to-surface.
• One thickness per body.
• T3 and Q4 elements only. T6 runs as T3; Q8 and Q9 run as Q4.
• 1,500,000 elements, 4,000,000 degrees of freedom, 60k nodes per mesh import.