Plates (Shell Elements)

Element type

Plates use flat Mindlin-Reissner shell elements: the four-node quadrilateral MITC4 and the three-node triangle MITC3, which can be mixed in one model. Both carry membrane, bending and transverse shear, have six DOFs per node like the beam elements, and report the same results. They suit thin to moderately thick plates and are not a substitute for solid elements where thickness is no longer small relative to span.

Each plate group has one uniform thickness and an isotropic elastic material. Concrete groups can also take directional kx / ky stiffness factors (see below); these are modifiers, not an orthotropic material.

Local axes and sign conventions

Local axes are set by plate geometry, independent of corner pick order, copying or mirroring. Toggle Plate Local Frame in the left sidebar to display them.

• Pressure: positive along local +z. On a slab a positive pressure acts upward, so enter gravity loads as negative values.
• Bending: Mx, My are moments per unit width producing bending stress in local x and y. They are sagging-positive, with tension on the −z face (the slab soffit), so a simply supported slab is positive at midspan and negative (hogging) over its supports. Mxy and the principal moments M1 ≥ M2 follow the same convention. In software that reports raw tensor moments, the principal moments appear swapped and negated.
• Membrane: Sx, Sy are tension-positive.

See Sign Conventions for all plate result signs.

Meshing limits

The default tile size is the smaller of the longest edge / 16 and 0.5 m. Analysis time and memory grow with mesh density, so refine only as far as convergence requires.

Mesh convergence

A successful solve does not prove that the mesh is adequate. Check convergence of each quantity used in design, because deflection, mid-panel moments and local support peaks converge at different rates.

1. Choose the result and location first, e.g. centre deflection, a support-line moment, a reaction sum or a group envelope. Keep the geometry, material, supports, loads, combinations and result recovery unchanged.
2. Run at least three successively finer meshes, roughly halving the tile size (doubling the edge divisions) at each step. Keep similar aspect ratios and compatible plate and member edges.
3. Compare the same signed result from the two finest meshes using |Rfine − Rprevious| / |Rfine| × 100%. Confirm reaction equilibrium, and check that the governing location has not moved only because the sampling grid changed.
4. Refine until the change is within a tolerance appropriate to the decision.

Concrete stiffness modifiers (cracked section)

Concrete plate groups have kx and ky stiffness factors along local x and y. Each factor scales both membrane and bending stiffness in its direction. Shear and twisting stiffness are scaled by the same factor when the two are equal, or by √(kx · ky) when they differ. Keep them equal for normal cracked concrete. Use different values only to make the model stiffer in one direction, e.g. a one-way slab or ribbed deck modelled as a plate.

Lower factors make the plate more flexible, so it attracts less force. In walls and diaphragms this changes the lateral force distribution as well as the deflection. Thickness, mass and self-weight are not changed. The presets apply the same factor to kx and ky, and a blank field means gross stiffness.

Factors range from 0.05 to 1.0. For other codes, such as AS 3600 or Eurocode 2, enter a custom factor.

Visual style by material

Plates are tinted by material family: blue-grey for steel, warm grey for concrete, tan for timber and blue for other materials. Edges are always drawn.

Editing and re-meshing

• Edit the thickness and material of each group in the list.
• Re-mesh (pencil icon) regenerates the grid from the original corners (4 for a quad, 3 for a triangle) at a new tile size, restoring any deleted sub-elements.
• Delete removes the group and its interior nodes.
• Groups whose tiles differ in thickness, material or modifiers show as mixed until a uniform value is set.

Connecting plates to beams

A beam or column connects to a plate wherever its line passes through plate corner or mesh nodes, with no manual links needed. A beam along a plate edge remains one member, and its force diagrams show the plate load transfer as a smoothly varying load. Member end forces are the solved values.

Columns connected to slabs

A column that meets a slab at a mesh node is connected over its cross-section rather than at a single node, so slab moments around the column stay finite as the mesh is refined. Column sections are shown hatched on plate contours.

Connection area. Rectangular, round, drawn and section-builder tee sections use their solid outline. Steel and other thin-walled sections use their bounding rectangle. The area is centred on the member axis and follows the member's rotation, sideways setting and end offsets. Where the columns above and below the slab differ, their common area is used. Any part of the area beyond a slab edge or over an opening carries no load, and a warning is shown if it extends more than 5 mm (or 2% of the section width, if larger) past the edge.

Single-node connections. A column connects at a single node instead when any of the following applies:

• A beam frames into the node, ending at it or passing through it.
• The node has a support, is a rigid diaphragm master, or is tied to a beam along the slab.
• The column is inclined more than 10° from the slab normal.
• The section has no defined size, or the slab mesh under the column is too irregular.

The Plate Analysis dialog lists these columns with the reason. A slab node that is only a diaphragm slave does not prevent a full-section connection. Members framing perpendicular into a wall or other plate are connected in the same way as columns.

Mesh density. Near columns, use tiles no larger than about the column width. A warning lists columns where the tiles exceed twice the width of the column section on the slab.

Effect on results. A full-section connection is stiffer than a single-node connection. In flat slabs without beams, edge and corner columns attract more moment, slab moments at the column faces are higher, span moments are slightly lower, and deflection and sway are smaller. Interior columns change little. Where a beam frames into the column, the beam already ties the joint and results are similar to a single-node connection.

Plate–beam connections

• Slabs and decks on beams: translations and bending rotations are continuous, so the joint is not an unintended hinge.
• Walls on beams: load and translation transfer fully, but the wall does not restrain beam rotation about the wall normal. Add restraint or framing if required.
• Offsets: a plate node a small numerical distance off a beam axis is still connected. A genuinely offset beam (e.g. a downstand) is not; set the member eccentricity to the real offset.
• Rigid, not bearing: an eccentric beam is rigidly connected and transfers uplift and tension as well as gravity load. Gap, lift-off, slip and friction are not modelled.

Loads on plates

Apply a surface pressure in the current pressure unit (e.g. kPa or psf), either uniformly to a group or to selected elements, or as a linear ramp over a group. See Plate Loads for ramp axes and mesh guidance.

Linear ramps are area-averaged per tile, so they are mesh-stepped. Like any applied load, a plate surface load contributes mass to modal analysis through its gravity-direction component.

Analysis support

Results

Contour results for any analysed plate group across its mesh. The legend's Smooth / Bands toggle switches between a continuous gradient (with steps kept at supports, beams, walls and columns) and discrete colour levels. It changes the display only, not the values.

Moments, shears and stresses are smoothed across neighbouring elements, but not across supports, connected beams, walls, columns or point loads, so real steps in shear are kept. Spring supports also break the smoothing, except mat foundation springs. At interior line supports, beams and walls, the moment across the line is recovered from each side's own elements, giving the peak at the line rather than the value half an element away. Smoothing can still soften sharp changes near concentrated loads, mesh edges and openings. Refine the mesh there, and use the Summary dialog or the Pro Excel export for per-element values.

The Summary dialog and Pro Excel reports tabulate per-element results and per-group envelopes; Pro PDF reports give per-group envelopes only. Envelopes give the peak sagging (max) and hogging (min) moments, Wood-Armer demands and, in envelope mode, the governing load combination.

Limitations

• Flat elements only. Curved surfaces are faceted, and warped (non-coplanar) quads are rejected. There are no curved-edge elements.
• Full composite action. A slab acts compositely with a beam only when the member eccentricity is set to the real offset, and then with full (rigid) shear interaction and no slip, which can be unconservative relative to partial-composite design.
• Members crossing plate interiors are not embedded. Split the mesh so the member lies on shared plate nodes or edges; otherwise no force transfers along it.
• Qx, Qy are mesh-sensitive. The resultant is more stable than the signed components, which can vary sharply near supports, corners, beam tie-ins and zero crossings. Refine where shear governs, and check punching and one-way shear on integrated shear (control perimeter or section cut from the reactions), not a single peak.
• Wood-Armer uses bending only. Bars are assumed along local x and y (or along and across a strip in Plate Analysis). In-plane forces (post-tensioning, transfer, diaphragm) are excluded; design for combined bending and in-plane force where significant.
• Peaks at concentrations are mesh-dependent. At point restraints, concentrated loads, beam/column tie-ins, sharp mesh corners and opening edges, design from averaged or integrated values, not a contour peak.
• Linear elastic, linearised stability. No cracking, yielding, contact, large displacement or post-buckling.

Model Health checks

Plate issues are reported in the Model Health dialog.