2. Modelling

This chapter is the reference for every modelling tool, its dialog fields and
defaults, the editing and selection mechanics, the material library, the grid
and setout system, validation, and the meshing rules applied before analysis.

All modelling is done in slab mode (the only mode); the semantic model is
stored under FloorModel and saved with the project.

2.1 Tools at a glance

While a drawing tool is active its options appear in a small draggable panel
(titled Slab, Column, Wall, …). The ×/Done button hides the panel
but keeps the tool armed - the next canvas click continues drawing. Press
Esc to leave the tool.

2.2 Slabs

A slab is a flat polygon at one elevation and one thickness. All structural
action starts from slabs.

Slab tool fields

Drawing a slab

1. Click the Slab tool.
2. Click each polygon corner. Corners snap to the grid/nodes per the Grid &
   Snap settings.
3. Finish with double-click, Enter, or by clicking within 0.5 m of the
   first corner. Fewer than 3 corners is rejected with
   slab outline needs at least 3 corners.
4. The slab gets the next name S<n> and a running numeric id. The status line
   suggests click MESH to generate the discretized mesh.

Editing

• Move a corner: click a corner handle and drag it (snaps live). On release
  the status reports Corner n moved to (x, y); the mesh/results are
  invalidated.
• Add a corner: open Edit slab shape for the slab and click a +
  handle on an edge.
• Delete a corner: open Edit slab shape, click the corner, then
  Delete node (or press Delete). A polygon must keep ≥ 3 corners
  (A polygon needs at least three corners).
• Offset edges: in Edit slab shape: distance (default 0.3 m, positive
  outward), edge selection All edges or Edge i (L m), then Apply
  offset. While the editor is open, every edge shows its number next to it
  in the canvas, and the edge picked in the dropdown is highlighted on the
  slab - the pick stays selected after each offset so repeated nudges keep
  working. Neighbours stretch to remain connected.
• Properties: Elevation, Thickness, Concrete grade, Span behaviour, E, ν,
  Density, Mesh size.

Slab shape editor (Edit slab shape)

Touching same-elevation slabs mesh together automatically: shared edge
segments and common coordinates merge within 1e-6 m, and the connected group
adopts the finest mesh size of its members.

2.3 Openings

Openings are axis-aligned rectangles cut from one slab. Steps:

1. Click Opening, then click two opposite corners.
2. The rectangle centre must lie inside a slab, else
   Opening must be drawn inside a slab region.
3. The opening is stored against that slab and named Opening <n>.

Validation at mesh/analysis time: the rectangle must be four-sided and
axis-aligned, lie fully within its slab, and not cover the entire slab.

Point loads inside an opening are rejected (point load N lies within a slab opening); area loads over openings apply only to elements outside them.

2.4 Columns and point supports

Column tool fields

Place with a single click. The status line reports the coordinates and Z range
(Column at (x, y), z = a → b) or the support type and spring.

How columns are modelled

• A column is a vertical beam stub of the given section and heights,
  meshed as a chain of beam elements (E = 30 GPa, ν 0.2, ρ 2400 unless the
  slab material applies). It carries self weight through its density and is
  included in the vertical load path.
• Its stiffness matrix uses Iy = w·d³/12, Iz = d·w³/12 and a Timoshenko
  rectangular torsion constant; Stiffness (%) scales all three.
• A point support restrains the nearest slab node
  (within max(0.2, 0.75 × mesh size)) in Z (fixed/pinned/spring) with no
  section or self weight.
• The column top/bottom restraints act on the stub ends; a Top = None
  column is laterally stable only through the slab (the solver's in-plane
  stabilisation handles it), so use pinning/fixing where the structure
  actually provides it.

Bulk edit: select several columns and edit Shape, b, h, d, Z bottom/top,
Bottom/Top boundary and Bending stiffness % together.

2.5 Piles

Pile tool fields

Placement: one click; the head sits at the host slab elevation and the tip at
head − length. Drawing a pile switches the model mode to pile_supported.

How piles are modelled

• If Diameter > 0 a vertical beam chain is generated (segment length ≈ 1 m,
  at most 20 segments), EI auto-derived from the diameter unless you give a
  value.
• Head springs: Kx = Ky = Lateral k, Kz = Axial k, Krx = Kry = Krz = Rotational k, placed at the tip node. The head link length is 0.05 m; a
  pinned head uses a tiny (0.001·I) link stiffness, a rotational spring uses
  I = k·L/E.
• With Diameter = 0 the pile is a set of head springs only (no shaft).
• Pile soil layers add distributed shaft springs: each meshed shaft node
  receives Kx = Ky = LateralK × tributary length and Kz = Skin × tributary length from the layer(s) it spans. Layers are global (shared by all piles).
• Pile head must land on the generated mesh within 1e-7 m, otherwise
  pile N head does not lie on the generated mesh (move the pile or refine the
  mesh so a node exists at the head).

Pile soil layers modal

Title Pile soil layers - columns Name, Top (m), Bottom (m),
Lateral k (kN/m/m), Skin (kN/m/m); delete × per row; + Add layer.

New-layer defaults: name Layer <id>; top = previous bottom (first layer top
starts at 0); bottom = top − 5; lateral k 5 000; skin 1 000.

Rules (enforced at validation): top must be above bottom; stiffnesses ≥ 0; at
least one of lateral/skin > 0. Layer elevations are measured in model Z
(elevations, not depth below head). Empty state text: "No layers - pile shaft
support comes from the tip springs in the pile inputs."

See Chapter 7 for the p-y/skin model and worked
numbers.

2.6 Soil zones

Draw with two clicks (rectangle); the panel has one field:

Drawing the first soil zone switches the model to slab_on_ground. Zones
auto-cycle through colours and can overlap; each zone may also display an
allowable bearing value used for the bearing result annotation.

Properties: Name, Subgrade modulus, No tension (compression-only
contact), Opacity slider (0.75 body / 0.2 for light ground), Colour.

Each meshed slab node inside a zone gets Kz = k × tributary area (kN/m).
Rules:

• slab_on_ground requires at least one soil zone; k must be > 0.
• subgrade modulus must be greater than zero - every zone needs k > 0.
  Tick Compression only for no-tension contact; the solver iterates it.

Typical k values (kN/m³): soft clay 5 000–15 000, firm clay 15 000–40 000,
loose sand 15 000–30 000, dense sand 40 000–100 000, rock 200 000+.
See §7.1.

2.7 Walls and line supports

Wall tool fields

Drawing: two clicks; length ≥ 0.1 m; start and end must lie inside the same
slab. The wall's z_bottom/z_top derive from the extent and height.

How walls behave

• A Wall is meshed with wall plates on the chosen side(s) of the slab,
  densified to the local mesh size; material follows the slab unless overridden
  in Properties (f′c, E, ν, ρ).
• Below-slab run: the base restraint acts at the foundation
  (z_bottom): Free, Pinned, Fixed, Point spring or Line spring.
  Support every base node applies the restraint along the whole base -
  uncheck it to model isolated corner restraints.
• Above-only wall: it bears on the slab. Its base edge shares the slab's
  mesh nodes, so the Base restraint is ignored (including base springs) and
  the wall cantilevers from the slab. The top edge is held only by an explicit
  Top restraint (Free / Pinned / Fixed) - use it to tie the wall to the
  structure above. This means an above-slab wall never supports the slab, and
  the ground/soil springs carry the model as drawn.
• A wall spanning both sides meshes below and above with one shared edge:
  the base restraint acts at z_bottom, the top restraint at z_top.
• Wall springs are vertical only (Kz) in the current implementation; there
  is no horizontal soil pressure.
• Wall self weight is applied as nodal line loads
  (w = width × height × density × 9.81/1000 kN/m) unless the wall has an
  explicit SelfWeightCase.
• Below-slab walls carry no density (their weight is not double-counted
  with the ground path); above-slab walls carry it.
• A wall's Top line load (kN/m, positive down) and its Load case are
  entered in Properties. The load belongs to that case like any other load:
  it is drawn and factored only when the case (or a combination containing it)
  is active. If the case is left unassigned, the first load case is used.
  When wall plates exist, the load is applied at the top edge; otherwise the
  load falls back to a slab line load.
• A Line support is not meshed: it is a restraint line (fixed/pinned/spring)
  on the nearest slab nodes, with no stiffness or weight of its own.

2.8 Edge beams (bands)

The Beam tool draws a band along an edge between two clicks inside the same
slab.

The beam hangs below the slab: z_bottom = slab elevation − depth,
z_top = elevation + 0.02; the slab thickness at that location is deducted
from the beam section (D − t) so stiffness and weight are not double counted.

Properties:

Design along bands uses the band total moment (kN·m, not per metre) and stays
out of the shell moment contour unless B± is enabled in the results pane.

2.9 Drop panels

Two-click rectangle inside a slab; field Thickness t (m, default 0.45,
≥ 0.1). Drop panels thicken the slab locally (element thickness = maximum
covering panel) and their outline becomes a mesh feature line. No extra self
weight beyond the thicker shell volume. Name Drop <n>.

Use them around punching columns, or the local head depth is picked up by the
punching check from either a drop panel or a band beam.

2.10 Vertical plates (steps)

Draw two clicks along the step line between two slabs at different elevations.

Preconditions:

• length ≥ 0.1 m (Vertical plate length too short);
• both slabs must exist under the midpoint
  (Vertical plate needs two slabs at different levels under the line (a step));
• both ends must lie over the lower slab
  (Plate ends must lie over <low slab name> (the lower slab));
• the step height (upper elevation − lower top) must be ≥ 0.05 m.

The plate closes the vertical face between the slabs, participating in bending
and in the load path.

2.11 Design strips

A design strip is a rectangle spanning between two points inside one slab,
over which results are integrated and design is performed.

Strip tool fields

Auto fields are not stored - the program sizes them. Drawing requires start
and end inside the same slab and width > 0
(Design strip width must be greater than zero).

Strips are repaired on save/load: endpoints clamp onto the owning polygon and
the width shrinks (binary search) until the strip rectangle lies inside the
slab (default 0.5 m minimum fallback). A strip must also satisfy
design strip must lie fully within its slab region after repair.

Width guidance: a column strip is typically 0.25·L each side of the column
line (total 0.5·L); the middle strip fills the rest of the bay. Draw one strip
per band and per direction, or use ＋ Add strips to materialise the
automatic centre strips the program shows when none exist (one X and one Y
through each slab's bbox centre, inset 5 %, width max(0.5, 0.5 × the other dimension)).

Strip Properties - four tabs

Geometry

Reinforcement

Top bar / Top spacing / Bottom bar / Bottom spacing (Auto or explicit), and a
Copy from strip… selector with Copy to clone another strip's bars.

Limits

Section

Two results are names you will see: B-span (bottom, spanning direction),
B-dist, T-span, T-dist in diagrams and reports.

2.12 Properties pane

Select one entity to edit it. Every field applies on change; Apply
persists; Delete removes it; Deselect clears. Geometry edits invalidate
the mesh and results; grid-line, measurement and strip edits do not.

Bulk editor

Select several entities of the same type (or click a type chip to edit one
type within a mixed selection). Fields that disagree show (Mixed). Numeric
fields per type:

• Columns: Shape, Width b, Depth h, Diameter, Z bottom, Z top, Bottom/Top
  boundary, Bending stiffness %
• Piles: Axial/Lateral k, Diameter, Bending EI, Rotational k
• Slabs: Elevation, Thickness, f′c, Span behaviour, E, ν, Density, Mesh size
• Strips: Width
• Walls: Width, Z bottom, Z top, Base restraint, Self wt case
• Edge beams: Width, Depth, Z bottom, Z top
• Drop panels / Vertical plates: Thickness
• Soil zones: Subgrade modulus
• Loads: Load case plus Fx/Fy/Fz (force, force/m or pressure by type)

Buttons: Delete N and Deselect.

2.13 Selection and editing

Picking

• Click replaces the selection; Shift+click adds; Ctrl/Cmd+click
  toggles.
• Overlapping entities: repeated clicks cycle through everything under the
  cursor (status: N items under the cursor - click again to cycle through them).
• Drag from empty space for a marquee: plain = replace, Shift = add, Ctrl =
  toggle. The marquee works correctly in tilted views.
• A selects all entities allowed by the type filter; X or Esc clears.
• The Filter chips limit what can be picked and what A selects. All
  cycles all-on → all-off → all-on; the dropdown shows a per-type list.

Moving and deleting

• Slab and soil-zone corners drag with snapping; whole entities move via
  Properties X/Y.
• Delete / Backspace deletes the selection (multiple entities supported).
• Deleting geometry clears the mesh and results. Rules worth knowing:
  • deleting the last pile returns the model to slab_on_ground/suspended;
  • deleting a grid line or measurement never invalidates results;
  • deleting a polygon corner below 3 corners is refused.
• There is no undo - Duplicate the project before wholesale edits if you
  need a safe point to return to.

2.14 Grid, setouts, dimensions and measurements

Background grid

The background grid is a visual snap aid (Settings → Grid & Snap):
major spacing 5.00 m, minor 1.00 m, minor colour #1b9eee, snap to grid on,
snap to nodes on, "Only snap at custom grid intersections" off. Grid spacing
and colour are stored per project; the toolbar shows the current snap mode
(Grid: …).

Manual grid lines (setouts)

• Grid line tool: click places an X line (vertical, bubbles A, B, C,
  …, AA…); Shift+click places a Y line (horizontal, bubbles 1, 2, 3…).
• Clicking near an existing same-axis line (< 0.3 m) cycles its bubble label.
• New lines span the model bounds plus max(1.5 m, 12 % of span).
• Grid lines are named setouts when created with the grid generator; manual
  lines belong to the ungrouped setout.

Grid generator (Create grid)

Opens Create grid:

• Setout name and Saved setouts (Save / Load / Delete) - saved setouts
  persist in localStorage['geomodel_grid_setouts'] and are reusable across
  projects. Errors: Enter a setout name first, Pick a saved setout to load,
  Pick a saved setout to delete.
• Show grids: per-setout visibility checkboxes (Show all, Hide all).
  Hiding is per project (geomodel.hiddenGridSetouts). A setout just created
  while hidden is automatically shown.
• X lines / Y lines: Start (m) plus rows of Spacing (m) × Count
  (0–500 each, + Add row; defaults 6 m × 3 and 4 m × 2, start 0). A live
  preview reads N lines: … m.
• Replace existing lines of each direction - default off; with a setout
  name it replaces only that setout.
• Reset restores the tables; Create grid commits (deduplicating within
  1e-3 m) and reports Created N grid lines for setout "…" or
  No new lines … (all coordinates already exist).

Dimensions and Measure

• Dimensions toggle shows span dimensions between the manual grid lines.
• Measure: click two points to add a permanent dimension annotation
  (snaps to grid lines and nodes, free direction). It must have two distinct
  points (Measurement needs two distinct points). Measurements are selectable
  and deletable, and never invalidate results.

2.15 Model tree

The Model sidebar tab lists every entity by type with concise labels
(e.g. Column C3 at (3.0, 3.0), Pile P1 ⌀0.6 L8, Opening 1 in S1,
no slab ⚠ for orphans). Rows support click / Ctrl / Shift selection, hover
highlight in the viewport, per-row × delete, and a selection bar with
Delete / Clear. Only non-empty groups are shown; an empty model shows
Empty model - draw a slab region to begin.

2.16 Materials

Open the Material library (cube button). It has three lists: Concrete
grades, Reinforcement steel, Custom.

Selecting a grade shows and edits:

Derived properties (shear modulus G, bulk modulus K) are shown live.

Custom materials: + New concrete / + New reinforcement, a name, and
scope Global (all projects) or This project only; Save/Delete.
Project-scope materials are stored on the model and travel with the file;
global ones live in the browser (and sync to the server materials library when
available). Custom rows show a project/global badge.

Apply to selected slab / wall copies the selected material onto the
selection (… applied to <name> - re-mesh to use it); with nothing selected:
Select a slab or wall in the model first (current: …).

Built-in grades per code:

EC2 (EN 1992-1-1) - concrete C20/25 … C90/105 (f′c 20–90 MPa;
E 30.0–43.6 GPa per EC2 Table 3.1); steel B500A, B500B, B500C.

AS 3600-2018 - N20, N25, N32, N40, N50, N65, N80, N100
(f′c 20–100 MPa; E 24.0/26.7/30.1/32.8/34.8/37.4/39.6/42.2 GPa);
D250N, D300E, D500N, D500L, D500E.

ACI 318-19 - 20–100 MPa (3000–14500 psi; Ec = 4700√f′c);
Grade 40 (280), 60 (420), 80 (550), 100 (690).

CSA A23.3-19 - 20–100 MPa (Ec = 4500√f′c); 400W, 500W, 600W.

Grade names always follow the active design code: switching code in
Settings → Design refreshes the slab tool, the Properties grade pickers and
the library lists to that code's names, and drops stored grade names that no
longer exist (the numeric f′c/E values on the model are kept).

Design defaults are separate and live in Settings → Design (see
§6.1).

2.17 Validation

CHK runs the full validation: semantic rules, mesh build, and mesh checks.
Results are titled:

• Model & mesh valid - no issues found
• Valid with N warning(s)
• Validation: N error(s)[, M warning(s)]

Each issue can be Located (highlights the offending entity). The full
message list:

Semantic errors (all errors, not warnings)

Mesh checks

Errors:

• N coincident mesh nodes share the same coordinates - connections through them are only partial
• N element node references point at nodes that do not exist in the mesh
• N degenerate elements (repeated nodes or zero area) would make the stiffness matrix singular - refine the mesh or adjust the geometry
• N duplicate elements (the same nodes meshed twice) - slab regions probably overlap; the doubled stiffness corrupts results
• N unrestrained mesh nodes carry supports, springs or loads but no elements - those restraints/loads have no effect
• the generated mesh has no elements

Warnings:

• N mesh nodes are not used by any element
• mesh has N disconnected components (largest X, smallest Y elements): loads on one do not transfer to the others - check that slabs touch along an edge and walls/columns connect, followed by island reports that name the slabs/extents and the nearest gap.

Fix-island advice: snap shared corners, use Edit slab shape to make edges
coincide, or add a column/beam that spans the gap.

2.18 Meshing rules

The mesher (internal/slab/generator.go) is feature-driven:

1. Feature lines are collected from: slab bounding boxes and polygon
   vertices; opening edges; column/pile/point-load X-Y stations; wall ends;
   edge-beam ends; vertical-plate ends; drop-panel footprints and design-strip
   edges.
2. Each feature interval is split into ceil(length / mesh_size) equal steps.
   A slab mesh size of 1.0 m therefore gives elements at most 1.0 m in
   feature-bounded regions; irregular boundaries are clipped.
3. Elements: full interior cells become quads (or two triangles with
   mesh_type = tri); cells clipped by boundaries become clean quads when
   convex with all interior angles > 15°, otherwise ear-clipped triangles.
4. Nodes merge within 1e-6 m; touching same-elevation slabs share feature
   lines and take the finest mesh size in the group.
5. Openings: element centroids strictly inside a rectangle are removed.
6. Drop panels set the element thickness to the covering panel's maximum.
7. Loads: point loads snap to the nearest node within 1e-7 m (else an error);
   line loads convert to equivalent nodal forces by tributary segment; area
   loads become pressures on every element whose centroid is inside the
   polygon; self weight is assembled from density × volume.

Mesh type is set in the Mesh Generation dialog (Quad (structured)
default or Triangle) and the element size writes to every slab's Mesh size
field; the modal pre-fills the average slab mesh size.

Quads are generally more accurate per node; triangles handle awkward
boundaries better but need a finer mesh for the same moment accuracy. Quads
are the default and are recommended wherever wall results are compared
against other software: both mesh types report membrane forces in the same
(wall run, vertical) frame, but triangles need roughly twice the refinement
for the same membrane smoothness.

2.19 A modelling walkthrough

A 16 × 12 m flat plate, 250 mm, columns 400 × 400 at the four corners and
mid-sides, a 2 × 2 m stair opening, a perimeter edge beam, and a 2.4 m grid:

1. New Project → "flat-plate-tutorial".
2. Settings → Design: EC2, C32/40, B500, cover 25 mm; Apply.
3. Slab tool: thickness 0.25, elevation 0, f′c 32, E 30, mesh 0.5; draw the
   16 × 12 rectangle (corners at (0,0), (16,0), (16,12), (0,12)). Finish with
   Enter.
4. Opening tool: two corners (6,4) and (8,6). Confirm the centre is inside;
   the status reads Opening added to S1.
5. Column tool: keep Column, 0.4 × 0.4, Z↓ 4 (below), Z↑ 3, Base Fixed,
   Top None; place at (0,0), (8,0), (16,0), (0,6), (16,6), (0,12), (8,12),
   (16,12).
6. Beam tool: b 0.3, h 0.6; draw along the four perimeter edges.
7. Grid generator: X rows 4 m × 5 (0 → 16); Y rows 4 m × 4 (0 → 12);
   setout name "Grid A"; Create grid.
8. MESH → CHK: expect "Model & mesh valid" (fix islands if any).
9. Save (Ctrl+S) - the file stores the semantic model, not the mesh.

The same sequence in screenshots would take a page; the command of record is
the numeric fields above. For a full analysis/design walkthrough see
Chapter 8.

2.20 Troubleshooting

→ Next: Chapter 3 - Loads