Element reference

Every lowercase JSX element tscad understands, generated from the type definitions: the same text your editor shows on hover. Lengths in mm, angles in degrees.

#Shared props

Placement (3D)

Where a solid goes. Applied in this order: mirror, scale, rotate (+ rotateX/Y/Z), then the translation (at + x/y/z). Available on every solid-producing element.

Prop	Type	Description
x	number	Move along X, mm (added to `at`).
y	number	Move along Y, mm (added to `at`).
z	number	Move along Z, mm (added to `at`).
at	Vec3	Move by `[x, y, z]`, mm.
rotate	Vec3	Rotate `[rx, ry, rz]` degrees about the fixed X, then Y, then Z axes (OpenSCAD's `rotate([rx, ry, rz])`), about the origin, before translating.
rotateX	number	Rotate about X, degrees (added to `rotate[0]`).
rotateY	number	Rotate about Y, degrees (added to `rotate[1]`).
rotateZ	number	Rotate about Z, degrees (added to `rotate[2]`).
scale	number	Uniform scale factor about the origin.
mirror	Axis	Mirror across the plane through the origin square to this axis (`"x"` negates X).
name	string	A name other elements can refer to (`".plate"`, `".bolt > .shank"`): `<subtract from tool>`, `<union of>`, `<intersect of>`, `<fillet target>`, `<chamfer target>`, `<shell target>`, `<draft target>`. Refs resolve within the enclosing `<part>`. Component calls take `name` too.
ghost	boolean	A tool for refs only: left out of the output unless a ref op uses it up (`<subtract tool>`, `<union of>`), with a warning when nothing does. Component calls take it too.

Placement (2D)

Where a 2D shape goes in its sketch: mirror, then rotate, then translate.

Prop	Type	Description
x	number	Move along sketch X, mm.
y	number	Move along sketch Y, mm.
at	Vec2	Move by `[x, y]`, mm (added to `x`/`y`).
rotate	number	Rotate CCW about the sketch origin, degrees (before translating).
mirror	"x" \| "y"	Mirror: `"x"` negates sketch X, `"y"` negates sketch Y.
z	number	Inside `<loft>`: the height of this section, mm.

#Containers

Parts, assemblies and groups: the structure of a model.

<assembly>

A collection of parts (may nest); placement props move every part in it.

Prop	Type	Description
allowFree	boolean	Don't warn about parts their mates leave free to move.
strict	boolean	Mates must fix every part (free parts are errors) and redundant mates are reported.
fixed	boolean	As a sub-assembly: ground it in the parent assembly's mates.
name	string	Assembly name (used as a prefix for loose solids' part name).

Also takes placement props, solid children.

<part>

One named, coloured solid: the unit of export. Several children are unioned.

Prop	Type	Description
name	string	Part name: unique within the model; used for meshes, STEP entities and export files.
color	string	Display colour, any CSS colour (default: from `material`).
material	MaterialName \| (string & {})	Material preset (`"pla"`, `"petg"`, `"abs"`, `"aluminum"`, `"steel"`, `"brass"`, `"wood"`...), giving a default colour and density. See `materials`.
density	number	Density in g/cm³ for mass estimates (default: from `material`).
visible	boolean	`false` leaves the part out of the document (and exports); default true.
fixed	boolean	Ground this part for `<mate>`s: it never moves (default: the first part is grounded).

Also takes placement props, solid children.

<group>

Groups solids (unioned) so they can be placed together.

Also takes placement props, solid children.

<drawing>

A flat 2D part (laser / CNC): exports to DXF/SVG; thickness also makes it a 3D part.

A flat 2D part for laser cutting / CNC: its 2D shapes compile straight to loops (no kernel) and export to DXF/SVG with tscad/drawing. Give it a thickness to also get a 3D part (the sheet, extruded up from z = 0) for the viewer and STEP/STL.

<drawing name="gasket" thickness={1.5}><rect w={50} h={30} /><circle r={8} /></drawing>

Prop	Type	Description
name	string	Drawing (and part) name; unique. Default `"drawing"`.
thickness	number	Sheet thickness, mm: also emit the drawing as an extruded part.
layer	string	Output layer in DXF/SVG, e.g. `"cut"` or `"engrave"` (SVG colours `engrave` blue). Default: the drawing's name.
color	string	Display colour of the part.
material	MaterialName \| (string & {})	Material preset of the part (see `<part material>`).
density	number	Density override, g/cm³.

Also takes 2D placement props, 2D shape children.

#Assemblies

Anchors and mates place parts for you (see Assemblies & mates).

<anchor>

A named frame on a part, for mates.

A named frame (connector) on a part: an origin and an axis (its local z), plus an x direction. It moves with everything around it, so a component can expose mounting points. Anchors build no geometry.

<anchor id="shaft" at={[0, 0, 24]} axis="z" />

Prop	Type	Description
id*	string	Name, unique within its part: the mate refers to `"part.id"`.
at	Vec3	Origin, mm (default the origin of where the anchor sits).
x	number	Added to `at[0]`.
y	number	Added to `at[1]`.
z	number	Added to `at[2]`.
axis	Direction	The anchor's axis (its local z). Default `"z"`.
xAxis	Direction	The anchor's x direction (projected square to `axis`). Default: X, or Y when `axis` is along X.

<mate>

A joint between two anchors (inside <assembly>).

Join anchor b (its part moves) to anchor a. Origins meet, axes align (opposed with flip) and, depending on type, x directions align: | type | free motion | driven by | |---|---|---| | fastened (default) | none | none | | revolute | rotation about the axis | angle | | slider | travel along the axis | offset | | cylindrical | rotation about + travel along the axis | angle, offset | | planar | travel in the plane, rotation about the normal | angle | | ball | any rotation about the origin | none |

Prop	Type	Description
a*	string \| AnchorRef	The first anchor: `"part.anchor"` or a handle (`A.motor.shaft`).
b*	string \| AnchorRef	The second anchor.
type	MateType	Joint type. Default `"fastened"`.
offset	number	Offset along `a`'s axis, mm (a slider's travel; a gap for the others).
distance	number	Alias of `offset`.
angle	number	Rotation of `b` about `a`'s axis, degrees (a revolute joint's angle).
flip	boolean	Axes opposed instead of aligned (face-to-face).
id	string	Name, for `<gear>`s relating this joint to another.
limits	[number, number]	Allowed range of the joint, `[min, max]`: degrees for revolute/cylindrical/planar (the angle), mm for a slider (the offset). Out-of-range positions warn.

<gear>

Couples two joints' angles (inside <assembly>).

Couples two revolute (or cylindrical) joints: b's angle = ratio × a's angle + phase. Negative ratios turn the other way (meshing spur gears).

<gear a="motor" b="wheel" ratio={-0.5} />

Prop	Type	Description
a*	string	`id` of the driving mate.
b*	string	`id` of the driven mate.
ratio*	number	b's angle per degree of a's.
phase	number	Angle offset, degrees.

#Primitives

Basic solids. Box, cylinder and cone sit centred in X/Y with their base on z = 0.

<box>

A box; centred in XY, base on z = 0.

A rectangular box. Default placement: centred in X and Y, base on z = 0 (ready to print). Size by size, or width/depth/height (aliases w/d/h).

Prop	Type	Description
size	number \| Vec3	`[x, y, z]` mm, or one number for a cube.
width	number	Size along X, mm.
depth	number	Size along Y, mm.
height	number	Size along Z, mm.
w	number	Alias of `width`.
d	number	Alias of `depth`.
h	number	Alias of `height`.
center	CenterSpec	Centring per axis. Default `[true, true, false]` (centred XY, base on z = 0).

Also takes placement props.

<cylinder>

A cylinder about +Z; base on z = 0.

A cylinder about +Z. Default placement: axis on Z, base on z = 0. Radius by r/radius or d/diameter; height by h/height.

Prop	Type	Description
r	number	Radius, mm.
radius	number	Radius, mm (alias of `r`).
d	number	Diameter, mm.
diameter	number	Diameter, mm (alias of `d`).
h	number	Height along +Z, mm.
height	number	Height along +Z, mm (alias of `h`).
center	CenterSpec	Centring per axis. Default `[true, true, false]`; `true` also centres in Z.

Also takes placement props.

<cone>

A cone / frustum about +Z; base on z = 0.

A cone or frustum about +Z, from radius r1 at the base to r2 at the top (either may be 0). Default placement: axis on Z, base on z = 0.

Prop	Type	Description
r1	number	Bottom radius, mm.
r2	number	Top radius, mm (0 for a point).
d1	number	Bottom diameter, mm.
d2	number	Top diameter, mm.
h	number	Height along +Z, mm.
height	number	Height along +Z, mm (alias of `h`).
center	CenterSpec	Centring per axis. Default `[true, true, false]`.

Also takes placement props.

<sphere>

A sphere centred on the origin.

A sphere, centred on the origin by default.

Prop	Type	Description
r	number	Radius, mm.
radius	number	Radius, mm (alias of `r`).
d	number	Diameter, mm.
diameter	number	Diameter, mm (alias of `d`).
center	CenterSpec	Centring per axis. Default `true`; `false` puts the bounding box's corner on the origin.

Also takes placement props.

<torus>

A torus about +Z centred on the origin.

A torus about +Z, centred on the origin.

Prop	Type	Description
R	number	Major radius (centre to tube centre), mm.
r	number	Minor radius (tube radius), mm.
major	number	Major radius, mm (alias of `R`).
minor	number	Minor radius, mm (alias of `r`).

Also takes placement props.

<step>

An imported STEP solid: <step data={text} />.

An imported STEP solid (exact B-rep), placed like any other solid. Get the text with an import attribute: import bracket from "./bracket.step" with { type: "text" }. Analytic models round-trip; some blended (filleted) files can't be read yet.

Prop	Type	Description
data*	string	The STEP file's text (ISO-10303-21).
solid	number	Which solid of the file, 0-based (default: all solids, unioned).

Also takes placement props.

#Booleans

Combine solids.

<union>

Union of the children.

Everything in any child.

Prop	Type	Description
of	string	By ref instead of children: unite the named solids (`".a, .b"`). The first keeps its place and name; the others are moved into it and removed from where they were.

Also takes placement props, solid children.

<difference>

First child minus the rest.

The first child minus every other child.

Prop	Type	Description
from	string	By ref instead of children: the named solid to cut (`".plate"`). The result keeps its name and place in the tree. Needs `tool`. `<subtract from=".plate" tool=".bolt > .shank" />`
tool	string	By ref: the solid(s) to cut away (`".hole"`, `".a, .b"`). They are used up: removed from the output.

Also takes placement props, solid children.

<subtract>

First child minus the rest (alias of <difference>).

The first child minus every other child.

Prop	Type	Description
from	string	By ref instead of children: the named solid to cut (`".plate"`). The result keeps its name and place in the tree. Needs `tool`. `<subtract from=".plate" tool=".bolt > .shank" />`
tool	string	By ref: the solid(s) to cut away (`".hole"`, `".a, .b"`). They are used up: removed from the output.

Also takes placement props, solid children.

<intersection>

Common volume of the children.

Only what every child shares.

Prop	Type	Description
of	string	By ref instead of children: keep what the named solids share (`".a, .b"`); the first keeps its place and name.

Also takes placement props, solid children.

<intersect>

Common volume of the children (alias of <intersection>).

Only what every child shares.

Prop	Type	Description
of	string	By ref instead of children: keep what the named solids share (`".a, .b"`); the first keeps its place and name.

Also takes placement props, solid children.

#Transforms

Move, turn, scale and mirror children (every solid also has placement props).

<translate>

Translate children.

Prop	Type	Description
x	number	Offset along X, mm.
y	number	Offset along Y, mm.
z	number	Offset along Z, mm.
by	Vec3	Offset `[x, y, z]`, mm (added to `x`/`y`/`z`).

Also takes solid children.

<rotate>

Rotate children (degrees, X then Y then Z; or axis + angle).

Prop	Type	Description
x	number	Angle about X, degrees (applied first).
y	number	Angle about Y, degrees (applied second).
z	number	Angle about Z, degrees (applied third).
by	Vec3	`[rx, ry, rz]` degrees, X then Y then Z (added to `x`/`y`/`z`).
axis	Vec3 \| Axis	Rotate by `angle` about this axis instead (right-hand rule).
angle	number	Angle about `axis`, degrees.
origin	Vec3	Rotate about this point instead of the origin.

Also takes solid children.

<scale>

Scale children (uniform or per axis).

Prop	Type	Description
by*	number \| Vec3	Scale factor: a number (uniform) or `[sx, sy, sz]`. Non-uniform scale turns analytic surfaces (cylinders, spheres) into NURBS.
origin	Vec3	Scale about this point instead of the origin.

Also takes solid children.

<mirror>

Mirror children across a plane (with keep, a symmetric pair).

Prop	Type	Description
axis*	Axis \| Vec3	The plane to mirror across, by its normal: an axis (`"x"` negates X) or a vector.
keep	boolean	Keep the original as well as the mirrored copy (a symmetric pair). Default false.
origin	Vec3	A point on the mirror plane (default origin).

Also takes solid children.

<transform>

Apply an arbitrary affine matrix (row-major, column-vector).

Apply an arbitrary affine matrix (OpenSCAD's multmatrix): row-major, column-vector (p' = M p, translation in the last column), exactly the IR's layout. Shear or non-uniform scale turns analytic faces into NURBS.

Prop	Type	Description
matrix*	readonly number[] \| readonly (readonly number[])[]	16 numbers (4×4), 12 (3×4, last row [0, 0, 0, 1] implied), or the rows as nested arrays.

Also takes solid children.

#Sketch shapes

2D shapes, used inside extrude, revolve, loft, sweep and drawing. Overlapping shapes union; nested loops become holes.

<rect>

2D: rectangle (centred).

A rectangle, centred on its position by default.

Prop	Type	Description
w	number	Width (sketch X), mm.
h	number	Height (sketch Y), mm.
width	number	Alias of `w`.
height	number	Alias of `h`.
size	number \| Vec2	`[w, h]`, or one number for a square.
center	boolean	`false` puts the lower-left corner on the position instead. Default true.

Also takes 2D placement props.

<roundedRect>

2D: rectangle with rounded corners (centred).

A rectangle with rounded corners (exact quarter arcs), centred.

Prop	Type	Description
w	number	Width (sketch X), mm.
h	number	Height (sketch Y), mm.
width	number	Alias of `w`.
height	number	Alias of `h`.
size	number \| Vec2	`[w, h]`, or one number for a square.
center	boolean	`false` puts the lower-left corner on the position instead. Default true.
r	number	Corner radius, mm (clamped to half the shorter side).
radius	number	Alias of `r`.

Also takes 2D placement props.

<circle>

2D: circle.

A circle (one exact arc), centred on its position. Inside a constraint sketch it is a solved circle (center, tangent, equal...).

Prop	Type	Description
center	PointLike	Centre point id (created if new) or `[x, y]` guess.
fixed	boolean	Pin the centre where drawn.
tangent	Refs<LineHandle \| Round>	Tangent to these lines/arcs/circles.
equal	Refs<Round>	Same radius as these arcs/circles.
concentric	Ref<Round>	Same centre as this arc/circle.
r	number	Radius, mm.
radius	number	Radius, mm (alias of `r`).
d	number	Diameter, mm.
diameter	number	Diameter, mm (alias of `d`).

Also takes 2D placement props.

<ellipse>

2D: ellipse.

An ellipse (one exact rational NURBS), centred.

Prop	Type	Description
rx*	number	Semi-axis along sketch X, mm.
ry*	number	Semi-axis along sketch Y, mm.

Also takes 2D placement props.

<polygon>

2D: polygon through points.

A polygon through points (closed automatically).

Prop	Type	Description
points*	readonly Vec2[]	Vertices `[x, y]` in order (either winding).

Also takes 2D placement props.

<regularPolygon>

2D: regular polygon.

A regular polygon (hexagon, ...), centred, first vertex on +X.

Prop	Type	Description
sides*	number	Number of sides (≥ 3).
r	number	Circumradius (centre to vertex), mm.
radius	number	Circumradius, mm (alias of `r`).
apothem	number	Inradius (centre to flat), mm: e.g. half a hex nut's across-flats size.
flats	number	Across-flats width, mm (= 2 × apothem).

Also takes 2D placement props.

<slot>

2D: stadium slot along X.

A stadium / slot (two half circles joined by straight sides) along sketch X, centred.

Prop	Type	Description
length*	number	Overall length end to end, mm.
width*	number	Width (= end diameter), mm.

Also takes 2D placement props.

<path>

2D: SVG path data.

An SVG-style path. Supports M L H V C S Q T A Z (absolute and relative). Each subpath must be closed (Z, or end where it began); subpaths nested in others become holes. Note: y points up (no SVG flip).

Prop	Type	Description
d*	string	Path data, e.g. `"M0 0 H20 V10 A5 5 0 0 1 10 10 Z"`.

Also takes 2D placement props.

<star>

2D: star.

A star with points tips, first tip on +Y, centred.

Prop	Type	Description
points*	number	Number of tips (≥ 2).
r1*	number	Tip radius, mm.
r2*	number	Valley radius, mm.

Also takes 2D placement props.

<text>

2D: text outlines (emboss / engrave).

Text outlines, for embossing (<extrude>) or engraving (<difference>). Glyph holes (o, a, e...) are handled like any nested loop. By default the first baseline starts at the position (align="left", valign="baseline"); \n starts a new line.

<extrude height={1}><text size={8} align="center" valign="middle">tscad</text></extrude>

Prop	Type	Description
size	number	Font size (em), mm. Default 10. In the default font capitals are about 0.73 × size tall and lowercase x about 0.55 × size.
font	ArrayBuffer \| Uint8Array \| object	A TTF/OTF/WOFF font's bytes (e.g. `import f from "./Font.ttf" with { type: "file" }` then read it, or `await Bun.file(...).arrayBuffer()`), or an opentype.js `Font`. Default: the built-in DejaVu Sans (Latin, Greek and common symbols such as ° ± × µ ⌀ Ø).
align	"left" \| "center" \| "right"	Horizontal alignment of each line about the position. Default `"left"`.
valign	"baseline" \| "top" \| "middle" \| "bottom"	Vertical alignment of the block: `"baseline"` (default: first baseline at the position), `"top"` (ascender), `"middle"` (centre of the capitals), `"bottom"` (last descender).
spacing	number	Letter advance multiplier (1 = the font's own spacing; 1.2 = 20 % looser).
lineHeight	number	Line pitch as a multiple of `size`. Default 1.2.
kerning	boolean	Apply the font's kerning. Default true.
ligatures	boolean	Apply standard ligatures (fi, fl...). Default true.

Also takes 2D placement props.

<dxf>

2D: an imported DXF drawing.

An imported DXF drawing as 2D shapes: LINE, ARC, CIRCLE, LWPOLYLINE/POLYLINE (bulges become exact arcs), SPLINE, ELLIPSE, INSERTed BLOCKs. $INSUNITS → mm. Loose entities are chained into closed loops; nested loops are holes.

import plate from "./plate.dxf" with { type: "text" } <extrude height={3}><dxf data={plate} layer="CUT" /></extrude>

Prop	Type	Description
data*	string	The DXF file's text.
layer	string \| readonly string[]	Only these layers.
units	"mm" \| "cm" \| "m" \| "in" \| "ft"	Override the file's units.
scale	number	Extra scale factor.
center	boolean	Move the drawing's bounding-box centre to the origin.
tolerance	number	End-point snapping tolerance when chaining, mm.

Also takes 2D placement props.

<svg>

2D: an imported SVG drawing.

An imported SVG as 2D shapes: paths (arcs stay exact), rect, circle, ellipse, polygon, closed polylines, nested groups with transforms. Units come from the viewBox and the width/height (else 1 px = 0.2646 mm); y is flipped to point up. Each element's fill-rule decides its holes; overlapping elements are unioned.

import logo from "./logo.svg" with { type: "text" } <extrude height={1}><svg data={logo} center /></extrude>

Prop	Type	Description
data*	string	The SVG file's text.
select	string	Only the element with this id (`"logo"`, `"#logo"`) or class (`".cut"`), with its children.
scale	number	Extra scale factor.
flipY	boolean	Flip y so the drawing reads the right way up. Default true.
center	boolean	Move the drawing's bounding-box centre to the origin.

Also takes 2D placement props.

<sketch>

2D: groups shapes to place them together.

Prop	Type	Description
prefer	"ccw" \| "cw"	Hint: which way round the closed loops are drawn (in declaration order).
strict	boolean	Make an under-constrained sketch an error instead of a warning.
allowFree	boolean	Don't warn about remaining degrees of freedom.

Also takes 2D placement props, 2D shape children.

<offset>

2D: offsets its shapes outward (+) or inward (−).

Offsets its 2D children: positive distance grows the shapes (clearance outlines, gaskets), negative shrinks them (insets, pockets). Holes move the other way, so the material grows/shrinks consistently. Lines and arcs stay exact; NURBS (ellipses, text, Béziers) are flattened to lines first. Holes that close up and islands that shrink away are removed.

<extrude height={2}><offset distance={1.5}><path d={outline} /></offset></extrude>

Prop	Type	Description
distance	number	Offset distance, mm: positive outward, negative inward.
d	number	Alias of `distance`.
round	boolean	Round convex corners with exact arcs (default true); `false` mitres them.

Also takes 2D placement props, 2D shape children.

<hull>

2D: the convex hull of the children (exact arcs and tangents).

The exact convex hull of the child shapes: polygons stay polygons, circles and arcs give tangent lines and arcs (two circles → a slot, three → a rounded triangle), NURBS and text are flattened.

<hull><circle r={10} /><circle r={4} x={25} /></hull>

Also takes 2D placement props, 2D shape children.

<sketchUnion>

2D: union of the child shapes (exact; arcs stay arcs).

An exact 2D boolean of its child shapes: each child is one operand (a <sketch> groups several shapes into one; nested loops in an operand are holes). Lines and arcs stay exact; NURBS (ellipses, text, Béziers) are flattened first. The result is a 2D shape like any other: use it in <extrude>, <revolve>, <drawing>, <offset>... - <sketchUnion> (<union2d>): everything in any child. - <sketchDifference> (<difference2d>): the first child minus the others. - <sketchIntersection> (<intersection2d>): only what every child shares.

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<sketchDifference>

2D: the first child shape minus the others (exact).

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<sketchIntersection>

2D: what every child shape shares (exact).

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<union2d>

2D: alias of <sketchUnion>.

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<difference2d>

2D: alias of <sketchDifference>.

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<intersection2d>

2D: alias of <sketchIntersection>.

<extrude height={8}><difference2d><circle d={6} /><rect w={6} h={3} y={3} /></difference2d></extrude> // a D-shaft profile

Also takes 2D placement props, 2D shape children.

<section>

2D: one loft section at height z.

A loft section: one 2D shape at height z.

Prop	Type	Description
z*	number	Height of the section, mm.

Also takes 2D shape children.

#Sketch → solid

Turn 2D shapes into solids.

<extrude>

Extrude 2D shapes (nested loops become holes).

Extrude 2D shapes into a solid. Every closed loop is extruded; loops nested inside an odd number of others are holes, and disjoint outlines are unioned: <extrude height={5}><rect w={40} h={30}/><circle r={5}/></extrude> is a plate with a hole.

Prop	Type	Description
height	number	Distance along the sketch normal, mm (negative extrudes the other way).
h	number	Alias of `height`.
distance	number	Alias of `height`.
draft	number	Taper angle, degrees: positive narrows the outline as it rises (mould draft).
plane	"XY" \| "XZ" \| "YZ"	Sketch plane. `"XY"` (default): normal +Z. `"XZ"`: sketch x → X, y → Z, normal −Y. `"YZ"`: sketch x → Y, y → Z, normal +X.
offset	number	Offset of the sketch plane along its normal, mm.
center	boolean	Extrude symmetrically about the sketch plane. Default false.

Also takes placement props, 2D shape children.

<revolve>

Revolve a 2D profile (x = radius, y = height) about Z.

Revolve 2D shapes about the Z axis: sketch x is the radius, sketch y is the height (the profile is placed in the XZ plane). Keep the profile at x ≥ 0.

Prop	Type	Description
angle	number	Sweep angle, degrees (0 < angle ≤ 360). Default 360.

Also takes placement props, 2D shape children.

<loft>

Loft through 2D sections along Z.

Skin through 2D sections stacked along Z. Give each shape a z, or wrap each in <section z={...}>. One loop per section, bottom to top.

Prop	Type	Description
ruled	boolean	Straight (ruled) walls between sections instead of a smooth skin. Default false.

Also takes placement props, 2D shape children.

<sweep>

Sweep a 2D profile along a 3D path.

Prop	Type	Description
path	Path3 \| readonly Vec3[]	The path: `helix({...})`, `polyline3([...])`, `arc3({...})`, or IR curves. Or draw it in 2D with a `<sweepPath>` child instead.
frame	"follow" \| "translate"	`"follow"` (default) turns the profile with the path; `"translate"` keeps its orientation (no twist; for threads along a helix, follow is usually right).

Also takes placement props, 2D shape children.

<sweepPath>

A sweep's path drawn in 2D (inside <sweep>).

A <sweep>'s path drawn in 2D on a plane: a constraint <sketch> (lines, arcs, splines; open, or closed for a ring) or <path d="M ..."> data. Keep it tangent-continuous (join lines with tangent arcs): the sweep is exact along lines and arcs, and sharp corners warn.

<sweep> <sweepPath plane="XZ"><path d="M0 0 V40 A15 15 0 0 0 30 40" /></sweepPath> <circle r={3} /> </sweep>

Prop	Type	Description
plane	"XY" \| "XZ" \| "YZ"	The plane the path is drawn on (as `<extrude plane>`). Default `"XY"`.
offset	number	Shift the plane along its normal, mm.

Also takes 2D placement props.

#Patterns

Repeat children.

<linearPattern>

Copies along a line.

count copies, each moved by step from the last.

Prop	Type	Description
count*	number	Number of copies (including the original).
step	Vec3	Offset between copies `[dx, dy, dz]`, mm.
dx	number	X offset between copies, mm.
dy	number	Y offset between copies, mm.
dz	number	Z offset between copies, mm.
center	boolean	Centre the pattern on the original position. Default false.
of	string \| readonly unknown[]	Inside a constraint `<sketch>`: the entities to copy (ids or handles); the copies stay tied by translation constraints. Without `of` it is the usual solid pattern.

Also takes placement props, solid children.

<gridPattern>

Copies on an XY grid.

An nx × ny grid of copies in XY.

Prop	Type	Description
nx*	number	Columns (along X).
ny*	number	Rows (along Y).
dx*	number	Column spacing, mm.
dy*	number	Row spacing, mm.
center	boolean	Centre the grid on the original position. Default true.

Also takes placement props, solid children.

<polarPattern>

Copies around an axis.

count copies rotated about an axis through the origin.

Prop	Type	Description
count*	number	Number of copies (including the original).
angle	number	Total angle, degrees. 360 (default) spaces copies evenly around the circle; anything less puts the first copy at 0 and the last at `angle`.
axis	Axis	Rotation axis. Default `"z"`.
radius	number	Move the children out along +X by this radius first, mm (bolt circles).
startAngle	number	Angle of the first copy, degrees. Default 0.

Also takes placement props, solid children.

#Features

Round, bevel, hollow, draft, push/pull and split. Edges and faces are picked with selectors.

<fillet>

Round edges.

Round edges of the children (unioned). radius 0 skips the fillet (handy for params).

Prop	Type	Description
target	string	By ref instead of children: the named solid to apply it to (`".plate"`); the result keeps its name.
radius	number	Fillet radius, mm.
r	number	Alias of `radius`.
edges	SelectorLike \| Selector	Which edges: `edges.top()`, `">Z or \|Z"`, or an IR selector. Default: all edges. The kernel fails if nothing matches.

Also takes placement props, solid children.

<chamfer>

Bevel edges.

Bevel edges of the children (unioned). distance 0 skips it.

Prop	Type	Description
target	string	By ref instead of children: the named solid to apply it to (`".plate"`); the result keeps its name.
distance	number	Setback along each face, mm.
d	number	Alias of `distance`.
edges	SelectorLike \| Selector	Which edges (see `fillet`). Default: all edges.

Also takes placement props, solid children.

<shell>

Hollow out.

Hollow the children (unioned) to a wall thickness, leaving the open faces open.

Prop	Type	Description
target	string	By ref instead of children: the named solid to apply it to (`".plate"`); the result keeps its name.
thickness*	number	Wall thickness, mm. Walls grow inward unless `outward` (the sign is ignored: −2 is also 2 mm inward).
open	SelectorLike \| Selector	Faces to remove: `faces.top()`, `">Z"`, ... Default: none (a closed hollow).
outward	boolean	Grow the walls outward (keep the inside size). Default false.

Also takes placement props, solid children.

<draft>

Mould draft on faces.

Mould draft: tilt the selected faces of the children (unioned) by angle so the part releases from a mould pulled along pull. Faces pivot about the neutral plane (default z = 0, square to pull); a positive angle leans them in as they rise along pull.

<draft angle={3}><box size={[40, 30, 20]} /></draft>

Prop	Type	Description
target	string	By ref instead of children: the named solid to apply it to (`".plate"`); the result keeps its name.
angle*	number	Draft angle, degrees (0 skips it).
faces	SelectorLike \| Selector	Faces to draft. Default: the walls square to `pull` (`"#Z"` for the default pull).
neutral	number \| PlaneSpec	Neutral plane: a height along `pull` (mm), or a plane. Default 0.
pull	Axis \| `-${Axis}` \| Vec3	Mould pull direction: an axis (`"z"`, `"-z"`) or a vector. Default `"z"`.

Also takes placement props, solid children.

<pushPull>

Move faces along their normals (push/pull).

Push or pull faces: move the selected faces of the children (unioned) along their normals by distance (negative: inward); neighbouring faces stretch or shrink to meet them. distance={0} skips it.

<pushPull distance={2} faces=">Z"><box size={10} /></pushPull> // 10 × 10 × 12

Prop	Type	Description
distance	number	How far to move the faces, mm (negative: into the solid). Give this or `d`.
d	number	Alias of `distance`.
faces*	SelectorLike \| Selector	Faces to move: `faces.top()`, `">Z"`, ...

Also takes placement props, solid children.

<offsetFaces>

Move faces along their normals (alias of <pushPull>; the IR name).

Push or pull faces: move the selected faces of the children (unioned) along their normals by distance (negative: inward); neighbouring faces stretch or shrink to meet them. distance={0} skips it.

<pushPull distance={2} faces=">Z"><box size={10} /></pushPull> // 10 × 10 × 12

Prop	Type	Description
distance	number	How far to move the faces, mm (negative: into the solid). Give this or `d`.
d	number	Alias of `distance`.
faces*	SelectorLike \| Selector	Faces to move: `faces.top()`, `">Z"`, ...

Also takes placement props, solid children.

<split>

Cut with a plane, keep one side.

Cut the children (unioned) with a plane and keep one side: section views, halves for printing, flat bottoms.

<split plane="XY" offset={5}><sphere r={10} /></split> // the cap above z = 5

Prop	Type	Description
plane	PlaneSpec	The cutting plane (in the children's own coordinates). Default `"XY"`.
offset	number	Move the plane along its normal, mm.
keep	"above" \| "below"	Keep the side the normal points to (`"above"`, default) or the other (`"below"`).

Also takes placement props, solid children.

#Sheet metal

Bent sheet parts from a base outline: flanges, edge flanges, hems and jogs, with the flat pattern as cut/bend drawings. See the sheet-metal guide.

<sheetMetal>

A sheet-metal part (folded + flat pattern).

A sheet-metal part: a base <flange> (a closed 2D outline) with <edgeFlange>, <hem> and <jog> children hanging from its edges, nested to any depth. Bends are exact cylindrical sections. Besides the folded part, the flat pattern comes out as drawings named <name>-flat (layer cut) and <name>-bends (layer bend: the bend centre lines as open paths, with an "UP 90° R2" text note beside each), so tscad build -o part.dxf gives a cut-and-bend-ready flat; engraveNotes adds the labels as text outlines (<name>-notes, layer engrave). Bend allowance: BA = θ·(R + K·T).

<sheetMetal name="bracket" thickness={2} bendRadius={2}> <flange> <rect w={60} h={40} /> <edgeFlange edge="+y" length={30} /> </flange> </sheetMetal>

Prop	Type	Description
thickness*	number	Sheet thickness, mm.
bendRadius	number	Inside bend radius, mm. Default: the thickness.
kFactor	number	Neutral-axis position as a fraction of the thickness from the inside. Default 0.44.
name	string	Name of the flat-pattern drawings (`<name>-flat`...). Default `"sheet"`.
flat	boolean	Show the flat pattern (extruded) instead of the folded part.
engraveNotes	boolean	Also emit the bend labels as text outlines (`<name>-notes`, layer `engrave`) for laser marking. Default false.

Also takes placement props.

<flange>

Sheet metal: the base flange.

The base flange: a closed 2D outline (holes allowed) on z = 0, plus edge flanges as children.

Also takes 2D placement props.

<edgeFlange>

Sheet metal: a flange folded from an edge.

A flange folded from an edge: length of flat beyond the bend. Where two 90° edge flanges meet at a corner of their parent, corner closes the gap between them and cornerRelief cuts a relief where their bends meet.

Prop	Type	Description
length	number	Flat length beyond the bend, mm. Optional with `profile` (the outline's height).
angle	number	Bend angle, degrees (0, 180]. Default 90.
bendRadius	number	Inside bend radius, mm. Default: the sheet's.
profile	boolean	The flange's 2D children are its outline (tapered tabs, holes inside it) instead of holes in a width × length rectangle. Drawn in flange coordinates (x along the edge from 0 to its width, y away from the bend); it must stand on the bend line: a straight edge along y = 0 from x = 0 to the width.
corner	"open" \| "closed" \| "overlap"	How it meets a neighbouring 90° edge flange at a corner: `"open"` (default, a gap of the bend's size), `"closed"` (both run on and meet on the corner's diagonal, mitred; the flat pattern cuts square at the inside of the mitre), `"overlap"` (this one runs past the corner flush with the neighbour's outside; the neighbour stops `cornerGap` short of it).
cornerGap	number	Gap left at a closed / overlapped corner, mm. Default min(0.2, thickness / 4).
cornerRelief	"round" \| "rect" \| "tear"	Relief where the bends meet at a corner: `"rect"` / `"round"` cut `cornerReliefSize` into the parent and cut the bends back; `"tear"` none.
cornerReliefSize	number	Corner relief size (square side / radius), mm. Default bend radius + thickness.

<hem>

Sheet metal: a 180° hem.

A hem: folded right back (180°) over the sheet.

Prop	Type	Description
length*	number	Flat length of the folded-back part, mm.
gap	number	Gap between the sheet and the hem, mm (bend radius = gap / 2). Default: the thickness.

<jog>

Sheet metal: a jog (Z-bend).

A jog (Z-bend): up by angle, a web, back down, so the flange continues offset higher.

Prop	Type	Description
offset*	number	Rise of the jogged flange's bottom face above the parent's, mm.
length*	number	Flat length of the jogged flange, mm.
angle	number	Bend angle of both bends, degrees. Default 90.
bendRadius	number	Inside bend radius, mm. Default: the sheet's.

#Features on faces

Sketch on a face of a solid, then pocket into it, raise a boss from it or cut through. The face is picked with a selector; x, y and rotate place the sketch in the face.

<pocket>

Cut a 2D profile depth into a face of the base.

Prop	Type	Description
face*	SelectorLike \| Selector	Which face: a selector matching planar faces.
index	number	Which of the matching faces. Default 0.
draft	number	Taper, degrees.
depth*	number	How deep into the face, mm.
d	number	Alias of `depth`.

Also takes 2D placement props.

<boss>

Raise a 2D profile height out of a face of the base.

Prop	Type	Description
face*	SelectorLike \| Selector	Which face: a selector matching planar faces.
index	number	Which of the matching faces. Default 0.
draft	number	Taper, degrees.
height*	number	How far out of the face, mm.
h	number	Alias of `height`.

Also takes 2D placement props.

<cutThrough>

Cut a 2D profile through the base, from a face.

Prop	Type	Description
face*	SelectorLike \| Selector	Which face: a selector matching planar faces.
index	number	Which of the matching faces. Default 0.
draft	number	Taper, degrees.
depth	number	How far to cut, mm. Default 2000 (through anything reasonable).

Also takes 2D placement props.

<onFace>

Model on a face of the first child (sketch on face).

Model on a face of another solid ("sketch on face"). The first child is the base; the other children are tools modelled in the face's frame (origin at the centre of the face's bounding box, +Z pointing out of the material, +X along model X projected onto the face (Y when the face is square to X), then combined with the base by op.

<onFace face=">Z" op="cut"> <box size={[40, 30, 10]} /> <cylinder r={3} h={4} z={-4} /> </onFace>

Prop	Type	Description
face*	SelectorLike \| Selector	Which face: a selector (`">Z"`, `faces.max("x")`...) matching planar faces.
index	number	Which of the matching faces (0-based, kernel order). Default 0.
op	"union" \| "add" \| "cut" \| "difference" \| "intersect" \| "intersection" \| "none"	How the tools combine with the base. Default `"union"`.

Also takes solid children.

#Constraint sketch

Elements of constraint-solved sketches (see Constraint sketches).

<point>

Constraint sketch: a point.

A sketch point. x/y are a rough guess unless fixed.

Prop	Type	Description
id	string
ref	PointHandle	A handle naming this point (`ref={s.o}`).
x	number	Rough (or, with `fixed`, exact) X, mm.
y	number	Rough (or, with `fixed`, exact) Y, mm.
at	Vec2	`[x, y]` (alias of `x`/`y`).
fixed	boolean	Pin the point at `x`, `y` (default 0, 0).
on	Ref<LineHandle \| Round>	Keep the point on this curve (line, arc or circle).

<line>

Constraint sketch: a line between two points.

Line-ish constraint props shared by <line>.

Prop	Type	Description
from*	PointLike	Start point: an id (created if new) or `[x, y]`.
to*	PointLike	End point: an id (created if new) or `[x, y]`.
horizontal	boolean	Keep the line horizontal.
vertical	boolean	Keep the line vertical.
length	number	Length, mm.
angle	number	Direction from `from` to `to`, degrees CCW from +X (lines are undirected: mod 180).
parallel	Refs<LineHandle>	Parallel to these lines.
perpendicular	Refs<LineHandle>	Perpendicular to these lines.
equal	Refs<LineHandle>	Same length as these lines.
tangent	Refs<Round> \| boolean	Tangent to these arcs/circles (`true`: the arc meeting this line's `from`).

<arc>

Constraint sketch: a circular arc.

A circular arc from from to to, counter-clockwise about center unless cw. Give center (an id) or leave it out and set radius / tangent: the centre is then an implicit point ("<id>.center").

Prop	Type	Description
from*	PointLike	Start point.
to*	PointLike	End point.
center	PointLike	Centre point (created if new).
radius	number	Radius, mm.
r	number	Alias of `radius`.
diameter	number	Diameter, mm.
d	number	Alias of `diameter`.
cw	boolean	Clockwise from `from` to `to`. Default: counter-clockwise (or as drawn, for tangent arcs).
ccw	boolean	Explicitly counter-clockwise.
angle	number	Sweep angle, degrees (constrained).
tangent	Refs<LineHandle \| Round> \| boolean	Tangent to these lines/arcs/circles; `true`: to the curve meeting this arc's `from`.
equal	Refs<Round>	Same radius as these arcs/circles.
concentric	Ref<Round>	Same centre as this arc/circle.
major	boolean	Hint: the long way round (sweep over 180°). Picks the branch when nothing is drawn.
minor	boolean	Hint: the short way round (sweep under 180°).

<spline>

Constraint sketch: a B-spline through control points.

A clamped B-spline through control points (ends on the first and last).

Prop	Type	Description
points*	readonly PointLike[]	Control points: ids (created if new) or `[x, y]`, at least 2.
degree	number	Degree (default 3, lowered for few points).

<dimension>

Constraint sketch: a driving dimension.

A driving dimension. Between two points: distance (or dx / dy, signed b − a); point–line: perpendicular distance; line–line: distance between (and so parallel) lines; an arc/circle stands for its centre. of + radius/diameter for circles, of + length for lines, a/b + angle for two lines.

Prop	Type	Description
distance	number	Distance, mm.
value	number	Alias of `distance`.
side	"left" \| "right"	For a distance from a line: which side of it (looking from its `from` to its `to`) the other point/line lies. Default: the side it is drawn on.
dx	number	Signed horizontal distance `b.x − a.x`, mm.
dy	number	Signed vertical distance `b.y − a.y`, mm.
angle	number	Angle from line a to line b, degrees CCW (mod 180).
of	Ref<AnyCurve>	The entity for `radius` / `diameter` / `length`.
radius	number
diameter	number
length	number

<distance>

Constraint sketch: a distance.

Distance between two things (see <dimension>).

Prop	Type	Description
value	number	Distance, mm.
side	"left" \| "right"	For a distance from a line: `"left"` / `"right"` of it (from → to). Default: as drawn.
distance	number	Alias of `value`.
dx	number
dy	number

<angle>

Constraint sketch: an angle between lines.

Angle from line a to line b, degrees CCW (lines undirected: mod 180).

Prop	Type	Description
value	number
angle	number

<coincident>

Constraint sketch: coincident points / point on curve.

Two points made one, or a point put on a curve.

<equal>

Constraint sketch: equal lengths / radii.

Equal length (lines) or radius (arcs/circles); of for several.

Prop	Type	Description
of	readonly Ref<LineHandle \| Round>[]

<parallel>

Constraint sketch: parallel lines.

Two lines parallel (of for several).

Prop	Type	Description
of	readonly Ref<LineHandle>[]

<perpendicular>

Constraint sketch: perpendicular lines.

Two lines perpendicular.

<tangent>

Constraint sketch: tangency.

Tangent: line–arc/circle or arc/circle–arc/circle.

Prop	Type	Description
side	"left" \| "right"	Line–arc/circle: the side of the line (looking from → to) the centre lies on.

<collinear>

Constraint sketch: collinear lines.

Lines on one infinite line.

<concentric>

Constraint sketch: concentric arcs/circles.

Same centre.

<horizontal>

Constraint sketch: horizontal.

A line (a) or two points (a, b) horizontal.

<vertical>

Constraint sketch: vertical.

A line (a) or two points (a, b) vertical.

<symmetric>

Constraint sketch: symmetry.

a and b mirror images: across line about; about point about (point symmetry); or, with axis, across the vertical ("x": x mirrored) or horizontal ("y") line through point about (default the origin).

Prop	Type	Description
about	Ref<PointHandle \| LineHandle>
axis	"x" \| "y"

<midpoint>

Constraint sketch: midpoint.

point at the middle of line of.

Prop	Type	Description
point*	PointId
of*	Ref<LineHandle>

<onCurve>

Constraint sketch: point on curve.

point on curve curve (line: the infinite line; arc: its circle).

Prop	Type	Description
point*	PointId
curve*	Ref<LineHandle \| Round>

<fix>

Constraint sketch: fix a point.

Pin a point (at x/y, or where it is drawn).

Prop	Type	Description
point	PointId
a	PointId
x	number
y	number

<mirrorEntities>

Constraint sketch: mirrored, constrained copies of entities.

Mirrored copies of entities across a line, kept symmetric by constraints: edit one side and the other follows. A mirrored point is named with a ' ("p" → "p'"), and a copy's id gets a ' too ("lug" → "lug'"). Points on the mirror line meet their own image, so a mirrored half profile closes.

<mirrorEntities about="axis" of={["lugTop", "lugEnd", "lugBottom"]} />

Prop	Type	Description
about*	Ref<LineHandle>	The mirror line (usually construction).
of*	Refs<LineHandle \| ArcHandle \| CircleHandle \| SplineHandle>	Entities to mirror.

<circularPattern>

Constraint sketch: copies turned about a centre, constrained.

Copies of entities turned about a centre, tied by rotation constraints (not baked coordinates). Copy k of a point "p" is "p~k" (wrapping round for a full turn, so a chain can end on the next copy's start: to="a~1"), and copy k of "lobe" is "lobe~k".

<circularPattern center="o" count={6} of={["hole"]} />

Prop	Type	Description
center*	PointId	The point to turn about.
count*	number	Number of instances, the original included.
angle	number	Total angle, degrees: 360 (default) spaces them evenly; less puts the last at `angle`.
of*	Refs<LineHandle \| ArcHandle \| CircleHandle \| SplineHandle>	Entities to copy.