Command reference

Generated by cargo xtask book from solidcraft-cli commands (390 commands). Every command runs the same way from the toolbar, a script, solidcraft-cli exec <id> '<json>', the control channel and MCP. Parameters marked ? are optional; expr is a number or an expression with units.

SOLID › CREATE

sketch.create Create Sketch
plane: XY|XZ|YZ | construction plane name or id | {origin, x_dir, y_dir} | {face: [world x,y,z], body?: exact world body, index?: face index, path?: complete occurrence ids, fixed?: bool}; new face attachments require a unique certified source (a flat face of a sheet metal body attaches to its panel instead, in the flat pattern's coordinates), fixed:true explicitly freezes the selected plane; offset?: expr, flip?: bool | "x" | "y" (not on a face: sketch the plane from its other side, so the normal and the default extrude direction are reversed; a half turn about the plane's own x or y axis, true picks the one keeping the sketch's y axis upward; offset still moves along the unflipped normal), project_edges?: bool, name?
solid.extrude Extrude (E)
distance: expr (or through_all: true); taper?: angle expr; sketch?: id|name (default: active or last sketch); profiles?: all | [index] | [{curves: [ids]}] (the profile whose outer loop is made of exactly these curves, or pieces of them; found again on every recompute, so it follows parameter changes; islands inside are its holes; an error when no profile or several match) | [{point:[x,y]}] (index and point picks are stored by their curves when that finds the same profile); face?: [x,y,z] (extrude a planar body face instead of a sketch profile); face_body?: name (whose face, where faces of several bodies meet at the point); direction?: positive|negative|symmetric (distance is total thickness, split evenly around the start plane); convention?: total_distance|legacy_per_side (default total_distance; legacy preserves older symmetric extents); distance2?; start_offset?: expr (along the sketch normal, also with direction: negative); to?: [x,y,z] (To Object: a face, vertex or point; to_offset?: expr past it); from?: [x,y,z] (From Object: start at that face or point); operation?: new|join|cut|intersect|auto (cut into a body, otherwise join existing solids; new in an empty component); targets?: [body] (Join from a face, or from a sketch on a body's face, defaults to that face's body; explicit targets or participants override); name?; body_name?; thin?: true (Thin: a wall along sketch curves instead of the profiles) with curves?: [curve ids] (open chains and closed loops, joined where they meet end to end; default: every drawn curve of the sketch), thickness: expr, side?: center|inside|outside|two_sides (a closed loop's inside is the area it encloses, an open chain's the side it bends toward, a straight line's the left of its first curve as drawn; default center), thickness2?: expr (two_sides: the thickness outside); corners are mitred, crossing walls are one
solid.revolve Revolve
axis: sketch line id | x | y (sketch axes) | X|Y|Z (world); angle?: expr (default 360 deg); angle2?: expr (Two Sides: the other side's angle); direction?: symmetric (angle split either side, independent of axis direction); convention?: sketch_normal|legacy_axis_start (default sketch_normal; legacy retains older angular starts); to?: [x,y,z] (To Object: turn until that face, vertex or point); sketch?, profiles? | face: [x,y,z] (a planar body face as the profile) and face_body?: name (whose face, where faces of several bodies meet), operation?, targets?, name?, body_name?
solid.sweep Sweep
sketch: profile sketch; profiles?; path_sketch: sketch; path: [curve ids in order]; orientation?: perpendicular (default: square to the path, turning with it) | parallel (as drawn: the profile moves without turning; the path must keep crossing its plane) | [x,y,z] (square to the path, its turn about the path fixed by this direction); twist?: angle expr (the profile turns this much about the path over its length; within 4 turns); scale?: expr (the profile's scale at the end, linear along the path; 0.01…100); operation?, targets?, name?, body_name?
solid.loft Loft
sections: [{sketch, profiles?} | {sketch, point: id} (an apex)] (2 or more, in order); operation?, targets?, name?, body_name?
solid.box Box
length, width, height: expr; corner?: [x,y,z] | center?: [x,y,z] (numbers in mm or length expressions; default: the origin); operation?, targets?: [body], name?, body_name?
solid.cylinder Cylinder
radius | diameter, height: expr; base?: [x,y,z] (centre of the bottom: numbers in mm or length expressions; default: the origin); axis?: X|Y|Z|[x,y,z] (default Z); operation?, targets?: [body], name?, body_name?
solid.sphere Sphere
radius | diameter: expr; center?: [x,y,z] (numbers in mm or length expressions; default: the origin); operation?, targets?: [body], name?, body_name?
solid.torus Torus
major, minor: expr (radii); center?: [x,y,z] (numbers in mm or length expressions; default: the origin); operation?, targets?: [body], name?, body_name?
solid.pattern.rectangular Rectangular Pattern
features: [names] | bodies: [names] | components: [names]; dir1: [x,y,z]; count1; spacing1; dir2?, count2?, spacing2?; alignment?, alignment2?: left|center|right (default right; counts include the original); reversed?, reversed2?: bool (Flip)
solid.pattern.circular Circular Pattern
features: [names] | bodies: [names] | components: [names]; axis: X|Y|Z | {origin, dir}; count; angle? (default 360 deg; partial arcs include both ends); alignment?: left|center|right (default right; original stays fixed); reversed?: bool (Flip; selects the extra side for even centered counts)
solid.pattern.path Pattern on Path
features: [names] | bodies: [names]; path_sketch: sketch; path: [curve ids in order]; count; spacing (between instances) | distance (first to last); orientation?: identical|path; flip?: bool
solid.mirror Mirror
features: [names] | bodies: [names] (combine?: join with the original); plane: XY|XZ|YZ|construction plane name or id|{origin, normal}|{origin, x_dir, y_dir} (origin coordinates may be length expressions; the mirror follows them, or a construction plane)
solid.hole Hole (H)
position: [x,y,z] on a face (numbers, or length expressions the hole follows) | sketch + points: [sketch point ids] (one hole each, perpendicular to the sketch, into the material on whichever side of the sketch plane it is) | sketch alone (every sketch point: standalone points and circle centres); flip?: bool (sketch points: drill to the other side); direction?: [x,y,z] (default: into the face, against its outward normal; one that leaves the face is mirrored into it; ignored with sketch points); diameter | thread (a tapped hole: the tap drill, major − pitch) | clearance: "M6" with fit?: close|normal|loose (ISO 273); depth? (default through all) | to?: [x,y,z] (To Object: drill to that face or point); type?: simple|drilled|counterbore|countersink; tip_angle?; cb_diameter?, cb_depth?; cs_diameter?, cs_angle?; thread?: "M6" (cosmetic)
solid.pipe Pipe
path_sketch: sketch; path: [curve ids in order]; diameter: expr; wall?: expr (hollow); operation?, targets?, name?, body_name?
solid.bounding_solid Bounding Solid
bodies?: [names] (default: all); margin?: expr; name?, body_name?
solid.thread Thread
face: [x,y,z] on a cylindrical face; designation?: ISO metric ("M8", "M8x1"; default: the size that fits); length?: expr (default: the whole face); modeled?: bool (default false). Cosmetic: the model is unchanged, model.threads lists it. Modeled: cuts the thread profile into the body
solid.boundary_fill Boundary Fill
tools: [bodies]; cells: [[x,y,z] a point inside each cell to fill (a cell: inside some tools, outside the rest)]; operation?: new|join|cut|intersect; remove_tools?: bool
solid.coil Coil
diameter; two of revolutions (or turns), height, pitch; section_size; section?: circular|square; section_position?: inside|center|outside; base?: [x,y,z] (numbers in mm or length expressions; default: the origin); axis?: X|Y|Z|[x,y,z] (default Z); start_angle?; clockwise?: bool; operation?, targets?, name?, body_name?
solid.rib Rib
sketch, curves: [open curve ids, in order]; thickness (across the sketch plane); depth? (default: to the next face); flip?: bool (fill to the other side)
solid.web Web
sketch, curves: [open curve ids] (one wall each); thickness; depth? (default: to the next face); flip?: bool
solid.emboss Emboss
sketch, profiles?; depth; mode?: emboss|deboss; targets?; face?: world point [x,y,z] selecting a planar or complete exterior cylindrical wall (inferred when exactly one supported tangent cylinder matches the selected profiles)
joint.origin Joint Origin
name?, occurrence?: id|name (default: from the pick), face: [x,y,z] (centre of a planar face) | circle: [x,y,z] (centre of a round end) | point: [x,y,z], z?: [x,y,z]

SOLID › MODIFY

solid.fillet Fillet (F)
edges: [[x,y,z] point on edge | {body, index}]; radius: expr; body?; type?: constant|curvature (alias g2: curvature-continuous quintic between planar faces along straight edges, one perpendicular planar end face at each end; radius sets the equivalent circular setback, not constant curvature; exact fit only)|chord (radius is the width across)|variable (radius at the end nearest start, radius2 at the other; one end may be 0, where the round closes to the corner)|spline (the radius along the edge is a clamped B-spline from the end nearest start: radius is its first control radius, radii the rest, knots its knot vector from 0 to 1; one end may be 0); radius2?; start?: [x,y,z]; radii?: [expr, …]; knots?: [number, …]; mid?: [[position 0…1 from start, radius expr], …] (variable radii between the ends); smooth?: bool (smooth instead of straight between the radii); corner?: rolling|g2 (rolling, the default: the corners where three blended edges meet are pieces of the rolling ball's sphere, tangent to each blend; g2: a patch repeating each blend's surface up to the second order, constant-radius exact fillets only, refused where it cannot be built); fit?: exact|reduce|taper (exact, the default: a radius too large for the geometry around the edges is refused; reduce: where it doesn't fit it is reduced to the largest that does, one radius for edges sharing a face; the smallest used is returned as `radius_applied`, each edge's as `radii_applied: [{edge: [x,y,z], radius}]`, and noted in the feature's warning; taper: along each straight edge between planar faces where it doesn't fit, the radius follows the room there as a smooth spline, down to 0 where a face closes to a point, noted in the feature's warning)
solid.chamfer Chamfer
edges: [[x,y,z] | {body, index}]; distance: expr; distance2?: expr (along the second face) | angle?: expr (from the first face); flip?: bool (which face is first: by default the one facing up most); body?
solid.combine Combine
target: body; tools: [body]; operation?: join|cut|intersect; keep_tools?: bool; new_component?: bool (the result goes into a new component; component_name?)
solid.scale Scale
bodies: [names]; factor: expr | factors: [x, y, z] exprs; origin?: [x,y,z]
face.delete Delete Face
faces: [[x,y,z] points on the faces, or face names from model.faces]; body?; heal?: bool (default true: the neighbouring planes close the gap, as when a rounded edge, hole or boss is taken off; false: the gap stays open and the faces left are a surface body)
solid.offset_face Offset Face
faces: [[x,y,z] points on planar faces, or face names from model.faces]; distance: expr (positive: outward); body?
solid.shell Shell
faces: [[x,y,z] points on the faces to remove, or face names from model.faces]; thickness: expr; direction?: inside|outside|both; tangent_chain?: bool (also open faces joined smoothly to the picked ones); body?
solid.draft Draft
faces: [[x,y,z] points, or face names from model.faces]; angle: expr; neutral: XY|XZ|YZ|plane name|{origin, normal}; pull?: [x,y,z] (default: neutral plane normal); body?
solid.split_face Split Face
faces: [[x,y,z] points on the faces to split, or face names from model.faces]; body?; and the splitting tool: plane: XY|XZ|YZ|plane name|{origin, normal} — or tool: {body, point} (a face of a body, its surface extended) — or sketch: id or name (its curves, along the sketch's normal)
solid.split_body Split Body
body: name; plane: XY|XZ|YZ|plane name|{origin, normal} — or tool: {body, point} (a face of a body, its surface extended) — or sketch: id, line: curve id (a straight sketch line, along the sketch's normal)
solid.press_pull Press Pull (Q)
face: [x,y,z] and distance: expr (positive adds material, negative cuts), or edges: [[x,y,z]…] and distance (a fillet)
solid.move Move/Copy (M)
bodies: [names]; translate?: [x,y,z] (exprs or numbers); axis?: [x,y,z]; angle?: expr; copy?: bool (default false: keeps the original bodies and transforms a new copy instead of moving them in place)
solid.replace_face Replace Face
faces: [[x,y,z] points on planar faces, or face names from model.faces]; target: plane (XY|XZ|YZ|construction plane|{origin, normal}) | target_face: [x,y,z] on a parallel planar face; body?
solid.align Align
bodies: [names]; from: [x,y,z] | {snap: vertex|edge_mid|face_center|circle_center, at: [x,y,z]} | from_face: [x,y,z]; to: (the same) | to_face: [x,y,z] (faces also turn to meet); flip?: bool
solid.remove Remove
bodies: [names] (removed from here on in the timeline)
timeline.compute_all Compute All
timeline.delete Delete (Delete)
features: [id or name] (a sketch takes its dependent features with it) → deleted: [ids]; failing?: [{feature, error}] (later features that worked and now fail)
parameters.change Change Parameters
name, expression (number or text), unit?: mm|cm|m|in|ft|deg|rad|"" (new parameters default to their value's unit), comment?, favorite?: bool, new_name?: rename (references follow); or delete: name → recomputed: features rebuilt, restored: features whose earlier result for the same inputs was reused (e.g. a value set back)
material.assign Physical Material
bodies: [names]; material: name (Steel, Aluminum, ABS Plastic, …, or one made with material.create; `material.list`)
appearance.assign Appearance (A)
bodies?: [names]; faces?: [[x,y,z] on faces] (body?: which body, default the nearest); components?: [names or ids, or occurrence names]; appearance?: library name (appearance.library) | color: "#rrggbb" or [r, g, b] (0–255), opacity? (0–1, default 1); pbr?: {metallic:0..1, roughness:0.045..1, dielectric_ior:1..3} (requires color/appearance and opacity 1); omitted/null uses legacy scalar shading. Neither appearance nor color (or color: null): clear, so the face follows its body, the body its component, the component its material

SOLID › CONSTRUCT

construct.plane.offset Offset Plane
base: XY|XZ|YZ|plane name, or a planar face {face: [x,y,z], body?, index?, path?}; offset: expr; name?
construct.plane.at_angle Plane at Angle
base: XY|XZ|YZ|plane name; axis: X|Y|Z|{origin, dir}; angle: expr; name?
construct.axis.through_cylinder Axis Through Cylinder/Cone/Torus
face: ref (a cylinder, cone or torus face, or a circular edge); name?
construct.axis.normal_to_face Axis Perpendicular To Face
face: ref; point: ref (the axis goes through it, square to the face); name?
construct.axis.two_planes Axis Through Two Planes
a, b: plane or planar face refs; name?
construct.axis.two_points Axis Through Two Points
a, b: point refs (vertices, sketch points, points); name?
construct.axis.edge Axis Through Edge
edge: ref (a straight edge or sketch line); name?
construct.point.vertex Point At Vertex
point: ref (vertex, sketch point, point); name?
construct.point.two_edges Point Through Two Edges
a, b: edge or line refs (where they meet, or come closest); name?
construct.point.three_planes Point Through Three Planes
a, b, c: plane or planar face refs; name?
construct.point.center Point At Center Of Circle/Sphere/Torus
of: ref (circular edge, sketch circle or arc, sphere or torus face); name?
construct.point.edge_plane Point At Edge And Plane
edge: edge or line ref; plane: plane or planar face ref; name?
construct.point.along_path Point Along Path
path: edge or sketch curve ref; t: expr, 0…1 along it (default 0.5); name?
construct.plane.midplane Midplane
a, b: plane or planar face refs (halfway between; bisecting when they meet at an angle); name?
construct.plane.two_edges Plane Through Two Edges
a, b: straight edge or line refs in one plane; name?
construct.plane.three_points Plane Through Three Points
a, b, c: point refs; name?
construct.plane.tangent Tangent Plane
face: ref (cylinder, cone, sphere or torus); at?: [x,y,z] where it touches (default: the face pick); name?
construct.plane.along_path Plane Along Path
path: edge or sketch curve ref; t: expr, 0…1 along it (default 0.5); name? The plane is square to the path there
construct.plane.perpendicular Perpendicular Plane
plane: plane or planar face ref; line: straight edge, sketch line or axis ref; name? The plane holds the line and is square to the plane

SOLID › ASSEMBLE

component.create New Component
name?, parent?: component id or name (default: the active one); parent_path?: exact parent placement; activate?: bool (default true)
component.insert_design Insert Design
path: a .solidcraft design → a new component linked to it, holding its solid bodies as placed in that design; name? (default: the design's name); parent?: component id or name (default: the active one); translate?: [x,y,z]
joint.create Joint (J)
type: rigid|revolute|slider|cylindrical|pin_slot|planar|ball; a, b: joint origins ({occurrence, face|circle|point: [x,y,z] in world} | origin name); values?: [angles in deg or expressions, distances]; limits?: [[min, max] | null…]; flip?: bool (default false: the origins are mated, b's z against a's as two faces meet; true: b's z along a's, so two origins given at one point with the same z stay as they are); offset?; angle?; name?; quiet?: bool (leave out dof and fixed)
joint.as_built As-Built Joint
type, a: occurrence, b: occurrence (stay where they are); at?: joint origin (default: b's origin) — the joint's frame; name?; limits?: [[min, max] | null…]; quiet?: bool
joint.rigid_group Rigid Group
occurrences: [ids or names] (move together, as they are)
joint.drive Drive Joints
joint: id|name; value | values: [angles in deg or expressions, distances] (values not given keep theirs; clamped to the limits; the other joints of a closed loop follow, and the motion stops where the loop can no longer close → stopped_by_loop); quiet?: bool (leave out dof and fixed) → values: [{name, value, unit: deg|mm, limits}] as joint.list gives them; moved: whether any occurrence moved; reason: why the joint can move nothing (suppressed, its origins lost, or its chain joined to nothing grounded → unconnected: the occurrence named)
joint.motion_link Motion Link
a, b: joints; ratio (b = ratio · a + offset): b's units per a's (mm per deg for an angle driving a distance); offset?: in b's units (deg for an angle, mm for a distance, or an expression); ia?, ib?: value indices (default 0)
joint.gear Gear
a, b: joints that turn (revolute), b driven by a; ra, rb: the gears' pitch radii (or tooth counts): mm, an expression, or {circle: [x,y,z], occurrence?}: the round face there, its radius (read again whenever the design changes, so the ratio follows edits); internal?: bool (one is a ring gear: both turn the same way; by default b turns the other way); reverse?: bool; link?: index (replace that motion link) → link, ratio (b's degrees per a's); b keeps where it is
joint.rack_pinion Rack and Pinion
a, b: a joint that turns (revolute: the pinion) and one that slides (slider: the rack), in either order, b driven by a; radius: the pinion's pitch radius (mm, an expression, or {circle: [x,y,z], occurrence?}): the rack travels radius × the turn in radians; reverse?: bool; link?: index (replace that motion link) → link, ratio (mm per degree, or degrees per mm); b keeps where it is
joint.screw Screw
joint: a cylindrical joint (its turn drives its travel) | a, b: a joint that turns and one that slides, b driven by a; pitch: travel per turn (mm or an expression); reverse?: bool (a left-hand thread); link?: index (replace that motion link) → link, ratio (mm per degree, or degrees per mm); b keeps where it is
joint.cam Cam
a: the cam's joint (revolute); b: the follower's joint, a slider (a translating follower) or a revolute (an oscillating one), b driven by a; profile: {sketch: id|name, index?: the profile (default: the largest)} | {edges: [[x,y,z]…] (points on edges of the cam's bodies forming one closed loop, world), occurrence?}: the cam's outline, in a plane square to its axis, read again whenever the design changes; follower?: knife|roller|flat (default knife; flat: a face square to a slider's line); radius?: the roller's radius (mm, an expression or {circle: [x,y,z], occurrence?}: the roller's round face, which is its tip too); tip?: a joint origin where the follower touches: its knife's point or its roller's centre, such as {circle: [x,y,z]} on the roller (needed for an oscillating follower; a translating one's line runs through it, by default along its slider's axis); flip?: bool (ride the cam from the other side than the one the follower is on now); link?: index (replace that motion link) → link, lift: {min, max, rise, unit} (b's travel over a turn of the cam), reverse (the side it rides from), follower_offset (mm: how far a translating follower's line passes from the cam's axis); b keeps where it is
contact.enable_sets Enable Contact Sets
enabled?: bool (default true) — driving joints and motion studies stop where bodies in one contact set would pass through each other
contact.enable_all Enable All Contact
every occurrence takes part in contact (one set of all)
contact.disable_all Disable Contact
contact off
contact.create New Contact Set
occurrences: [ids or names] (two or more); name?
motion.study Motion Study
name?; study? (edit an existing one); steps? (timeline length, default 100); keys: [{joint, index?, points: [[step, value], …]}] (values: degrees for angles, mm for distances, or expressions)
motion.trace Motion Trace
occurrence: id|name, or an occurrence path [ids] (an instance inside sub-assemblies); point: [x,y,z] world point on it, where it is placed now; study: id|name, or joint: id|name with from and to (degrees for angles, mm for distances, or expressions) and index? (which value, default 0); samples? (2…500, default the study's steps + 1, or 100) - the point's path as the study plays or the joint is driven, closed loops following → points: [[x,y,z]…] world positions, samples (taken), stopped_at (the sample where the motion stopped short; the trace ends there), stopped_by_loop, stopped_by_contact (the design is not changed)
explode.create Exploded View
name?; scale? (automatic: each occurrence pushed away from the assembly's centre by scale × its offset, default 1); moves?: [{occurrence, translate: [x,y,z]}] (instead of automatic)

SOLID › POSITION

component.capture_position Capture Position
keeps pending occurrence moves
component.revert_position Revert Position
occurrences?: [ids] (default all); drops selected pending occurrence moves

SOLID › INSPECT

inspect.interference Interference
bodies?: [names] (default: all, in world placement) → interferences: pairs that overlap with the overlap volume, area, bounding box and centre; unchecked: pairs that could not be checked, with the reason. Bodies are pruned by bounding box first, so any number of bodies is fine; at most 20000 pairs whose boxes overlap are intersected per call (truncated: true and skipped_pairs: n say when more were left out)
inspect.measure Measure (I)
bodies?: [names] (default all); or items: [1-2 selections] → length/area/volume; diameter, radius, circumference or arc_length/angle_deg of circles, arcs and cylinders; slot sizes; min (distance_mm, from, to), max, center_distance (centre to centre, or from an axis) and angle
inspect.section Section Analysis
plane: XY|XZ|YZ | construction plane name or id | {origin, normal}; offset?: expr along the plane's normal (XY: +Z, XZ: +Y, YZ: +X); at?: expr, the cut's world coordinate on the named plane's axis (XY: Z, XZ: Y, YZ: X), instead of offset; flip?: bool; or clear: true. Returns the cut's origin and normal, and for a named plane its axis and at

SOLID › CONFIGURE

config.configure Configure
params?: [parameter names]; features?: [feature names]; materials?: [body names]; appearances?: [body names] (columns to add; with no rows yet, a "Default" row takes the current values)
config.table Display Configuration Table
→ columns (param:<name> or suppress:<feature>), rows, the active row and whether the design still matches it

SOLID › INSERT

parts.fastener Insert Fastener
the Insert Part dialog's command (same as parts.insert): family, size, length?, at?|point?+direction?, name?
file.insert_step Insert STEP
path: STEP, IGES, FreeCAD .FCStd or Rhino .3dm file (its bodies join the design as an Import base feature in a new component named after the file, placed in the active component; an assembly's products become nested components, a repeated part one component with an occurrence per placement, all held as one rigid group until component.unlock → component, component_name, occurrence, subcomponents?, rigid_joints?); name? (the feature's and the component's); up?: z|y (default z: the file's axes are kept; y: the file has Y up, so the import's component is turned a quarter turn about X, Y becoming Z → stand_up: its occurrence); names?: solid|product|instance (what the bodies are named after: the solid's own name, else the product's (default); the name of the product (part) that holds the body; the name of the assembly occurrence (instance), else the product's)
file.insert_mesh Insert Mesh
path: .3mf, .stl, .obj, .glb or .gltf file (its meshes join the design as mesh bodies in a new component named after the file → component, component_name, occurrence; a glTF file's node tree becomes nested components held as one rigid group until component.unlock, a mesh placed again another occurrence, its materials the bodies' appearances, and its metres millimetres); name?; up?: z|y for a glTF file (default y: glTF has Y up, so the import's component is turned a quarter turn about X, Y becoming Z → stand_up: its occurrence; z: the file's axes are kept)

SKETCH › FINISH SKETCH

sketch.finish Finish Sketch
sketch.finish_auto_constrain Finish with AutoConstrain
like AutoConstrain, then Finish Sketch

SKETCH › CREATE

sketch.line Line (L)
points: [[x,y] | "l1.end" | {at, ref}…], closed?: bool, construction?: bool, ids?: [..], infer?: bool (add horizontal/vertical); connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.rectangle.two_point 2-Point Rectangle (R)
p0, p1: opposite corners [x,y]; construction?. Returns sides {bottom, right, top, left} (line ids) and corners {bottom_left, bottom_right, top_right, top_left} (point ids); connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.rectangle.three_point 3-Point Rectangle
p0, p1: first edge; p2: point on the opposite edge; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.rectangle.rounded Rounded Rectangle
p0, p1: opposite corners [x,y]; radius: expr (the corner radius, less than half the shorter side); construction?. A 2-point rectangle whose four corners are filleted alike: one radius dimension (`param`), the other arcs equal to it. Returns sides {bottom, right, top, left} (line ids) and arcs (the corner arcs: bottom-left, bottom-right, top-right, top-left); connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.rectangle.center Center Rectangle
center, corner. Returns sides {bottom, right, top, left} (line ids) and corners {bottom_left, bottom_right, top_right, top_left} (point ids); connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.circle.center Center Diameter Circle (C)
center: [x,y] or point ref, radius | diameter: number; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.circle.two_point 2-Point Circle
p0, p1: diameter ends; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.circle.three_point 3-Point Circle
p0, p1, p2; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.arc.three_point 3-Point Arc
start, end, through; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.arc.center_point Center Point Arc
center, start, end (counter-clockwise from start) | center, start, sweep: signed degrees; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.polygon.inscribed Inscribed Polygon
center, radius (to vertices), sides, angle?: deg; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.polygon.circumscribed Circumscribed Polygon
center, radius (to edge midpoints), sides, angle?: deg; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.polygon.edge Edge Polygon
p0, p1: one edge, sides; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.slot.center_to_center Center to Center Slot
p0, p1: arc centres, width; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.slot.overall Overall Slot
p0, p1: overall ends, width; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.point Point
point: [x,y], id?; connect?: bool (default true: a new point landing exactly on an existing point, the origin too, is made coincident with it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.dimension Sketch Dimension (D)
entities: [refs], type?: auto|distance|horizontal|vertical|length|radius|diameter|angle, value?: number or expression (default: current; a bare number is in the design's units, e.g. 2 means 2 in in an inch design; give a unit such as "50 mm" to override); text_at?: [x, y]. Two points or a line off the axes: with auto, text_at across from them is the distance between them, above or below them horizontal, beside them vertical. Two lines: the angle between them (acute, or 180° − it when the value is nearer that) unless text_at picks a sector. A dimension the sketch already determines is refused (naming what determines it); if_redundant?: "driven" places it as a driven (reference) dimension instead. scale_sketch?: bool (the dimension tool sends true): when this is the sketch's first length dimension and nothing in the sketch fixes a size (no other driving length dimension, nothing fixed or projected), the whole sketch scales about its origin to the value instead of distorting. Returns measured in unit (mm or deg), and scaled: the factor when the sketch was scaled
sketch.construction Normal/Construction (X)
curves: [ids], value?: bool (default: construction unless all of them already are)
sketch.line.midpoint Midpoint Line
mid: [x,y] or point ref, end: [x,y]; construction?. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.arc.tangent Tangent Arc
start: end point of a line or arc ("l1.end"), end: [x,y]; curve?: the curve to be tangent to (default: the one ending at start). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.circle.two_tangent 2-Tangent Circle
curves: [two lines/circles/arcs], radius | diameter: expr, near: [x,y] (which of the solutions). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.circle.three_tangent 3-Tangent Circle
curves: [three lines/circles/arcs], near: [x,y] (which of the solutions). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.slot.center_point Center Point Slot
center: slot centre, end: one arc centre, width. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.slot.arc_three_point Three Point Arc Slot
start, through, end: points on the centre arc, width. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.slot.arc_center Center Point Arc Slot
center, start: centre arc start, end: direction of the centre arc end (counter-clockwise), width. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.ellipse Ellipse
center, major: end of the major axis [x,y], minor: a point the ellipse passes through on the minor side [x,y] | minor_radius. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.spline.fit_point Fit Point Spline
points: [[x,y] or point refs…] (2…500): the spline passes through them, periodic?: boolean (default false); periodic cubic fit closes smoothly through at least 3 distinct samples. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.spline.control_point Control Point Spline
points: control points (2…500), cubic. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.spline.control_point_5 Control Point Spline (Degree 5)
points: control points (2…500), degree 5. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.conic Conic Curve
start, end, apex: [x,y] or point refs; rho?: 0…1 (default 0.5: parabola). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.centerline Centerline
curves: [line ids], value?: bool (default toggles): centerline line type (not in profiles; an axis)
sketch.text Text
text: string (\n breaks lines), at: baseline start [x,y], height?: capital height mm (default 5), angle?: deg; at's x and y, height and angle each take a number or an expression over the design's parameters as a string ("plate_width / 2", "label_size"): the text keeps the expression, follows the parameters, and returns it in `exprs`; an expression naming no parameter is the number it comes to, a bare number in one is in the design's units, font?: an installed font's family or full name, or a .ttf/.otf file path (~ and %VAR% expand; default: the built-in Liberation Sans), bold?, italic?: bool (an installed family's bold or italic face; italic without one is slanted), align?: left|center|right (the lines against `at`, or along the path), letter_spacing?: extra mm between letters, line_spacing?: times the font's line distance (default 1), path?: a curve id of the sketch the baseline follows ("": none; `at` and `angle` then do not place the text; the curve becomes construction, a guide the letters stand on), reverse?: bool (the other way along the path). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.constrainer Sketch Constrainer
entities: [one or two sketch entity ids]: applies the constraint the geometry nearly has (horizontal/vertical, parallel, perpendicular, collinear, coincident, concentric, equal, tangent)
sketch.project Project (P)
refs: [{edge: [x,y,z], body?} | {face: [x,y,z], body?} (its edge loops) | {body: name} (silhouette) | {vertex: [x,y,z], body?} | {sketch, curve} | {sketch, point} | "origin" | {axis: X|Y|Z} | {plane: XY|XZ|YZ|name}]. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.intersect Intersect
refs: [{body}, {face: [x,y,z], body?}, {edge: [x,y,z], body?}, {sketch, curve}]: section curves (or points) with the sketch plane, linked. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.include_3d Include 3D Geometry
refs: like Project (edges, vertices, sketch curves and points); curves out of the sketch plane are flattened onto it. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.project_to_surface Project To Surface
curves: [{sketch, curve}…] (curves of other sketches), face: [x,y,z] point on the target face, body?: projected along the active sketch's normal onto the face, as linked 3D curves. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.intersection_curve Intersection Curve
a, b: {body} | {face: [x,y,z], body?}: where they meet, as linked 3D curves. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.spun_profile Spun Profile
body: name, axis: a line of the active sketch (curve id) | X|Y|Z: the body's outline revolved about the axis, in the sketch plane. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.isoparametric_curve Isoparametric Curve
face: [x,y,z] point on the face (the curve passes through it), body?, direction?: u|v|[x,y,z] (default u): linked 3D curve. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.fit_curves_to_section Fit Curves to Mesh Section
body: name (a mesh or solid body): its section with the sketch plane, fitted with lines and arcs, as normal (unlinked) geometry. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)

SKETCH › CONSTRAINTS

sketch.constraint.horizontal_vertical Horizontal/Vertical
line: id | points: [a, b]; mode?: horizontal|vertical
sketch.constraint.coincident Coincident
a, b: points, a point and a curve or sketch axis (x / y: the sketch's own axes, unless a curve has that id; an axis becomes a linked construction line on it, reported in created), or two distinct lines (joins their closest endpoints)
sketch.constraint.tangent Tangent
a, b: curves or sketch axes (x / y: the sketch's own axes, unless a curve has that id; an axis becomes a linked construction line on it, reported in created)
sketch.constraint.equal Equal
a, b: lines or circles/arcs
sketch.constraint.parallel Parallel
a, b: lines or sketch axes (x / y: the sketch's own axes, unless a curve has that id; an axis becomes a linked construction line on it, reported in created)
sketch.constraint.perpendicular Perpendicular
a, b: lines or sketch axes (x / y: the sketch's own axes, unless a curve has that id; an axis becomes a linked construction line on it, reported in created)
sketch.constraint.fix Fix/UnFix
entity: point or curve | entities: [points and curves]; fixed?: bool (default: fix them all unless all are fixed, then unfix)
sketch.constraint.midpoint MidPoint
point, line
sketch.constraint.concentric Concentric
a, b: circles/arcs
sketch.constraint.collinear Collinear
a, b: lines or sketch axes (x / y: the sketch's own axes, unless a curve has that id; an axis becomes a linked construction line on it, reported in created)
sketch.constraint.symmetry Symmetry
a, b: two points or two curves (lines mirror their ends, circles/arcs their centres); line: symmetry line id, or x / y for the sketch's own axes (a curve with that id wins; an axis becomes a linked construction line on it, reported in created); or point (or a point id as line, "origin" too): symmetric about that point, each pair joined by a construction line it is the midpoint of
sketch.constraint.curvature Curvature
a, b: two curves sharing an end point (curvature continuous, G2)
sketch.constraint.polygon Polygon
lines: [line ids] of a closed chain: equal sides with every corner on one circle (a regular polygon)
sketch.auto_constrain AutoConstrain
tolerance?: mm (default 0.01), angle_tolerance?: deg (default 1), dimensions?: bool (default true): infer constraints, then dimension until fully constrained
sketch.auto_constrain_from_datum AutoConstrain from datum
datum: point ref (default origin); like AutoConstrain with positions measured from the datum

SKETCH › MODIFY

sketch.blend_curve Blend Curve
a, b: end points of two curves ("l1.end", "a2.start"), continuity?: g1|g2|g3|g4 (default g1: a tangent spline; g2…g4 match the reference curves' curvature, curvature rate and 4th derivative as well, as one Bézier of degree 5, 7 or 9). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.fillet Fillet
point: corner shared by two curves ("l1.end") | points: [corners] (all rounded alike: one radius, the rest equal) | a, b: two lines or arcs meeting at a corner; radius: expr. A corner that dimensions or constraints measure to stays as a virtual sharp corner on both curves' extensions (`virtual_corners`; the moved ones in `moved_to_virtual_corner`). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.chamfer.equal_distance Equal Distance Chamfer
point | a, b: a corner of two lines; distance. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.chamfer.distance_angle Distance and Angle Chamfer
point | a, b: a corner of two lines; distance: along a, angle: deg from a. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.chamfer.two_distance Two Distance Chamfer
point | a, b: a corner of two lines; distance: along a, distance2: along b. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.offset Offset (O)
curves: [ids], distance: number in mm or length expression (creates an editable dimension; positive = left of the chain, or toward `side`), side?: [x,y], chain?: bool (default true: the connected chain); direction?: one_side|symmetric (default one_side) or symmetric?: bool (the same distance each way; no `side`, whose job it takes over), distance2?: positive length expression (Two Sides: an independent distance the other way, as for `solid.extrude`). Each side is its own offset association, listed in `sides`; flip?: bool reverses the primary side; `param`/`param2` name the driving dimensions. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.trim Trim (T)
curve: id, at: [x,y] (the piece to remove: between the nearest intersections around it). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.extend Extend
curve: id, at: [x,y] near the end to extend (to the nearest curve)
sketch.break Break
curve: id, at: [x,y] (split at intersections) | points: [[x,y]…] (1…1000 positions projected onto the curve; duplicates are merged). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.scale Sketch Scale
entities: [curve/point ids], base: [x,y] or point ref, factor: number
sketch.move Move/Copy Sketch Entities
entities: [ids], translate?: [dx,dy], angle?: deg, center?: [x,y], copy?: bool; picking a text outline or linked point transforms its whole text source once, and copies remain editable text. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)

SKETCH › INSERT

sketch.insert_dxf Insert DXF
path | text: ASCII DXF (blocks expanded); at?: [x,y] offset, scale?, tolerance?: mm within which ends join (default 0.0001); plane?: (when no sketch is active, a new sketch on it; default XY). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.insert_svg Insert SVG
path | text: SVG; at?: [x,y] offset, scale?, tolerance?: mm within which ends join (default 0.0001); plane?: (when no sketch is active, a new sketch on it; default XY). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
canvas.insert Canvas
path | data (base64 PNG or JPEG); plane?: XY|XZ|YZ|{face: [x,y,z]}|… (default XY); center?: [x,y] on the plane, or at?: [x,y,z]; width?: mm (default 100); angle?: deg; opacity?: 0…1 (default 0.5); flip?; name?
canvas.decal Decal
path | data; face: [x,y,z] on a planar face (the image is centred there); width?: mm; angle?: deg; opacity?: (default 1)
canvas.edit Edit Canvas
canvas: id or name; center?, width?, angle?: deg, opacity?, flip?, visible?, name?

SKETCH › INSPECT

inspect.curvature_comb Curvature Comb Analysis
curves?: [sketch curve ids] (sketch?: id|name, default active) | edges?: [[x,y,z] points on body edges]; density?: teeth per curve (default 40), scale?: comb length per unit curvature (default auto)
inspect.minimum_radius Minimum Radius Analysis
curves?: [sketch curve ids] (sketch?) | edges?: [[x,y,z]…] | faces?: [[x,y,z]…] (default: every face of every body); the smallest radius of curvature of each and where it is
inspect.isocurve Isocurve Analysis
faces: [[x,y,z]…] points on faces; count?: curves each way (default 8): the faces' isoparametric curves
inspect.center_of_mass Center of Mass
bodies?: [names] (default all): the centre of mass (uniform density) of each and of all together
inspect.zebra Zebra Analysis
stripes?: number across the view (default 12); clear?: true turns the analysis off
inspect.draft Draft Analysis
pull?: [x,y,z] direction (default Z); angle?: degrees (default 1); clear?: true turns the analysis off
inspect.environment_map Environment Map Analysis
clear?: true turns the analysis off
inspect.accessibility Accessibility Analysis
direction?: [x,y,z] the tool comes from (default Z, from above); clear?: true turns the analysis off
inspect.curvature_map Curvature Map Analysis
radius?: mm shown red (default: a tenth of the model's size); clear?: true turns the analysis off

SKETCH › PATTERN

sketch.mirror Mirror
entities: [curve/point ids], line: mirror line id (symmetry constraints are added). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.pattern.circular Circular Pattern
entities: [ids], center: [x,y] or point ref, count: 2…500, angle?: total deg (default 360); alignment?: left|center|right (default right); reversed?: bool (default false). Quantity includes the original. Center balances copies around it; reversed flips the direction and extra side for even totals. Partial arcs span angle with angle/(count-1) spacing; full turns use angle/count. Adds associative pattern constraints; a coordinate center creates a constrainable point. Returns pattern and center ids. pattern?: existing pattern id to edit (omitted values retained; surviving instance ids retained). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.pattern.rectangular Rectangular Pattern
entities: [ids], count, spacing; count2?, spacing2?; direction?, direction2?: sketch line ids (live references); dir?, dir2?: [x,y] vectors (defaults: sketch x, perpendicular to direction 1); alignment?, alignment2?: left|center|right (default right). Signed spacings reverse each direction. reversed?, reversed2?: bool (default false); reverses placement and the extra side of even centered totals. Quantities include the original. Adds associative pattern constraints. Returns pattern id. pattern?: existing pattern id to edit (omitted values retained; surviving instance ids retained). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)

SURFACE › INSPECT

inspect.continuity Continuity Analysis
body?: name (default: the visible bodies); edges?: [x,y,z] points or {"index": i} (default: every edge of the body; a pick must match one body); samples?: 3…257 stations along each edge, ends included (default 33); gap_tolerance_mm? (default 0.001), angle_tolerance_deg? (default 1), curvature_tolerance_per_mm? (default 0.01); clear?: true turns the analysis off. → each edge's worst gap (G0), normal angle (G1) and curvature jump (G2) as {value, at: [x,y,z], edge_fraction}, its verdict (smooth, curvature_jump, sharp or gap) and a summary; the seams are shaded in the viewport

SURFACE › CREATE

surface.boundary Boundary Surface
sketch?: id|name (default: the sketch being edited); curves: [2 to 4 sketch curve ids in loop order] (each one ends where the next begins and the last where the first does; the patch runs through them and leaves each boundary along the tangent across it); continuity?: g0|g1|g2|g3 | [one per curve] (default g1: how much of the surface across each boundary the patch repeats — a sketch curve's own plane, so g1 and up hold exactly and g0 lets the middle bow); crown?: number -0.9…3 (default 0: how full the middle is, without touching a boundary); samples?: 8…512 stations per boundary (default 25); name?, body_name? (a surface body)
surface.patch Patch
sketch?: id|name and profiles? (planar patches of sketch regions) | edges: [[x,y,z]] (points on a closed loop of a body's edges: one face on them, planar when the loop is, else a smooth B-spline surface) and body?; continuity?: g0|g1|g2 (edges only, default g0: how the patch meets the faces beside the loop — g1 their tangent planes, g2 also their curvature across the edges) or [{edge: [x,y,z], g: g0|g1|g2}] (those edges so, the rest g0) or {all, edges}; points?: [[x,y,z]] (edges only, up to 64: points the patch passes through); crown?: number −0.9…3 (default 0: only a fitted patch, whose middle becomes fuller by this many times the loop's size — the bump vanishes on the loop, so the face still meets the picked edges and the continuity across them; a loop that is planar and g0 is the exact plane whatever the crown; with points, crown needs a g1 or g2 edge); name?, body_name?
surface.thicken Thicken
bodies: [surface names]; thickness: expr (negative: against the normal); symmetric?: bool; operation?: new|join|cut|intersect; targets?
surface.extrude Surface Extrude
sketch?: id|name; curves?: [curve ids] (open or closed chains of curves meeting end to end) and/or profiles? (their boundaries; the default when no curves are given); distance: expr; direction?: positive|negative|symmetric; distance2?: expr; start_offset?: expr; name?, body_name? (a surface body: walls only, no caps)
surface.revolve Surface Revolve
sketch?: id|name; curves?: [curve ids] and/or profiles? (as surface.extrude); axis: sketch line id|x|y|X|Y|Z|{origin, dir}; angle?: expr (default 360 deg); angle2?: expr (the other side); symmetric?: bool; name?, body_name? (a surface body, no caps; a solid where a full turn closes it)
surface.sweep Surface Sweep
sketch?: id|name; curves?: [curve ids] and/or profiles? (as surface.extrude); path_sketch: sketch; path: [curve ids in order] (a path with corners, or 3D curves, gives ruled walls mitred at the corners); orientation?, twist?, scale? (as solid.sweep); name?, body_name? (a surface body, no caps)
surface.loft Surface Loft
sections: [{sketch, curves?: [curve ids], profiles?} | {body, edges: [[x,y,z]]}] (2…50 in order; each one chain: a profile without holes, or curves meeting end to end; all open or all closed; a body edge chain takes the face the chain bounds as the surface the end repeats); continuity?: [g0|g1|g2|g3, g0|g1|g2|g3] (each end, default g0: how much of the surface at the first and last section the loft repeats — the tangent plane, the curvature, or how that curvature changes); crown?: [number, number] (default 0: how full each end leaves, -0.9 flattest to 3 fullest); name?, body_name? (a surface body: ruled between two sections, smooth through three or more; no caps)
surface.offset Offset Surface
faces: [[x,y,z]] (points on the faces); body?; distance: expr (signed, along the faces' normals; 0 copies the faces); chain?: bool (each pick's whole smooth chain of faces); tolerance?: expr (how far a fitted face may stray, default 0.01 mm). Planes and cylinders move exactly; other faces are fitted. A new surface body (a solid where its faces close)
surface.ruled Ruled Surface
body; edges: [[x,y,z]] (points on a chain of its edges, open or closed); distance: expr (how far the strip reaches); mode?: normal|tangent|angle|direction (default normal: along the normal of the face beside each edge; tangent: continuing it); angle?: expr (angle mode: from `direction`, else from the face's normal, turned away from the face; 90 deg from the normal is tangent); direction?: [x,y,z] (direction mode: the rulings; angle mode: the reference, e.g. a pull direction for a draft); face?: [x,y,z] (a point on the face the directions come from; default: the face beside the most picked edges); flip?: bool (the other side); corners?: mitre|round (sharp corners of the chain; inside corners are always cut back). Lines and arcs give exact planes, cylinders and cones, other edges a fitted ruled B-spline. A new surface body
surface.blend Blend Surface
from, to: {body, edges: [[x,y,z]]} (points on the edges of one chain of each body: two picks on the same edge is that one edge, more chain up); continuity?: [g0|g1|g2|g3, g0|g1|g2|g3] (each end, default g1: how much of the surface at the picked edges the blend repeats — the tangent plane, the curvature, or how that curvature changes); bulge?: [number, number] (default 0: how full each end leaves, -0.9 flattest to 3 fullest); align?: [[x,y,z], [x,y,z]] (a point each end leaves towards, when the faces at the picks do not say); stitch?: bool (sew the blend onto its two bodies where the boundaries meet, replacing them); name?, body_name?

SURFACE › MODIFY

surface.stitch Stitch
bodies: [names] (surfaces sewn into the first; a solid when they close); tolerance?: expr (default: tight)
surface.extend Extend
body: surface name; edges: [[x,y,z]] (points on boundary edges to push out); distance: expr (unless up_to); mode?: natural (the surface itself continued: exact for planes and surfaces of revolution, a B-spline's end spans continued; the default) | tangent (a ruled run-off face along each edge, G1) | curvature (a run-off face keeping the surface's curvature across the edge, G2); up_to?: plane (XY|XZ|YZ|plane name|{origin, normal}) | {body, point} (a face, its surface extended) | "bounds" (natural: back to the surface's own bounds, undoing a trim); neighbours?: bool (default true: the edges next to an extended edge are lengthened to meet it; false: the extension's sides run square to the edge)
surface.trim Trim
body: surface name; plane: XY|XZ|YZ|plane name|{origin, normal} or tool: {body, point} (a face, its surface extended); keep: [x,y,z] (a point on the side to keep)
surface.untrim Untrim
face: {body, point}; holes?: all|[[x,y,z]] (points on the inner loops to remove; default: all); outer?: bool (restore the outer boundary to the surface's natural bounds: a free-form surface's own, an analytic surface's span of the face); in_place?: bool (untrim a surface body's face where it is; a solid's face is always copied out). A surface body; the face keeps its name
surface.unstitch Unstitch
body; faces?: [[x,y,z]] (points on the faces to take out, each its own surface body; the rest stay together under the body's name; default: every face its own surface body). A solid comes apart into surfaces
surface.reverse_normal Reverse Normal
body (a surface); faces?: [[x,y,z]] (points on the faces to turn over; default: all of them)
surface.fair Fair Surface
body: surface name; faces?: [[x,y,z]] points on the faces to fair (default: every face); strength?: number (0..1 of the full fairing step, default 1); iterations?: number (1..1000 steps, default 1); keep_edges?: bool (default true: hold the boundary row and the row next to it, so a face keeps meeting its neighbours in position and in tangent); tolerance?: expr mm (how far a control vertex may move, default 0.001 of the body's size). Moves the interior control vertices of each B-spline face to flatten its curvature variation while the boundary stays put: the face keeps its edges and the body its shape within the tolerance, and the warning in the reply carries the energy before and after; name?
surface.fillet Surface Fillet
planned: a, b: {body, point} (two faces of separate bodies that meet or cross; the points pick the side the ball rolls on); radius: expr; trim?: both|first|none
surface.match Match Surface
body: surface name (the body whose face is rebuilt); faces?: [[x,y,z]] (points on that face, default: the body's first); target: body name (the body the seam must meet); edges: [[x,y,z]] (points on one edge chain of the target: the rebuilt boundary takes its place); order?: g1|g2|g3 (default g2: position and tangent plane, the curvature too, or how that curvature changes along the seam). The far boundary stays where it was and the body keeps its name

SHEET METAL › CREATE

sheet.flange Flange
base: sketch + profiles? (rule?, flip?) | contour: sketch + curves (open chain of lines) + distance (rule?, flip?, reverse?) | edge: edges: [[x,y,z] on top/bottom edges, or {point: [x,y,z], angle?, height?} for an edge with its own angle and height] + height (to the outer face), angle? (default 90 deg), radius? (default: rule), position?: inside|outside|middle, flip?, body?, corner_relief_shape?: notch|round|rectangular|tear and corner_relief? (size across): the relief at the corners these flanges make (default: the rule's); type?: base|edge|contour (default from the inputs); name?, body_name? (the new body). Thickness, K-factor and bend radius come from the rule (sheet.manage_rules); passing them here is refused, and so is the corner relief on a base or contour flange
sheet.perforate Perforate
diameter, pitch: expr; margin?: expr (clear of edges, cut-outs and bends; default: the diameter); pattern?: staggered (60°, default) | square; body? - a perforation field over the whole flat sheet: holes in the flat pattern (perforations), the DXF (layer PERFORATION) and the measured volume, not cut into the B-rep (#732)
sheet.hem Hem
edges: [[x,y,z] on sheet edges]; length (to the outer face); gap? (inner radius, default: rule); flip?; body?
sheet.fold Fold
line: sketch + curve (a sketch line on the sheet's base face; followed when the sketch changes) or points: [[x,y,z], [x,y,z]]; angle? (default 90 deg); radius? (default: rule); position?: centerline|start|end|mould (where the line sits in the bend, default centerline); fixed?: [x,y,z] on the side that stays (default: the larger side); flip? (fold the other way); body?
sheet.convert Convert to Sheet Metal
body; face: [x,y,z] on its large flat face (a plate of even thickness; recesses in one face up to half the thickness deep, such as an engraved label, become pockets of the sheet), or that face's name from model.faces; rule?; bends?: [[x,y,z] on sharp edges] (a solid or a shelled body: `face` is the fixed face and the flat faces reached from it across these edges become the sheet; a shell keeps its thickness, a solid takes the rule's inward; edges between two of those faces that are no bends are cut open with the rule's gap; a point in the middle of a chamfer between two faces, or on a bend modelled with its radius (a cylinder between two flat faces tangent to it, either skin), makes it one bend of the rule's radius at their virtual sharp; the faces' holes become cut-outs and their engravings, up to half the thickness deep, pockets)
sheet.flat_pattern Create Flat Pattern
body? → flat size, outline loops and cut-outs (flat coordinates, as point lists), cutout_shapes (the same cut-outs exactly, in the same order: {circle: {center, radius}} for a round hole, else {segments: [{line: [a, b]} | {arc: {center, radius, start_deg, sweep_deg}} | {polyline: [...]}]}), pockets (with their own cutout_shapes), bend lines and the bend table

SHEET METAL › MODIFY

sheet.unfold Unfold
body? (default: the last sheet body) — all bends
sheet.refold Refold
body? (default: the last unfolded sheet)
sheet.manage_rules Sheet Metal Rules
name (new or existing); thickness?, k_factor?, bend_radius?, relief_width?, relief_depth?, corner_relief?, hem_gap?, gap? (expressions; `Thickness` is the rule's; gap: between flanges that meet at a corner, whose ends are closed toward each other at any angle); corner_relief_shape?: notch|round|rectangular|tear (what is cut where two bends meet at a corner of the base: round and rectangular a relief `corner_relief` across; tear none, each bend's end is cut straight from the corner to its flange's end; default notch); active?: bool; delete?: bool

PLASTIC › CREATE

plastic.boss Boss
position: [x,y,z] on a face; direction? (default: out of the face); diameter, height; hole_diameter?, hole_depth? (default: to the face); draft? (angle), fillet? (root radius); ribs? (count), rib_thickness?, rib_length? (out from the wall), rib_offset? (below the top); body?
plastic.lip Lip
face: [x,y,z] on the rim face of a shelled body; width, height; type?: lip|groove; gap? (groove clearance); side?: inside|outside (which rim edge); body?
plastic.snap_fit Snap Fit
position: [x,y,z] on a face; direction? (default: out of the face); hook: [x,y,z] (the catch's direction); length, thickness, width, catch_depth, catch_length; body?
plastic.rest Rest
position: [x,y,z] on a face (the rest's centre); direction? (default: out of the face); width (round: the diameter); length? (a rectangle, along `along`); along?: [x,y,z]; height; draft? (angle; default: the body's plastic rule); thickness? (wall of a hollow rest); body?

PLASTIC › SETUP

plastic.manage_rules Manage Plastic Rules
name (library or new rule; a new one starts from `from`, default ABS (1.5mm)); from?; material?; thickness?, nominal_radius?, clearance?, knife_edge?, reveal_height?, thickness_variation?, draft?, max_thickness?, min_thickness?, min_draft? (expressions; `Thickness` is the rule's); active?: bool (rule for bodies without one); delete?: bool (a design rule; a library rule goes back to the library values)
plastic.assign_rule Assign Plastic Rule
bodies: [names]; rule: name (empty: no rule) — plastic features on these bodies take its draft and clearance as defaults

Other: sketch.*

sketch.edit Edit Sketch
sketch: id or name
sketch.draw.dimensioned Draw Dimensioned Sketch Geometry
command: sketch creation command, params: object, dimensions: object of role to numeric or expression value; creates geometry and all driving dimensions atomically in one undo step. Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.delete Delete Sketch Entities
entities: [curve, point or constraint ids]
sketch.move_point Drag Sketch Point
point: ref, to: [x,y]
sketch.drag Drag Sketch Geometry
entity: point or curve, from: [x,y] where it was grabbed, to: [x,y], live?: bool: a point goes to `to`, a line (spline, conic) slides by to - from, a circle or arc grabbed on its edge takes the radius to `to`; the rest moves as little as it can and keeps its solution branch (a long move is followed in short steps, each solved with the entity held; a step that cannot be solved that way is approached as far as it can be and the next ones tried; when none past it solves, the last one is left to the sketch's ordinary solve, which may pull it back or leave the sketch unsolved; a step that would sweep an arc through its start is undone and the drag ends there). Returns `reached`: how much of the way from `from` to `to` the geometry followed (0..1), and `at`: where the grabbed spot went (`from` moved as the dragged points did), the `from` of the next move. `live: true` (each frame of an interactive drag) solves the sketch once and leaves the features after it as they were (stale) until `sketch.drag_end` or any command that reads the model; `dof` is then the one from before the drag
sketch.drag_end End Sketch Drag
constraint?: {command: a sketch.constraint.* id, params}: ends a drag made of `sketch.drag` `live: true` frames: adds the constraint it let go on (not kept if it over-constrains the sketch), then evaluates the whole model once; returns the constraint's result and the sketch's solved state and degrees of freedom
sketch.dimension_text Move Dimension Text
dimension: constraint id or parameter name; at: [x,y] text centre (sketch coordinates) | reset: true (default place)
sketch.options Sketch Palette Options
sketch?: id|name (default active); any of show_profile, show_points, show_dimensions, show_constraints, show_projected, show_construction, grid, snap, slice, sketch_3d: bool. Returns them all
sketch.chain Chain
curve: id: the curves joined to it end to end (what a double-click selects)
sketch.solve Solve Sketch
reports the solver status and degrees of freedom
sketch.infinite Infinite Line
curves: [line ids], value?: bool (default toggles): infinite line type (#1359): construction geometry drawn across the whole view through the line's two points; off, a normal line
sketch.edit_text Edit Text
link: the text's link id (or entity: one of its curves), text?, at?, height?, angle?: deg (numbers or expressions as in sketch.text; a number replaces an expression, and so does moving the text), font?: family or file path (empty: the built-in font), bold?, italic?: bool (an installed family's bold or italic face; italic without one is slanted), align?: left|center|right (the lines against `at`, or along the path), letter_spacing?: extra mm between letters, line_spacing?: times the font's line distance (default 1), path?: a curve id of the sketch the baseline follows ("": none; `at` and `angle` then do not place the text; the curve becomes construction, a guide the letters stand on), reverse?: bool (the other way along the path) (each kept when left out); live?: bool: one frame of an interactive change (the sketch is solved, the features after it stay as they were until `sketch.drag_end`). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.toggle_driven Toggle Driven Dimension
constraint: dimension id, driven?: bool (default toggles); a driving dimension gets a parameter with its current value
sketch.glyphs Constraint Glyphs
sketch?: id|name: every constraint with where to draw its glyph (sketch coordinates)
sketch.snap Snap Inference
at: [x,y], from?: [x,y] (previous click), radius?: mm (snap distance, default 1): what a click there would snap to and infer
sketch.export_dxf Save As DXF
sketch?: id|name (default active); path?: file to write (else the DXF text is returned)
sketch.line3d 3D Line
points: [[x,y,z]…] world points (2 or more): one 3D line per segment, joined end to end (needs 3D Sketch on). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.spline3d 3D Spline
points: [[x,y,z]…] world fit points (2 or more): a smooth 3D curve through them (needs 3D Sketch on). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.point3d 3D Point
point: [x,y,z] world point (needs 3D Sketch on). Returns created: {points, curves, constraints, dimensions}: the ids of what it added (stable and never reused: usable right away in sketch.dimension, sketch.constraint.*, sketch.delete…)
sketch.move3d Move 3D Point
wire: drawn 3D curve or point id, index?: fit point (default 0), to: [x,y,z] | by: [dx,dy,dz]; points joined to it move too
sketch.offset.break Break Offset Association
curve: derived offset curve id (retains geometry and makes its points editable)
sketch.break_link Break Link
link?: link id (j1) | entities?: [curve or point ids]: linked geometry becomes normal sketch geometry
sketch.auto_project Auto-Project Edges on Reference
value?: bool (default toggles): project a face's edges when a sketch is created on it
sketch.redefine Redefine Sketch Plane
sketch: id or name; plane: as sketch.create; author_path?: exact owner occurrence ids; explicitly rebinds or freezes the plane while preserving geometry and dimension names
sketch.copy Copy Sketch Entities
entities?: [curve or point ids] (default: the selected sketch geometry); the constraints and dimensions among them come along
sketch.cut Cut Sketch Entities
entities?: [curve or point ids] (default: the selected sketch geometry): copies them as sketch.copy does, then deletes them (one undo step)
sketch.paste Paste Sketch Entities
at?: [x, y] (sketch point the copy's centre goes to) | translate?: [x, y]; without either, offset from the original in its own sketch and at the same coordinates in another; sketch?: target (default: the active sketch)
sketch.inspect Inspect Sketch
sketch?: id|name (default active)

Other: canvas.*

canvas.calibrate Calibrate Canvas
canvas: id or name; a, b: two points on the canvas plane [x,y]; distance: their true distance (mm): scales the image about a
canvas.delete Delete Canvas
canvas: id or name

Other: mesh.*

mesh.convert Convert Mesh
body: mesh body name; tolerance?: length expression (default 0.05 mm): reconstruct a closed constant-section mechanical mesh as editable planar and cylindrical faces, with a parametric timeline feature; name?

Other: sheet.*

sheet.rules List Sheet Metal Rules
→ rules with their expressions and values, and the active one
sheet.export_dxf Export Flat Pattern as DXF
body?, path?, curves?: exact|arcs (default exact: an ellipse as ELLIPSE, splines, text outlines and other Béziers as SPLINE; arcs: tangent arcs and lines within 0.001 mm, for machines that read only those), text?: cut|etch (default cut: letters that text cut through the sheet are cut contours on layer TEXT; etch: single contours on layer ETCH and the sheet keeps its material there; text machined to a depth is always on ETCH), bend_notes?: bool (default false: a note beside each bend line on layer BEND_NOTES, `B1 UP 90%%d R1`), note_height?: mm (default 3), per_body?: bool (a file for every sheet body, `<path>-<body>.dxf`, or their DXF texts without a path → files: [{body, path | dxf, bends}]; not with `body`) → DXF (AutoCAD 2000, mm): layers OUTLINE (the outer contour), CUT (what is cut out inside it), TEXT or ETCH (letters), BEND_UP and BEND_DOWN (dashed centre lines), BEND_NOTES, POCKET_<BOTTOM|TOP|INTERNAL>_Z<from>_TO_<to>_MM (one per side and depth) and PERFORATION; inner contours come before the outline
sheet.export_bend_table Export Bend Table
body?, format?: csv|json (default csv), path? → bend table in mm and degrees, including rule and flat centre-line coordinates; a bend that cut-outs split has a row for each piece

Other: plastic.*

plastic.rules List Plastic Rules
→ rules with their expressions and values, the active rule and the rules assigned to bodies

Other: component.*

component.from_bodies Create Components from Bodies
bodies: [names] → one new component per body, named after it
component.activate Activate Component
component: id or name (0 or "root" for the design); occurrence?, path?: exact placement used to author shared geometry
component.list List Components
compact?: bool (counts of bodies, features, sketches and construction planes instead of their names; occurrences leave out identity transforms; children as occurrence ids); bodies?: bool (with compact: body names, not their count)
component.properties Component Physical Properties
component?: id or name (default active); descendants?: bool (default true). Measures the first placement, or all placements for root, including pending moves; material-aware mass and center of mass in world coordinates
component.rename Rename Component
component, name
component.delete Delete Component
component: deletes it, its subcomponents, occurrences and features
component.unlock Unlock Contents
component: removes the rigid joints that hold its contents together (an imported assembly's rigid group), so its parts move and take joints one by one → joints (the ids removed)
component.move_bodies Move Bodies to Component
bodies: [names], component
component.move_sketches Move Sketches to Component
sketches: [ids or names], component
component.paste_new Paste New
component: independently copy its nested definition graph and history, materials and styles; occurrence?, path?: selected source placement; translate?: [x,y,z]. Reassigned external bodies become base geometry; retained external links and omitted boundary joints are reported
component.update_links Update Links
component?: id or name (default: every linked component) — reads the linked designs again and replaces their bodies where they changed
component.break_link Break Link
component: id or name of a linked component — keeps its bodies as they are and forgets the design file
component.links List Links
→ linked components: component, name, path, file (resolved), found

Other: occurrence.*

occurrence.properties Occurrence Physical Properties
occurrence: id or name; path?: [occurrence ids] (required if nested under multiple instances); descendants?: bool (default true). Physical properties of this placement in world coordinates, including pending moves
occurrence.copy Paste (Instance)
component (or occurrence): what to place again; path?: validates selected occurrence; parent?: component (default: the same parent); translate?: [x,y,z]. Copies the selected effective transform, including pending moves
occurrence.move Move Occurrence
occurrence; path?: exact placement; space?: local|world (default local); translate?: [x,y,z]; axis?: [x,y,z], angle?: radians or "30 deg", origin?: [x,y,z]; capture?: bool (default true; false keeps it pending until Capture Position). Nested occurrence definitions remain shared
occurrence.ground Ground
occurrence; grounded?: bool (default toggles)

Other: joint.*

joint.reach Reach Point
occurrence: id|name; point: [x,y,z] (where its point goes, world); at?: [x,y,z] (its point, in the world where it is now; default: the centre of its bodies' box); z?: [x,y,z] (the way its axis then points); axis?: [x,y,z] (that axis, in the world now; default: its own z); joints?: [ids or names] (only these move toward the point; the other joints of a closed loop they are in follow); quiet?: bool; continuous?: bool (a frame of a drag: the answer says continuous, and the app's command line doesn't echo it). Moves the values of the joints on its chain from where they are to the nearest pose, within their limits, through motion links, keeping closed loops closed as joint.drive does (contact sets are not checked) → reached; error_mm (and error_deg with z): how close it got; point: where its point is; values: [{joint, name, values}] of the joints that moved, as joint.list gives them; moved; stopped_by_limit: [{joint, value, limit: min|max}]: the limits it rests on short of the point; stopped_by_loop: {joint}: the closed loop that stopped it (its chain alone gets closer); reason: why nothing can move
joint.limits Joint Limits
joint; index?: value index (default 0); min?, max? (omit both to clear)
joint.edit Edit Joint
joint; type?, flip?, offset?, angle?, suppressed?, name?
joint.delete Delete Joint
joint: id|name (or origin: name, link: index)
joint.list List Joints
→ joints (type, occurrences, values, limits), origins, links, degrees of freedom, conflicts, floating: [{occurrences, joints}] (joint chains joined to nothing grounded: the solver places none of them, so driving them moves nothing)
joint.solve Solve Joints
re-place the occurrences from the joints → conflicts, errors, dof

Other: contact.*

contact.edit Edit Contact Set
set: id|name; occurrences?; name?; suppressed?: bool; delete?: bool
contact.list List Contact Sets
→ sets, enabled, all
contact.check Check Contact
→ pairs in contact sets that pass through each other now

Other: motion.*

motion.play Play Motion Study
study: id|name; step (0…steps) — sets the joints to the study's values there (contact sets stop them); quiet?: bool (positions of only the occurrences that moved) → values: [{joint, values: [{name, value, unit}]}], positions, moved: whether any occurrence moved, unmoved: [{joint, name, reason}] (keyed joints that can move nothing, such as a chain joined to nothing grounded)
motion.export Export Motion Study
study; samples? (default steps + 1); path? (.json or .csv) → occurrence positions per step (the design is not changed)
motion.export_animation Export Motion Animation
study: id|name, or joint: id|name with from and to (degrees for angles, mm for distances, or expressions) and index?; path: a .gif file, or a folder for PNG frames (frame-0001.png, frame-0002.png, …); samples? (frames, 2…1000; default the study's steps + 1, or 100); width?, height? (16…4096 pixels, default 800 × 500); camera?: {target, yaw, pitch, roll?, distance, fov?, up?} (ui.camera's reply; fields left out keep the default view: view.apply's camera, or the home view framing the model); fps? (1…50, default 20); grid?, axes? (default true: the ground grid and the origin's axes) - draws the study as it plays, or the joint as it is driven, with the headless renderer → path, format, frames, width, height, fps (GIF), bytes, renderer, stopped_at, stopped_by_loop, stopped_by_contact (the design is not changed)
motion.trace.keep Keep Motion Trace
occurrence: id|name, or an occurrence path [ids] (an instance inside sub-assemblies); point: [x,y,z] world point on it, where it is placed now; study: id|name, or joint: id|name with from and to (degrees for angles, mm for distances, or expressions) and index? (which value, default 0); samples? (2…500, default the study's steps + 1, or 100) - the point's path as the study plays or the joint is driven, closed loops following; name? (default Motion TraceN) - keeps the trace as a 3D sketch spline through its points (a new sketch with 3D Sketch on, in the root component, where no joint moves it; a fixed curve, it does not follow later changes) → sketch, name, curves, points
motion.plot Plot Motion Study
study: id|name; joints?: [id|name] (default: every joint that moves); occurrence? and point? (a point of a part to follow, as motion.trace takes them); samples? (3…1000, default the study's steps + 1); duration?: seconds the whole study takes, 0.001 or more (velocities and accelerations then per second, else per step) → step: [the study step of each sample], time?: [s], joints: [{joint, name, index, dof, unit, value, velocity, acceleration, velocity_unit, acceleration_unit}] (degrees for angles, mm for distances; angles unwrapped), point?: {occurrence, position: [[x,y,z]…], velocity, acceleration (vectors), speed, acceleration_norm, unit, velocity_unit, acceleration_unit}, samples (taken), stopped_at, stopped_by_loop, stopped_by_contact. The study plays as motion.play plays it, each sample driven from the one before, on a copy (the design is not changed); velocities and accelerations are finite differences between samples (central, one-sided at the ends)
motion.interference Motion Interference
study: id|name; occurrences?: [ids or names] (two or more, checked against each other; default every occurrence), with against?: [ids or names] (then each of `occurrences` is checked only against these, such as an arm against the parts it must miss), or contact_sets?: true (the pairs of the design's contact sets); samples? (2…1000, default the study's steps + 1) → collisions: [{a, b, first_step, last_step, steps: [[from, to]…] (the step ranges where they overlap), depth_mm (how far into each other, the most at deepest_step), volume_mm3 (their overlap there; null when it was not cheap to work out)}], clear, pairs (checked), samples (taken), truncated (the work budget ran out; checked_to: the last step checked), stopped_at, stopped_by_loop. The study plays as motion.play plays it but contact sets do not stop it, on a copy (the design is not changed). Parts are tested at the samples only: one that passes wholly through another between two samples is missed
motion.list List Motion Studies
motion.delete Delete Motion Study
study

Other: explode.*

explode.show Show Exploded View
view: id|name (or none: back to the assembled placement) — shown only; the design keeps its placements
explode.list List Exploded Views
explode.delete Delete Exploded View
view

Other: config.*

config.column Configuration Column
param? | feature? | material? | appearance? (target name); delete?: bool
config.row Configuration Row
name; from? (row to copy; default current values); values?: {column key: expression, suppression, material name, appearance name or Look object}; rename?; delete?: bool
config.activate Activate Configuration
row: name — sets its parameter values and suppressions
config.preview Preview Configuration
row: name — validates a rebuild without changing the design or history
config.rule Configuration Rule
rule?: {id,name,enabled,condition,effect}; id? + delete?; id? + index? (ordered move)
config.rules Configuration Rules
ordered typed rules, rows and active state

Other: parts.*

parts.library Standard Parts
family? → families (name, standard, sizes, lengths) and, with family, each size's dimensions (mm)
parts.insert Insert Part
family (socket_head_cap_screw | hex_bolt | hex_nut | washer | set_screw | dowel_pin | bearing); size ("M6", or "608" for bearings); length? (mm; screws, bolts, set screws, pins; default a standard length near 2.5 d); at?: [x,y,z] on a hole's rim or wall (the part seats on the hole's face with a rigid joint) | point?: [x,y,z] with direction?: [x,y,z] (no joint); name?
parts.resize Change Part Size
component: id|name of an inserted part; size?; length? — rebuilds it (joints keep it seated)

Other: body.*

body.rename Rename Body
body: its name, name: the new name (features that use the body follow)

Other: browser.*

browser.group New Group
folder: bodies|sketches|construction; component?: id (default 0); name?; items?: [keys] (they leave other groups)
browser.ungroup Ungroup
group: id (its items go back to the folder)
browser.rename_group Rename Group
group: id, name
browser.move Move Browser Items
folder, component?, items: [keys]; group?: id (into it; omit to take them out of groups); before?: key (position in the group)
browser.order Order Browser Items
folder, component?, order: [keys] (the folder's items in display order)
browser.visibility Show/Hide
visible: bool; items?: [sketch id or name | body name | construction name | joint name | O|X|Y|Z|XY|XZ|YZ]; or joints?: [joint id or name] (their glyphs; they still constrain and move parts); or folder?: bodies|sketches|construction|origin|joints (all of it); or paths?: [[occurrence ids]] (exact placements and descendants), isolate?: bool (requires paths and visible:true). Saved with the design; not an undo step

Other: document.*

document.units Change Design Units
units: mm|cm|m|in|ft (display and unit-less parameters; values keep their meaning)
document.metadata Design Properties
→ metadata: the design's metadata object as saved (other tools' keys too); properties: project, part_number, revision, author, organization, description and license, each its text or null (absent, or not text)
document.metadata.set Change Design Properties
key and value, or values: {key: value, …} (all or nothing, one undo step). SolidCraft's keys: project, part_number, revision, author, organization, description, license (text; "" or null removes); another tool's data goes under its reverse-DNS key such as com.example.tool (an object; null removes) → metadata, changed: [keys]
document.metadata.remove Remove Design Property
key, or keys: [keys] (any key, also one another tool wrote) → metadata, removed: [keys that were there]
document.inspect Inspect Design
measure?: bool (include body measurements)

Other: view.*

view.save New Named View
name?; camera: {target: [x,y,z], yaw, pitch, distance, fov?} (replaces a view of the same name)
view.rename Rename Named View
view: name, name
view.delete Delete Named View
view: name
view.list List Named Views
view.apply Restore Named View
view?: front|back|top|bottom|left|right|iso|home (frames the model) | a named view's name; or camera?: {target: [x,y,z], yaw, pitch, distance, fov?} (radians, mm) → camera. The viewport (and the MCP screenshot) moves there. View state: not saved, not an undo step
view.navigate Navigate View
camera: Camera; direction?: [x,y,z] in the camera's up-axis frame; or action: left|right|up|down|clockwise|counterclockwise|home|fit, degrees?: 0..180 (how far left|right|up|down turn; default 90); or motion: pan|orbit|zoom, delta?: [dx,dy] (pixels, each ±10000), viewport?: [width,height] (1..1000000, required for pan or pivot), pivot?: [x,y,z], factor?: 0.05..20 (required for zoom), anchor?: [x,y,z] → camera, fit, continuous?

Other: selection.*

selection.delete Delete
items?: [selection items]; components?, occurrences?, canvases?: [ids or names]; dry_run?: bool → deleted, would_fail, skipped (one undo step)

Other: edit.*

edit.undo Undo (Ctrl+Z)
edit.redo Redo (Ctrl+Y)
edit.checkpoint Checkpoint
→ {checkpoint: id}: remember the design, active sketch and undo history (restore with edit.restore_checkpoint)
edit.restore_checkpoint Restore Checkpoint
checkpoint: id; forget?: bool (true = drop it without going back). Goes back to it, undo history included

Other: timeline.*

timeline.rename Rename
feature: id|name, name (references to it follow)
timeline.group New Feature Folder
name?; features?: [id|name]; parent?: folder id (features leave any other timeline folder)
timeline.ungroup Remove Feature Folders
group: id | groups: [ids] (features remain in the timeline)
timeline.rename_group Rename Feature Folder
group: id, name
timeline.move_to_group Move Features to Folder
features?: [id|name], groups?: [ids], group?: id (omit or null to move to the timeline root)
timeline.move_many Move Timeline Items
features?: [id|name], groups?: [folder ids], group?: folder id, position: insertion slot; atomically changes folder membership and moves all selected contents as one block
timeline.rollback Move Timeline Marker
position: number of features to keep active (omit = end)
timeline.roll_to Roll History Marker
position: number of features to keep active (omit = end) | feature: id|name (the marker goes right after it)
timeline.reorder Reorder Feature
feature: id|name, position: its new index; refused when a feature that worked would fail
timeline.reorder_many Reorder Features
features: [id|name], position: insertion slot in the current history; selected features keep their relative order; refused when a feature that worked would fail
timeline.redefine Edit Feature
feature: id|name, command: the feature's command id, params: its parameters (the feature is rebuilt in place)
timeline.dependents Feature Dependents
feature: id|name → features deleted with it, and features that would fail without it
timeline.suppress Suppress Feature
feature: id|name, suppressed?: bool (default toggles)
timeline.edit Edit Feature
feature: id|name, set: {fields to change, merged into the feature's definition as timeline.inspect returns it, e.g. {"extent": {"distance": "30"}} (extrude), {"angle": "90 deg"} (revolve); expressions are text} → recomputed: features rebuilt, restored: features whose earlier result for the same inputs was reused
timeline.inspect Inspect Feature
feature: id|name → type, definition (the fields timeline.edit's set changes, with their current values), inputs: [{label, param, expression, unit}] (named inputs parameters.change can also set), error, warning
timeline.copy Copy Features
features: [ids or names] (in timeline order on paste)
timeline.paste Paste Features
translate?: [x,y,z] (moves the copies' geometry); the copies go at the marker
timeline.add Add Recorded Feature
feature: a feature as the design file and timeline.inspect hold it ({type, name?, id?, …}; id and name are kept when free, so later steps can refer to them); params?: [{name, expression, unit?, comment?}] (the model parameters its sketch dimensions use); the feature goes at the marker → feature, name, error, warning
timeline.export_script Export Command Script
path?: write the script to this file → script: {commands: [...]} that rebuilds the design (solidcraft-cli eval/run), steps, omitted: what the script leaves out (appearances, folders, views, configurations); components and assemblies are not supported yet

Other: select.*

select.set Select
items: [{type: body|edge|face|feature|sketch_curve|sketch_point|profile, …}], add?: bool
select.clear Clear Selection

Other: parameters.*

parameters.list List Parameters
favorites?: bool (only favourites), filter?: all|user|sketch|feature|favorites → parameters (name, expression, unit, value in its unit, source, feature/input, comment, favorite, uses, used_by, error) and cycles
parameters.add Add User Parameter
name, expression, unit?, comment?, favorite?: bool
parameters.rename Rename Parameter
name, new_name (expressions, feature inputs and dimensions that use it follow)
parameters.delete Delete Parameter
name (refused while something uses it; the error lists the users)
parameters.favorite Favourite Parameter
name, favorite?: bool (default true)
parameters.move Move Parameter
name, before | after: another user parameter; the user parameter is listed just before or after it
parameters.comment Comment Parameter
name, comment
parameters.users Parameter Users
name → users (parameters, feature inputs, dimensions) and the features it drives
parameters.graph Parameter Graph
→ nodes, edges [user, used] (users include Feature:<name>), cycles, errors
parameters.export Export Parameters
format?: csv|json (default csv, or from the path), path?: write to a file → text
parameters.import Import Parameters
text: CSV (header with name, expression, unit?, comment?) or JSON [{name, expression, unit?, comment?}] | path; all or nothing
parameters.complete Complete Expression
prefix?: the text before the cursor → word, suggestions [{text, kind: parameter|function|unit|constant, detail}]

Other: expr.*

expr.evaluate Evaluate Expression
expression, kind?: length|angle|unitless (or unit?: mm|in|deg…) → ok, value (mm/rad), display_value, references, error

Other: file.*

file.new New Design (Ctrl+N)
name?
file.save Save (Ctrl+S)
path? (default: current file); format?: container|json (default: json for .json, otherwise container); compression?: fast|compact (default: fast); cache?: bool (warm native geometry, default: false); preview?: bool (saved display meshes, default: false)
file.save_as Save As
path; format?: container|json (default: json for .json, otherwise container); compression?: fast|compact (default: fast); cache?: bool (warm native geometry, default: false); preview?: bool (saved display meshes, default: false)
file.export Export
path; format?: stl|stla|obj|step|3mf|3mf-tagged|urdf|json (default from extension; 3mf-tagged: 3MF whose triangles carry their B-rep face, at full precision, for meshing and analysis tools; docs/formats/3mf-face-tags.md; urdf: the whole assembly as a robot, with STL meshes written next to it; docs/urdf.md); bodies?: [names] (JSON and URDF export the complete design); urdf only: mesh_prefix? (before each mesh file name, e.g. package://robot/meshes/), effort? (default 1000), velocity? (default 10)
file.save_mesh Save As Mesh
path; format?: stl|3mf|3mf-tagged (default from the extension, else stl; 3mf-tagged: docs/formats/3mf-face-tags.md); bodies?: [names] (default: all); ascii?: bool (STL); slicer?: id, name or program path from file.slicers (open the saved file there)
file.slicers Installed Slicers
``→ the slicers found on this machine: [{id, name, icon?}]; pass an id or name as file.save_mesh’s `slicer```
file.export_view_dxf Export Current View as DXF
camera: Camera (current view); hidden?: omit|dashed (default omit); tolerance?: 0.0001..1 mm (curve chord tolerance, default 0.01); path?: .dxf file (else returns dxf text). Visible placed bodies only; 2D LINE/LWPOLYLINE entities on VISIBLE/HIDDEN layers, mm; perspective projected onto the camera target plane; no viewport crop or overlays.

Other: doc.*

doc.open Open (Ctrl+O)
path: .solidcraft design, or a .step/.stp/.igs/.fcstd/.3dm/.3mf/.stl/.obj/.glb/.gltf file (STEP, IGES, FreeCAD, Rhino, 3MF, STL, OBJ or glTF; opens as a new design holding the file as a component named after it, as file.insert_step and file.insert_mesh make); up?: z|y for a STEP, IGES, FreeCAD, Rhino or glTF file (see file.insert_step and file.insert_mesh); names?: solid|product|instance for a STEP, IGES, FreeCAD or Rhino file (see file.insert_step)
doc.recovery_list Recoverable Designs
dir? (default: the recovery folder) → designs autosaved by apps that crashed or closed with unsaved changes
doc.recover Recover Design
id (from doc.recovery_list); dir?; discard?: bool (delete the entry once open) — opens it with its file path, unsaved
doc.recovery_discard Discard Recovered Design
id, or all: true; dir?

Other: model.*

model.edges List Edges
body: name
model.faces List Faces
body: name → per face: index, name (what face.delete, sheet.convert `face`, solid.shell … take in place of a point), exact, area, centroid (not always on the face), plane_normal, point (a point on the face that picks it), cylinder? ({origin, axis, radius} of a cylindrical face)
model.threads List Threads

Other: appearance.*

appearance.library Appearance Library
→ the built-in appearances (name, colour, opacity)
appearance.list List Appearances
body?: name → assigned appearances; with body, its resolved look and its faces' (face index, look)

Other: material.*

material.list List Materials
→ the built-in materials, then the design's own (user: true, with their look)
material.create New Physical Material
name (not a built-in material's); density_g_cm3: (0, 1000]; appearance?: library name (appearance.library) | color?: "#rrggbb" or [r, g, b] (0–255), opacity? (0–1), pbr?: {metallic:0..1, roughness:0.045..1, dielectric_ior:1..3} (opaque only, needs color/appearance): the default look. Optical edits do not change density. Assign it with material.assign
material.edit Edit Physical Material
material: a material defined in this design; name? (bodies and configuration cells follow); density_g_cm3?; appearance? | color?, opacity?, pbr? (as material.create; color: null clears the look). Omitted appearance/color retains the entire current look
material.delete Delete Physical Material
material: a material defined in this design; replace?: material for the bodies and configuration cells that use it (without it, a material in use is refused)
material.properties.validate Validate Physical Material Data
card: schema_version 1 engineering material card in SI units. Returns numerical consistency, derived isotropic moduli, missing conditions and sources needing review. Read-only; does not assign/save properties or provide an analysis solver. See docs/physical-material-cards.md
material.properties.directional Directional Elastic Modulus
card: schema_version 1 engineering material card; direction: three finite nonzero-vector components in the card's material-local axes. Returns normalized direction, Young modulus in Pa and source/condition review. Read-only constitutive query; no structural solver, persistence or body-axis assignment. See docs/physical-material-cards.md

Other: engine.*

engine.commands List Commands

Other: inspect.*

inspect.compare Compare Bodies
a, b: body names (default: the two selected bodies, or the design's only two), in world placement; tolerance?: mm (0.001 to 10, default 0.01): surfaces closer than this agree; spacing?: mm (default 0.5): the largest piece of a face sampled as one point, coarser for a body that would need more than max_points? (default 8 million, up to 50 million) samples; max_regions? (default 50); color?: true | {only_in_a?, only_in_b?: "#rrggbb"} (colours the faces that hold a region, red where only a has material and green where only b has: the faces mostly beyond the tolerance, else the one with the largest share; an undo step) → a, b: volume_mm3, area_mm2, center_of_mass, bbox; difference: b − a; deviation: a_to_b, b_to_a (max_mm, mean_mm, at, area_beyond_mm2); regions, largest first: side (only_in_a | only_in_b), volume_mm3 (integrated along lines through the region: resolution), area_mm2, max_deviation_mm, at, center, bbox, faces_a, faces_b (face indices, as model.faces lists them); identical; verdict; warnings (a body whose surface does not enclose what it measures, lines left out). Works from the two surfaces, without a boolean of the bodies, so near-identical bodies compare too

Other: library.*

library.inspect Inspect Local Library
path: scalar library JSON; returns validated catalog and exact entry revisions, without changing the design
library.export Export Design Library
path: .json; id? (default user.local), name?, provenance?, overwrite? false. Copies assigned looks and design-local physical definitions; never changes the design
library.apply Apply Local Library Entry
path, entry: qualified ID, revision: exact content SHA-256; targets?: {bodies?, faces?: [{body,point}], components?}; name?: physical material name on import. Copies values in one undo step; material conflicts are explicit

Other: diagnostics.*

diagnostics.crash_reports Crash Reports
``limit?: number (default 20). Lists this computer’s crash reports, newest first: {dir, reports: [{id, kind, time, message, command, count, version, path, replayable}]}. kind: command_panic | panic | kernel_panic_recovered | unclean_exit. Read one with diagnostics.crash_report; reproduce it with `solidcraft-cli crashes replay ```
diagnostics.crash_report Crash Report
id: report id. The whole report: message, location, backtrace, app version and commit, system, the command that crashed and the recent ones, notes, and design_path / replay_path when the crash can be replayed (`solidcraft-cli run <replay_path> --in <design_path>`)
diagnostics.crash_reports.clear Delete Crash Reports
id?: one report (default: all). Returns {deleted}
diagnostics.crash_test Crash Test
mode: panic | kernel | abort. Checks that crash reports work: panic = an internal error in this command (caught; the design is unchanged), kernel = one inside the geometry kernel (caught), abort = the app ends at once (reported at the next start). Only when the SOLIDCRAFT_CRASH_TEST environment variable is set

Other: render.*

render.preflight Check Render Request
setup?: saved name OR settings?: full RenderSetup; transparent_background?: false; replace?: false. Validates the installed image host and bounded captured product scene without starting work. Stale geometry is rejected. See docs/render-jobs.md
render.start Render Image
Same request as render.preflight. Captures an immutable product scene and queues a bounded image job. Returns its session-scoped job identity, captured scene_generation and progress. Does not change the design. See docs/render-jobs.md
render.status Render Progress
job: {session, serial, generation}. Non-blocking progress, error and completed frame metadata; no image bytes and no rendering in this call.
render.cancel Cancel Render
job: {session, serial, generation}. Requests cooperative cancellation; completed jobs remain completed. Late cancelled frames cannot be published.
render.export Export Render Image
job: {session, serial, generation}, path: PNG destination, overwrite?: false. Exports a retained completed image atomically; an existing destination is preserved on failure. See docs/render-jobs.md
render.backends Render Backends
No parameters. Returns {schema_version: 1, default_backend: builtin, backends: [{id, label, availability, executors: [{id, availability, profiles, limits, scratch}]}]}. Metadata only; does not start rendering or probe a GPU. See docs/render-backends.md
render.settings.get Render Settings
name?: saved setup. Without name returns {setups, defaults}; with name returns {name, setup}. Does not evaluate the model or apply a camera. See docs/render-settings.md
render.settings.set Save Render Settings
name: setup name, set: object of fields to replace (backend, mode, camera, width, height, format, exposure_ev, environment_rotation, environment_intensity, background). Creates from defaults, validates atomically, one undo step; identical edits are no-ops. See docs/render-settings.md
render.scene Inspect Render Scene
No parameters. Authoritative product-scene metadata, without modelling overlays or mesh payloads. Explicitly settles stale geometry; does not render an image. See docs/render-workspace.md
render.settings.apply Apply Render Camera
name: saved setup. Applies its existing Camera snapshot including roll/up as view state, without modifying the document or starting a render.