SolidCraft

Parameter	Type	Required	Description
name		No
occurrence	id\|name	No	default: from the pick, or the named face's component
path	[occurrence ids from the root]	No	the placement picked on, ending at the occurrence: a part in a sub-assembly placed more than once is then on that copy; default: the occurrence's first placement, or with no occurrence the placement nearest the pick
face	[x,y,z] \| "<name>"	Yes	centre of a planar face
circle	[x,y,z] \| "<name>"	Yes	centre of a round end: a point on its wall or rim, the end's centre, or the round face's name as model.faces lists it
edge	[x,y,z]	Yes	a point on an edge of a planar face: the edge's middle, z out of the face, y into it; on?: [x,y,z] a point on the face (default: the larger planar face beside the edge); corner?: [x,y,z] near one end: the corner there, x and y along its two edges into the face; found again by name, so it follows the face as it changes size; z?: [x,y,z] the frame's z instead of the face's normal, along the edge when it runs that way, x chosen from z: an edge or corner picked as it is, kept as a point where it can't be found by name
point	[x,y,z]	Yes
z	[x,y,z]	No
plane	"XY"\|"XZ"\|"YZ"\|"o:<ids>/origin/<item>"\|"<name>"	Yes
axis	"X"\|"Y"\|"Z"\|"o:<ids>/origin/<item>"\|"<name>"	Yes
body	the named face's body	No
end	"<name>"	No	a circle's end: the face across its rim there; default the end nearer the pick

Automation details

Command ID: joint.origin

Parameters:

name?, occurrence?: id|name (default: from the pick, or the named face's component), path?: [occurrence ids from the root] (the placement picked on, ending at the occurrence: a part in a sub-assembly placed more than once is then on that copy; default: the occurrence's first placement, or with no occurrence the placement nearest the pick), face: [x,y,z] | "<name>" (centre of a planar face) | circle: [x,y,z] | "<name>" (centre of a round end: a point on its wall or rim, the end's centre, or the round face's name as model.faces lists it) | edge: [x,y,z] (a point on an edge of a planar face: the edge's middle, z out of the face, y into it; on?: [x,y,z] a point on the face (default: the larger planar face beside the edge); corner?: [x,y,z] near one end: the corner there, x and y along its two edges into the face; found again by name, so it follows the face as it changes size; z?: [x,y,z] the frame's z instead of the face's normal, along the edge when it runs that way, x chosen from z: an edge or corner picked as it is, kept as a point where it can't be found by name) | point: [x,y,z], z?: [x,y,z] | plane: "XY"|"XZ"|"YZ"|"o:<ids>/origin/<item>"|"<name>" | axis: "X"|"Y"|"Z"|"o:<ids>/origin/<item>"|"<name>"; a circle's z?: [x,y,z] (a round edge's centre with the way out of it: its end by name when that is the frame it shows, else a point there); body?: the named face's body; end?: "<name>" (a circle's end: the face across its rim there; default the end nearer the pick); x?: [x,y,z] (a direction, world) | "<face name>" | {face: [x,y,z]} (the frame's x: a direction, a plane's normal, or the way to another hole's axis; keeps a round origin's turn; a point's x is a direction, laid square to its z, default: chosen from z alone). Faces are kept by name: the origin follows its face, and a circle its end, when the design changes

SOLID › INSERT

Insert Point Cloud

Command group: SOLID › INSERT

Read the solid features guide.

Automation details

Command ID: pointcloud.insert

Parameters:

path: .ply, .xyz or .pts file (its points join the design as a point cloud: drawn as points, never a body; a PLY's red, green and blue are its colours, its other properties can colour and filter it; its edge and face elements become segments and triangles, a segment with width and height properties drawn as a bead) → cloud, name, points, segments, triangles, source_points, bounds, warnings; name?; units?: mm|cm|m|in|ft (the file's length unit, default mm); max_points?: most points kept (default 5000000, at most 20000000; a larger file is thinned evenly); center?: bool (move the cloud so the middle of its base sits at the origin); point_size?: pixels (0.5…16, default 2); color_by?: file|single|height or a property's name (the file's colours, the default; one colour; a ramp by height, blue low to red high; or by any property of the file, a ramp over its values or a palette for whole numbers); color?: [r, g, b] 0…1 (the single colour; given alone it sets color_by single, null sets color_by file); color_range?: [low, high] the ramp runs between (design Z in mm by height), or null for the automatic range (by height all but the lowest and highest 2 % of the points; by a property the values it takes over what the filters keep); height_range?: the same as color_range; filters?: [{property, range: [low, high]} or {property, values: [whole numbers]} for a property with named values], or null (only what every filter keeps is shown)

Insert Fastener

Command group: SOLID › INSERT

Read the solid features guide.

Automation details

Command ID: parts.fastener

Parameters:

the Insert Part dialog's command (same as parts.insert): family, size, length?, at?|point?+direction? (from the shank's tip toward the head), flip?, name?

Insert STEP

Command group: SOLID › INSERT

Read the import and export guide.

Parameter	Type	Required	Description
folder	bool	No	default false; true: an import that brings more than one item into the history (its Import feature and the rigid joints holding its parts) goes into a new history folder named `Group #N`
name		No	the feature's and the component's
up	z\|y	No	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	auto\|solid\|product\|instance	No	default auto: keep meaningful solid names, replace placeholders with the nearest named product, else instance; solid: the solid's own name; product: the part's name; instance: the occurrence's name, else the product's
history	features\|solids for a FreeCAD file	No	default features: its sketches and the Pad, Pocket, Revolution, Groove, Fillet, Chamfer and primitive features that use them are rebuilt as features in the new component, when every one can be and they build what the file holds → features_added, history: "features"; else, or with solids, the file's solids come in as an Import feature, and a warning says why the history was not rebuilt
matrix	[12 or 16 numbers]	No	where the new component's occurrence sits in the active component, after `up`: a rigid row-major 3x4 rotation-and-translation or 4x4 matrix, flat or as rows, as occurrence.move takes it; a scale, shear or mirror is refused before the file is read
tolerance		No	see occurrence.move

Automation details

Command ID: file.insert_step

Parameters:

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?, group?: the folder); folder?: bool (default false; true: an import that brings more than one item into the history (its Import feature and the rigid joints holding its parts) goes into a new history folder named `Group #N`); 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?: auto|solid|product|instance (default auto: keep meaningful solid names, replace placeholders with the nearest named product, else instance; solid: the solid's own name; product: the part's name; instance: the occurrence's name, else the product's); history?: features|solids for a FreeCAD file (default features: its sketches and the Pad, Pocket, Revolution, Groove, Fillet, Chamfer and primitive features that use them are rebuilt as features in the new component, when every one can be and they build what the file holds → features_added, history: "features"; else, or with solids, the file's solids come in as an Import feature, and a warning says why the history was not rebuilt); matrix?: [12 or 16 numbers] (where the new component's occurrence sits in the active component, after `up`: a rigid row-major 3x4 rotation-and-translation or 4x4 matrix, flat or as rows, as occurrence.move takes it; a scale, shear or mirror is refused before the file is read); tolerance? (see occurrence.move)

Insert Mesh

Command group: SOLID › INSERT

Read the import and export guide.

Parameter	Type	Required	Description
name		No
up	z\|y for a glTF file	No	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
origin	bool	No	default false: the mesh keeps its file's coordinates; true: once read, scaled and stood up, the import's occurrence is moved so the box around its bodies is centred on X and Y of the active component with its lowest point on Z = 0 → moved_to_origin: [x, y, z], the shift made
crease_angle_degrees	0..180	No	0 clears imported shading normals for the previous flat-shading behavior; positive angles regenerate angle-weighted normals across manifold edges below this crease angle; omitted keeps authored OBJ normals/smoothing groups, or flat shading when absent; geometry stays unchanged

Automation details

Command ID: file.insert_mesh

Parameters:

path: .3mf, .stl, .obj, .ply (with faces), .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); units?: mm|cm|m|in|ft for an STL or OBJ file, or a PLY file with faces (default mm): the unit its coordinates are in, scaled to millimetres as the file is read (a 3MF or glTF file states its own). The design keeps the millimetre mesh and not the unit, so insert the file again to try another; origin?: bool (default false: the mesh keeps its file's coordinates; true: once read, scaled and stood up, the import's occurrence is moved so the box around its bodies is centred on X and Y of the active component with its lowest point on Z = 0 → moved_to_origin: [x, y, z], the shift made); crease_angle_degrees?: 0..180 (0 clears imported shading normals for the previous flat-shading behavior; positive angles regenerate angle-weighted normals across manifold edges below this crease angle; omitted keeps authored OBJ normals/smoothing groups, or flat shading when absent; geometry stays unchanged)

SOLID › MODIFY

Fillet

Command group: SOLID › MODIFY

Default keyboard shortcut: F

Round the edges of a solid: the “R.03 typ” or “break all edges R.015” callout on a print, or the corner radius left in a pocket by the end mill. You pick the edges and the radius.

Before you start

You need a solid body with edges to round.
Pick edges one at a time, or click a face to round every edge around it.
Round the larger radii first. Do the vertical corners of a block before its top edges, so the small top round runs smoothly around the big corner.
An inside corner on a milled part can’t be sharper than the cutter. Make inside radii a little larger than the end mill’s radius, so the tool doesn’t bury itself in the corner.

Options

Choice in the dialog	Meaning	Example or reason to choose it
Edges	The edges to round. Click edges one by one, or click a face to take all of its edges.	The four vertical corners of a block, or the top face.
Radius	The radius of the round. A new fillet starts at 2 mm, shown in the design’s unit.	0.03 in for a typical edge break.
Type	Constant radius: one radius all along the edge. Chord length: the width across the round stays the same whatever angle the faces meet at. Variable radius: a radius at each end, and more along the edge if you add them. Curvature continuous: a smoother section where it meets flat faces (G2). Spline: the radius follows control radii you set along the edge.	Constant radius for almost everything on a machined part. Variable radius for a round that has to grow along an edge.
Corners (Constant radius)	Shown when three or more of the picked edges meet at one corner, such as rounding every edge of a block in one Fillet. Tangent makes a rolling-ball corner. Curvature makes a smooth patch set back along each edge, with a Setback box.	Leave it on Tangent. That is the corner a ball end mill leaves.
Face limits (Constant radius)	What happens when the radius is too big for the faces beside an edge. Exact radius stops and says why. Largest radius rounds every edge with the largest radius that fits, and shows the Applied Radius. Narrowed radius keeps the radius and narrows the round only where the faces run out.	Leave it on Exact radius, so a radius that doesn’t fit is caught instead of quietly changed.
Turns (Constant radius)	Where two rounds turn around a sharp corner edge, such as the rounds along the base of a boss at its upright edges. Mitre runs the rounds on until they meet. Swept turns them around the corner edge.	Mitre unless you want the corner rolled around.
End Radius, Swap Ends, Mid Radius (Variable radius)	The radius at the far end of the first edge, which end gets the start radius, and extra radii along the edge (Add Mid Radius). Smooth radius change blends between them instead of running straight.	A round that goes from 0.06 in at one end to 0.25 in at the other.
Tangent chain	Follows the edge around smooth (tangent) bends, so one pick rounds the whole run.	Leave it on for edges that flow into an existing round.
Preview	Shows the round on the part while you set it up.	Leave it on.

Try it: round the corners and break the top edges of a plate

Make a 3 in × 2 in × 0.75 in block (sketch a rectangle, Extrude 0.75 in).
Click Fillet and click the four vertical corner edges. Set Radius to 0.25 in and click OK.
Click Fillet again and click the top face. Edges shows 8 selected: the four straight edges and the four rounded corners.
Set Radius to 0.03 in and click OK. The top edge has a 0.03 in round all the way around.

Tips and common mistakes

Do type the unit with the number when the print uses another unit. In a millimetre design, typing 0.03 in enters 0.762 mm.
Do round all the edges of one size in a single Fillet. It’s one feature to change when the print changes.
Do round the big corners before the small edge breaks. Done the other way, the small round has to turn a sharp corner and can fail or leave an odd shape.
Don’t make a round bigger than the faces beside it allow. With Face limits on Exact radius, the dialog says “The radius is too large for the faces beside these edges” and OK stays grayed out; use a smaller radius, or set Face limits to Largest radius.
Don’t model a round you’ll never see just to look finished. Every fillet adds rebuild time and can get in the way of later features.

Chamfer

Command group: SOLID › MODIFY

Cut a flat bevel along edges of a solid: the “break all edges” or “0.03 × 45°” callout on a print. You pick the edges and how the chamfer is sized.

Before you start

You need a solid body with edges to chamfer.
Pick edges one at a time, or click a face to chamfer every edge around it.
Chamfer edges before you add other features that touch them. An edge that already meets a small chamfer or fillet has little room left, and a chamfer there can fail.

Options

Choice in the dialog	Meaning	Example or reason to choose it
Edges	The edges to chamfer. Click edges one by one, or click a face to take all of its edges.	The four top edges of a block, or the top face.
Chamfer Type	Equal Distance: the same leg on both faces. That is a 45° chamfer only where the faces meet at 90°. Two Distances: a different leg on each face. Distance and Angle: one leg and an angle.	Equal Distance for a standard edge break on a square corner. Distance and Angle whenever the print gives an angle, like 0.06 × 30°, and for any chamfer on a sloped face.
Distance (Equal Distance)	The leg length on both faces.	0.03 in for a typical edge break.
Distance 1 and Distance 2 (Two Distances)	The leg on each face.	0.06 in by 0.03 in.
Distance 1 and Angle (Distance and Angle)	The leg on the first face, and the angle off that face.	0.06 in at 45°.
Flip	Swaps which face the first distance is measured on. Shown for Two Distances and Distance and Angle.	Turn it on if the long leg ends up on the wrong face.
Tangent chain	Follows the edge around smooth (tangent) bends, such as a fillet, so one pick chamfers the whole run.	Leave it on for edges that flow into a fillet.
Preview	Shows the chamfer on the part while you set it up.	Leave it on.

Try it: break the top edges of a plate

Make a 3 in × 2 in × 0.75 in block (sketch a rectangle, Extrude 0.75 in).
Click Chamfer and click the four top edges. Edges shows 4 selected.
Set Chamfer Type to Equal Distance and Distance to 0.03 in.
Click OK. All four top edges have a 0.03 × 45° chamfer.
To change it, edit the chamfer and set Chamfer Type to Distance and Angle, Distance 1 to 0.06 in and Angle to 30. Use Flip to swap which face takes the 0.06 in leg.

Tips and common mistakes

Do type the unit with the number when the print uses another unit. In a millimetre design, typing 0.03 in enters 0.762 mm.
Do chamfer all the edges of one size in a single Chamfer. It’s one feature to change when the print changes.
Don’t chamfer an edge right next to an existing small chamfer with a larger size. If the chamfer would run past the neighbouring face, the dialog says so; make the chamfer smaller or chamfer those edges together in one feature.

Combine

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
target	body	Yes
tools	[body]	Yes
operation	join\|cut\|intersect	No
touching	separate\|one_body	No	what a join makes of pieces that share no face: separate, the default, makes each piece that touches another only along an edge or at a point a body of its own and keeps pieces that touch nothing in one body; one_body keeps every piece in one body
keep_tools	bool	No
new_component	bool	No	the result goes into a new component; component_name?

Automation details

Command ID: solid.combine

Parameters:

target: body; tools: [body]; operation?: join|cut|intersect; touching?: separate|one_body (what a join makes of pieces that share no face: separate, the default, makes each piece that touches another only along an edge or at a point a body of its own and keeps pieces that touch nothing in one body; one_body keeps every piece in one body); keep_tools?: bool; new_component?: bool (the result goes into a new component; component_name?)

Scale

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required
bodies	[names]	Yes
factor	expr	Yes
factors	[x, y, z] exprs	Yes
origin	[x,y,z]	No

Automation details

Command ID: solid.scale

Parameters:

bodies: [names]; factor: expr | factors: [x, y, z] exprs; origin?: [x,y,z]

Delete Face

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
faces	[[x,y,z] points on the faces, or face names from model.faces]	Yes
body		No
heal	bool	No	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

Automation details

Command ID: face.delete

Parameters:

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)

Offset Face

Command group: SOLID › MODIFY

Push faces of a solid in or out by a set distance, and the faces around them follow. Use it to add finish stock, open up a pocket or bore, make a pocket deeper or a wall thicker, without going back into the sketch.

Before you start

You need a solid body. The faces can be flat or curved, such as the wall of a bore.
A positive Distance pushes the face out of the material and adds stock. A negative Distance pulls it into the material and removes stock.
On an inside wall, such as the side of a pocket or the wall of a bore, out of the material means into the opening. A negative Distance opens the pocket or bore up; a positive one closes it in.

Options

Choice in the dialog	Meaning	Example or reason to choose it
Faces	The faces to move. You can pick more than one.	The floor of a pocket, or the wall of a bore.
Distance	How far each face moves, square to the face. Positive adds material, negative removes it.	0.010 in to leave stock on a face for finishing. -0.005 in on a bore wall to open the bore 0.010 in on the diameter.

Try it: deepen and widen a pocket

Make a 3 in × 2 in × 0.75 in block and cut a 1 in × 1 in pocket 0.25 in deep into the top.
Click Offset Face (in the Modify menu) and click the floor of the pocket. Set Distance to -0.125 in. The arrow points down into the part. Click OK. The pocket is now 0.375 in deep.
Click Offset Face again and click one side wall of the pocket. Set Distance to -0.25 in. The arrow points into the material, away from the pocket. Click OK. The pocket is now 1.25 in wide that way.

Tips and common mistakes

Do remember a bore moves on the radius. To open a bore 0.010 in on the diameter, offset its wall -0.005 in.
Do watch the arrow before clicking OK. It shows which way the face will move.
Do type the unit with the number when the print uses another unit. In a millimetre design, typing 0.010 in enters 0.254 mm.
Do use Offset Face for a quick size change on a finished model, such as a stock allowance or a fit adjustment. If the size will change again, change the sketch or the feature instead, so the dimension lives where the print puts it.

Shell

Command group: SOLID › MODIFY

Hollow out a solid to an even wall thickness, leaving the faces you pick open: a box with an open top, an enclosure, or a cup.

Before you start

You need a solid body.
Pick the faces to remove. They become the openings. Pick the top face of a block to get an open box.
To make a closed hollow part with no openings, click the body instead of a face.
Round or chamfer the edges around the opening after you shell, not before. Shell can fail on a round that runs into the opening.

Options

Choice in the dialog	Meaning	Example or reason to choose it
Faces/Body	The faces to remove, or the body for a closed hollow part.	The top face of a block for an open box.
Thickness	The wall thickness.	0.125 in for a small enclosure.
Direction	Inside keeps the outside size and builds the wall inward. Outside keeps the inside size and builds the wall outward. Both splits the wall across the original faces.	Inside when the outside size is on the print. Outside when the inside size matters, such as a pocket a part must fit in.
Tangent chain (under Options)	Also removes faces that run smoothly into the ones you picked, such as a fillet around the top edge.	On by default. Turn it off to remove only the faces you clicked.

Try it: an open-top box

Make a 4 in × 3 in × 2 in block (sketch a rectangle, Extrude 2 in).
Click Shell and click the top face. Faces/Body shows 1 selected.
Set Thickness to 0.125 in and Direction to Inside.
Click OK. The block is an open box, still 4 in × 3 in × 2 in outside, with 0.125 in walls and floor.
To try Outside, edit the shell and set Direction to Outside. The inside is now 4 in × 3 in and the outside grows by the wall.

Tips and common mistakes

Do pick Direction from the dimension that matters. Inside holds the outside size, Outside holds the inside size.
Do shell first and round the rim after. Shell then doesn’t have to follow the rounds.
Don’t click the body when you want an opening. Clicking the body makes a closed hollow part with no way in.

Draft

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
faces	[[x,y,z] points, or face names from model.faces]	Yes
angle	expr	Yes
neutral	XY\|XZ\|YZ\|plane name\|{origin, normal}	Yes
pull	[x,y,z]	No	default: neutral plane normal
body		No

Automation details

Command ID: solid.draft

Parameters:

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?

Split Face

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
faces	[[x,y,z] points on the faces to split, or face names from model.faces]	Yes
body		No

Automation details

Command ID: solid.split_face

Parameters:

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; each curve on its own, an open one extended past its ends) and loops?: bool (default false: true joins the curves end to end first, so a closed loop cuts along itself only)

Split Body

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body	name	Yes
plane	XY\|XZ\|YZ\|plane name\|{origin, normal} — or tool: {body, point}	Yes	a face of a body, its surface extended
line	curve id	Yes	a straight sketch line, along the sketch's normal

Automation details

Command ID: solid.split_body

Parameters:

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)

Press Pull

Command group: SOLID › MODIFY

Default keyboard shortcut: Q

Read the solid features guide.

Parameter	Type	Required	Description
face	[x,y,z] and distance: expr	Yes	positive adds material, negative cuts
edges	[[x,y,z]…] and distance	Yes	a fillet
body	the body the face or edges are on	No	for edges, as for solid.fillet

Automation details

Command ID: solid.press_pull

Parameters:

face: [x,y,z] and distance: expr (positive adds material, negative cuts), or edges: [[x,y,z]…] and distance (a fillet); body?: the body the face or edges are on (for edges, as for solid.fillet)

Move/Copy

Command group: SOLID › MODIFY

Default keyboard shortcut: M

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	Yes
translate	[x,y,z]	No	length exprs or numbers, applied after rotation
axis	[x,y,z]	No	default: world Z with origin, else the body's component's Z, world Z at the root
angle	angle expr	No
origin	[x,y,z]	No	length exprs or numbers in world coordinates; default: the body's component's origin, the world origin at the root
tolerance	matrix rotation tolerance	No	default 1e-9, at most 1e-3
copy	bool	No	default false; true keeps originals and transforms copies
occurrences	[occurrence paths, root first]	No	only with copy: copies each component independently and transforms the copies in world space; reply lists them in occurrences
name		No
body_name		No
body_names		No

Automation details

Command ID: solid.move

Parameters:

bodies: [names]; translate?: [x,y,z] (length exprs or numbers, applied after rotation); axis?: [x,y,z] (default: world Z with origin, else the body's component's Z, world Z at the root); angle?: angle expr; origin?: [x,y,z] (length exprs or numbers in world coordinates; default: the body's component's origin, the world origin at the root); matrix?: rigid row-major 3x4 or 4x4, flat or rows (instead of translate/axis/angle/origin); tolerance?: matrix rotation tolerance (default 1e-9, at most 1e-3); copy?: bool (default false; true keeps originals and transforms copies); occurrences?: [occurrence paths, root first] (only with copy: copies each component independently and transforms the copies in world space; reply lists them in occurrences); name?, body_name?, body_names?

Replace Face

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
faces	[[x,y,z] points on planar faces, or face names from model.faces]	Yes
target	plane	Yes	XY\|XZ\|YZ\|construction plane\|{origin, normal}
target_face	[x,y,z] on a parallel planar face	Yes
body		No

Automation details

Command ID: solid.replace_face

Parameters:

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?

Align

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	Yes
from	[x,y,z] \| "origin" \| {snap: vertex\|edge_mid\|face_center\|circle_center, at: [x,y,z]}	Yes
from_face	[x,y,z]	Yes
from_plane	XY\|XZ\|YZ\|construction or offset plane name or id\|{origin, normal}	Yes
to		Yes	the same
to_face	[x,y,z]	Yes
to_plane		Yes	a plane as from_plane; the point or face goes onto it along its normal, and the plane may move later: the bodies follow
flip	bool	No
axes	[x, y, z]	No	point-to-point only: which world axes the offset moves along; default all three, at least one true
angle	expr	No	a turn about the target's direction after the move

Automation details

Command ID: solid.align

Parameters:

bodies: [names]; from: [x,y,z] | "origin" | {snap: vertex|edge_mid|face_center|circle_center, at: [x,y,z]} | from_face: [x,y,z] | from_plane: XY|XZ|YZ|construction or offset plane name or id|{origin, normal}; to: (the same) | to_face: [x,y,z] | to_plane: (a plane as from_plane; the point or face goes onto it along its normal, and the plane may move later: the bodies follow); from_frame / to_frame: a frame found again whenever the design changes, so the bodies follow it, in place of that side's point, face or plane: a joint origin as joint.create takes one ({face|circle|edge|point: [x,y,z]}, a face's name, a named joint origin) or {sketch, point|curve} (a sketch point, or a circle's, arc's or ellipse's centre, z along the sketch's normal), on the bodies' own component; faces, planes and frames also turn to meet; flip?: bool; axes?: [x, y, z] (point-to-point only: which world axes the offset moves along; default all three, at least one true); angle?: expr (a turn about the target's direction after the move)

Remove

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	Yes	removed from here on in the timeline

Automation details

Command ID: solid.remove

Parameters:

bodies: [names] (removed from here on in the timeline)

Compute All

Command group: SOLID › MODIFY

Read the solid features guide.

Automation details

Command ID: timeline.compute_all

No parameter description is provided by the command registry.

Delete

Command group: SOLID › MODIFY

Default keyboard shortcut: Delete

Read the solid features guide.

Parameter	Type	Required	Description
feature	id\|name	Yes
features	[id\|name]	Yes
groups	[timeline folder ids]	Yes	a folder goes with all its features, joints and nested folders; one undo step; a sketch takes its dependent features with it

Automation details

Command ID: timeline.delete

Parameters:

feature: id|name | features: [id|name] | groups: [timeline folder ids] (a folder goes with all its features, joints and nested folders; one undo step; a sketch takes its dependent features with it) → deleted: [feature ids]; joints?: [joint ids]; groups?: [folder ids deleted]; failing?: [{feature, error}] (later features that worked and now fail)

Change Parameters

Command group: SOLID › MODIFY

Parameter	Type	Required	Description
name		Yes
expression		Yes	number or text
unit	mm\|cm\|m\|in\|ft\|deg\|rad\|""\|text	No	new parameters default to their value's unit, a length the design's units; a text parameter's expression is its text, quotes round it optional: sketch texts' words are built from it
comment		No
favorite	bool	No
new_name	rename	No	references follow; an expression `new = value` renames to `new` and sets value, or sets `new` when the expression is just `new`
delete	name	Yes
changes	{name: expression, …}	Yes	existing parameters, checked together and rebuilt once, all or nothing

Automation details

Command ID: parameters.change

Parameters:

name, expression (number or text), unit?: mm|cm|m|in|ft|deg|rad|""|text (new parameters default to their value's unit, a length the design's units; a text parameter's expression is its text, quotes round it optional: sketch texts' words are built from it), comment?, favorite?: bool, new_name?: rename (references follow; an expression `new = value` renames to `new` and sets value, or sets `new` when the expression is just `new`); or delete: name; or changes: {name: expression, …} (existing parameters, checked together and rebuilt once, all or nothing) → changed?: {name: value} (with changes), recomputed: features rebuilt, restored: features whose earlier result for the same inputs was reused (e.g. a value set back), switched?: [{feature, name, suppressed}] (the configuration rules that switch a feature's suppression and read a parameter whose value changed run in their order, as on activation; driven parameters and restrictions wait for a configuration edit or activation)

Physical Material

Command group: SOLID › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	Yes
material	name	Yes	Steel, Aluminum, ABS Plastic, …, or one made with material.create; `material.list`

Automation details

Command ID: material.assign

Parameters:

bodies: [names]; material: name (Steel, Aluminum, ABS Plastic, …, or one made with material.create; `material.list`)

Appearance

Command group: SOLID › MODIFY

Default keyboard shortcut: A

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	No
faces	[[x,y,z] on faces]	No	body?: which body, default the nearest
components	[names or ids, or occurrence names]	No
appearance	library name or stable starter.* ID	No	appearance.library
color	"#rrggbb" or [r, g, b]	Yes	0–255
opacity		No	0–1, default 1
name	inert copied look label	No	requires color, mutually exclusive with appearance
pbr	{metallic:0..1, roughness:0.045..1, dielectric_ior:1..3}	No	requires color/appearance and opacity 1

Automation details

Command ID: appearance.assign

Parameters:

bodies?: [names]; faces?: [[x,y,z] on faces] (body?: which body, default the nearest); components?: [names or ids, or occurrence names]; appearance?: library name or stable starter.* ID (appearance.library) | color: "#rrggbb" or [r, g, b] (0–255), opacity? (0–1, default 1); name?: inert copied look label (requires color, mutually exclusive with appearance); pbr?: {metallic:0..1, roughness:0.045..1, dielectric_ior:1..3} (requires color/appearance and opacity 1); a starter ID or registered starter name resolves its recipe before color overrides; omitted pbr retains that response and pbr: null explicitly clears it. Unavailable glass recipes refuse through either selector. Other custom labels with an explicit color retain legacy scalar behavior. Neither appearance nor color (or color: null): clear, so the face follows its body, the body its component, the component its material

SOLID › CONSTRUCT

Offset Plane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
name		No

Automation details

Command ID: construct.plane.offset

Parameters:

base: XY|XZ|YZ|plane name, or a planar face {face: [x,y,z], body?, index?, path?}; offset: expr, or through: a point ref (vertex, sketch point, construction point) the plane goes through, parallel to base; name?

Plane at Angle

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
axis	X\|Y\|Z\|construction axis name\|{origin, dir} \| {edge\|face: [x,y,z]}	Yes	where it is now; a straight or circular edge, or a cylinder, cone or torus face: about its axis, followed as the model changes
angle	expr	Yes
direction_only	bool	No	default false: turn about the axis as a line; true: project the axis direction onto base and turn about the line through pivot, or the base origin
pivot	point ref	No	only with direction_only; vertex, sketch point, construction point
name		No

Automation details

Command ID: construct.plane.at_angle

Parameters:

base: XY|XZ|YZ|plane name, or a planar face {face: [x,y,z], body?, index?, path?}; axis: X|Y|Z|construction axis name (where it is now)|{origin, dir} | {edge|face: [x,y,z]} (a straight or circular edge, or a cylinder, cone or torus face: about its axis, followed as the model changes); angle: expr; direction_only?: bool (default false: turn about the axis as a line; true: project the axis direction onto base and turn about the line through pivot, or the base origin); pivot?: point ref (only with direction_only; vertex, sketch point, construction point); name?

Plane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
refs	1-3 refs in any order	Yes
with	{the method's other parameters: offset, angle, t, name…}	No

Automation details

Command ID: construct.plane

Parameters:

refs: 1-3 refs in any order; with?: {the method's other parameters: offset, angle, t, name…}. Builds with the first of the family's CONSTRUCT commands that takes the refs in its reference parameters (and every key of `with`). Returns method: the command used

Axis

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
refs	1-3 refs in any order	Yes
with	{the method's other parameters: offset, angle, t, name…}	No

Automation details

Command ID: construct.axis

Parameters:

refs: 1-3 refs in any order; with?: {the method's other parameters: offset, angle, t, name…}. Builds with the first of the family's CONSTRUCT commands that takes the refs in its reference parameters (and every key of `with`). Returns method: the command used

Point

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
refs	1-3 refs in any order	Yes
with	{the method's other parameters: offset, angle, t, name…}	No

Automation details

Command ID: construct.point

Parameters:

refs: 1-3 refs in any order; with?: {the method's other parameters: offset, angle, t, name…}. Builds with the first of the family's CONSTRUCT commands that takes the refs in its reference parameters (and every key of `with`). Returns method: the command used

Axis Through Cylinder/Cone/Torus

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
face	ref	Yes	a cylinder, cone or torus face, or a circular edge
name		No

Automation details

Command ID: construct.axis.through_cylinder

Parameters:

face: ref (a cylinder, cone or torus face, or a circular edge); name?

Axis Perpendicular To Face

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
face	ref	Yes
point	ref	Yes	the axis goes through it, square to the face
name		No

Automation details

Command ID: construct.axis.normal_to_face

Parameters:

face: ref; point: ref (the axis goes through it, square to the face); name?

Axis Through Two Planes

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required
a	plane or planar face refs	Yes
b	plane or planar face refs	Yes
name		No

Automation details

Command ID: construct.axis.two_planes

Parameters:

a, b: plane or planar face refs; name?

Axis Through Two Points

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
a	point refs	Yes
b	point refs	Yes	vertices, sketch points, points
name		No

Automation details

Command ID: construct.axis.two_points

Parameters:

a, b: point refs (vertices, sketch points, points); name?

Axis Through Edge

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
edge	ref	Yes	a straight edge or sketch line
name		No

Automation details

Command ID: construct.axis.edge

Parameters:

edge: ref (a straight edge or sketch line); name?

Point At Vertex

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
point	ref	Yes	vertex, sketch point, point
name		No

Automation details

Command ID: construct.point.vertex

Parameters:

point: ref (vertex, sketch point, point); name?

Point Through Two Edges

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
a	edge or line refs	Yes
b	edge or line refs	Yes	where they meet, or come closest
name		No

Automation details

Command ID: construct.point.two_edges

Parameters:

a, b: edge or line refs (where they meet, or come closest); name?

Point Through Three Planes

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required
a	plane or planar face refs	Yes
b	plane or planar face refs	Yes
c	plane or planar face refs	Yes
name		No

Automation details

Command ID: construct.point.three_planes

Parameters:

a, b, c: plane or planar face refs; name?

Point At Center Of Circle/Sphere/Torus

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
of	ref	Yes	circular edge, sketch circle or arc, sphere or torus face
name		No

Automation details

Command ID: construct.point.center

Parameters:

of: ref (circular edge, sketch circle or arc, sphere or torus face); name?

Point At Edge And Plane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required
edge	edge or line ref	Yes
plane	plane or planar face ref	Yes
name		No

Automation details

Command ID: construct.point.edge_plane

Parameters:

edge: edge or line ref; plane: plane or planar face ref; name?

Point Along Path

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
path	edge or sketch curve ref	Yes
name		No

Automation details

Command ID: construct.point.along_path

Parameters:

path: edge or sketch curve ref; t: expr, 0…1 along it (default 0.5); name?

Midplane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
a	plane or planar face refs	Yes
b	plane or planar face refs	Yes	halfway between; bisecting when they meet at an angle
name		No

Automation details

Command ID: construct.plane.midplane

Parameters:

a, b: plane or planar face refs (halfway between; bisecting when they meet at an angle); name?

Plane Through Two Edges

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required
a	straight edge or line refs in one plane	Yes
b	straight edge or line refs in one plane	Yes
name		No

Automation details

Command ID: construct.plane.two_edges

Parameters:

a, b: straight edge or line refs in one plane; name?

Plane Through Axis And Point

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
point	off-axis point ref	Yes
name		No

Automation details

Command ID: construct.plane.axis_point

Parameters:

axis: origin axis, construction axis, straight edge or sketch line ref; point: off-axis point ref; name?

Plane Through Three Points

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required
a	point refs	Yes
b	point refs	Yes
c	point refs	Yes
name		No

Automation details

Command ID: construct.plane.three_points

Parameters:

a, b, c: point refs; name?

Tangent Plane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
face	ref	Yes	cylinder, cone, sphere or torus
at	[x,y,z] where it touches	No	default: the face pick
reference	plane or planar face ref	No	the plane touches where the face turns towards it: parallel to it, on the side of `at`
angle	expr	No	with reference, default 0 deg: turned that far about the face's axis; not on a sphere
name		No

Automation details

Command ID: construct.plane.tangent

Parameters:

face: ref (cylinder, cone, sphere or torus); at?: [x,y,z] where it touches (default: the face pick); reference?: plane or planar face ref (the plane touches where the face turns towards it: parallel to it, on the side of `at`); angle?: expr (with reference, default 0 deg: turned that far about the face's axis; not on a sphere); name?

Plane Along Path

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
path	edge or sketch curve ref	Yes

Automation details

Command ID: construct.plane.along_path

Parameters:

path: edge or sketch curve ref; t: expr, 0…1 along it (default 0.5); name? The plane is square to the path there

Perpendicular Plane

Command group: SOLID › CONSTRUCT

Read the solid features guide.

Parameter	Type	Required	Description
plane	plane or planar face ref	Yes

Automation details

Command ID: construct.plane.perpendicular

Parameters:

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

New Component

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
name	component id or name	No
parent	component id or name	No	default: the active one
parent_path	exact parent placement	No
activate	bool	No	default true
grounded	bool	No	default: true for the design's first part, false otherwise

Automation details

Command ID: component.create

Parameters:

name?, parent?: component id or name (default: the active one); parent_path?: exact parent placement; activate?: bool (default true); grounded?: bool (default: true for the design's first part, false otherwise)

Insert Design

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
path	a .sc design	Yes

Automation details

Command ID: component.insert_design

Parameters:

path: a .sc design → a new component linked to it, holding its solid bodies as placed in that design and a copy of its design properties; name? (default: the design's name); parent?: component id or name (default: the active one); translate?: [x,y,z] in mm from the destination parent's origin (default [0,0,0], also with reuse); reuse?: bool (default false): insert a free occurrence, reusing an existing link to the same file when available

Joint

Command group: SOLID › ASSEMBLE

Default keyboard shortcut: J

Parameter	Type	Required	Description
a	joint origins	Yes
b	joint origins	Yes	{occurrence, face\|circle\|edge\|point: [x,y,z] in world, or face\|circle: "<face name>", plane: "XY"\|"o:<ids>/origin/<item>"\|"<name>", axis: "Z"\|"o:<ids>/origin/<item>"\|"<name>"; z? for a point, end?, x? as joint.origin} \| origin name
values	[angles in deg or expressions, distances]	No
limits	[[min, max] \| null…]	No
flip	bool	No	default false: the origins are mated, b's z against a's as two faces meet - two plane or axis datums mate aligned, each part keeping its side of the datum, and flip mates them; true: b's z along a's, so two origins given at one point with the same z and x stay as they are; a point origin without x takes its x from z, so give x on both, or use joint.as_built, to keep a turned part where it is
offset	mm or an expression	No
angle	deg or an expression	No	an angle relation's tilt from mated; for other joints the default is none, or a half turn where that turns b less, so faces that already meet stay as they are
name		No

Automation details

Command ID: joint.create

Parameters:

type: rigid|revolute|slider|cylindrical|pin_slot|planar|ball, or a relation: parallel|perpendicular|angle|point_on_plane|point_on_line|line_on_plane (ties only some directions or points, made where the parts are; several between two parts add up); a, b: joint origins ({occurrence, face|circle|edge|point: [x,y,z] in world, or face|circle: "<face name>", plane: "XY"|"o:<ids>/origin/<item>"|"<name>", axis: "Z"|"o:<ids>/origin/<item>"|"<name>"; z? for a point, end?, x? as joint.origin} | 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 - two plane or axis datums mate aligned, each part keeping its side of the datum, and flip mates them; true: b's z along a's, so two origins given at one point with the same z and x stay as they are; a point origin without x takes its x from z, so give x on both, or use joint.as_built, to keep a turned part where it is); offset?: mm or an expression; angle?: deg or an expression (an angle relation's tilt from mated; for other joints the default is none, or a half turn where that turns b less, so faces that already meet stay as they are); name?; quiet?: bool (leave out dof and fixed). An expression (text) is kept with the joint and worked out again whenever the design changes, so the joint follows the parameters it names; a joint whose expression no longer works out (a parameter deleted) is left out of the solve with the reason in its errors

As-Built Joint

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
type		Yes
a	occurrence	Yes
b	occurrence	Yes	stay where they are
at	joint origin	No	default: b's origin
name		No
limits	[[min, max] \| null…]	No
quiet	bool	No

Automation details

Command ID: joint.as_built

Parameters:

type, a: occurrence, b: occurrence (stay where they are); at?: joint origin (default: b's origin) — the joint's frame; one on a or b is kept on its face or hole there, so the joint follows it as the design changes; name?; limits?: [[min, max] | null…]; quiet?: bool

Rigid Group

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
occurrences	[ids or names]	Yes	move together, as they are

Automation details

Command ID: joint.rigid_group

Parameters:

occurrences: [ids or names] (move together, as they are)

Drive Joints

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
joint	id\|name	Yes
value	[angles in deg or expressions, distances]	Yes	values not given keep theirs; a value driven drops the expression joint.create gave it; 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
values	[angles in deg or expressions, distances]	Yes	values not given keep theirs; a value driven drops the expression joint.create gave it; 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	No	leave out dof and fixed

Automation details

Command ID: joint.drive

Parameters:

joint: id|name; value | values: [angles in deg or expressions, distances] (values not given keep theirs; a value driven drops the expression joint.create gave it; 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; requested: the values asked for, in the same form; held: [{name, requested, value, unit, why}] for each driven value that ended up elsewhere (a motion link sets it, as a screw's travel follows its turn; a limit; contact; a closed loop); moved: whether any occurrence moved; reason: why the joint can move nothing (suppressed: nothing is stored; its origins lost; its chain joined to nothing grounded → unconnected: the occurrence named; or, when nothing moved, the first held value's why); index?: zero-based coordinate to drive with value (the other coordinates follow); continuous?: bool (drag frame, suppress UI echo); stop_at_budget?: bool (default false: a contact check past its sample or work budget fails the drive; true: the drive stops at the last placement checked clear → stopped_by_budget {budget: samples|work|intersections, fraction})

Motion Link

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
a	joints	Yes
b	joints	Yes
ratio		Yes	b = ratio · a + offset
offset	in b's units	No	deg for an angle, mm for a distance, or an expression
ia	value indices	No
ib	value indices	No	default 0

Automation details

Command ID: joint.motion_link

Parameters:

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)

Gear

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
internal	bool	No	one is a ring gear: both turn the same way; by default b turns the other way
reverse	bool	No
link	index	No	replace that motion link

Automation details

Command ID: joint.gear

Parameters:

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, also when the link replaces another (at the current pose)

Rack and Pinion

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
radius	the pinion's pitch radius	Yes	mm, an expression, or {circle: [x,y,z], occurrence?}
reverse	bool	No
link	index	No	replace that motion link

Automation details

Command ID: joint.rack_pinion

Parameters:

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, also when the link replaces another (at the current pose)

Screw

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
pitch	travel per turn	Yes	mm or an expression
reverse	bool	No	a left-hand thread
link	index	No	replace that motion link

Automation details

Command ID: joint.screw

Parameters:

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, also when the link replaces another (at the current pose)

Cam

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
a	the cam's joint	Yes	revolute
follower	knife\|roller\|flat	No	default knife; flat: a face square to a slider's line
radius	the roller's radius	No	mm, an expression or {circle: [x,y,z], occurrence?}: the roller's round face, which is its tip too
flip	bool	No	ride the cam from the other side than the one the follower is on now
link	index	No	replace that motion link

Automation details

Command ID: joint.cam

Parameters:

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, also when the link replaces another (at the current pose)

Constrain

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Parameter	Type	Required	Description
type	mate\|flush\|distance\|concentric\|insert\|parallel\|perpendicular\|angle\|tangent\|point_on_axis	Yes
offset	the gap	No	mm or an expression; needed for distance
angle	deg or an expression	No	needed for angle
flip	turn b over	No
name		No	default: the rule and a number, Mate1

Automation details

Command ID: assembly.constraint.create

Parameters:

type: mate|flush|distance|concentric|insert|parallel|perpendicular|angle|tangent|point_on_axis; a, b: references, as joint.create's origins (a face or a datum plane for a plane, a circle or an axis for an axis, a point; b moves); offset?: the gap (mm or an expression; needed for distance); angle?: deg or an expression (needed for angle); flip?: turn b over; name? (default: the rule and a number, Mate1); quiet?. Kept as a joint of the kind the rule needs (mate and flush planar, distance planar or point on plane, concentric cylindrical, insert revolute, tangent line on plane, point on axis point on line), made where the parts are, so b moves no further than the rule needs → joint, name, dof, conflicts, fixed as joint.create

Enable Contact Sets

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Parameter	Type	Required	Description
enabled	bool	No	default true

Automation details

Command ID: contact.enable_sets

Parameters:

enabled?: bool (default true) — driving joints and motion studies stop where bodies in one contact set would pass through each other

Enable All Contact

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Automation details

Command ID: contact.enable_all

Parameters:

every occurrence takes part in contact (one set of all)

Disable Contact

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Automation details

Command ID: contact.disable_all

Parameters:

contact off

New Contact Set

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Parameter	Type	Required	Description
occurrences	[ids or names]	Yes	two or more
name		No

Automation details

Command ID: contact.create

Parameters:

occurrences: [ids or names] (two or more); name?

Motion Study

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
name		No
study		No	edit an existing one
steps		No	timeline length, default 100
keys	[{joint, index?, points: [[step, value], …]}]	Yes	values: degrees for angles, mm for distances, or expressions

Automation details

Command ID: motion.study

Parameters:

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

Command group: SOLID › ASSEMBLE

Parameter	Type	Required	Description
study	id\|name	Yes
joint	id\|name with from and to	Yes	degrees for angles, mm for distances, or expressions

Automation details

Command ID: motion.trace

Parameters:

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)

Exploded View

Command group: SOLID › ASSEMBLE

Read the solid features guide.

Parameter	Type	Required	Description
name		No
scale		No	automatic: each occurrence pushed away from the assembly's centre by scale × its offset, default 1
moves	[{occurrence, translate: [x,y,z]}]	No	instead of automatic

Automation details

Command ID: explode.create

Parameters:

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

Capture Position

Command group: SOLID › POSITION

Automation details

Command ID: component.capture_position

Parameters:

keeps pending occurrence moves and saves every moving joint's values → captured, joints

Revert Position

Command group: SOLID › POSITION

Parameter	Type	Required	Description
occurrences	[ids]	No	default all

Automation details

Command ID: component.revert_position

Parameters:

occurrences?: [ids] (default all); drops selected pending occurrence moves; with no occurrences the joints also go back to the values Capture Position saved (clamped to limits) → reverted, joints

SOLID › INSPECT

Interference

Command group: SOLID › INSPECT

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	No	default: all, in world placement; a name that is no body is refused
budget_s	seconds	No	default 240, at most 86400: pairs not finished by then are listed in unchecked as "not checked: the time budget … ran out" and the call returns
exclude_pairs	[[a, b]]	No	pairs left out, such as a pin in its hole: each side a body's world name or an occurrence id\|name, matching every body under it; pairs_excluded counts them

Automation details

Command ID: inspect.interference

Parameters:

bodies?: [names] (default: all, in world placement; a name that is no body is refused); budget_s?: seconds (default 240, at most 86400: pairs not finished by then are listed in unchecked as "not checked: the time budget … ran out" and the call returns); exclude_pairs?: [[a, b]] (pairs left out, such as a pin in its hole: each side a body's world name or an occurrence id|name, matching every body under it; pairs_excluded counts them) → interferences: pairs that overlap with the overlap volume, area, bounding box and centre, and a_part, b_part: {component, path: [occurrence names], path_ids} where each body sits (also on unchecked pairs); unchecked: [{a, b, reason}], the pairs that could not be checked, with the reason, and each mesh body (STL, 3MF or OBJ import: not intersected) as {a: name, b: null, reason: "mesh body: not checked"}, so count: 0 is not read as no overlap (checked counts the solid bodies). Bodies are pruned by bounding box first, then by their display meshes (pairs whose meshes stay apart by more than their chord tolerances, neither inside the other, are clear without a boolean), so any number of bodies is fine; the pairs left are intersected exactly, in parallel on desktop, the slowest first; at most 20000 pairs whose boxes overlap are intersected per call (truncated: true and skipped_pairs: n say when more were left out). Also: pairs_candidate (boxes overlap), pairs_cleared (by the meshes), pairs_intersected, pairs_not_checked, pairs_excluded, budget_exceeded, threads (worker threads; 0: on the calling thread), boolean_ms and tessellate_ms (kernel time summed over the pairs), slowest: [{a, b, ms, boolean_ms, tessellate_ms}] and ms

Bill of Materials

Command group: SOLID › INSPECT

Read the solid features guide.

Parameter	Type	Required	Description
component	id or name	No	default the design
levels	flat\| top	No	default: every part at any depth, counted through its subassemblies; the component's direct children, subassemblies as one row each
group_by	["part_number"]\| ["definition"]	No	default; components without a part number get a row per definition
group_children	true	No	a component with a part number is one row, the parts placed inside it listed under it as children: [{item, part_number, description, revision, each, count, definition}], not as rows of their own
path	write a .csv or .json file	No	children as items 1.1, 1.2…

Automation details

Command ID: assembly.bom

Parameters:

component?: id or name (default the design); levels?: flat (default: every part at any depth, counted through its subassemblies) | top (the component's direct children, subassemblies as one row each); group_by?: ["part_number"] (default; components without a part number get a row per definition) | ["definition"]; group_children?: true (a component with a part number is one row, the parts placed inside it listed under it as children: [{item, part_number, description, revision, each, count, definition}], not as rows of their own); path?: write a .csv or .json file (children as items 1.1, 1.2…); format?: csv|json (default from the path). Each component's bom_type counts: phantom has no row (what it holds counts here), reference counts nowhere, purchased and inseparable are one row (in flat, an inseparable one's purchased parts are listed too, under it with group_children and a part number) → rows: [{item, part_number, description, revision, bom_type, count, definition, components, properties, children?}] sorted by part number, total_occurrences (children included)

Component Colors

Command group: SOLID › INSPECT

Read the solid features guide.

Parameter	Type	Required	Description
enabled	bool	No	omitted: toggle

Automation details

Command ID: inspect.colored_components

Parameters:

enabled?: bool (omitted: toggle); temporary component colours, without changing appearances

Measure

Command group: SOLID › INSPECT

Default keyboard shortcut: I

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	No	default all
names_only	bool	No	each world body's name and its definition's, nothing measured

Automation details

Command ID: inspect.measure

Parameters:

bodies?: [names] (default all); names_only?: bool (each world body's name and its definition's, nothing measured) → closed per body; volume_mm3, center_of_mass, density_g_cm3 and mass_g only for closed, consistently oriented bodies; area, bbox and counts for all; total.open_bodies_skipped counts bodies excluded from volume/mass totals; or items: [1-2 selections] (face/edge: type, body, and point on it or index from model.faces/model.edges, or both) → length/area/volume; a face's perimeter_mm, with outer_perimeter_mm and inner_perimeter_mm on a flat face with holes; 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

Section Analysis

Command group: SOLID › INSPECT

Read the solid features guide.

Parameter	Type	Required	Description
plane	XY\|XZ\|YZ \| construction plane name or id \| {origin, normal}	Yes
offset	expr along the plane's normal	No	XY: +Z, XZ: +Y, YZ: +X
flip	bool	No
hatch	bool	No	hatch the cut faces, in each body's colour; default true

Automation details

Command ID: inspect.section

Parameters:

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; hatch?: bool (hatch the cut faces, in each body's colour; default true); or clear: true. Returns the cut's origin and normal, and for a named plane its axis and at

SOLID › CONFIGURE

Configure

Command group: SOLID › CONFIGURE

Parameter	Type	Required	Description
params	[parameter names]	No
features	[feature names]	No
materials	[body names]	No
appearances	[body names]	No	columns to add; with no rows yet, a "Default" row takes the current values

Automation details

Command ID: config.configure

Parameters:

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)

Display Configuration Table

Command group: SOLID › CONFIGURE

Automation details

Command ID: config.table

Parameters:

→ columns (param:<name> or suppress:<feature>), rows (each with its fixed id), the active row's name and whether the design still matches it

SKETCH › FINISH SKETCH

Finish Sketch

Command group: SKETCH › FINISH SKETCH

Parameter	Type	Required	Description
restore_marker	bool	No	default true

Automation details

Command ID: sketch.finish

Parameters:

restore_marker?: bool (default true); false transfers the temporary marker directly to another editor without rebuilding the intervening timeline

Cancel Sketch

Command group: SKETCH › FINISH SKETCH

Automation details

Command ID: sketch.cancel

Parameters:

Leaves the sketch without keeping what changed since it was created or opened for editing: the design goes back to how it was then (a new sketch is removed), as one step that Undo brings back. Refused when the undo history no longer leads back to that point (use Undo instead). restore_marker?: bool (default true); false transfers the temporary marker to another editor

Finish with AutoConstrain

Command group: SKETCH › FINISH SKETCH

Automation details

Command ID: sketch.finish_auto_constrain

Parameters:

like AutoConstrain, then Finish Sketch

SKETCH › CREATE

Line

Command group: SKETCH › CREATE

Default keyboard shortcut: L

Parameter	Type	Required	Description
points	[[x,y] \| "l1.end" \| {at, ref}…]	Yes	x and y each a number or an expression over the design's parameters, "W / 2": such a point is fixed where it comes to and follows the parameters, while text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the point; likewise wherever a point argument also takes a point id
closed	bool	No
construction	bool	No
ids	[..]	No
infer	bool	No	add horizontal/vertical
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.line

Parameters:

points: [[x,y] | "l1.end" | {at, ref}…] (x and y each a number or an expression over the design's parameters, "W / 2": such a point is fixed where it comes to and follows the parameters, while text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the point; likewise wherever a point argument also takes a point id), 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…)

2-Point Rectangle

Command group: SKETCH › CREATE

Default keyboard shortcut: R

Parameter	Type	Required	Description
p0	opposite corners [x,y]	Yes
p1	opposite corners [x,y]	Yes	a coordinate may be an expression over the design's parameters: the corner is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the corner
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.rectangle.two_point

Parameters:

p0, p1: opposite corners [x,y] (a coordinate may be an expression over the design's parameters: the corner is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the corner); 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…)

3-Point Rectangle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0	first edge	Yes
p1	first edge	Yes
p2	point on the opposite edge	Yes
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.rectangle.three_point

Parameters:

p0, p1: first edge; p2: point on the opposite edge; construction?: bool; 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…)

Rounded Rectangle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0	opposite corners [x,y]	Yes
p1	opposite corners [x,y]	Yes	a coordinate may be an expression over the design's parameters: the corner is fixed and follows them, as in `sketch.rectangle.two_point`; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the corner
radius	expr	Yes	the corner radius, less than half the shorter side
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.rectangle.rounded

Parameters:

p0, p1: opposite corners [x,y] (a coordinate may be an expression over the design's parameters: the corner is fixed and follows them, as in `sketch.rectangle.two_point`; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the corner); 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), diagonal (construction, between the bottom-left and top-right arc centres) and centre (the point held at its midpoint); 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…)

Center Rectangle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
center	[x,y]	Yes
corner	[x,y]	Yes	a coordinate may be an expression over the design's parameters: the point is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the point
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.rectangle.center

Parameters:

center, corner: [x,y] (a coordinate may be an expression over the design's parameters: the point is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the point); construction?: bool. 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…)

Center Diameter Circle

Command group: SKETCH › CREATE

Default keyboard shortcut: C

Parameter	Type	Required	Description
center	[x,y] or point ref	Yes	a coordinate may be an expression over the design's parameters: the centre is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the centre
radius	number or expression	Yes	an expression naming a parameter is a dimension driven by it; with `through` a point ref, that and the point both fix the radius
diameter	number or expression	Yes	an expression naming a parameter is a dimension driven by it; with `through` a point ref, that and the point both fix the radius
through	point ref	No	a point the circle passes through, kept on it: where the tool's second click snapped
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.circle.center

Parameters:

center: [x,y] or point ref (a coordinate may be an expression over the design's parameters: the centre is fixed and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the centre), radius | diameter: number or expression (an expression naming a parameter is a dimension driven by it; with `through` a point ref, that and the point both fix the radius); through?: point ref (a point the circle passes through, kept on it: where the tool's second click snapped); construction?: bool; 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…)

2-Point Circle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0	diameter ends	Yes
p1	diameter ends	Yes
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.circle.two_point

Parameters:

p0, p1: diameter ends; construction?: bool; 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…)

3-Point Circle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0	[x,y] or point ref	Yes
p1	[x,y] or point ref	Yes
p2	[x,y] or point ref	Yes	a referenced point stays on the circle
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.circle.three_point

Parameters:

p0, p1, p2: [x,y] or point ref (a referenced point stays on the circle); construction?: bool; 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…)

3-Point Arc

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
start	[x,y] or point ref	Yes
end	[x,y] or point ref	Yes
through	[x,y] or point ref	Yes	a referenced through point stays on the arc
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.arc.three_point

Parameters:

start, end, through: [x,y] or point ref (a referenced through point stays on the arc); construction?: bool; 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…)

Center Point Arc

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
center		Yes
start		Yes
end		Yes	counter-clockwise from start; clockwise?: bool for clockwise
center		Yes
start		Yes
sweep	signed degrees	Yes
construction	bool	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.arc.center_point

Parameters:

center, start, end (counter-clockwise from start; clockwise?: bool for clockwise) | center, start, sweep: signed degrees; construction?: bool; 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…)

Inscribed Polygon

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
center		Yes
radius		Yes	to vertices
sides		Yes
angle	deg	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.polygon.inscribed

Parameters:

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…)

Circumscribed Polygon

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
center		Yes
radius		Yes	to edge midpoints
sides		Yes
angle	deg	No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.polygon.circumscribed

Parameters:

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…)

Edge Polygon

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0		Yes
p1	one edge	Yes
sides		Yes
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.polygon.edge

Parameters:

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…)

Center to Center Slot

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0		Yes
p1	arc centres	Yes
width		Yes
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.slot.center_to_center

Parameters:

p0, p1: arc centres, width; returns centre_line (construction, between the arc centres) and middle (the point held at its midpoint); 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…)

Overall Slot

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
p0		Yes
p1	overall ends	Yes
width		Yes
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.slot.overall

Parameters:

p0, p1: overall ends, width; returns centre_line (construction, between the arc centres) and middle (the point held at its midpoint); 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…)

Point

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
id		No
connect	bool	No	default true: a new point landing exactly on an existing point, the origin too, is made coincident with it

Automation details

Command ID: sketch.point

Parameters:

point: [x,y] (each a number or an expression over the design's parameters: the point is then fixed where it comes to and follows them; text naming no parameter, such as "5", is just that number, in the design's length unit (a JSON number is mm), and does not itself fix the point) or a snap: "mid:<line>" (held at the line's midpoint), "on:<curve>:x,y" (on the curve near x,y), "x:<a>+<b>:x,y" (at the crossing of two curves near x,y), {vertex: [x,y,z]} or {on_edge: [x,y,z]} of the model; 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

Command group: SKETCH › CREATE

Default keyboard shortcut: D

Parameter	Type	Required	Description
half_axes	bool	No	default true; false: with auto, the minor radius wherever text_at is, as before half-axes, which the Dimension tool sends with Draw ellipses with their axes off

Automation details

Command ID: sketch.dimension

Parameters:

entities: [refs] (a line midpoint is "mid:line_id"; a model edge or vertex, {edge: [x,y,z], body?} or {vertex: [x,y,z], body?}, is projected into the sketch first and measured there: a point against the projected edge measures the distance to it), type?: auto|distance|horizontal|distance_x|vertical|distance_y|length|radius|diameter|major|minor|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), or `name = expression` (e.g. "width = 40"; also `#name = expression`), which adds the user parameter `name` with that expression and dimensions with `name` (refused when the name is taken or reserved; the reply's `defined` names it); text_at?: [x, y]. Two points or a line off the axes: with auto, text_at across from them (between the perpendiculars through them, or a tenth of their distance past) is the distance between them; pulled further past an end, up or down from it horizontal, sideways vertical. Two midpoints: placing text above or below their bounding box measures horizontally, beside it vertically, anywhere else (inside it or past its corners) the distance between them. Two lines: the angle between them (acute, or 180° − it when the value is nearer that) unless text_at picks a sector. A line and a circle or arc: the distance from the line to its edge (the gap, or how far the edge reaches past a line that cuts it; 0 is tangent); dimension the centre point for the distance to the centre. A point and a circle or arc: the distance from the point to its edge (or how far within it a point inside lies). Two circles or arcs: the gap between their edges (or how far they overlap when they cross, or the narrowest gap between them when one lies inside the other), or the centre-to-centre distance when they are the two caps of a slot. An ellipse: a half-axis, the distance from the centre to an axis end (major or minor; with auto, text_at pulled across the major axis gives the major half-axis, pulled out past an end of it the minor one, the minor without text_at; previous_axis?: major|minor, the half-axis an earlier placement chose, kept while text_at is near the boundary between them; the reply's axis names the one chosen; with auto, when a driving dimension already holds one half-axis (or its whole axis), the other one, wherever text_at is; without its major axis line the major half-axis goes to the ellipse's own major end, without its minor axis line the minor half-axis is the minor radius); any other type, radius among them, the minor radius; an ellipse's axis line with auto: its length, the whole axis, wherever text_at is; half_axes?: bool (default true; false: with auto, the minor radius wherever text_at is, as before half-axes, which the Dimension tool sends with Draw ellipses with their axes off). An arc and one of its end points: the arc's length (type arc_length does it from the arc alone). 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 the Sketch preference, on by default): 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 to the value instead of distorting: about the origin when the drawing is tied to it (joined to the origin, or constrained to a sketch axis), otherwise about the middle of the drawing, so it stays where it was drawn (#11043); scale_about_origin?: bool (default false; the dimension tool sends the Sketch preference) scales about the origin always, as before #11043. Returns measured in unit (mm or deg), and scaled: the factor when the sketch was scaled

Normal/Construction

Command group: SKETCH › CREATE

Default keyboard shortcut: X

Parameter	Type	Required	Description
curves	[ids]	Yes
value	bool	No	default: construction unless all of them already are

Automation details

Command ID: sketch.construction

Parameters:

curves: [ids], value?: bool (default: construction unless all of them already are)

Midpoint Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
end	[x,y]	Yes

Automation details

Command ID: sketch.line.midpoint

Parameters:

mid: [x,y], point ref or snap ("mid:<line>", "on:<curve>:x,y", model vertex/edge); 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…)

Tangent Arc

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
start	end point of a line or arc	Yes	"l1.end"
end	[x,y] or an existing point's id	Yes	"l2.start": the arc ends on that point
curve	the curve to be tangent to	No	default: the one ending at start

Automation details

Command ID: sketch.arc.tangent

Parameters:

start: end point of a line or arc ("l1.end"), end: [x,y] or an existing point's id ("l2.start": the arc ends on that point); 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…)

2-Tangent Circle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
curves	[two lines/circles/arcs]	Yes
radius	expr	Yes
diameter	expr	Yes
near	[x,y]	Yes	which of the solutions

Automation details

Command ID: sketch.circle.two_tangent

Parameters:

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…)

3-Tangent Circle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
curves	[three lines/circles/arcs]	Yes
near	[x,y]	Yes	which of the solutions

Automation details

Command ID: sketch.circle.three_tangent

Parameters:

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…)

Center Point Slot

Command group: SKETCH › CREATE

Parameter	Type	Required
center	slot centre	Yes
end	one arc centre	Yes
width		Yes

Automation details

Command ID: sketch.slot.center_point

Parameters:

center: slot centre, end: one arc centre, width; returns centre_line and middle. 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…)

Three Point Arc Slot

Command group: SKETCH › CREATE

Parameter	Type	Required
start		Yes
through		Yes
end	points on the centre arc	Yes
width		Yes

Automation details

Command ID: sketch.slot.arc_three_point

Parameters:

start, through, end: points on the centre arc, width; returns centre_arc and middle. 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…)

Center Point Arc Slot

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
center		Yes
start	centre arc start	Yes
end	direction of the centre arc end	Yes	counter-clockwise
sweep	degrees	Yes	0 < sweep < 360
width		Yes

Automation details

Command ID: sketch.slot.arc_center

Parameters:

center, start: centre arc start, end: direction of the centre arc end (counter-clockwise) or sweep: degrees (0 < sweep < 360), width; returns centre_arc and middle. 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…)

Ellipse

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
axes	bool	No	default true; false: the ellipse alone, as the Ellipse tool draws it with Draw ellipses with their axes off

Automation details

Command ID: sketch.ellipse

Parameters:

center, major: end of the major axis [x,y], minor: a point the ellipse passes through on the minor side [x,y] | minor_radius. Also adds its major and minor axes as construction lines through the centre (their ends: the major end and the point opposite it, and the two ends of the minor axis on the ellipse), held by midpoint, perpendicular and point-on-curve constraints, so a half-axis is the distance from the centre to an axis end and an axis line's length is a full axis; axes?: bool (default true; false: the ellipse alone, as the Ellipse tool draws it with Draw ellipses with their axes off). 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…)

Fit Point Spline

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
points	[[x,y] or point refs…]	Yes	2…500

Automation details

Command ID: sketch.spline.fit_point

Parameters:

points: [[x,y] or point refs…] (2…500): the spline passes through them; each fit point has an editable tangent handle whose direction and length control curvature, 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…)

Control Point Spline

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.spline.control_point

Parameters:

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…)

Control Point Spline (Degree 5)

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.spline.control_point_5

Parameters:

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…)

Conic Curve

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
start	[x,y] or point refs	Yes
end	[x,y] or point refs	Yes
apex	[x,y] or point refs	Yes
rho	0…1	No	default 0.5: parabola

Automation details

Command ID: sketch.conic

Parameters:

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…)

Centerline

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
curves	[line ids]	Yes
value	bool	No	default toggles

Automation details

Command ID: sketch.centerline

Parameters:

curves: [line ids], value?: bool (default toggles): centerline line type (not in profiles; an axis)

Text

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
at	baseline start [x,y]	Yes
height	capital height mm	No	default 5
angle	deg	No

Automation details

Command ID: sketch.text

Parameters:

text: string (\n breaks lines), or text_expression: the words built from text parameters (parameters.add with unit text), number parameters and quoted texts joined by + ("Label + '-L'", "'W' + Width"; a number parameter shows its value in the design's units, "85 mm", an angle in degrees, "30°"; number(Width) is the number alone and number(Width, 2) has 2 decimals): the text keeps it, its words follow the parameters (a parameter edit or a configuration row relabels it) and `exprs` returns it as `text`; 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), vertical_align?: baseline|top|middle|bottom (the block of lines against `at` or the path: the first line's baseline (default), its capitals' tops, halfway between those and the last line's baseline, or the bottom of the last line's descenders), 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…)

Construction Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line

Parameters:

Construction line, free. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Horizontal Construction Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.horizontal

Parameters:

Construction line, horizontal. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Vertical Construction Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.vertical

Parameters:

Construction line, vertical. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Construction Line at Angle

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.angle

Parameters:

Construction line, angle. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Parallel Construction Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.parallel

Parameters:

Construction line, parallel. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Perpendicular Construction Line

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.perpendicular

Parameters:

Construction line, perpendicular. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Tangent through External Point

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.tangent_external

Parameters:

Construction line, tangent_external. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Tangent at Curve Point

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.tangent_at

Parameters:

Construction line, tangent_at. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Common Tangent

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.tangent_two

Parameters:

Construction line, tangent_two. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Angle Bisector

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
through	second point	No
curve	sketch references	No
curve2	sketch references	No
angle	degrees from sketch X	No
offset	positive length	No	parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at
solution	zero-based solution index	No

Automation details

Command ID: sketch.construction_line.bisector

Parameters:

Construction line, bisector. at: point; through?: second point; curve?, curve2?: sketch references; angle?: degrees from sketch X; offset?: positive length (parallel: distance from the reference line; horizontal: distance from sketch X; vertical: distance from sketch Y; the side follows at) and a driving dimension at that value; near?: solution selector, and the side a line with a length runs towards; solution?: zero-based solution index; length?: a segment of this length from `at`, held by a length dimension, instead of an infinite line (horizontal, vertical, angle, parallel, perpendicular); construction?: false makes that segment a normal line. Tangents take circles/arcs, or an open spline/conic endpoint for tangent_at.. 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…)

Divide Curve

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
curve	id	Yes
curves	[ids]	Yes	each divided on its own

Automation details

Command ID: sketch.point.divide

Parameters:

curve: id | curves: [ids] (each divided on its own); segments: whole number from 2 to 500. Places points that divide each curve into `segments` pieces of equal length along it (arc length): segments − 1 points on an open curve (line, arc, spline, conic), `segments` points on a closed one (a circle from its point on sketch +X, an ellipse from its major-axis end, a closed spline from its first point). Each point is constrained to its share of the curve's length, so it stays on the curve and keeps equal spacing as the curve changes; the curve is not changed. Infinite lines are refused. Returns points: [ids], per curve in order, and constraints: [ids]. 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…)

Equation Curve

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
x	x	Yes	t
y	y	Yes	t
explicit	true and y: f	Yes	x
alone		Yes	no x
start	the range of t	Yes
end	the range of t	Yes	or of x
tolerance	mm	No	default 0.01
construction	bool	No
variable_unit	"number"	No	default

Automation details

Command ID: sketch.equation_curve

Parameters:

x: x(t), y: y(t): formulas of t in the design's expression language and parameters ("r * (cos(t) + t * sin(t))"); or explicit: true and y: f(x) alone (no x); start, end: the range of t (or of x): a number or an expression ("2 * pi", "360 deg" is 2·pi, a length is in the design's unit); tolerance?: mm (default 0.01): how far the curve may stray from the formulas (0.0001 to 10); construction?: bool; variable_unit?: "number" (default) or "range". The variable is a plain number: sin(t) reads it in radians; a result without a unit is in the design's length unit. With variable_unit "range" it is a length, so a ^ 2 / (4 * t) is a length when a is one: start and end must both be lengths, or one a length and the other a plain number, which is then in the design's unit. Makes a fit point spline through fixed points, as many as the tolerance needs (up to 500), closed smoothly when it ends where it starts; the points are placed again from the formulas whenever the parameters change. Returns curve, points (how many), closed, deviation (mm). 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

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
entities	[one or two sketch entity ids]: applies the constraint the geometry nearly has	Yes	horizontal/vertical, parallel, perpendicular, collinear, coincident, concentric, equal, tangent

Automation details

Command ID: sketch.constrainer

Parameters:

entities: [one or two sketch entity ids]: applies the constraint the geometry nearly has (horizontal/vertical, parallel, perpendicular, collinear, coincident, concentric, equal, tangent)

Project

Command group: SKETCH › CREATE

Default keyboard shortcut: P

Parameter	Type	Required	Description
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} \| {point: name} (a construction point) \| "origin" \| {axis: X\|Y\|Z\|name} \| {plane: XY\|XZ\|YZ\|name}]	Yes
projection_link	bool	No	default true
construction	bool	No	default the session's preference, off: the created curves are construction geometry

Automation details

Command ID: sketch.project

Parameters:

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} | {point: name} (a construction point) | "origin" | {axis: X|Y|Z|name} | {plane: XY|XZ|YZ|name}]; projection_link?: bool (default true); construction?: bool (default the session's preference, off: the created curves are construction 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…)

Intersect

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
refs	[{body}, {face: [x,y,z], body?}, {edge: [x,y,z], body?}, {sketch, curve}]: section curves	Yes	or points
projection_link	bool	No	default true
construction	bool	No	default the session's preference, off: the created curves are construction geometry

Automation details

Command ID: sketch.intersect

Parameters:

refs: [{body}, {face: [x,y,z], body?}, {edge: [x,y,z], body?}, {sketch, curve}]: section curves (or points) with the sketch plane; projection_link?: bool (default true); construction?: bool (default the session's preference, off: the created curves are construction 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…)

Include 3D Geometry

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
refs	like Project	Yes	edges, vertices, sketch curves and points
construction	bool	No	default the session's preference, off: the created curves are construction geometry

Automation details

Command ID: sketch.include_3d

Parameters:

refs: like Project (edges, vertices, sketch curves and points); curves out of the sketch plane are flattened onto it; construction?: bool (default the session's preference, off: the created curves are construction 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…)

Project To Surface

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.project_to_surface

Parameters:

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…)

Intersection Curve

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.intersection_curve

Parameters:

a, b: {body} | {face: [x,y,z], body?} | {sketch, curve} (a curve of another sketch, standing in for its extrusion along that sketch's normal): 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…)

Spun Profile

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.spun_profile

Parameters:

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…)

Isoparametric Curve

Command group: SKETCH › CREATE

Parameter	Type	Required	Description
face	[x,y,z] point on the face	Yes	the curve passes through it
body		No
direction	u\|v\|[x,y,z]	No	default u

Automation details

Command ID: sketch.isoparametric_curve

Parameters:

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…)

Fit Curves to Mesh Section

Command group: SKETCH › CREATE

Automation details

Command ID: sketch.fit_curves_to_section

Parameters:

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

Horizontal/Vertical

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
line	id	Yes
points	[a, b]	Yes	point ids or {midpoint: line_id}; accepted midpoints reuse or create a point with a Midpoint constraint
mode	horizontal\|vertical	No

Automation details

Command ID: sketch.constraint.horizontal_vertical

Parameters:

line: id | points: [a, b] (point ids or {midpoint: line_id}; accepted midpoints reuse or create a point with a Midpoint constraint); mode?: horizontal|vertical

Coincident

Command group: SKETCH › CONSTRAINTS

Automation details

Command ID: sketch.constraint.coincident

Parameters:

a, b: points (or a line's middle as {midpoint: line}, which becomes a point tied there), 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), or two circles/arcs (the second lies on the first: concentric and equal, `constraints` lists both); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Tangent

Command group: SKETCH › CONSTRAINTS

Automation details

Command ID: sketch.constraint.tangent

Parameters:

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), or the end point of a line or an arc: that end then lies on the other curve (or on the other end point), and its curve is tangent there, in one step (`constraints` lists both); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Equal

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	lines or circles/arcs	Yes
b	lines or circles/arcs	Yes

Automation details

Command ID: sketch.constraint.equal

Parameters:

a, b: lines or circles/arcs; or curves: [2 to 200 lines or circles/arcs], each made equal to the first, in one step; any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Parallel

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	lines or sketch axes	Yes
b	lines or sketch axes	Yes	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

Automation details

Command ID: sketch.constraint.parallel

Parameters:

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); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Perpendicular

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	lines or sketch axes	Yes
b	lines or sketch axes	Yes	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

Automation details

Command ID: sketch.constraint.perpendicular

Parameters:

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); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Fix/Unfix

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
entity	point or curve	Yes
entities	[points and curves]	Yes
fixed	bool	No	default: fix them all unless all are fixed, then unfix

Automation details

Command ID: sketch.constraint.fix

Parameters:

entity: point or curve | entities: [points and curves]; fixed?: bool (default: fix them all unless all are fixed, then unfix)

MidPoint

Command group: SKETCH › CONSTRAINTS

Automation details

Command ID: sketch.constraint.midpoint

Parameters:

point, line | a, b in pick order: a point and a line (either way round), or two lines whose midpoints meet (the first stays, the second moves); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Concentric

Command group: SKETCH › CONSTRAINTS

Automation details

Command ID: sketch.constraint.concentric

Parameters:

a, b: two circles/arcs, or a circle/arc and a sketch point (including origin), in either order; the point and the curve's centre become coincident; any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Collinear

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	lines or sketch axes	Yes
b	lines or sketch axes	Yes	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

Automation details

Command ID: sketch.constraint.collinear

Parameters:

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); any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Symmetry

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	two points or two curves	Yes
b	two points or two curves	Yes	lines mirror their ends, circles/arcs their centres

Automation details

Command ID: sketch.constraint.symmetry

Parameters:

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; any of them may be a model edge {edge: [x,y,z], body?} or vertex {vertex: [x,y,z], body?}, projected into the sketch first (reported in created)

Curvature

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
a	two curves sharing an end point	Yes
b	two curves sharing an end point	Yes	curvature continuous, G2

Automation details

Command ID: sketch.constraint.curvature

Parameters:

a, b: two curves sharing an end point (curvature continuous, G2)

Polygon

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
lines	[line ids] of a closed chain: equal sides with every corner on one circle	Yes	a regular polygon

Automation details

Command ID: sketch.constraint.polygon

Parameters:

lines: [line ids] of a closed chain: equal sides with every corner on one circle (a regular polygon)

AutoConstrain

Command group: SKETCH › CONSTRAINTS

Automation details

Command ID: sketch.auto_constrain

Parameters:

tolerance?: mm (default 0.01), angle_tolerance?: deg (default 1), dimensions?: bool (default true): infer constraints, then dimension until fully constrained

AutoConstrain from Datum

Command group: SKETCH › CONSTRAINTS

Parameter	Type	Required	Description
datum	point ref	Yes	default origin

Automation details

Command ID: sketch.auto_constrain_from_datum

Parameters:

datum: point ref (default origin); like AutoConstrain with positions measured from the datum

SKETCH › MODIFY

Blend Curve

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
a		Yes
b	end points of two curves	Yes	"l1.end", "a2.start"
continuity	g1\|g2\|g3\|g4	No	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

Automation details

Command ID: sketch.blend_curve

Parameters:

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…)

Fillet

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
point	corner shared by two curves	Yes	"l1.end"
points	[corners]\| a	Yes	all rounded alike: one radius, the rest equal; a corner is a point reference or {a, b}, the two curves meeting there
b	two lines or arcs meeting at a corner	Yes	two lines that share no end are first brought to where they meet: the nearer end of a line that stops short moves there, and a line that runs past is cut there, losing its shorter piece
radius	expr	Yes

Automation details

Command ID: sketch.fillet

Parameters:

point: corner shared by two curves ("l1.end") | points: [corners] (all rounded alike: one radius, the rest equal; a corner is a point reference or {a, b}, the two curves meeting there) | a, b: two lines or arcs meeting at a corner (two lines that share no end are first brought to where they meet: the nearer end of a line that stops short moves there, and a line that runs past is cut there, losing its shorter piece); 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`). An ellipse's axis line is never a side of a corner (also for the chamfers). 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…)

Equal Distance Chamfer

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
point	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}
points	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}
b	a corner of two lines	Yes	two that share no end are first brought to where they meet, as in sketch.fillet

Automation details

Command ID: sketch.chamfer.equal_distance

Parameters:

point | points: [corners] (every corner cut alike; a corner is a point reference or {a, b}) | a, b: a corner of two lines (two that share no end are first brought to where they meet, as in sketch.fillet); 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…)

Distance and Angle Chamfer

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
point	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order
points	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order
b	a corner of two lines	Yes	two that share no end are first brought to where they meet, as in sketch.fillet
distance	along a	Yes
angle	deg from a	Yes

Automation details

Command ID: sketch.chamfer.distance_angle

Parameters:

point | points: [corners] (every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order) | a, b: a corner of two lines (two that share no end are first brought to where they meet, as in sketch.fillet); 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…)

Two Distance Chamfer

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
point	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order
points	[corners]\| a	Yes	every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order
b	a corner of two lines	Yes	two that share no end are first brought to where they meet, as in sketch.fillet
distance	along a	Yes
distance2	along b	Yes

Automation details

Command ID: sketch.chamfer.two_distance

Parameters:

point | points: [corners] (every corner cut alike; a corner is a point reference or {a, b}, and a point's `a` is the first of its two lines in curve order) | a, b: a corner of two lines (two that share no end are first brought to where they meet, as in sketch.fillet); 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…)

Offset

Command group: SKETCH › MODIFY

Default keyboard shortcut: O

Parameter	Type	Required	Description
flip	bool reverses the primary side	No

Automation details

Command ID: sketch.offset

Parameters:

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, including ends that only coincide). A corner is trimmed back to the crossing when the offset runs past it, and extended until the offset curves intersect when the corner falls short; 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; instances?: whole number or unitless expression, 1…100 (default 1): each instance after the first offsets the instance before it by the same distance again, so instance n stands n distances from the curves picked. Every instance of a side is driven by that side's own dimension, and each entry of `sides` names its `instance`; an instance the shape cannot take refuses the whole command. 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…)

Trim

Command group: SKETCH › MODIFY

Default keyboard shortcut: T

Automation details

Command ID: sketch.trim

Parameters:

curve: id, at: [x,y] (the piece to remove: between the nearest intersections around it). Trimming a line source or its single-line offset releases linked extents (offset_released: curve ids), retaining their driving normal-distance dimensions and parallel relations. 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…)

Extend

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
curve	id	Yes
at	[x,y] near the end to extend	Yes	a line runs on to the nearest curve, or the previewed reach when nothing is in the way; an arc grows along its circle and closes into a whole circle when nothing stops it
curves	[id, id]	Yes	two lines or arcs of this sketch, grown until they meet and joined there
at	[[x,y],[x,y]]	No	one point per curve: the end to grow; default the end nearest the meeting point

Automation details

Command ID: sketch.extend

Parameters:

curve: id, at: [x,y] near the end to extend (a line runs on to the nearest curve, or the previewed reach when nothing is in the way; an arc grows along its circle and closes into a whole circle when nothing stops it) | curves: [id, id] (two lines or arcs of this sketch, grown until they meet and joined there), at?: [[x,y],[x,y]] (one point per curve: the end to grow; default the end nearest the meeting point). `curve` and `curves` exclude each other; the two-curve form returns moved: the meeting point's id

Break

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
curve	id	Yes
at	[x,y]	Yes	split at intersections; at a point where the curve ends and another curve meets, the curve gets its own end there and the two are no longer joined
points	[[x,y]…]	Yes	1…1000 positions projected onto the curve; duplicates are merged

Automation details

Command ID: sketch.break

Parameters:

curve: id, at: [x,y] (split at intersections; at a point where the curve ends and another curve meets, the curve gets its own end there and the two are no longer joined) | 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

Command group: SKETCH › MODIFY

Parameter	Type	Required
entities	[curve/point ids]	Yes
base	[x,y] or point ref	Yes
factor	number	Yes

Automation details

Command ID: sketch.scale

Parameters:

entities: [curve/point ids], base: [x,y] or point ref, factor: number; the driving length and radius dimensions wholly inside the selection scale too (a formula becomes `(formula) * factor`)

Transform

Command group: SKETCH › MODIFY

Default keyboard shortcut: G

Parameter	Type	Required	Description
entities	[curve/point ids]	Yes
factor	number	No	scale
angle	degrees	No	turn
center	[x,y] or point ref	No	what scales and turns stay put; default [0,0]
translate	[dx,dy]	No	applied last

Automation details

Command ID: sketch.transform

Parameters:

entities: [curve/point ids], factor?: number (scale), angle?: degrees (turn), center?: [x,y] or point ref (what scales and turns stay put; default [0,0]), translate?: [dx,dy] (applied last); scales, turns and moves in one step

Move/Copy Sketch Entities

Command group: SKETCH › MODIFY

Parameter	Type	Required	Description
entities	[ids]	Yes
translate	[dx,dy]	No
angle	deg	No
center	[x,y]	No
copy	bool	No
rotate_constraints	bool	No	default true; false keeps constraints unchanged

Automation details

Command ID: sketch.move

Parameters:

entities: [ids], translate?: [dx,dy], angle?: deg, center?: [x,y], copy?: bool, rotate_constraints?: bool (default true; false keeps constraints unchanged); a rotation turns the constraints tied to the sketch axes when all their geometry moves (horizontal and vertical relations and dimensions swap at odd quarter turns and stay at half turns, line angles turn with the line) and removes the horizontal and vertical ones that cannot hold at other angles; picking a text outline or linked point transforms its whole text source once, and copies remain editable text; copy also accepts drawn 3D curves, preserving exact arcs and height above the sketch plane; a turned rectangle keeps its shape: parallel and perpendicular relations replace the horizontal and vertical ones lost; returns `released`: the constraints tying the moved geometry to what stays that the move let go, as {id, kind}, and `added`: the relations put in their place, as {id, kind}. 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

Insert DXF

Command group: SKETCH › INSERT

Parameter	Type	Required	Description
path	ASCII DXF	Yes	blocks expanded
text	ASCII DXF	Yes	blocks expanded
align	"origin"\| "center"	No	default: `at` is where the file's origin goes; `at` is where the drawing's middle goes and it turns and scales about it
tolerance	mm within which ends join	No	default 0.0001
fixed	bool	No	a Fix constraint on every point the drawing adds, as sketch.constraint.fix puts one; a circle's or ellipse's radius stays free; default false
plane		No	when no sketch is active, a new sketch on it; default XY

Automation details

Command ID: sketch.insert_dxf

Parameters:

path | text: ASCII DXF (blocks expanded); at?: [x,y] offset, scale? | width? | height?: mm, the size of the drawn geometry's bounds before rotation, aspect kept (win over scale); angle?: degrees, about the drawing's origin (or its centre); align?: "origin" (default: `at` is where the file's origin goes) | "center" (`at` is where the drawing's middle goes and it turns and scales about it); tolerance?: mm within which ends join (default 0.0001); fixed?: bool (a Fix constraint on every point the drawing adds, as sketch.constraint.fix puts one; a circle's or ellipse's radius stays free; default false); 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…)

Insert SVG

Command group: SKETCH › INSERT

Parameter	Type	Required	Description
path	SVG	Yes
text	SVG	Yes
size_from	"geometry"\| "viewbox"	No	default: width and height are the bounds of the drawn geometry; the SVG sheet: its viewBox, else its width and height; a drawing smaller than its sheet then comes out smaller than width or height say
align	"origin"\| "center"	No	default: `at` is where the file's origin goes; `at` is where the drawing's (or sheet's) middle goes and it turns and scales about it
tolerance	mm within which ends join	No	default 0.0001
fixed	bool	No	every point it adds gets a Fix constraint, so the drawing stays where it is put
plane		No	when no sketch is active, a new sketch on it; default XY

Automation details

Command ID: sketch.insert_svg

Parameters:

path | text: SVG; at?: [x,y] offset, scale? | width? | height?: mm, the drawing's size before rotation, aspect kept (win over scale); size_from?: "geometry" (default: width and height are the bounds of the drawn geometry) | "viewbox" (the SVG sheet: its viewBox, else its width and height; a drawing smaller than its sheet then comes out smaller than width or height say); angle?: degrees, about the drawing's origin (or its centre); align?: "origin" (default: `at` is where the file's origin goes) | "center" (`at` is where the drawing's (or sheet's) middle goes and it turns and scales about it); tolerance?: mm within which ends join (default 0.0001); fixed?: bool (every point it adds gets a Fix constraint, so the drawing stays where it is put); 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

Command group: SKETCH › INSERT

Parameter	Type	Required	Description
path		Yes	base64 PNG or JPEG
data		Yes	base64 PNG or JPEG
plane	XY\|XZ\|YZ\|{face: [x,y,z]}\|…	No	default XY
center	[x,y] on the plane	No
at	[x,y,z]	No
width	mm	No	default 100
angle	deg	No
opacity	0…1	No	default 0.5
flip		No
name		No

Automation details

Command ID: canvas.insert

Parameters:

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?

Decal

Command group: SKETCH › INSERT

Parameter	Type	Required	Description
path		Yes
data		Yes
width	mm	No
angle	deg	No
opacity		No	default 1

Automation details

Command ID: canvas.decal

Parameters:

path | data; face: [x,y,z] on a planar face (the image is centred there), or the picked face as sketch.create's plane takes it ({face, body, index, path?}); width?: mm; angle?: deg; opacity?: (default 1)

Edit Canvas

Command group: SKETCH › INSERT

Parameter	Type	Required	Description
canvas	id or name	Yes
center		No
width		No
angle	deg	No
opacity		No
flip		No
visible		No
name		No
locked		No	a locked canvas refuses center, width, angle, flip, Calibrate and Delete

Automation details

Command ID: canvas.edit

Parameters:

canvas: id or name; center?, width?, angle?: deg, opacity?, flip?, visible?, name?, locked? (a locked canvas refuses center, width, angle, flip, Calibrate and Delete)

SKETCH › INSPECT

Curvature Comb Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
curves	[sketch curve ids]	No	sketch?: id\|name, default active
edges	[[x,y,z] points on body edges: the edge whose exact curve passes nearest]	No
faces	[[x,y,z] points on faces] with count?: isoparametric curves each way	No	default 4; combs along the face's iso grid
scale	comb length per unit curvature	No	default auto: the longest tooth a fifth of the combs' size

Automation details

Command ID: inspect.curvature_comb

Parameters:

curves?: [sketch curve ids] (sketch?: id|name, default active) | edges?: [[x,y,z] points on body edges: the edge whose exact curve passes nearest] | faces?: [[x,y,z] points on faces] with count?: isoparametric curves each way (default 4; combs along the face's iso grid); density?: teeth per curve, 2…2000 (default 40; on an edge or an iso curve exactly that many, evenly spaced along its parameter); scale?: comb length per unit curvature (default auto: the longest tooth a fifth of the combs' size); length?: a multiplier on the automatic scale, 0.01…100 (default 1; ignored with `scale`); add?: true keeps the combs shown and adds these, every comb again at one scale (with nothing picked it draws those shown again with this call's options, or turns the analysis on with none); clear?: true turns the analysis off. Every comb of a call shares one scale, so tooth lengths compare across curves; the viewport draws them. The curvature is exact: from each sketch curve, edge curve (line, circle, ellipse, B-spline, NURBS, intersection curve) or face surface's own derivatives, never from the display mesh; a face's teeth are the surface's normal curvature along each iso curve, along the surface normal. → combs: [{curve, teeth: [[foot, tip]], envelope: [tip], max_curvature, min_radius}] (those shown, with `add`), scale

Minimum Radius Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
curves	[sketch curve ids]	No	sketch?
edges	[[x,y,z]…]	No
faces	[[x,y,z]…]	No	default: every face of every body

Automation details

Command ID: inspect.minimum_radius

Parameters:

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

Isocurve Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
faces	[[x,y,z]…] points on faces	Yes	1…100
add	true keeps the faces already shown	No
clear	true turns the analysis off.	No

Automation details

Command ID: inspect.isocurve

Parameters:

faces: [[x,y,z]…] points on faces (1…100); count?: whole number of curves each way, 1…100 (default 8); add?: true keeps the faces already shown; clear?: true turns the analysis off. → each face's isoparametric curves, u = const and v = const of its surface, evenly spaced across it and cut to its trims, as points (`curves`) and per face (`faces`); the viewport draws them

Center of Mass

Command group: SKETCH › INSPECT

Automation details

Command ID: inspect.center_of_mass

Parameters:

bodies?: [names] (default all): the centre of mass (uniform density) of each and of all together, from the exact mass properties `inspect.measure` takes → center, volume, bodies: [{body, center, volume}], skipped: [{body, reason}] (bodies that enclose no volume or could not be measured)

Zebra Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
stripes	number across the view	No	default 12
clear	true turns the analysis off	No

Automation details

Command ID: inspect.zebra

Parameters:

stripes?: number across the view (default 12); clear?: true turns the analysis off

Draft Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
pull	[x,y,z] direction	No	default Z
angle	degrees	No	default 1
clear	true turns the analysis off	No

Automation details

Command ID: inspect.draft

Parameters:

pull?: [x,y,z] direction (default Z); angle?: degrees (default 1); clear?: true turns the analysis off

Environment Map Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
clear	true turns the analysis off	No

Automation details

Command ID: inspect.environment_map

Parameters:

clear?: true turns the analysis off

Accessibility Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
direction	[x,y,z] the tool comes from	No	default Z, from above
clear	true turns the analysis off	No

Automation details

Command ID: inspect.accessibility

Parameters:

direction?: [x,y,z] the tool comes from (default Z, from above); clear?: true turns the analysis off

Curvature Map Analysis

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
radius	mm shown red	No	default: a tenth of the model's size
clear	true turns the analysis off	No

Automation details

Command ID: inspect.curvature_map

Parameters:

radius?: mm shown red (default: a tenth of the model's size); clear?: true turns the analysis off

Inspect Sketch

Command group: SKETCH › INSPECT

Parameter	Type	Required	Description
sketch	id\|name	No	default active

Automation details

Command ID: sketch.inspect

Parameters:

sketch?: id|name (default active)

SKETCH › PATTERN

Mirror

Command group: SKETCH › PATTERN

Automation details

Command ID: sketch.mirror

Parameters:

entities: [curve/point ids], line: straight curve id, x / y for a sketch axis, or {axis: X|Y|Z} for an origin axis (the mirror line is the axis's projection into the sketch plane; an axis perpendicular to the plane is refused) (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…)

Circular Pattern

Command group: SKETCH › PATTERN

Parameter	Type	Required	Description
alignment	left\|center\|right	No	default right
reversed	bool	No	default false

Automation details

Command ID: sketch.pattern.circular

Parameters:

entities: [ids], center: [x,y] or point ref, count: 2…500 (number or unitless expression, retained through edits), angle?: total deg, number or expression (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…)

Rectangular Pattern

Command group: SKETCH › PATTERN

Parameter	Type	Required	Description
entities	[ids]	Yes
count		Yes
spacing		Yes
count2		No
spacing2		No
spacings	length numbers or expressions	Yes
direction	sketch line ids	No
direction2	sketch line ids	No	live references
dir	[x,y] vectors	No
dir2	[x,y] vectors	No	defaults: sketch x, perpendicular to direction 1
alignment		No
alignment2	left\|center\|right	No	default right
reversed2	bool	No	default false

Automation details

Command ID: sketch.pattern.rectangular

Parameters:

entities: [ids], count, spacing; count2?, spacing2?; counts: positive integer numbers or expressions, at most 500 instances total; spacings: length numbers or expressions; 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

Continuity Analysis

Command group: SURFACE › INSPECT

Read the solid features guide.

Parameter	Type	Required	Description
body	name	No	default: the visible bodies
edges	[x,y,z] points or {"index": i}	No	default: every edge of the body; a pick must match one body
gap_tolerance_mm		No	default 0.001
angle_tolerance_deg		No	default 1
curvature_tolerance_per_mm		No	default 0.01
curvature_change_tolerance_per_mm2		No	default 0.001
curvature_change_rate_tolerance_per_mm3		No	default 0.0001
add	true keeps the seams already shaded and adds these	No	measuring an edge again replaces it
clear	true turns the analysis off.	No

Automation details

Command ID: inspect.continuity

Parameters:

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), curvature_change_tolerance_per_mm2? (default 0.001), curvature_change_rate_tolerance_per_mm3? (default 0.0001); add?: true keeps the seams already shaded and adds these (measuring an edge again replaces it); clear?: true turns the analysis off. → each edge's worst gap (G0), normal angle (G1), curvature jump (G2), jump of the curvature's change across the seam dκ/ds (G3) and of that change's rate d²κ/ds² (G4), from the faces' exact derivatives, as {value, at: [x,y,z], edge_fraction}; its order (g0…g4: the highest every station meets within the tolerances, null where the faces do not meet), its verdict (smooth: g2 or better, curvature_jump, sharp or gap) and a summary; the seams are shaded in the viewport

SURFACE › CREATE

Boundary Surface

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
curves	[2 to 4 sketch curve ids in loop order]	Yes	each one ends where the next begins and the last where the first does; two: the patch spans between them and leaves each boundary along the tangent across it; three or four: the flat patch of the loop, three collapsing the side opposite the first curve to the corner there
continuity	g0\|g1\|g2\|g3 \| [one per curve]	No	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	No	default 0: how full the middle is, without touching a boundary; two curves only
operation	new\|join	No	default new; join sews the surface into the body of its first edge curve, a solid when it closes the gap
body_name		No	a surface body

Automation details

Command ID: surface.boundary

Parameters:

Either a loop of one sketch's curves — 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; two: the patch spans between them and leaves each boundary along the tangent across it; three or four: the flat patch of the loop, three collapsing the side opposite the first curve to the corner there); 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; two curves only); samples?: 8…512 stations per boundary (default 25) — or a curve network — u: [curve] (two or more one way: the surface lofts through them), v?: [curve] (crossing every u-curve once: two each way give a Coons patch, more a Gordon surface through every curve; a curve that misses another by more than 0.01 mm is refused, naming the pair), each curve "id" (a curve of `sketch`) | {sketch?: id|name, curves: [ids meeting end to end]} (planar or 3D sketch curves) | {body: name, edges: [[x,y,z]] (points on a chain of its edges), continuity?: g0|g1|g2 (default g0; g1 the surface leaves tangent to the face beside a surface's open edges, g2 with its curvature too; on curves of one direction only)} | {point: [x,y,z]} (a side collapsed to a point: a three-sided patch); operation?: new|join (default new; join sews the surface into the body of its first edge curve, a solid when it closes the gap). name?, body_name? (a surface body)

Patch

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
sketch	id\|name and profiles?	No	planar patches of sketch regions
profiles_3d	[indices]	Yes	the sketch's planar 3D-sketch loops, each patched in its own plane, as listed by sketch.inspect
edges	[[x,y,z]]	Yes	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
continuity	g0\|g1\|g2\|g3\|g4	No	edges only, default g0: how the patch meets the faces beside the loop — g1 their tangent planes, g2 also their curvature across the edges, g3 also its rate of change, g4 the change of that rate
points	[[x,y,z]]	No	edges only, up to 64: points the patch passes through
crown	number −0.9…3	No	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 higher edge
name		No
body_name		No

Automation details

Command ID: surface.patch

Parameters:

sketch?: id|name and profiles? (planar patches of sketch regions) or profiles_3d: [indices] (the sketch's planar 3D-sketch loops, each patched in its own plane, as listed by sketch.inspect) | 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|g3|g4 (edges only, default g0: how the patch meets the faces beside the loop — g1 their tangent planes, g2 also their curvature across the edges, g3 also its rate of change, g4 the change of that rate) or [{edge: [x,y,z], g: g0|g1|g2|g3|g4}] (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 higher edge); name?, body_name?

Thicken

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[surface names]	Yes
thickness	expr	Yes	negative: against the normal
symmetric	bool	No
operation	new\|join\|cut\|intersect	No
targets		No

Automation details

Command ID: surface.thicken

Parameters:

bodies: [surface names]; thickness: expr (negative: against the normal); symmetric?: bool; operation?: new|join|cut|intersect; targets?

Surface Extrude

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
sketch	id\|name	No
curves	[curve ids]	No	open or closed chains of curves meeting end to end
distance	expr	Yes
direction	positive\|negative\|symmetric	No	symmetric: distance is the total, split evenly around the start plane, as solid.extrude
convention	total_distance\|legacy_per_side	No	as solid.extrude; default total_distance; legacy_per_side: the distance on each side, as older symmetric surface extrudes keep
distance2	expr	No
start_offset	expr	No
name		No
body_name		No	a surface body: walls only, no caps

Automation details

Command ID: surface.extrude

Parameters:

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 (symmetric: distance is the total, split evenly around the start plane, as solid.extrude); convention?: total_distance|legacy_per_side (as solid.extrude; default total_distance; legacy_per_side: the distance on each side, as older symmetric surface extrudes keep); distance2?: expr; start_offset?: expr; name?, body_name? (a surface body: walls only, no caps)

Surface Revolve

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
sketch	id\|name	No
curves	[curve ids] and/or profiles?	No	as surface.extrude
axis	sketch line id\|x\|y\|X\|Y\|Z\|{type: world, axis: X\|Y\|Z}\|{sketch, curve}\|construction axis name\|{origin, dir}\| {edge\|face: [x,y,z]}	Yes	a line of another sketch, followed in that sketch; origin: numbers or length expressions, followed when parameters change; a straight or circular edge, or a cylinder, cone or torus face: about its axis, followed as the model changes
angle	expr	No	default 360 deg
angle2	expr	No	the other side
symmetric	bool	No
name		No
body_name		No	a surface body, no caps; a solid where a full turn closes it

Automation details

Command ID: surface.revolve

Parameters:

sketch?: id|name; curves?: [curve ids] and/or profiles? (as surface.extrude); axis: sketch line id|x|y|X|Y|Z|{type: world, axis: X|Y|Z}|{sketch, curve} (a line of another sketch, followed in that sketch)|construction axis name|{origin, dir} (origin: numbers or length expressions, followed when parameters change) | {edge|face: [x,y,z]} (a straight or circular edge, or a cylinder, cone or torus face: about its axis, followed as the model changes); 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

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
sketch	id\|name	No
curves	[curve ids] and/or profiles?	No	as surface.extrude
path_sketch	sketch	Yes
path	[curve ids in order]	Yes	a path with corners, or 3D curves, gives ruled walls mitred at the corners
path_body	body name	No
path_edges	[points on its edges]	No	the path is a chain of that body's edges, instead of a sketch's curves
orientation		No
twist		No
scale		No
rails		No
rail_fit		No	as solid.sweep
name		No
body_name		No	a surface body, no caps

Automation details

Command ID: surface.sweep

Parameters:

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); path_body?: body name; path_edges?: [points on its edges] (the path is a chain of that body's edges, instead of a sketch's curves); orientation?, twist?, scale?, rails?, rail_fit? (as solid.sweep); name?, body_name? (a surface body, no caps)

Surface Loft

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
sections	[{sketch, curves?: [curve ids], profiles?} \| {body, edges: [[x,y,z]]}]	Yes	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]	No	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]	No	default 0: how full each end leaves, -0.9 flattest to 3 fullest
rails		No
rail_fit		No	as solid.loft; sketch sections only, both ends g0
name		No
body_name		No	a surface body: ruled between two sections, smooth through three or more; no caps

Automation details

Command ID: surface.loft

Parameters:

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); rails?, rail_fit? (as solid.loft; sketch sections only, both ends g0); name?, body_name? (a surface body: ruled between two sections, smooth through three or more; no caps)

Offset Surface

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
faces	[[x,y,z]]	Yes	points on the faces
body		No
distance	expr	Yes	signed, along the faces' normals; 0 copies the faces
chain	bool	No	each pick's whole smooth chain of faces
tolerance	expr	No	how far a fitted face may stray, default 0.01 mm

Automation details

Command ID: surface.offset

Parameters:

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)

Ruled Surface

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
body		Yes
edges	[[x,y,z]]	Yes	points on a chain of its edges, open or closed
distance	expr	Yes	how far the strip reaches
mode	normal\|tangent\|angle\|direction	No	default normal: along the normal of the face beside each edge; tangent: continuing it
angle	expr	No	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]	No	direction mode: the rulings; angle mode: the reference, e.g. a pull direction for a draft
face	[x,y,z]	No	a point on the face the directions come from; default: the face beside the most picked edges
flip	bool	No	the other side
corners	mitre\|round	No	sharp corners of the chain; inside corners are always cut back

Automation details

Command ID: surface.ruled

Parameters:

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); far?: [null|[[x,y,z]]] (per chain edge, the interior control points of a free strip's far curve, as the default curve's handles list them; null: the default). A constant ruling, or one keeping its angle to an arc's axis, gives an exact plane, cylinder or cone; where the rulings turn freely along an edge, the strip is the exact ruled surface to a far curve of its own (from corner to corner, fair, near the rulings' ends). A new surface body

Blend Surface

Command group: SURFACE › CREATE

Read the solid features guide.

Parameter	Type	Required	Description
from	{body, edges: [[x,y,z]]}	Yes
to	{body, edges: [[x,y,z]]}	Yes	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]	No	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]	No	default 0: how full each end leaves, -0.9 flattest to 3 fullest
align	[[x,y,z], [x,y,z]]	No	a point each end leaves towards, when the faces at the picks do not say
seam	[[x,y,z], [x,y,z]]	No	a point on each chain its stations start from: two closed chains otherwise pair the way that keeps the blend from twisting; an open chain starts at the end nearer its point; a closed chain blends only to a closed chain
stitch	bool	No	sew the blend onto its two bodies where the boundaries meet, replacing them
name		No
body_name		No

Automation details

Command ID: surface.blend

Parameters:

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); seam?: [[x,y,z], [x,y,z]] (a point on each chain its stations start from: two closed chains otherwise pair the way that keeps the blend from twisting; an open chain starts at the end nearer its point; a closed chain blends only to a closed chain); stitch?: bool (sew the blend onto its two bodies where the boundaries meet, replacing them); name?, body_name?

SURFACE › MODIFY

Stitch

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
bodies	[names]	Yes	surfaces sewn into the first; a solid when they close
tolerance	expr	No	default: tight

Automation details

Command ID: surface.stitch

Parameters:

bodies: [names] (surfaces sewn into the first; a solid when they close); tolerance?: expr (default: tight)

Extend

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body	surface name	Yes
edges	[[x,y,z]]	Yes	points on boundary edges to push out
distance	expr	Yes	unless up_to
mode	natural\| tangent\| curvature	No	the surface itself continued: a B-spline's end spans continued, which keeps planes and surfaces of revolution on themselves; the default; the face continued tangent to its surface across the edge, G1; continued keeping the surface's curvature across the edge too, G2
up_to	plane\| {body, point}\| "bounds"	No	XY\|XZ\|YZ\|plane name\|{origin, normal}; a face, its surface extended; natural: back to the surface's own bounds, undoing a trim
neighbours	bool	No	default true: the edges next to an extended edge are lengthened to meet it; false: the extension's sides run square to the edge

Automation details

Command ID: surface.extend

Parameters:

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: a B-spline's end spans continued, which keeps planes and surfaces of revolution on themselves; the default) | tangent (the face continued tangent to its surface across the edge, G1) | curvature (continued keeping the surface's curvature across the edge too, 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)

Trim

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body	surface name	Yes
plane	XY\|XZ\|YZ\|plane name\|{origin, normal} or tool: {body, point}	Yes	a face, its surface extended
curves	{sketch, curves?: [curve ids] (chains of curves meeting end to end; default every curve), direction?: normal\|[x,y,z] (swept onto the surface along the sketch's normal, the default, or this direction)}	Yes
keep	[x,y,z]	Yes	a point on the side to keep
keep_with	[x,y,z] or [[x,y,z], …]	Yes	what to keep of it
extend	bool	No	a surface that stops short of the other is extended to meet it
stitch	bool	No	the kept pieces sewn into `body`; `with` is then gone

Automation details

Command ID: surface.trim

Parameters:

body: surface name; plane: XY|XZ|YZ|plane name|{origin, normal} or tool: {body, point} (a face, its surface extended) or curves: {sketch, curves?: [curve ids] (chains of curves meeting end to end; default every curve), direction?: normal|[x,y,z] (swept onto the surface along the sketch's normal, the default, or this direction)}; keep: [x,y,z] (a point on the side to keep) or [[x,y,z], ...] (points on the regions to keep: the pieces that hang together once cut). Mutual trim: with: another surface (one face each; leave out plane, tool and curves), keep_with: [x,y,z] or [[x,y,z], ...] (what to keep of it); each is cut where the other's surface (extended) meets it; extend?: bool (a surface that stops short of the other is extended to meet it); stitch?: bool (the kept pieces sewn into `body`; `with` is then gone)

Untrim

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
face	{body, point}	Yes
holes	all\|[[x,y,z]]	No	points on the inner loops to remove; default: all
outer	bool	No	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	No	untrim a surface body's face where it is; a solid's face is always copied out

Automation details

Command ID: surface.untrim

Parameters:

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

Unstitch

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body		Yes
faces	[[x,y,z]]	No	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

Automation details

Command ID: surface.unstitch

Parameters:

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

Reverse Normal

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body		Yes	a surface
faces	[[x,y,z]]	No	points on the faces to turn over; default: all of them

Automation details

Command ID: surface.reverse_normal

Parameters:

body (a surface); faces?: [[x,y,z]] (points on the faces to turn over; default: all of them)

Fair Surface

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body	surface name	Yes
faces	[[x,y,z]] points on the faces to fair	No	default: every face
strength	number	No	0..1 of the full fairing step, default 1
iterations	number	No	1..1000 steps, default 1
keep_edges	bool	No	default true: hold the boundary row and the row next to it, so a face keeps meeting its neighbours in position and in tangent
name		No

Automation details

Command ID: surface.fair

Parameters:

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

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
planned	a	Yes
b	{body, point}	Yes	two faces of separate bodies that meet or cross; the points pick the side the ball rolls on
radius	expr	Yes
trim	both\|first\|none	No

Automation details

Command ID: surface.fillet

Parameters:

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

Match Surface

Command group: SURFACE › MODIFY

Read the solid features guide.

Parameter	Type	Required	Description
body	surface name	Yes	the body whose face is rebuilt
faces	[[x,y,z]]	No	points on that face, default: the body's first
target	body name	Yes	the body the seam must meet
edges	[[x,y,z]]	Yes	points on one edge chain of the target: the rebuilt boundary takes its place
order	g1\|g2\|g3	No	default g2: position and tangent plane, the curvature too, or how that curvature changes along the seam

Automation details

Command ID: surface.match

Parameters:

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

Flange

Command group: SHEET METAL › CREATE

Create a sheet metal base, bend an existing edge into a wall, or build a contour from an open sketch. The sheet metal rule supplies the material thickness and bend settings so the folded and flat versions describe the same part.

Before you start

Flange type	What you need to select	Result
Base	A closed region in a finished sketch.	A new flat sheet metal body.
Edge	One or more supported edges of an existing sheet metal body.	Bent walls along those edges. A sketch is not required for this mode.
Contour	An open chain of straight sketch lines.	A sheet following that outline, extended by the chosen distance.

Choose or create a Sheet Metal Rule before building the part. To work from an ordinary solid plate, use Convert to Sheet Metal first. An arbitrary solid edge does not become a sheet metal edge just by selecting Flange.

Options

Choice	Meaning
Type	Base, Edge or Contour. The selection determines which input is appropriate.
Rule	Sets thickness, bend radius, K-factor and the gaps/reliefs that keep bends manufacturable. Change thickness in the rule, not as a flange height.
Height	Sets the edge flange’s height. Check the height reference and preview when matching a drawing dimension.
Angle	Sets how far the edge bends; 90° makes a right-angle wall.
Per-edge angle and height	Lets selected edges in one feature have different dimensions. Empty values use the common setting.
Position	Places the flange relative to the selected edge. The preview shows which material remains inside or outside the original outline.
Flip	Bends toward the other side of the sheet.
Corner Relief Shape and size	Use the rule’s setting or override relief between edge flanges of this feature. These overrides are not available for base or contour flanges.
Distance	Sets the length of a contour flange’s extrusion along the open sketch.

Try it: two sides of a tray

Set a sheet rule with 1.5 mm thickness and 1.5 mm bend radius.
Draw and finish an 80 × 50 mm rectangular sketch.
Choose Flange, select the rectangle’s region and make a Base flange.
Choose Flange again, select an edge and set its height to 20 mm.
Add another 20 mm flange on the opposite edge. Check the bend directions before confirming each feature.
Use Create Flat Pattern to inspect the developed part and bend lines.

Tips and common mistakes

Do use one edge flange feature for adjoining walls whose shared corners should close together. Flanges made as separate features keep their own ends.
Do inspect warnings and the flat pattern; a relief that cannot fit may be left out with a warning.
Don’t confuse height with sheet thickness. The rule owns thickness.
Don’t select a sketch point for an edge flange: choose an edge of the sheet. For a base flange, select a closed sketch region instead.

Examples and community resources

An 80 by 50 mm sheet with two opposite 20 mm edge flanges

Resource	What to explore	Author and licence
Editable sheet metal demo	The rule, base sketch and two edge flanges used in this illustration.	SolidCraft contributors; MIT OR Apache-2.0.

Contribute a tip, demo, model or screenshot, explaining the edge or region that must be selected.

Path Flange

Command group: SHEET METAL › CREATE

Read the sheet metal guide.

Parameter	Type	Required	Description
edge	[x,y,z] on a top or bottom edge of the sheet	Yes
radius		No	default: rule

Automation details

Command ID: sheet.path_flange

Parameters:

edge: [x,y,z] on a top or bottom edge of the sheet; sketch + curves: an open chain of sketch lines drawn on a plane across that edge, from the edge out (each line one flange as long as the line, to the outer face from the virtual sharp; each corner one bend, turning the way the lines turn); radius? (default: rule); body?. One feature, one body

Perforate

Command group: SHEET METAL › CREATE

Read the sheet metal guide.

Parameter	Type	Required	Description
diameter	expr	Yes
pitch	expr	Yes
margin	expr	No	clear of edges, cut-outs, bends and the outline; default: the diameter
pattern	staggered\| square	No	60°, default
body		No

Automation details

Command ID: sheet.perforate

Parameters:

diameter, pitch: expr; margin?: expr (clear of edges, cut-outs, bends and the outline; default: the diameter); pattern?: staggered (60°, default) | square; body?; sketch? + profiles? (the outline: closed profiles of a sketch on a face of the sheet; holes only inside them, out of their inner loops) - a perforation field over the whole flat sheet or inside the outline: holes in the flat pattern (perforations), the DXF (layer PERFORATION) and the measured volume, not cut into the B-rep (#732)

Hem

Command group: SHEET METAL › CREATE

Fold a sheet metal edge back through a half turn to form a return. Use a hem when you need a doubled-over edge, rather than an upright wall.

Before you start

You need an existing sheet metal body and a supported free sheet edge. Make a base flange or convert a suitable solid plate first.
Select the edge, not a sketch line, face or point. Hem does not require a new sketch. A bend along a line inside the sheet uses Fold instead.
Leave room for the return so it does not run into another wall or return.

Options

Choice	Meaning
Edges	The sheet edges to turn back. Check that the preview changes the intended edge.
Length	The return’s length, measured to its outer face. It is not the thickness of the sheet.
Gap	Controls the inner radius of the return bend. Leave it empty to use the sheet rule’s hem setting.
Flip	Turns the return toward the other side of the sheet.

Try it: a returned edge

Create an 80 × 50 mm base flange in 1.5 mm sheet.
Choose Hem and select a free 80 mm edge of the sheet.
Set Length to 8 mm and Gap to 1.5 mm.
Check which side receives the return; use Flip if necessary, then confirm.
Inspect Create Flat Pattern to see the material needed for the bend.

Tips and common mistakes

Do check the bend in the preview: an edge returning toward another feature needs enough clearance.
Don’t draw a sketch line to tell Hem where to bend. Its input is an existing sheet edge; use Fold for a bend line through a panel.
Don’t use Hem for an ordinary right-angle wall. That is an edge Flange.

Examples and community resources

A sheet metal plate with one edge returned back toward the plate

Resource	What to explore	Author and licence
Editable hem demo	The sheet rule, base flange and 8 mm return used in this illustration.	SolidCraft contributors; MIT OR Apache-2.0.

Contribute a tip, demo, model or screenshot, explaining the selected edge and dimensions.

Fold

Command group: SHEET METAL › CREATE

Read the sheet metal guide.

Parameter	Type	Required	Description
line	sketch + curve	Yes	a sketch line on the sheet's base face; followed when the sketch changes
points	[[x,y,z], [x,y,z]]	Yes
angle		No	default 90 deg
radius		No	default: rule
position	centerline\|start\|end\|mould	No	where the line sits in the bend, default centerline
fixed	[x,y,z] on the side that stays	No	default: the larger side
flip		No	fold the other way
body		No

Automation details

Command ID: sheet.fold

Parameters:

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?

Convert to Sheet Metal

Command group: SHEET METAL › CREATE

Read the sheet metal guide.

Parameter	Type	Required	Description
body		Yes
rule		No
bends	[[x,y,z] on sharp edges]	No	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

Automation details

Command ID: sheet.convert

Parameters:

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)

Create Flat Pattern

Command group: SHEET METAL › CREATE

Read the sheet metal guide.

Parameter	Type	Required	Description
body		No

Automation details

Command ID: sheet.flat_pattern

Parameters:

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

Unfold

Command group: SHEET METAL › MODIFY

Read the sheet metal guide.

Parameter	Type	Required	Description
body		No	default: the last sheet body

Automation details

Command ID: sheet.unfold

Parameters:

body? (default: the last sheet body) — all bends

Refold

Command group: SHEET METAL › MODIFY

Read the sheet metal guide.

Parameter	Type	Required	Description
body		No	default: the last unfolded sheet

Automation details

Command ID: sheet.refold

Parameters:

body? (default: the last unfolded sheet)

Sheet Metal Rules

Command group: SHEET METAL › MODIFY

Read the sheet metal guide.

Parameter	Type	Required	Description
name		Yes	new or existing
thickness		No
k_factor		No
bend_radius		No
relief_width		No
relief_depth		No
corner_relief		No
hem_gap		No
gap		No	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	No	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
angle_display	bend\|included	No	how the DXF bend notes read the bend angles: the bend angle, default, or the included angle left between the bend's sides, 180° less it; the bend table gives both, and a flange's `angle` is always the bend angle
active	bool	No
delete	bool	No

Automation details

Command ID: sheet.manage_rules

Parameters:

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); angle_display?: bend|included (how the DXF bend notes read the bend angles: the bend angle, default, or the included angle left between the bend's sides, 180° less it; the bend table gives both, and a flange's `angle` is always the bend angle); active?: bool; delete?: bool

WELDMENTS › CREATE

Frame Member

Command group: WELDMENTS › CREATE

Parameter	Type	Required	Description
sketch	the frame sketch	Yes	id or name; 2D or 3D
lines	[curve ids]	No	one member each; default: every straight line drawn in the sketch: not construction, not projected or otherwise linked, not of no length
anchor	origin\|center\|centroid\|top_left\|top\|top_right\|left\|right\|bottom_left\|bottom\|bottom_right	No	the profile point that sits on each line, default origin
locate	[x,y]	No	the profile point that sits on each line, in mm from the profile's own origin: a bar's or an angle's bottom-left corner, a channel's web back at mid-height, the centre of other profiles; takes precedence over `anchor` and keeps the member attached at that point when the profile size changes
angle	angle expr	No	the profile turned about the line; default 0: its y as near world up as the line allows, a vertical member's x along world X
mirror	bool	No	the profile mirrored across its y axis
name		No
body_name		No	what the members are named after, then numbered: `Rail`, `Rail (2)`…; default the size's name, `RSC 203x89`, the profile's description, `Rect Tube 40x40x3`, or the profile sketch's name

Automation details

Command ID: frame.member

Parameters:

sketch: the frame sketch (id or name; 2D or 3D); lines?: [curve ids] (one member each; default: every straight line drawn in the sketch: not construction, not projected or otherwise linked, not of no length); profile: {kind: bar|round_bar|rect_tube|round_tube|angle|channel|i_beam, …its dimensions: each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"); a channel's flange_slope is an angle (a number of degrees)} (frame.profile.list gives each kind's dimensions and an example; dimensions left out take defaults from the profile's size) | {size: a standard steel size by name, such as "RSC 203x89", "PFC 200x90x30", "RSA 50x50x5", "SHS 100x100x5", "RHS 200x100x6.3" or "CHS 42.4x3.2" (frame.profile.list lists them), alone: it brings its dimensions} | profile_sketch: a sketch whose profile is the section, in its own x and y around its origin, with profiles?: picks as solid.extrude takes them (default: its material, nested loops alternating, so two circles make a tube); anchor?: origin|center|centroid|top_left|top|top_right|left|right|bottom_left|bottom|bottom_right (the profile point that sits on each line, default origin); locate?: [x,y] (the profile point that sits on each line, in mm from the profile's own origin: a bar's or an angle's bottom-left corner, a channel's web back at mid-height, the centre of other profiles; takes precedence over `anchor` and keeps the member attached at that point when the profile size changes); angle?: angle expr (the profile turned about the line; default 0: its y as near world up as the line allows, a vertical member's x along world X); mirror?: bool (the profile mirrored across its y axis); name?; body_name? (what the members are named after, then numbered: `Rail`, `Rail (2)`…; default the size's name, `RSC 203x89`, the profile's description, `Rect Tube 40x40x3`, or the profile sketch's name); names?: {line id: name} (names to keep, as Edit Feature keeps them). One body per line, from its start to its end; each member keeps its name when other lines are added or deleted. Returns the feature and the bodies it made

End Cap

Command group: WELDMENTS › CREATE

Parameter	Type	Required	Description
thickness	length in design units or a parameter expression	Yes
ratio	the inset as a share of the thickness	No	give offset or ratio, not both; neither: the plate is flush with the outside of the profile
chamfer	corner chamfer length along each edge from the corner	No	default 0; a rounded corner needs at least its rounding

Automation details

Command ID: frame.end_cap

Parameters:

faces: [{face:[x,y,z],body,index,path?}] planar end faces of frame members, picked in world mm (1–256); thickness: length in design units or a parameter expression; offset?: inset of the plate from the outside of the profile, a length; ratio?: the inset as a share of the thickness (give offset or ratio, not both; neither: the plate is flush with the outside of the profile); chamfer?: corner chamfer length along each edge from the corner (default 0; a rounded corner needs at least its rounding); direction?: outward|inward (default outward: past the end; inward: the member is cut back by the thickness and the cap takes its place). One separate body per face, named `<member> End Cap`; the plate is the profile's outer outline on a closed section (tube, pipe, bar), its outside on an open one (angle, channel, beam, slotted extrusion): the edges on the rectangle round the profile with their rounds and chamfers, inward stretches closed along the rectangle. Common name/body_names fields supported.

PLASTIC › CREATE

Boss

Command group: PLASTIC › CREATE

Read the plastic parts guide.

Parameter	Type	Required	Description
position	[x,y,z] on a face	Yes
direction		No	default: out of the face
diameter		Yes
height		Yes
hole_diameter		No
hole_depth		No	default: to the face
draft		No	angle
fillet		No	root radius
ribs		No	count
rib_thickness		No
rib_length		No	out from the wall
rib_offset		No	below the top
body		No

Automation details

Command ID: plastic.boss

Parameters:

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?

Lip

Command group: PLASTIC › CREATE

Read the plastic parts guide.

Parameter	Type	Required	Description
face	[x,y,z] on the rim face of a shelled body	Yes
width		Yes
height		Yes
type	lip\|groove	No
gap		No	groove clearance
side	inside\|outside	No	which rim edge
body		No

Automation details

Command ID: plastic.lip

Parameters:

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?

Snap Fit

Command group: PLASTIC › CREATE

Read the plastic parts guide.

Parameter	Type	Required	Description
position	[x,y,z] on a face	Yes
direction		No	default: out of the face
hook	[x,y,z]	Yes	the catch's direction
length		Yes
thickness		Yes
width		Yes
catch_depth		Yes
catch_length		Yes
base_height		No	extends the base below the face
new_body	bool	No	make a separate body instead of joining
body		No

Automation details

Command ID: plastic.snap_fit

Parameters:

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; base_height? (extends the base below the face); new_body?: bool (make a separate body instead of joining); body?

Rest

Command group: PLASTIC › CREATE

Read the plastic parts guide.

Parameter	Type	Required	Description
position	[x,y,z] on a face	Yes	the rest's centre
direction		No	default: out of the face
width		Yes	round: the diameter
length		No	a rectangle, along `along`
along	[x,y,z]	No
height		Yes
draft		No	angle; default: the body's plastic rule
thickness		No	wall of a hollow rest
body		No

Automation details

Command ID: plastic.rest

Parameters:

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

Manage Plastic Rules

Command group: PLASTIC › SETUP

Read the plastic parts guide.

Parameter	Type	Required	Description
name		Yes	library or new rule; a new one starts from `from`, default ABS (1.5mm)
from		No
material		No
thickness		No
nominal_radius		No
clearance		No
knife_edge		No
reveal_height		No
thickness_variation		No
draft		No
max_thickness		No
min_thickness		No
min_draft		No	expressions; `Thickness` is the rule's
active	bool	No	rule for bodies without one
delete	bool	No	a design rule; a library rule goes back to the library values

Automation details

Command ID: plastic.manage_rules

Parameters:

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)

Assign Plastic Rule

Command group: PLASTIC › SETUP

Read the plastic parts guide.

Parameter	Type	Required	Description
bodies	[names]	Yes
rule	name	Yes	empty: no rule

Automation details

Command ID: plastic.assign_rule

Parameters:

bodies: [names]; rule: name (empty: no rule) — plastic features on these bodies take its draft and clearance as defaults

Other commands: sketch

Edit Sketch

Parameter	Type	Required	Description
sketch	id or name	Yes
restore_marker	nonnegative timeline position	No
null		Yes	end

Automation details

Command ID: sketch.edit

Parameters:

sketch: id or name; restore_marker?: nonnegative timeline position, null (end) or false. A position or null: temporarily roll to this sketch and restore that position on Finish or Cancel; Finish groups the edit into one Undo step. Omitted: the same with the current position when features come after the sketch, so they rebuild once at Finish rather than after every sketch command. false: leave the timeline in place (later features rebuild after every sketch command)

Draw Dimensioned Sketch Geometry

Automation details

Command ID: sketch.draw.dimensioned

Parameters:

command: sketch creation command, params: object, dimensions: object of role to numeric or expression value, or `name = expression` (also `#name = expression`), which defines the user parameter `name` as sketch.dimension does (the reply's `defined` lists the names) (optional with as_drawn or locate), as_drawn?: bool (also dimension every other role of the shape at its size as drawn; a radius or diameter given takes the place of the other, as an edge polygon's side length does its radius, a circle otherwise takes its diameter, and a size the sketch already determines, such as the angle of a line inferred horizontal, is left out), locate?: bool (then place the shape from the sketch origin until nothing of it is left free: horizontal and vertical distances from the origin to its points, centres first, each kept only where it removes freedom, so a shape anchored to the origin or to placed geometry gets none; a point on an axis goes onto that axis instead of a 0 distance; the reply's located lists them); 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…)

Delete Sketch Entities

Parameter	Type	Required	Description
entities	[curve, point or constraint ids]	Yes

Automation details

Command ID: sketch.delete

Parameters:

entities: [curve, point or constraint ids]

Drag Sketch Point

Parameter	Type	Required	Description
point	ref	Yes
to	[x,y]	Yes

Automation details

Command ID: sketch.move_point

Parameters:

point: ref, to: [x,y]

Move Sketch Points

Parameter	Type	Required	Description
moves	[{point: ref \| near: [x,y], to: [x,y]}]	Yes	each point to its own target; `near`: the sketch point closest to it, refused when none lies within `tolerance` or two are as close
tolerance	mm	No	default 0.1
sketch		No

Automation details

Command ID: sketch.move_points

Parameters:

moves: [{point: ref | near: [x,y], to: [x,y]}] (each point to its own target; `near`: the sketch point closest to it, refused when none lies within `tolerance` or two are as close), tolerance?: mm (default 0.1); sketch? → moved: [{point, to, at, reached}] (`at`: where it ended up after the one solve; `reached`: whether that is `to`)

Drag Sketch Geometry

Automation details

Command ID: sketch.drag

Parameters:

entity: point or curve, from: [x,y] where it was grabbed, to: [x,y], live?: bool: points and the material point grabbed on a line move toward `to` within the design constraints. When exact placement is impossible, bounded feasible steps minimize cursor distance. Splines slide by to - from; a circle or arc grabbed on its edge takes the radius to `to`. `with?`: [point or curve ids] moves the rest of a selection with the entity as one translation (circles keep their radii). Long moves retain the solution branch; arcs cannot sweep through their starts. Returns `reached`: progress projected onto the requested move (0..1), `at`: the grabbed position for the next frame, and `retry`: budget-limited progress can continue in another frame. `live: true` shares a work budget across held-solve decomposition and cursor correction; ordinary recovery and the final model evaluation retain their existing limits, not a wall-clock deadline. Later features stay stale until `sketch.drag_end`; `dof` stays from before the drag

End Sketch Drag

Automation details

Command ID: sketch.drag_end

Parameters:

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

Move Dimension Text

Parameter	Type	Required	Description
dimension	constraint id or parameter name	Yes
at	[x,y] text centre	Yes	sketch coordinates
reset	true	Yes	default place

Automation details

Command ID: sketch.dimension_text

Parameters:

dimension: constraint id or parameter name; at: [x,y] text centre (sketch coordinates) | reset: true (default place)

Sketch Palette Options

Parameter	Type	Required	Description
sketch	id\|name	No	default active

Automation details

Command ID: sketch.options

Parameters:

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

Chain

Parameter	Type	Required	Description
curve	id: the curves joined to it end to end	Yes	what a double-click selects

Automation details

Command ID: sketch.chain

Parameters:

curve: id: the curves joined to it end to end (what a double-click selects)

Solve Sketch

Automation details

Command ID: sketch.solve

Parameters:

reports the solver status and degrees of freedom

Add Spline Point

Automation details

Command ID: sketch.spline.insert_point

Parameters:

curve: fit point spline id, at: [x,y]: a fit point is inserted where the curve passes nearest to it, between its neighbours (the curve still runs through it and all its old points; constraints on them stay); end?: start|end: `at` becomes the spline's new first or last point instead, and the curve runs on to it (refused when that end is joined to other geometry). Control point splines take no new points yet. Returns point: the new point's id

Remove Spline Point

Automation details

Command ID: sketch.spline.remove_point

Parameters:

curve: spline id, point: one of its points (a point id, or the curve's start or end such as s1.end): the spline runs through (or over) its other points only, and the point goes with the constraints on it unless another curve uses it. Fit point, control point and closed splines. Refused for a closed spline's closing point, for an end joined to other geometry or held by a constraint, when fewer than 2 points would be left (3 on a closed spline), and for a projected, offset or patterned spline. Returns curve, point: the point's id, deleted: whether the point went too

Add Tangent Handles

Automation details

Command ID: sketch.spline.handles

Parameters:

curve: fit point spline id: gives it a tangent handle at each fit point (a free point joined to it by a construction line) where the curve already runs, so its shape does not change until a handle is moved; moving a fit point moves the handles nobody has turned with it. In the app a selected spline shows its handles and the first drag of one adds them. Refused for a spline that has handles already, a control point, projected, offset, patterned or equation spline. Returns curve, handles: the handle point ids in fit point order

Reset Tangent Handles

Automation details

Command ID: sketch.spline.reset_handles

Parameters:

curve: fit point spline id: removes its tangent handles (the handle points, their construction lines and the constraints on them), so the curve runs through its fit points as if the handles had never been moved; selected, it shows them again where they start. Refused for a spline without tangent handles. Returns curve, removed: the removed handle point ids in fit point order

Reverse Spline Direction

Parameter	Type	Required	Description
curve	spline id	Yes	fit point, control point or closed

Automation details

Command ID: sketch.spline.reverse

Parameters:

curve: spline id (fit point, control point or closed): its last point becomes its first and the curve runs the other way along the same path; its points and the constraints on them stay. Refused for a projected spline and for one an offset uses or makes. Returns curve

Infinite Line

Parameter	Type	Required	Description
curves	[line ids]	Yes
value	bool	No	default toggles

Automation details

Command ID: sketch.infinite

Parameters:

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

Edit Text

Parameter	Type	Required	Description
live	bool: one frame of an interactive change	No	the sketch is solved, the features after it stay as they were until `sketch.drag_end`

Automation details

Command ID: sketch.edit_text

Parameters:

link: the text's link id (or entity: one of its curves), text? or text_expression? (as in sketch.text; typed words replace the expression), 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), vertical_align?: baseline|top|middle|bottom (the block of lines against `at` or the path: the first line's baseline (default), its capitals' tops, halfway between those and the last line's baseline, or the bottom of the last line's descenders), 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); or edits: [{link or entity, text?, at?, …}]: several texts changed together, the design rebuilt once (all or nothing; returns edits: each one's result); 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…)

Edit Equation Curve

Parameter	Type	Required	Description
curve	an equation curve's id	Yes

Automation details

Command ID: sketch.equation_curve.edit

Parameters:

curve: an equation curve's id; x?, y?, explicit?, start?, end?, tolerance?, variable_unit?: as in sketch.equation_curve, each kept when left out (explicit: true drops x; false needs x). The points are chosen again for the new formulas; the curve's start point (and the end point of an open curve) keeps its id, so geometry joined there stays joined. Returns curve, points, closed, deviation

Toggle Driven Dimension

Parameter	Type	Required	Description
constraint	dimension id	Yes
driven	bool	No	default toggles

Automation details

Command ID: sketch.toggle_driven

Parameters:

constraint: dimension id, driven?: bool (default toggles); a driving dimension gets a parameter with its current value

Toggle Radius / Diameter

Parameter	Type	Required	Description
constraint	a circle's or an arc's radius or diameter dimension id	Yes
diameter	bool	No	default: the other one
sketch	id\|name	No	default: the one being edited

Automation details

Command ID: sketch.toggle_diameter

Parameters:

constraint: a circle's or an arc's radius or diameter dimension id; diameter?: bool (default: the other one); sketch?: id|name (default: the one being edited). The circle stays the same size: its parameter is halved or doubled (a plain value is rewritten, an expression becomes `(e) / 2` or `2 * (e)`); refused when anything else uses that parameter

Constraint Glyphs

Parameter	Type	Required	Description
sketch	id	No
name	every constraint with where to draw its glyph	Yes	sketch coordinates

Automation details

Command ID: sketch.glyphs

Parameters:

sketch?: id|name: every constraint with where to draw its glyph (sketch coordinates)

Snap Inference

Parameter	Type	Required	Description
at	[x,y]	Yes
from	[x,y]	No	previous click
radius	mm	No	snap distance, default 1

Automation details

Command ID: sketch.snap

Parameters:

at: [x,y], from?: [x,y] (previous click), radius?: mm (snap distance, default 1): what a click there would snap to and infer

Drawing Size

Parameter	Type	Required	Description
path	SVG or DXF	Yes	by `format`: "svg" \| "dxf", default by the file name, else SVG
text	SVG or DXF	Yes	by `format`: "svg" \| "dxf", default by the file name, else SVG

Automation details

Command ID: sketch.drawing_bounds

Parameters:

path | text: SVG or DXF (by `format`: "svg" | "dxf", default by the file name, else SVG); returns min, max, width and height of the drawn geometry in the file's own size, and for an SVG with a viewBox (or width and height) its sheet: {min, max, width, height}

Save As DXF

Parameter	Type	Required	Description
sketch	id\|name	No	default active
path	file to write	No	else the DXF text is returned
units	"design" \| "in" \| "inch" \| "mm" \| "cm" \| "m" \| "ft"	No	default mm
layer	profile layer name	No	default "0"
layers	"single" \| "roles"	No	default "single": all on `layer`; "roles": outer on "OUTLINE", holes on "CUT"
join	bool	No	default false: R12 LINE/ARC; true: closed loops as LWPOLYLINE with arc bulges

Automation details

Command ID: sketch.export_dxf

Parameters:

sketch?: id|name (default active); path?: file to write (else the DXF text is returned); units?: "design" | "in" | "inch" | "mm" | "cm" | "m" | "ft" (default mm); layer?: profile layer name (default "0"); layers?: "single" | "roles" (default "single": all on `layer`; "roles": outer on "OUTLINE", holes on "CUT"); join?: bool (default false: R12 LINE/ARC; true: closed loops as LWPOLYLINE with arc bulges)

Loose Ends

Parameter	Type	Required	Description
sketch	id\|name	No	default active
untied	[{point, curve, at, touches: {point}\|{curve}}] ends that touch another curve only by position	Yes	the profile closes now, but nothing keeps it closed when a dimension changes

Automation details

Command ID: sketch.loose_ends

Parameters:

sketch?: id|name (default active): the ends of profile curves (not construction, projected or text) that can make a profile fail. open: [{point, curve, at}] ends that touch no other profile curve (no profile runs through them); untied: [{point, curve, at, touches: {point}|{curve}}] ends that touch another curve only by position (the profile closes now, but nothing keeps it closed when a dimension changes)

Tie Loose Ends

Parameter	Type	Required	Description
sketch	id\|name	No	default active

Automation details

Command ID: sketch.loose_ends.tie

Parameters:

sketch?: id|name (default active); points?: [point ids] (default: every untied end): ties each untied end to what it touches, coincident with another curve's end or on another curve. Returns constraints: [ids added], and the untied ends left

3D Line

Automation details

Command ID: sketch.line3d

Parameters:

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…)

3D Spline

Parameter	Type	Required	Description
points	[[x,y,z]…] world fit points	Yes	2 or more

Automation details

Command ID: sketch.spline3d

Parameters:

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…)

3D Arc

Automation details

Command ID: sketch.arc3d

Parameters:

start, through, end: [x,y,z] world points: an exact circular arc through them, from start through through to end (needs 3D Sketch on). Stored exactly (centre, radius, angles), so path consumers can treat it as a true arc. 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…)

3D Point

Parameter	Type	Required	Description
point	[x,y,z] world point	Yes	needs 3D Sketch on

Automation details

Command ID: sketch.point3d

Parameters:

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…)

Move 3D Point

Parameter	Type	Required	Description
wire	drawn 3D curve or point id	Yes
index	fit point	No	default 0
to	[x,y,z]	Yes
by	[dx,dy,dz]	Yes

Automation details

Command ID: sketch.move3d

Parameters:

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

Break Offset Association

Parameter	Type	Required	Description
curve	derived offset curve id	Yes	retains geometry and makes its points editable

Automation details

Command ID: sketch.offset.break

Parameters:

curve: derived offset curve id (retains geometry and makes its points editable)

Trim Along Path

Automation details

Command ID: sketch.trim.path

Parameters:

points: [[x,y]…] (2…2000 positions: a path drawn across the sketch). Every piece the path crosses is removed as `sketch.trim` removes the piece at that crossing, in the order the path crosses them; a piece crossed again after it is gone is not trimmed twice; eligible single-line offset outputs are trimmed while preserving their distance; projected geometry, infinite lines, other offset outputs and pieces trim refuses are passed over (why in `skipped`). dry_run?: bool (report without changing the design). One undo step → trimmed: [each trim's result], removed: [[[x,y]…]] (each removed piece as a polyline). 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…)

Break Link

Parameter	Type	Required	Description
link	link id	No	j1
entities	[curve or point ids]: linked geometry becomes normal sketch geometry	No

Automation details

Command ID: sketch.break_link

Parameters:

link?: link id (j1) | entities?: [curve or point ids]: linked geometry becomes normal sketch geometry

Auto-Project Edges on Reference

Parameter	Type	Required	Description
value	bool	No	default toggles

Automation details

Command ID: sketch.auto_project

Parameters:

value?: bool (default toggles): project a face's edges when a sketch is created on it

Redefine Sketch Plane

Parameter	Type	Required
sketch	id or name	Yes
plane	as sketch.create	Yes
frame	as sketch.create	No
author_path	exact owner occurrence ids	No

Automation details

Command ID: sketch.redefine

Parameters:

sketch: id or name; plane: as sketch.create; frame?: as sketch.create; author_path?: exact owner occurrence ids; explicitly rebinds or freezes the plane while preserving geometry and dimension names

Copy Sketch Entities

Parameter	Type	Required	Description
entities	[curve or point ids]	No	default: the selected sketch geometry

Automation details

Command ID: sketch.copy

Parameters:

entities?: [curve or point ids] (default: the selected sketch geometry); the constraints and dimensions among them come along

Cut Sketch Entities

Automation details

Command ID: sketch.cut

Parameters:

entities?: [curve or point ids] (default: the selected sketch geometry): copies them as sketch.copy does, then deletes them (one undo step)

Paste Sketch Entities

Parameter	Type	Required	Description
at	[x, y]	No	sketch point the copy's centre goes to
translate	[x, y]	No
sketch	target	No	default: the active sketch

Automation details

Command ID: sketch.paste

Parameters:

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)

Replace Sketch

Parameter	Type	Required	Description
sketch	the sketch to replace	No	default: the active sketch
from	the sketch whose contents take its place	Yes	id or name

Automation details

Command ID: sketch.replace

Parameters:

sketch?: the sketch to replace (default: the active sketch); from: the sketch whose contents take its place (id or name); file?: a design file `from` is in (default: this design). The sketch keeps its plane, place in the timeline and the features built on it; its curves, points, constraints, dimensions and texts become a copy of `from`'s, at the same sketch coordinates (one undo step)

Other commands: canvas

Calibrate Canvas

Parameter	Type	Required	Description
canvas	id or name	Yes
a	two points on the canvas plane [x,y]	Yes
b	two points on the canvas plane [x,y]	Yes
distance	their true distance	Yes	mm

Automation details

Command ID: canvas.calibrate

Parameters:

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

Straighten Canvas

Parameter	Type	Required
canvas	id or name	Yes
a	two points on the canvas plane [x,y] along a line of the image	Yes
b	two points on the canvas plane [x,y] along a line of the image	Yes

Automation details

Command ID: canvas.straighten

Parameters:

canvas: id or name; a, b: two points on the canvas plane [x,y] along a line of the image; angle?: deg, the direction that line should have (0 horizontal, the default; 90 vertical): turns the image about a, the shorter way

Delete Canvas

Parameter	Type	Required	Description
canvas	id or name	Yes

Automation details

Command ID: canvas.delete

Parameters:

canvas: id or name

Canvas to Sketch

Parameter	Type	Required	Description
canvas	id or name	No	default: the last canvas

Automation details

Command ID: canvas.to_sketch

Parameters:

canvas?: id or name (default: the last canvas); name?: the new sketch's name. Traces the canvas image (dark drawing on a light background, or the reverse) into a new sketch on the canvas plane, lying exactly on the image: lines, splines and holes

Other commands: pointcloud

Edit Point Cloud

Parameter	Type	Required	Description
cloud	id or name	Yes
name		No
visible		No
point_size	pixels	No	0.5…16
color_by	file\|single\|height or a property's name	No	the file's colours, the default; one colour; a ramp by height, blue low to red high; or by any property of the file, a ramp over its values or a palette for whole numbers
color	[r, g, b] 0…1	No	the single colour; given alone it sets color_by single, null sets color_by file
height_range	the same as color_range	No
units	mm\|cm\|m\|in\|ft	No	the file's length unit: the points are scaled from the unit they came in as
matrix	[12 or 16 numbers]	No	where the cloud sits: a rigid row-major 3x4 or 4x4 matrix, as occurrence.move takes it
tolerance		No

Automation details

Command ID: pointcloud.edit

Parameters:

cloud: id or name; name?; visible?; point_size?: pixels (0.5…16); color_by?: file|single|height or a property's name (the file's colours, the default; one colour; a ramp by height, blue low to red high; or by any property of the file, a ramp over its values or a palette for whole numbers); color?: [r, g, b] 0…1 (the single colour; given alone it sets color_by single, null sets color_by file); color_range?: [low, high] the ramp runs between (design Z in mm by height), or null for the automatic range (by height all but the lowest and highest 2 % of the points; by a property the values it takes over what the filters keep); height_range?: the same as color_range; units?: mm|cm|m|in|ft (the file's length unit: the points are scaled from the unit they came in as); matrix?: [12 or 16 numbers] (where the cloud sits: a rigid row-major 3x4 or 4x4 matrix, as occurrence.move takes it); tolerance?; filters?: [{property, range: [low, high]} or {property, values: [whole numbers]} for a property with named values], or null (only what every filter keeps is shown) → cloud

Reload Point Cloud

Parameter	Type	Required	Description
cloud	id or name	Yes	its file is read again from where it was inserted; name, placement, units, colouring and the filters on properties it still has are kept; read under the limit it was inserted with, so a file that grew is thinned only past that limit

Automation details

Command ID: pointcloud.reload

Parameters:

cloud: id or name (its file is read again from where it was inserted; name, placement, units, colouring and the filters on properties it still has are kept; read under the limit it was inserted with, so a file that grew is thinned only past that limit) → cloud, points, segments, triangles, warnings

Delete Point Cloud

Parameter	Type	Required	Description
cloud	id or name	Yes

Automation details

Command ID: pointcloud.delete

Parameters:

cloud: id or name → deleted

Point Clouds

Automation details

Command ID: pointcloud.list

Parameters:

→ clouds: [{cloud, name, file, source (the file's path, read again by pointcloud.reload), points, segments, triangles, source_points, units, visible, point_size, color_by (file, single, height or a property's name), color, colored, properties: [{name, integer, span, names}], filters, color_range (the ramp's now, exact over what the filters keep), height_range (the ramp's own range or the automatic one by height), height_auto, bounds: [[x,y,z], [x,y,z]] in the design, matrix}]

Other commands: inspect

View Analysis

Parameter	Type	Required	Description
off	true turns the view analysis on now off.	No

Automation details

Command ID: inspect.analysis

Parameters:

off?: true turns the view analysis on now off. → active: the command id of the view analysis on (inspect.zebra, inspect.draft, inspect.curvature_map, inspect.environment_map, inspect.accessibility, inspect.continuity, inspect.isocurve or inspect.curvature_comb), or null. One is on at a time: turning one on turns the one on before off. Read-only without `off`

Clearance

Parameter	Type	Required	Description
bodies	[names]	No	default: every solid body, in world placement, but those in `against`; mesh bodies are not measured
against	[names]	No	only pairs with one body in `bodies` and the other here
min_volume	mm³	No	default 0.01: smaller overlaps count as contact
clearance	mm	No	default 0: report pairs closer than this
nearest	n	No	each body of `bodies` gets its n nearest others
skip_within	"occurrence"\| "component"\| null	No	pairs of bodies of one occurrence; pairs of bodies inside one placed component, its subcomponents included
tolerance	mm	No	default 1e-6: a gap below it is contact, 0

Automation details

Command ID: inspect.clearance

Parameters:

bodies?: [names] (default: every solid body, in world placement, but those in `against`; mesh bodies are not measured); against?: [names] (only pairs with one body in `bodies` and the other here); min_volume?: mm³ (default 0.01: smaller overlaps count as contact); clearance?: mm (default 0: report pairs closer than this); nearest?: n (each body of `bodies` gets its n nearest others); skip_within?: "occurrence" (pairs of bodies of one occurrence) | "component" (pairs of bodies inside one placed component, its subcomponents included) | null; tolerance?: mm (default 1e-6: a gap below it is contact, 0) → overlaps: [{a, b, volume_mm3, area_mm2, bbox, center}]; near: [{a, b, distance_mm, from, to, overlap_mm3?: a contact's shared volume below min_volume, exact?: false when measured on the meshes}], nearest by body (the same for pairs that overlap: 0); nearest: {body: [{body, distance_mm}]}; unchecked: [{a, b, reason}] (pairs whose overlap could not be worked out; each mesh body, STL/3MF/OBJ import, is not measured and is listed as {a: name, b: null, reason: "mesh body: not checked"}, also when named in `bodies` or `against`; the result's `bodies` counts the solid bodies only); pairs_checked; pairs_reused (of those, measured by an earlier call: neither body changed or moved since); pairs_pruned (ruled out by their boxes); ms. Distances are measured on the exact faces and edges, the meshes only rule pairs out

Parameter Sweep

Parameter	Type	Required	Description
parameter	name	Yes
values	[number \| expression]\| from	Yes	at most 200
to	numbers	Yes
steps		No	default 10, at most 199: steps + 1 values

Automation details

Command ID: inspect.parameter_sweep

Parameters:

parameter: name; values: [number | expression] (at most 200) | from, to: numbers, steps? (default 10, at most 199: steps + 1 values) → for each value, in a copy of the design (the design itself is not changed): {value, ms (the rebuild), ok, failed: [{feature, name, error}], warned: [{feature, name, warning}] (features that build at the current value and fail or warn at this one), joints_lost: [{joint, name, origin?: a|b, why}], joints_flipped: [{joint, name, origin: a|b, degrees}] (an origin's z turned more than 90° on its own part from where it is now), sketches_flipped: [{sketch, name, degrees}] (the sketch plane's normal turned more than 90°), sketches_failed: [{sketch, name, failing, folded}] (a solve that fails, or keeps a triangle's turn or an offset's side only by flipping it)} (or {value, ms, ok: false, error} where the parameter takes no such value); summary: {values, ok, slowest_ms, failed, joints_lost, joints_flipped, sketches_flipped, sketches_failed} (how many values show each)

Compare Parameter Variants

Automation details

Command ID: inspect.parameter_variants

Parameters:

variants: [{name, set: {parameter: number | expression}}] (1 to 12; up to 16 existing parameters each). Rebuild each set together in a separate copy of the open design. Returns baseline and ordered results with volume, mass, body counts and rebuild regressions. No edits are kept.

Compare Bodies

Parameter	Type	Required	Description
tolerance	mm	No	0.001 to 10, default 0.01
max_regions		No	default 50
color	true \| {only_in_a?, only_in_b?: "#rrggbb"}	No	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

Automation details

Command ID: inspect.compare

Parameters:

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, center and bbox (measured_by: "boolean": exact, the pieces of a − b or b − a there, measured as inspect.measure does; "not measured": the cut could not be made, so volume_mm3 and center are null and not_measured says why, never an estimate), area_mm2, max_deviation_mm, at, 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, a cut that could not be made). The regions are found from the two surfaces, so near-identical bodies compare too

Compare Picture

Parameter	Type	Required	Description
reference	path to a PNG or JPEG the model should match	Yes
crop_px	[x, y, w, h] in pixels	No
crop_fraction	[x, y, w, h] as fractions 0..1 of the picture	No	to take one view off a board
overlay	false leaves the overlay PNG out	No

Automation details

Command ID: inspect.compare_picture

Parameters:

reference: path to a PNG or JPEG the model should match; view?/camera?/bodies?/rows? as inspect.silhouette; crop_px?: [x, y, w, h] in pixels, or crop_fraction?: [x, y, w, h] as fractions 0..1 of the picture (to take one view off a board); part_fills_crop?: false — with true the crop box is the part itself and no background search runs, for a crop that tightly frames the part; fit?: "width" | "height" | "both" (default "width"): one uniform scale, taken from the named dimension ("both" claims both and scales by width, reporting aspect_mismatch when the shapes differ); overlay?: false leaves the overlay PNG out → overlap (0..1), edges: top|bottom|left|right in mm at nine stations (positive where the model reaches past the picture, null where a station misses one of the two), the grid and its mm_per_px, and overlay_png (red model, blue picture) as base64 PNG. The compare is outline only: holes are not compared — both the picture's and the model's holes are filled

Silhouette

Parameter	Type	Required	Description
view	front\|back\|left\|right\|top\|bottom\|iso	No	default front
camera	{target: [x,y,z], yaw, pitch, distance, fov?}	No	mm, radians; fov 0 means parallel
bodies	[world body names]	No	default visible bodies, named hidden bodies included
rows	mask height in pixels	No	default 240, clamped to 16..1024

Automation details

Command ID: inspect.silhouette

Parameters:

view?: front|back|left|right|top|bottom|iso (default front); or camera?: {target: [x,y,z], yaw, pitch, distance, fov?} (mm, radians; fov 0 means parallel); bodies?: [world body names] (default visible bodies, named hidden bodies included); rows?: mask height in pixels (default 240, clamped to 16..1024) → tightly framed run-length mask, box_mm, mm_per_px, right/up, projection, body and triangle counts

Other commands: solid

Cell Grid

Parameter	Type	Required	Description
size	expr	Yes	a cell's inscribed diameter
web	expr	Yes	the wall between cells
depth	expr	Yes	or through_all: true
shape	hexagon\|square\|triangle\|circle\|polygon	No	default hexagon
sides	expr	No	polygon cells, 3 to 64; default 8
dot_grid	hexagonal\|square	No	where circle and polygon cells sit; default hexagonal
angle	expr	No	the grid's rotation about the anchor; angle 45 deg with square cells gives a diamond layout
anchor	[x,y,z]	No	a cell's centre, projected onto the sketch plane; default the sketch origin: grids with the same anchor, angle, size and web line up
clip	whole\|snap\|free	No	cells the field's edge crosses: only whole cells; cells cut along the grid's own lines; cells trimmed to the edge as drawn; default snap
direction	positive\|negative\|symmetric	No	default positive
sketch	id\|name	No	default: active or last sketch; its closed profiles hold the field: a loop inside another is a keep-out
profiles	as solid.extrude	No
targets	[body]	No
mode	cut	No	the only mode so far

Automation details

Command ID: solid.cell_grid

Parameters:

size: expr (a cell's inscribed diameter); web: expr (the wall between cells); depth: expr (or through_all: true); shape?: hexagon|square|triangle|circle|polygon (default hexagon); sides?: expr (polygon cells, 3 to 64; default 8); dot_grid?: hexagonal|square (where circle and polygon cells sit; default hexagonal); angle?: expr (the grid's rotation about the anchor; angle 45 deg with square cells gives a diamond layout); anchor?: [x,y,z] (a cell's centre, projected onto the sketch plane; default the sketch origin: grids with the same anchor, angle, size and web line up); clip?: whole|snap|free (cells the field's edge crosses: only whole cells; cells cut along the grid's own lines; cells trimmed to the edge as drawn; default snap); direction?: positive|negative|symmetric (default positive); sketch?: id|name (default: active or last sketch; its closed profiles hold the field: a loop inside another is a keep-out); profiles?: as solid.extrude; targets?: [body]; mode?: cut (the only mode so far); name?. Cuts at most 250 cells in one operation; not for sheet metal (use sheet.perforate). The faces cut have no stable names yet

Other commands: mesh

Convert Mesh

Parameter	Type	Required	Description
body	mesh body name	No	default: the selected mesh body
name		No

Automation details

Command ID: mesh.convert

Parameters:

body?: mesh body name (default: the selected mesh body); tolerance?: length expression (default 0.05 mm): rebuild a closed mesh as an editable solid — a constant-section part as planar and cylindrical faces, any other closed mesh as the faceted solid its triangles describe — with a parametric timeline feature in the mesh body's owning component (the active component must be that component or an ancestor; otherwise activate the named component first); the active component is unchanged; name?

Other commands: model

Read Body Mesh

Parameter	Type	Required	Description
body	finite positive chord tolerance in mm	Yes
tolerance	finite positive chord tolerance in mm	No	default 0.05

Automation details

Command ID: model.mesh

Parameters:

body, tolerance?: finite positive chord tolerance in mm (default 0.05); evaluated component-local mesh, at most 8192 vertices and 16384 triangles; no files or model changes

List Edges

Parameter	Type	Required	Description
body	name	Yes

Automation details

Command ID: model.edges

Parameters:

body: name

List Faces

Parameter	Type	Required	Description
body	name	Yes

Automation details

Command ID: model.faces

Parameters:

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), sheet_face? (a folded sheet's face: `sheet:<body>:<panel>:<side>`, panel base or a flange's tag F<feature>.<k>, side top | bottom | rim.<edge> | bend.inner | bend.outer; taken wherever a face name is, and it holds while sizes change and flanges come and go)

List Threads

Automation details

Command ID: model.threads

No parameter description is provided by the command registry.

List Body Features

Parameter	Type	Required	Description
body	name	No	a placed copy's name means the body it shows; default every body

Automation details

Command ID: model.body_features

Parameters:

body?: name (a placed copy's name means the body it shows; default every body) → bodies: [{body, features: [{id, name}]}], in timeline order the feature that created each body, every later one that changed it, and those of bodies consumed into it. Read-only

Other commands: plugin

Inspect Plugin

Parameter	Type	Required	Description
path	plugin package folder	Yes

Automation details

Command ID: plugin.inspect

Parameters:

path: plugin package folder; returns inert manifest and approval hash covering manifest and component; runs no plugin code

Install Plugin

Parameter	Type	Required	Description
path	plugin .zip	Yes
replace	bool	No	required to replace an installed plugin of the same id
dry_run	bool	No

Automation details

Command ID: plugin.install

Parameters:

path: plugin .zip, replace?: bool (required to replace an installed plugin of the same id), dry_run?: bool; checks the .zip (one plugin, safe paths, size caps, manifest) and unpacks it into the plugins folder; runs no plugin code

List Plugins

Automation details

Command ID: plugin.list

Parameters:

List inspected and installed plugin manifests, namespaced entries, declared effects and input schemas; no plugin code runs

Run Plugin

Parameter	Type	Required
path		Yes
approval	exact hash from plugin.inspect after reviewing permissions	Yes
entry		Yes
params	JSON	No

Automation details

Command ID: plugin.run

Parameters:

path, approval: exact hash from plugin.inspect after reviewing permissions, entry, params?: JSON; explicit native Wasm component execution, one undo step; errors discard all edits

Other commands: sheet

List Sheet Metal Rules

Automation details

Command ID: sheet.rules

Parameters:

→ rules with their expressions and values, and the active one

Export Flat Pattern as DXF

Parameter	Type	Required	Description
body		No
path		No
curves	exact\|arcs	No	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	No	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	No	default false: a note beside each bend line on layer BEND_NOTES, `B1 UP 90%%d R1`, its angle the included angle when the body's rule has angle_display: included
note_height	mm	No	default 3
bend_lines	bool	No	default true; false leaves BEND_UP and BEND_DOWN out, for a cutter that would cut them
layers	roles\|single	No	default roles, the layers below; single: every entity on layer 0
per_body	bool	No	a file for every sheet body, `<path>-<body>.dxf`, or their DXF texts without a path → files: [{body, path \| dxf, bends}]; not with `body`

Automation details

Command ID: sheet.export_dxf

Parameters:

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`, its angle the included angle when the body's rule has angle_display: included), note_height?: mm (default 3), bend_lines?: bool (default true; false leaves BEND_UP and BEND_DOWN out, for a cutter that would cut them), layers?: roles|single (default roles, the layers below; single: every entity on layer 0), 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

Export Bend Table

Parameter	Type	Required	Description
body		No
format	csv\|json	No	default csv
path		No

Automation details

Command ID: sheet.export_bend_table

Parameters:

body?, format?: csv|json (default csv), path? → bend table in mm and degrees, including rule and flat centre-line coordinates; angle_deg is the bend angle and included_angle_deg the angle left between the bend's sides (180° less it); a bend that cut-outs split has a row for each piece

Other commands: plastic

List Plastic Rules

Automation details

Command ID: plastic.rules

Parameters:

→ rules with their expressions and values, the active rule and the rules assigned to bodies

Other commands: frame

Profile Library

Automation details

Command ID: frame.profile.list

Parameters:

family?: RSC|PFC|RSA|SHS|RHS|CHS (list only that family's sizes). Returns kinds: [{kind, label, required, optional, example}]: the built-in profiles, each SolidCraft's own parametric definition; and sizes: [{family, kind, standard, source, names, additional?}]: the standard steel sizes by name, each family with the published table its dimensions come from (frame.profile.properties with {profile: {size}} gives a size's dimensions and section)

Profile Properties

Parameter	Type	Required	Description
profile	{kind: bar\|round_bar\|rect_tube\|round_tube\|angle\|channel\|i_beam, …its dimensions: each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"); a channel's flange_slope is an angle (a number of degrees)}\| {size: a standard steel size by name, such as "RSC 203x89", "PFC 200x90x30", "RSA 50x50x5", "SHS 100x100x5", "RHS 200x100x6.3" or "CHS 42.4x3.2" (frame.profile.list lists them), alone: it brings its dimensions}	Yes	frame.profile.list gives each kind's dimensions and an example; dimensions left out take defaults from the profile's size

Automation details

Command ID: frame.profile.properties

Parameters:

profile: {kind: bar|round_bar|rect_tube|round_tube|angle|channel|i_beam, …its dimensions: each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"); a channel's flange_slope is an angle (a number of degrees)} (frame.profile.list gives each kind's dimensions and an example; dimensions left out take defaults from the profile's size) | {size: a standard steel size by name, such as "RSC 203x89", "PFC 200x90x30", "RSA 50x50x5", "SHS 100x100x5", "RHS 200x100x6.3" or "CHS 42.4x3.2" (frame.profile.list lists them), alone: it brings its dimensions}; density?: kg/m³ (adds mass_per_m, kg/m). Returns profile (every default filled in), area (mm²), centroid [x,y] (mm, from the bounding box centre), ixx, iyy, ixy (mm⁴ about the centroid), width, height

Insert Profile

Parameter	Type	Required	Description
profile	{kind: bar\|round_bar\|rect_tube\|round_tube\|angle\|channel\|i_beam, …its dimensions: each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"); a channel's flange_slope is an angle (a number of degrees)}\| {size: a standard steel size by name, such as "RSC 203x89", "PFC 200x90x30", "RSA 50x50x5", "SHS 100x100x5", "RHS 200x100x6.3" or "CHS 42.4x3.2" (frame.profile.list lists them), alone: it brings its dimensions}	Yes	frame.profile.list gives each kind's dimensions and an example; dimensions left out take defaults from the profile's size
at	[x,y]	No	sketch mm, default the origin
anchor	origin\|center\|centroid\|top_left\|top\|top_right\|left\|right\|bottom_left\|bottom\|bottom_right	No	the profile point placed on `at`: its origin, the default and a built-in profile's centre, its bounding box's centre, its centroid, or a corner or edge middle of its bounding box
fixed	bool	No	default true: the curves are locked, so solving the sketch keeps the shape
sketch	id\|name	No	default: the sketch being edited

Automation details

Command ID: frame.profile.insert

Parameters:

profile: {kind: bar|round_bar|rect_tube|round_tube|angle|channel|i_beam, …its dimensions: each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"); a channel's flange_slope is an angle (a number of degrees)} (frame.profile.list gives each kind's dimensions and an example; dimensions left out take defaults from the profile's size) | {size: a standard steel size by name, such as "RSC 203x89", "PFC 200x90x30", "RSA 50x50x5", "SHS 100x100x5", "RHS 200x100x6.3" or "CHS 42.4x3.2" (frame.profile.list lists them), alone: it brings its dimensions}; at?: [x,y] (sketch mm, default the origin); anchor?: origin|center|centroid|top_left|top|top_right|left|right|bottom_left|bottom|bottom_right (the profile point placed on `at`: its origin, the default and a built-in profile's centre, its bounding box's centre, its centroid, or a corner or edge middle of its bounding box); angle?: radians, counter-clockwise; fixed?: bool (default true: the curves are locked, so solving the sketch keeps the shape); sketch?: id|name (default: the sketch being edited). Returns the section as frame.profile.properties does. 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…)

Other commands: component

Cycle Component Color

Parameter	Type	Required	Description
component	id or name	Yes

Automation details

Command ID: component.cycle_color

Parameters:

component: id or name; saves the next identification colour and turns Component Colors on; shared by every instance, separate from appearances

Hide Component History

Parameter	Type	Required	Description
component	id or name	Yes

Automation details

Command ID: component.hide_history

Parameters:

component: id or name; keeps the component's features in the design but leaves them out of the History bar (#10393)

Show Component History

Parameter	Type	Required	Description
component	id or name	Yes

Automation details

Command ID: component.show_history

Parameters:

component: id or name; puts a component's features back in the History bar after Hide Component History (#10393)

Create Components from Bodies

Parameter	Type	Required	Description
bodies	[names]	Yes

Automation details

Command ID: component.from_bodies

Parameters:

bodies: [names] → one new component per body, named after it

Activate Component

Parameter	Type	Required	Description
component	id or name	Yes	0 or "root" for the design
occurrence	exact placement used to author shared geometry	No
path	exact placement used to author shared geometry	No

Automation details

Command ID: component.activate

Parameters:

component: id or name (0 or "root" for the design); occurrence?, path?: exact placement used to author shared geometry

Edit in Place

Parameter	Type	Required	Description
component	id or name of a linked component	Yes
path	its placement	No	occurrence ids, default its first

Automation details

Command ID: component.edit_in_place

Parameters:

component: id or name of a linked component; path?: its placement (occurrence ids, default its first) → in the app window: open the design it links in a tab of its own with the assembly drawn around it (component.finish_edit goes back); fails when it is not linked, the assembly has no file yet, something is open or running in it, or the file is missing, on a network location not allowed yet or open in another SolidCraft; asked during the agent's turn it opens once the turn ends (queued: true); elsewhere it only checks

Finish Edit

Automation details

Command ID: component.finish_edit

Parameters:

no parameters → in the app window: go back from the linked design edited in place to its assembly, which reads it again; fails while the design has unsaved changes (run file.save first) or something is open in it; asked during the agent's turn it finishes once the turn ends (queued: true); elsewhere nothing changes

List Components

Parameter	Type	Required	Description
compact	bool	No	counts of bodies, features, sketches and construction planes instead of their names; occurrences leave out identity transforms; children as occurrence ids
bodies	bool	No	with compact: body names, not their count

Automation details

Command ID: component.list

Parameters:

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 Physical Properties

Parameter	Type	Required	Description
component	id or name	No	default active
descendants	bool	No	default true

Automation details

Command ID: component.properties

Parameters:

component?: id or name (default active); descendants?: bool (default true); about?: [x, y, z] (mm). Measures the first placement, or all placements for root, including pending moves; material-aware mass and center of mass in world coordinates; volume, density, mass, center of mass and inertia_g_mm2 (the inertia tensor about the body's center of mass, world axes, from its tessellation) only for closed, consistently oriented bodies; total.open_bodies_skipped counts open bodies excluded from volume/mass totals; total.first_moment_g_mm (mass × center of mass), inertia_g_mm2 about the total center of mass, principal_moments_g_mm2 (smallest first) and principal_axes (unit, right-handed); with about, total.inertia_about {point, inertia_g_mm2}

Rename Component

Parameter	Type	Required	Description
component		Yes
name		Yes

Automation details

Command ID: component.rename

Parameters:

component, name

Delete Component

Automation details

Command ID: component.delete

Parameters:

component: deletes it, its subcomponents, occurrences and features

Unlock Contents

Automation details

Command ID: component.unlock

Parameters:

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)

Move Bodies to Component

Parameter	Type	Required	Description
bodies	[names]	Yes
component		Yes
component_path	its placement to place them by	No	default: its only one, else the active one; a component placed more than once gets them in every instance
from_path	the placement of their component they move from	No	default: its only one, else its first, where its bodies have their own names

Automation details

Command ID: component.move_bodies

Parameters:

bodies: [names], component; component_path?: its placement to place them by (default: its only one, else the active one; a component placed more than once gets them in every instance); from_path?: the placement of their component they move from (default: its only one, else its first, where its bodies have their own names)

Paste Bodies

Parameter	Type	Required	Description
bodies	[names, as the Browser shows them: a body seen in another placement of its component (`Cube (B:2)`) is copied from there]	Yes
component	where the copies go	No	default: the active one
component_path	its placement to place them by	No	default: its only one, else the active one; a component placed more than once gets them in every instance

Automation details

Command ID: component.copy_bodies

Parameters:

bodies: [names, as the Browser shows them: a body seen in another placement of its component (`Cube (B:2)`) is copied from there]; component?: where the copies go (default: the active one); component_path?: its placement to place them by (default: its only one, else the active one; a component placed more than once gets them in every instance). Each copy stays where its body is in the world; the copies' names come back as `bodies`

Paste from Another Design

Parameter	Type	Required	Description
component	where it goes	No	default: the active one

Automation details

Command ID: component.paste_from_design

Parameters:

component?: where it goes (default: the active one); component_path?: its placement (default: the active one, else its only one). Pastes what was copied in another design, at the same world coordinates: its bodies as imported bodies (no history) in one Import feature, or its components as independent copies with their history, appearances, joints and motion (as `component.paste_new`); the user parameters they use come along, renamed `w_2` when taken. A component that uses what isn't in it (another body, sketch or parameter) is refused, saying what. Returns `bodies` and `feature`, or the pasted components' `paths`

Move Sketches to Component

Parameter	Type	Required	Description
sketches	[ids or names]	Yes	a number is an id; a string is an exact name, then an id
component		Yes

Automation details

Command ID: component.move_sketches

Parameters:

sketches: [ids or names] (a number is an id; a string is an exact name, then an id), component; the sketches keep their own coordinates (component.move_features keeps them where they are in the world), except that a sketch on an exactly attached face stays where it is on the face

Move Sketches to Their Parts

Parameter	Type	Required	Description
sketches	[ids or names]	No	default: every sketch in the design

Automation details

Command ID: component.move_sketches.to_parts

Parameters:

sketches?: [ids or names] (default: every sketch in the design) → moved, stayed, sketches [{sketch, name, component, part}], kept [{sketch, name, code, reason}]. Each sketch whose plane is an exactly attached face of a part's body goes to that part, as component.move_sketches moves it, and stays where it is on the face; the others (on an origin, construction or fixed plane, on a body of the design itself, or already in their part) stay where they are. One undo step

Move Features to Component

Parameter	Type	Required	Description
features	[ids or names]	Yes	sketches too
component	where they go	No	default: the active one

Automation details

Command ID: component.move_features

Parameters:

features: [ids or names] (sketches too); component?: where they go (default: the active one) → moved, component, bodies. Ids, names and timeline order stay; the geometry stays where it is in the world; the bodies the features made move with them. Refused while the timeline is rolled back, for a component placed more than once, and for a move that would break a feature (nothing changes)

Paste New

Parameter	Type	Required	Description
occurrence	selected source placement	No
path	selected source placement	No
parent	component the copy goes in	No	default: the source placement's; not the component or one inside it
in_place	as occurrence.copy	No
parent_path	as occurrence.copy	No
translate	[x,y,z]	No

Automation details

Command ID: component.paste_new

Parameters:

component: independently copy its nested definition graph and history, materials and styles; occurrence?, path?: selected source placement; parent?: component the copy goes in (default: the source placement's; not the component or one inside it); in_place?, parent_path?: as occurrence.copy; translate?: [x,y,z]. Reassigned external bodies become base geometry; retained external links and omitted boundary joints are reported

Update Links

Parameter	Type	Required	Description
component	id or name	No	default: every linked component

Automation details

Command ID: component.update_links

Parameters:

component?: id or name (default: every linked component); components?: a list of ids or names, which goes on past a design it cannot read (that one keeps its bodies, is named in failed and gets a warning) — reads the linked designs again and replaces their bodies where they changed, as one undo step; → updated, unchanged, failed ([{component, name, error}]), warnings (also joints whose faces are gone or that no longer solve)

Relink Source

Parameter	Type	Required	Description
component	id or name of a linked component	Yes

Automation details

Command ID: component.relink

Parameters:

component: id or name of a linked component; path: a saved design (.sc or .json) — replaces the source and linked bodies for all its occurrences, preserving identities and placements; occurrence?: one of its placements — when it has others, only that placement comes to show the design, as a placement of the component already linked to it or of a new one under the same parent, keeping its position and joints (component is then the one it shows, previous_component the one it showed); returns path, previous_path, warnings, joint_errors and joint_conflicts

Break Link

Parameter	Type	Required	Description
component	id or name of a linked component — keeps its bodies as they are and forgets the design file	Yes

Automation details

Command ID: component.break_link

Parameters:

component: id or name of a linked component — keeps its bodies as they are and forgets the design file

Extract to File

Parameter	Type	Required	Description
component	id or name of a component that is not linked	Yes
path	the .sc design to write	Yes

Automation details

Command ID: component.extract

Parameters:

component: id or name of a component that is not linked; path: the .sc design to write → its history, subcomponents and their joints move to that design, and the component becomes linked to it (as component.insert_design makes it); returns path, file, feature, bodies, notices (what stays behind), warnings and copies (components that build the same bodies: see component.replace_with_link)

Find Identical Copies

Parameter	Type	Required	Description
component	id or name of a linked component	Yes

Automation details

Command ID: component.copies

Parameters:

component: id or name of a linked component → copies: [{component, name}], the components not linked whose own history builds the same bodies

Replace with Link

Parameter	Type	Required	Description
with	a linked component	Yes
path	a .sc design	Yes	its link here, else a new linked component

Automation details

Command ID: component.replace_with_link

Parameters:

component or components: [ids or names] of components that are not linked; with: a linked component, or path: a .sc design (its link here, else a new linked component) → each component's history goes and its placements become placements of the linked component; refused when its bodies are not the same as the link's; returns component, name, replaced and warnings

List Links

Automation details

Command ID: component.links

Parameters:

→ linked components: component, name, path, file (resolved), found (null when the file is on a network location not allowed, or names a device: it is not looked for), changed (whether the file is no longer what this design last read: Update Links reads it again; null when not found or the link is older than this record), then host (the network location); state (missing, unreadable, not_allowed: a network location not allowed or outside the folders this agent may use) and reason when the file can't be reached

Part Properties

Parameter	Type	Required	Description
component	id or name	Yes	0 or "root": the design's own properties

Automation details

Command ID: component.metadata

Parameters:

component: id or name (0 or "root": the design's own properties) → component, name, part_number, description, revision, bom_type (components only), metadata (as saved, other tools' keys too), properties: {name: text}

Change Part Properties

Parameter	Type	Required	Description
component	id or name	Yes	not the root: use document.metadata.set
part_number	text	No
description	text	No
revision	text	No	empty or null removes
bom_type	normal\|phantom\|reference\|purchased\|inseparable	No	empty or null: normal
values	{key: value}	No	SolidCraft's keys, as document.metadata's properties lists them, bom_type, or a reverse-DNS key holding an object

Automation details

Command ID: component.metadata.set

Parameters:

component: id or name (not the root: use document.metadata.set); part_number?, description?, revision?: text (empty or null removes); bom_type?: normal|phantom|reference|purchased|inseparable (empty or null: normal); values?: {key: value} (SolidCraft's keys, as document.metadata's properties lists them, bom_type, or a reverse-DNS key holding an object); properties?: {name: text, …} (free properties; empty or null removes). All or nothing, one undo step → component, metadata, properties, changed: [keys]

Other commands: occurrence

Occurrence Physical Properties

Parameter	Type	Required	Description
occurrence	id or name	Yes
path	[occurrence ids]	No	required if nested under multiple instances
descendants	bool	No	default true

Automation details

Command ID: occurrence.properties

Parameters:

occurrence: id or name; path?: [occurrence ids] (required if nested under multiple instances); descendants?: bool (default true); about?: [x, y, z] (mm). Physical properties of this placement in world coordinates, including pending moves; volume, density, mass, center of mass and inertia_g_mm2 only for closed, consistently oriented bodies; total.open_bodies_skipped counts open bodies excluded from volume/mass totals; total inertia as in component.properties

Paste (Instance)

Parameter	Type	Required	Description
component		Yes	or occurrence
path	validates selected occurrence	No
parent	component	No	default: the same parent
translate	[x,y,z]	No

Automation details

Command ID: occurrence.copy

Parameters:

component (or occurrence): what to place again; path?: validates selected occurrence; parent?: component (default: the same parent); translate?: [x,y,z]; in_place?: bool (default false: the selected transform within the parent; true: where the selected placement is in the world, translate in world axes; a parent placed more than once is placed by parent_path?, else the active placement, and every instance gets the copy). Copies the selected effective transform, including pending moves

Move Occurrence

Parameter	Type	Required	Description
occurrence		Yes
path	exact placement	No
space	local\|world	No	default local
translate	[x,y,z]	No	numbers or length expressions: an occurrence moved by expressions that name parameters keeps them and moves with them when the parameters change, along the axes the move was given in; other moves of it stay; a parameter they use can't be deleted, and a renamed one carries into them
axis	[x,y,z]	No
angle	radians or "30 deg"	No
origin	[x,y,z]	No
to	{position: [x,y,z], axis?: [x,y,z], angle?} or to_matrix?: [12 or 16 numbers]	No	absolute placement: where it goes in space, not a move; not with translate/axis/angle/origin/matrix
matrix	[12 or 16 numbers]	No	instead of translate/axis/angle/origin: a rigid move as a row-major 3x4 rotation-and-translation or 4x4 matrix, flat or as rows; one that is a rotation only up to rounding is orthonormalised, a scale, shear or mirror is refused
tolerance	largest accepted \|RᵀR − I\|	No	default 1e-9, at most 1e-3
capture	bool	No	default true; false keeps it pending until Capture Position
move_grounded	bool	No	default false: a grounded occurrence refuses; true moves it and it stays grounded

Automation details

Command ID: occurrence.move

Parameters:

occurrence; path?: exact placement; space?: local|world (default local); translate?: [x,y,z] (numbers or length expressions: an occurrence moved by expressions that name parameters keeps them and moves with them when the parameters change, along the axes the move was given in; other moves of it stay; a parameter they use can't be deleted, and a renamed one carries into them); axis?: [x,y,z], angle?: radians or "30 deg", origin?: [x,y,z]; to?: {position: [x,y,z], axis?: [x,y,z], angle?} or to_matrix?: [12 or 16 numbers] (absolute placement: where it goes in space, not a move; not with translate/axis/angle/origin/matrix); matrix?: [12 or 16 numbers] (instead of translate/axis/angle/origin: a rigid move as a row-major 3x4 rotation-and-translation or 4x4 matrix, flat or as rows; one that is a rotation only up to rounding is orthonormalised, a scale, shear or mirror is refused); tolerance?: largest accepted |RᵀR − I| (default 1e-9, at most 1e-3); capture?: bool (default true; false keeps it pending until Capture Position); move_grounded?: bool (default false: a grounded occurrence refuses; true moves it and it stays grounded). Nested occurrence definitions remain shared. Replies {occurrence, transform, pending}; when joints hold it to something fixed and put it back, transform is where it is and the reply adds reverted: true and a warning naming the joint

Drag Occurrence

Parameter	Type	Required	Description
at	[x,y,z] world point on it	Yes
point	[x,y,z] where it goes	Yes

Automation details

Command ID: occurrence.drag

Parameters:

occurrence or path: exact placement; at: [x,y,z] world point on it; point: [x,y,z] where it goes. Moves the placement by point - at (with any chain of joints it is in that is joined to nothing grounded) and captures its position; other pending moves stay pending. Shared definitions move in all placements. Grounded parts and parts joints hold to something fixed are refused (joint.reach moves those)

Align Occurrence

Parameter	Type	Required	Description
occurrence	placements to move together	No
occurrences	placements to move together	No
path	placements to move together	No
paths	placements to move together	No
from		Yes
from_face		Yes
from_plane		Yes
to		Yes
to_face		Yes
to_plane		Yes
flip	bool	No
capture	bool	No	default true
move_grounded	bool	No	default false

Automation details

Command ID: occurrence.align

Parameters:

occurrence?, occurrences?, path?, paths?: placements to move together; from | from_face | from_plane; to | to_face | to_plane; flip?: bool; capture?: bool (default true); move_grounded?: bool (default false). Moves only the chosen occurrence placements in world coordinates without changing shared component geometry; a placement inside a component placed more than once moves in every placement of it, and the reply's `shared` lists those paths

Ground

Parameter	Type	Required	Description
occurrence		Yes
grounded	bool	No	default toggles

Automation details

Command ID: occurrence.ground

Parameters:

occurrence; grounded?: bool (default toggles)

Move to Component

Parameter	Type	Required	Description
occurrence		Yes
path	exact placement	No
parent	component id or name	Yes	0 or "root" for the design
parent_path	the parent's placement to place it by	No	default: its only one, else the active one; every instance of the parent gets it

Automation details

Command ID: occurrence.reparent

Parameters:

occurrence; path?: exact placement; parent: component id or name (0 or "root" for the design); parent_path?: the parent's placement to place it by (default: its only one, else the active one; every instance of the parent gets it). The placement keeps its world position; a move that would break a feature is refused

Other commands: browser

Move to Component

Read the window tour.

Automation details

Command ID: browser.reparent

Parameters:

Moves placements, features and bodies into a component. occurrences?: [ids or paths], features?: [ids or names], bodies?: [names], component?: where they go (default: the active one), component_path?: its placement → component, occurrences, features, bodies (what moved). One undo step, all or nothing: placements move first (taking what they hold), then features (taking the bodies they made), then the bodies still elsewhere (a body transfer, which leaves its features behind)

New Group

Read the window tour.

Parameter	Type	Required	Description
folder	bodies\|sketches\|construction	No
component	id	No	default 0
parent	group id	No	the new group nests in it, taking its component and folder; at most 8 levels
name		No
items	[keys]	No	they leave other groups

Automation details

Command ID: browser.group

Parameters:

folder?: bodies|sketches|construction; component?: id (default 0); parent?: group id (the new group nests in it, taking its component and folder; at most 8 levels); name?; items?: [keys] (they leave other groups)

Ungroup

Read the window tour.

Parameter	Type	Required	Description
group	id	Yes	its items and child groups go up to the group that holds it, or the folder

Automation details

Command ID: browser.ungroup

Parameters:

group: id (its items and child groups go up to the group that holds it, or the folder)

Rename Group

Read the window tour.

Parameter	Type	Required	Description
group	id	Yes
name		Yes

Automation details

Command ID: browser.rename_group

Parameters:

group: id, name

Move Browser Items

Read the window tour.

Parameter	Type	Required	Description
folder	[keys (strings) and group ids (numbers)]	Yes
component	[keys (strings) and group ids (numbers)]	No
items	[keys (strings) and group ids (numbers)]	Yes
group	id	No	into it; omit for the folder's top level
before	key or group id	No	position in it; default the end

Automation details

Command ID: browser.move

Parameters:

folder, component?, items: [keys (strings) and group ids (numbers)]; group?: id (into it; omit for the folder's top level); before?: key or group id (position in it; default the end). A group cannot go into itself or past 8 levels

Order Browser Items

Read the window tour.

Parameter	Type	Required	Description
folder	bodies\|sketches\|construction\|components	Yes
component		No
order	[keys (strings) and top-level group ids (numbers)]	Yes	display order; for `components`, the ids of the components placed in it

Automation details

Command ID: browser.order

Parameters:

folder: bodies|sketches|construction|components, component?, order: [keys (strings) and top-level group ids (numbers)] (display order; for `components`, the ids of the components placed in it)

Show/Hide

Read the window tour.

Parameter	Type	Required	Description
visible	bool	Yes
items	[sketch id or name \| body name \| construction name \| joint name \| O\|X\|Y\|Z\|XY\|XZ\|YZ]	No
joints	[joint id or name]	No	their glyphs; they still constrain and move parts
features	[feature id or name]	No	the bodies they made; path?: [occurrence ids] for only that placement's
folder	bodies\|sketches\|construction\|origin\|joints\|all	No	all of it; showing also shows its browser folders and groups, and `all` takes in the occurrence hides too
tree_folders	[browser folder or group key: c0/bodies, o:4/sketches, o:4/origin, c0/g7, c0/joints, c0/canvases, c0/point_clouds]	No	the folder or group itself: its items keep their own state; component origin items use o:4/origin/XY etc. in items
paths	[[occurrence ids]]	No	exact placements and descendants
isolate	bool	No	with paths or items of bodies, and visible:true: everything else is hidden, other placements as placements

Automation details

Command ID: browser.visibility

Parameters:

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 features?: [feature id or name] (the bodies they made; path?: [occurrence ids] for only that placement's); or folder?: bodies|sketches|construction|origin|joints|all (all of it; showing also shows its browser folders and groups, and `all` takes in the occurrence hides too); or tree_folders?: [browser folder or group key: c0/bodies, o:4/sketches, o:4/origin, c0/g7, c0/joints, c0/canvases, c0/point_clouds] (the folder or group itself: its items keep their own state; component origin items use o:4/origin/XY etc. in items); or paths?: [[occurrence ids]] (exact placements and descendants), isolate?: bool (with paths or items of bodies, and visible:true: everything else is hidden, other placements as placements). Saved with the design and undone like any other change (the camera is not)

Expand All

Read the window tour.

Parameter	Type	Required	Description
path	[occurrence ids]	No	that placement and its descendants
component	id	No	that component's own folders

Automation details

Command ID: browser.expand_all

Parameters:

path?: [occurrence ids] (that placement and its descendants); component?: id (that component's own folders); omit both for the whole tree, including folders that start closed (Origin, Named Views, Features). Display only: open/closed rows are not saved in the design and are not an undo step → open, open_by_default, closed_by_default

Collapse All

Read the window tour.

Parameter	Type	Required	Description
path	[occurrence ids]	No	that placement's branch
component	id	No

Automation details

Command ID: browser.collapse_all

Parameters:

path?: [occurrence ids] (that placement's branch); component?: id; omit both for the whole tree: every placement, folder and group at every level. The row it starts from (the design row for the whole tree) stays open, so its first level remains visible. Display only; not an undo step → open, open_by_default, closed_by_default

Other commands: joint

Reach Point

Parameter	Type	Required	Description
occurrence	id\|name	Yes
point	[x,y,z]	Yes	where its point goes, world
at	[x,y,z]	No	its point, in the world where it is now; default: the centre of its bodies' box
z	[x,y,z]	No	the way its axis then points
axis	[x,y,z]	No	that axis, in the world now; default: its own z
joints	[ids or names]	No	only these move toward the point; the other joints of a closed loop they are in follow
quiet	bool	No

Automation details

Command ID: joint.reach

Parameters:

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

Parameter	Type	Required	Description
joint		Yes
index	value index	No	default 0
min		No
max		No	omit both to clear

Automation details

Command ID: joint.limits

Parameters:

joint; index?: value index (default 0); min?, max? (omit both to clear)

Edit Joint

Parameter	Type	Required	Description
joint		Yes
a	joint origins as joint.create takes them	No
b	joint origins as joint.create takes them	No	a side left out keeps its place; the two must stay on different occurrences
type		No
flip		No
offset		No
angle		No	a number, or an expression the joint then follows
suppressed		No
name		No

Automation details

Command ID: joint.edit

Parameters:

joint; a?, b?: joint origins as joint.create takes them (a side left out keeps its place; the two must stay on different occurrences); type?, flip?, offset?, angle? (a number, or an expression the joint then follows), suppressed?, name?; the joint re-solves, keeping its limits and expressions (a relation's values start again where its parts are); an edit that places it again (not a rename alone) meets a loop it closes as joint.create does, turning an angle a half turn where only that meets it

Delete Joint

Parameter	Type	Required	Description
joint	id\|name	Yes	or origin: name, link: index

Automation details

Command ID: joint.delete

Parameters:

joint: id|name (or origin: name, link: index)

List Joints

Automation details

Command ID: joint.list

Parameters:

→ joints (type, occurrences, values, limits; expressions: {offset?, angle?, values?} when they were typed as expressions), 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)

Inspect Joint

Parameter	Type	Required	Description
joint	id\|name	No	default: every joint

Automation details

Command ID: joint.inspect

Parameters:

joint?: id|name (default: every joint) → joints: [{id, name, type, suppressed, visible, flip, offset (mm), angle (deg), values: as joint.list gives them, dofs, expressions?: {offset?, angle?, values?}, a, b: {occurrence, occurrence_name, component, component_name, path (occurrence names from the top, `/` between), snap (as saved: type, pick, face, end, edge, corner, x, point, z, in the component's coordinates), references: [{role: face|end|x|edge|corner, name, role_in_feature?: (top, side:c1…), feature?: {id, name, type} (the feature that made the face; error when it is gone), sketch?: {id, name, curve, curve_type} (a face swept from a sketch curve), faces?: [an edge's two faces], unverified?: a name saved before exact names}], resolves, frame?: {origin, z, x} in the world, error?: why the origin is lost}, links: [{index, role: driver|driven, …as joint.list}], errors, conflicts}] (reads only: nothing changes)

Solve Joints

Automation details

Command ID: joint.solve

Parameters:

re-place the occurrences from the joints → conflicts, errors, dof

Sweep Joint

Parameter	Type	Required	Description
joint	id\|name	Yes
from	its value the sweep runs between	Yes
to	its value the sweep runs between	Yes	degrees for angles, mm for distances, or expressions
index		No	which value, default 0
step		No	between samples, in the joint's unit; default: fine enough that no part passes through another between two
refine	mm	No	the first contact is bisected until no part moves more than this between the last clear value and the touching one; default 0.01
occurrences	[ids or names]	No	checked against each other; default every occurrence
against	[ids or names]	No	the parts that stay: each of `occurrences` only against these
contact_sets	true	No	the pairs of the design's contact sets
exclude_pairs	[[a, b]]	No	occurrences by id or name: pairs of bodies under a and b are not checked, such as a pin in its hole
budget_s	seconds	No	at most 86400; past them the sweep stops with what it found; its work is then not capped. Without it the work caps, 4096 samples, 64 bisection steps and 500 million triangle tests, stop it the same way
report_gaps	bool	No	the nearest gap at every sample, default false
apply	bool	No	leave the design where the sweep stopped; default false: the design is not changed

Automation details

Command ID: joint.sweep

Parameters:

joint: id|name; from, to: its value the sweep runs between (degrees for angles, mm for distances, or expressions); index? (which value, default 0); step? (between samples, in the joint's unit; default: fine enough that no part passes through another between two); refine?: mm (the first contact is bisected until no part moves more than this between the last clear value and the touching one; default 0.01); occurrences?: [ids or names] (checked against each other; default every occurrence), with against?: [ids or names] (the parts that stay: each of `occurrences` only against these), or contact_sets?: true (the pairs of the design's contact sets); exclude_pairs?: [[a, b]] (occurrences by id or name: pairs of bodies under a and b are not checked, such as a pin in its hole); budget_s?: seconds (at most 86400; past them the sweep stops with what it found; its work is then not capped. Without it the work caps, 4096 samples, 64 bisection steps and 500 million triangle tests, stop it the same way); report_gaps?: bool (the nearest gap at every sample, default false); apply?: bool (leave the design where the sweep stopped; default false: the design is not changed) → stopped_at (the last value clear of contact, or where a loop or limit stopped it; null: it reached `to`), stopped_by: {a, b, at: [x,y,z] (where they touch, world), a_part, b_part: {component, path: [occurrence names], path_ids} (where each touching body sits)} | "loop" | "limit" | "budget" (stopped_at: the last value checked clear) | null, samples: [{value, min_gap_mm?, pair?, parts?}], min_gap? (report_gaps: {part: {mm, at_value, to}}, the nearest each part came to another), unit, gap_method ("mesh": distances between the tessellations), gap_tolerance_mm (how far those can be off: 0 when every face is flat), pairs (checked), touching_at_start: [[a, b]] (pairs already touching at `from`, such as parts joined face to face or a door on its frame: these stop it only once they pass into each other deeper than they start), touching_parts (where their bodies sit), budget_s, budget_exceeded, budget_ran_out: "time" | "samples" | "bisections" (a contact reported less refined than `refine`) | "intersections" | "work" | null, applied. The parts are tested at the samples and through the bisection; the motion is on a copy (closed loops follow, contact sets do not stop it)

Find Joint Limits

Parameter	Type	Required	Description
joint	id\|name	Yes
index		No	one value; default every value
refine		No
step		No
occurrences		No
against		No
contact_sets		No
exclude_pairs		No	as joint.sweep

Automation details

Command ID: joint.find_limits

Parameters:

joint: id|name; index? (one value; default every value); refine?, step?, occurrences?, against?, contact_sets?, exclude_pairs? (as joint.sweep) → values: [{index, dof, unit, value (now), min, max, min_by, max_by, range}], each value swept both ways from where it is, its own limits ignored, closed loops following; each side stops at the first contact (bisected to `refine`), where a loop cannot close, or at another limit (another value's, or another joint's through a motion link): min_by/max_by {a, b, at} | "loop" | "limit" | "budget" (its work ran out: the last value checked clear) | "turn" (an angle with no contact within a turn: a turn from the other side, or ±180° from now when nothing is met at all) | "range" (a distance with no contact within the parts' reach: min/max null); touching_at_start, overlapping_at_start: [{a, b, depth_mm}] (already passing into each other: they stop it only going deeper), refine_mm, gap_method, gap_tolerance_mm, pairs (0: no two parts to check, so nothing is swept). The design is not changed

Other commands: assembly

Edit Constraint

Parameter	Type	Required	Description
constraint	id\|name	Yes	a joint made with assembly.constraint.create
type	a rule as assembly.constraint.create takes it	No	the references it has must fit it; the gap carries over
offset	the gap	No	mm or an expression
angle	an angle rule's angle	No
flip	true turns b over	No	from the new rule's way after a type change, else from how it faces now
name		No
suppressed		No

Automation details

Command ID: assembly.constraint.edit

Parameters:

constraint: id|name (a joint made with assembly.constraint.create); type?: a rule as assembly.constraint.create takes it (the references it has must fit it; the gap carries over); offset?: the gap (mm or an expression); angle?: an angle rule's angle; flip?: true turns b over (from the new rule's way after a type change, else from how it faces now); name?; suppressed?; quiet?. Changed as joint.edit changes a joint: its values start again where its parts are → conflicts, errors, dof, fixed as joint.edit

Mass Properties

Automation details

Command ID: assembly.mass_properties

Parameters:

no parameters → occurrences: [{occurrence (0: the design's own bodies), name, component, path, group, fixed, frame {origin, x, y, z}, bodies: [{name, material, density_g_cm3, closed, volume_mm3, mass_kg}], open_bodies_skipped, mass}], groups: [{group, occurrences, fixed, frame_occurrence, frame, mass}] (occurrences an unsuppressed rigid joint ties together, and a nested occurrence no joint places with its parent; fixed: holds the design or a grounded occurrence), warnings. mass: {mass_kg, center_of_mass_mm (world), center_of_mass_local_mm, inertia_world_kg_mm2, inertia_local_kg_mm2 (about the centre of mass, in world and frame axes)} or null when massless. Read-only; pending moves count; each body at its material's density (the default material's when none is assigned)

Other commands: contact

Edit Contact Set

Parameter	Type	Required
set	id\|name	Yes
occurrences		No
name		No
suppressed	bool	No
delete	bool	No

Automation details

Command ID: contact.edit

Parameters:

set: id|name; occurrences?; name?; suppressed?: bool; delete?: bool

List Contact Sets

Automation details

Command ID: contact.list

Parameters:

→ sets, enabled, all

Check Contact

Automation details

Command ID: contact.check

Parameters:

→ pairs in contact sets that pass through each other now

Other commands: motion

Play Motion Study

Parameter	Type	Required	Description
study	id\|name	Yes
step		Yes	0…steps
quiet	bool	No	positions of only the occurrences that moved

Automation details

Command ID: motion.play

Parameters:

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)

Export Motion Study

Parameter	Required	Description
study	Yes
samples	No	default steps + 1
path	No	.json or .csv

Automation details

Command ID: motion.export

Parameters:

study; samples? (default steps + 1); path? (.json or .csv) → occurrence positions per step (the design is not changed)

Export Motion Animation

Parameter	Type	Required	Description
study	id\|name	Yes
joint	id\|name with from and to	Yes	degrees for angles, mm for distances, or expressions
view	id\|name	Yes	an exploded view, coming apart from the assembled placement
samples		No	frames, 2…1000; default the study's steps + 1, 100 for a joint, 41 for a view or 81 with back
width		No
height		No	16…4096 pixels, default 800 × 500
camera	{target, yaw, pitch, roll?, distance, fov?, up?}	No	ui.camera's reply; fields left out keep the default view: view.apply's camera, or the home view framing the model, for a view both assembled and exploded
fps		No	1…50, default 20

Automation details

Command ID: motion.export_animation

Parameters:

study: id|name, or joint: id|name with from and to (degrees for angles, mm for distances, or expressions) and index?, or view: id|name (an exploded view, coming apart from the assembled placement) with back? (default false; true: back together too, exploded at the middle frame of an odd count); 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, 100 for a joint, 41 for a view or 81 with back); 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, for a view both assembled and exploded); fps? (1…50, default 20); grid?, axes? (default true: the ground grid and the origin's axes) - draws the study as it plays, the joint as it is driven or the view as it explodes, 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, nor its placements)

Keep Motion Trace

Parameter	Type	Required	Description
study	id\|name	Yes
joint	id\|name with from and to	Yes	degrees for angles, mm for distances, or expressions
name		No	default Motion TraceN
auto_update	bool	No	default true
point_ref	joint origin snap - keeps the trace as a root 3D sketch spline	No

Automation details

Command ID: motion.trace.keep

Parameters:

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); auto_update?: bool (default true); point_ref?: joint origin snap - keeps the trace as a root 3D sketch spline. Associative curves follow mechanism and driving-input edits; false keeps a fixed curve. point_ref retains a geometry snap; otherwise point is retained in component coordinates → sketch, name, curves, points

Edit Motion Trace

Parameter	Type	Required	Description
sketch	id\|name	Yes
index		No
samples		No	2…500
auto_update	false to detach	No

Automation details

Command ID: motion.trace.edit

Parameters:

sketch: id|name; joint? with from and to, or study?; index?; samples? (2…500); auto_update?: false to detach. Edits a saved associative trace's driving conditions in one undo step

Plot Motion Study

Parameter	Type	Required	Description
study	id\|name	Yes
joints	[id\|name]	No	default: every joint that moves
samples		No	3…1000, default the study's steps + 1

Automation details

Command ID: motion.plot

Parameters:

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

Parameter	Type	Required	Description
study	id\|name	Yes
occurrences	[ids or names]	No	two or more, checked against each other; default every occurrence
against	[ids or names]	No	then each of `occurrences` is checked only against these, such as an arm against the parts it must miss
contact_sets	true	No	the pairs of the design's contact sets
exclude_pairs	[[a, b]]	No	occurrences by id or name: pairs of bodies under a and b are not checked
samples		No	2…1000, default the study's steps + 1

Automation details

Command ID: motion.interference

Parameters:

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); exclude_pairs?: [[a, b]] (occurrences by id or name: pairs of bodies under a and b are not checked); samples? (2…1000, default the study's steps + 1); budget_s?: seconds (above 0, at most 86400; default a fixed work budget): the time the check may take instead, looked at between samples, for a mechanism such as a gear train that needs longer → collisions: [{a, b, first_step, last_step, steps: [[from, to]…] (the step ranges where they overlap), volume_mm3 (the most volume they share at a sample, worked out exactly from the bodies), deepest_step (the first sample sharing that volume), not_measured (null, or why the volume was not worked out at every sample they overlap, such as a budget it ran past: then volume_mm3 and deepest_step are null, never an estimate), depth_mm (how far into each other at most: an estimate from points of the bodies' contact meshes, not exact)}], clear (every sample checked and none collide; never while truncated), pairs (checked), samples (taken), truncated (the work budget, or budget_s, ran out; checked_to: the last step checked), budget_s (when given), 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

List Motion Studies

Automation details

Command ID: motion.list

No parameter description is provided by the command registry.

Delete Motion Study

Parameter	Type	Required	Description
study		Yes

Automation details

Command ID: motion.delete

Parameters:

study

Other commands: explode

Show Exploded View

Parameter	Type	Required	Description
view	id\|name	Yes	or none: back to the assembled placement

Automation details

Command ID: explode.show

Parameters:

view: id|name (or none: back to the assembled placement) — shown only; the design keeps its placements

List Exploded Views

Automation details

Command ID: explode.list

No parameter description is provided by the command registry.

Delete Exploded View

Parameter	Type	Required	Description
view		Yes

Automation details

Command ID: explode.delete

Parameters:

view

Other commands: layout

Apply Layout

Parameter	Type	Required	Description
name	apply preset to current workspace through retained runtime	Yes
expected_revision	apply preset to current workspace through retained runtime	No

Automation details

Command ID: layout.apply

Parameters:

name, expected_revision?: apply preset to current workspace through retained runtime

Inspect Layout

Automation details

Command ID: layout.get

Parameters:

{}: committed state and registered workspace summaries

Reset Layout

Parameter	Type	Required	Description
expected_revision	restore current workspace's registered default	No

Automation details

Command ID: layout.reset

Parameters:

expected_revision?: restore current workspace's registered default

Save Layout

Parameter	Type	Required	Description
name		Yes
replace	false	No	overwrite accepted for compatibility
expected_revision	save complete envelope in injected catalogue	No

Automation details

Command ID: layout.save

Parameters:

name, replace?: false (overwrite accepted for compatibility), expected_revision?: save complete envelope in injected catalogue

Select Layout Workspace

Parameter	Type	Required	Description
workspace	atomically remember outgoing and replace with destination	Yes
expected_revision	atomically remember outgoing and replace with destination	No

Automation details

Command ID: layout.workspace.select

Parameters:

workspace, expected_revision?: atomically remember outgoing and replace with destination

Other commands: panel

Run Panel Header Action

Automation details

Command ID: panel.action

Parameters:

target or legacy id, action, expected_revision?: invoke a registered owning-controller action

Activate Panel Tab

Automation details

Command ID: panel.activate

Parameters:

target or legacy id, expected_revision?: activate open tab without focus

Close Panel

Automation details

Command ID: panel.close

Parameters:

target or legacy id, expected_revision?: explicit guarded close

Collapse Panel Section

Automation details

Command ID: panel.collapse

Parameters:

target or legacy id, collapsed, expected_revision?

Dismiss Panel Peek

Parameter	Type	Required	Description
expected_revision	dismiss temporary collapsed-panel presentation	No

Automation details

Command ID: panel.dismiss

Parameters:

expected_revision?: dismiss temporary collapsed-panel presentation

Float Panel

Automation details

Command ID: panel.float

Parameters:

target or legacy id, destination: new_section with floating location, expected_revision?

Focus Panel

Automation details

Command ID: panel.focus

Parameters:

target or legacy id, expected_revision?: reopen retained state, activate and request focus

Focus Next Panel

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.focus.next

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Focus Previous Panel

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.focus.previous

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

List Panels

Automation details

Command ID: panel.list

Parameters:

{}: committed state, active tabs, capabilities, availability and registered kinds

Move Panel

Automation details

Command ID: panel.move

Parameters:

target or legacy id, destination: new_section, join_tab or relative, activate?: false, expected_revision?

Move Panel to Next Zone

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.move.next_zone

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Redock Native Panel Section

Parameter	Type	Required	Description
target	native_host	Yes
expected_revision	native close redocks without cancelling content	No

Automation details

Command ID: panel.native_close

Parameters:

target: native_host, expected_revision?: native close redocks without cancelling content

Open Panel

Parameter	Type	Required
kind		Yes
instance		Yes
destination	required for new instance	No
expected_revision		No

Automation details

Command ID: panel.open

Parameters:

kind, instance, destination?: required for new instance, expected_revision?

Peek Collapsed Panel

Automation details

Command ID: panel.peek

Parameters:

target or legacy id, expected_revision?: transient presentation without resizing

Pop Out Panel

Automation details

Command ID: panel.popout

Parameters:

target or legacy id, destination: new_section with window location, expected_revision?: web lowers to floating

Reset Panel Sash

Parameter	Type	Required
first	reset adjacent dock pair to registered default ratio	Yes
second	reset adjacent dock pair to registered default ratio	Yes
expected_revision	reset adjacent dock pair to registered default ratio	No

Automation details

Command ID: panel.reset_pair

Parameters:

first, second, expected_revision?: reset adjacent dock pair to registered default ratio

Resize Panel Section

Automation details

Command ID: panel.resize

Parameters:

target or legacy id, size: {width,height}, thickness_only?: false by default; true changes Bottom height or side column width and ignores the other valid size component, expected_revision?

Resize Panel Sash

Parameter	Type	Required
first	conserve adjacent dock pair extent	Yes
second	conserve adjacent dock pair extent	Yes
first_size	conserve adjacent dock pair extent	Yes
second_size	conserve adjacent dock pair extent	Yes
expected_revision	conserve adjacent dock pair extent	No

Automation details

Command ID: panel.resize_pair

Parameters:

first, second, first_size, second_size, expected_revision?: conserve adjacent dock pair extent

Resize Panel Sash Down

Default keyboard shortcut: Down

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.sash.down

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Resize Panel Sash Left

Default keyboard shortcut: Left

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.sash.left

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Reset Focused Panel Sash

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.sash.reset

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Resize Panel Sash Right

Default keyboard shortcut: Right

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.sash.right

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Resize Panel Sash Up

Default keyboard shortcut: Up

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.sash.up

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Toggle Focused Panel

Parameter	Type	Required	Description
expected_revision	resolve the focused shared panel control in the live host	No

Automation details

Command ID: panel.toggle

Parameters:

expected_revision?: resolve the focused shared panel control in the live host

Other commands: config

Configuration Column

Parameter	Type	Required	Description
param		No	target name
feature		No	target name
material		No	target name
appearance		No	target name
delete	bool	No

Automation details

Command ID: config.column

Parameters:

param? | feature? | material? | appearance? (target name); delete?: bool

Configuration Row

Parameter	Type	Required	Description
name		Yes	a row's name, or its id from config.table
from		No	row to copy, by name or id; default current values
values	{column key: expression, suppression, material name, appearance name or Look object}	No
rename		No
delete	bool	No

Automation details

Command ID: config.row

Parameters:

name (a row's name, or its id from config.table); from? (row to copy, by name or id; default current values); values?: {column key: expression, suppression, material name, appearance name or Look object}; rename?; delete?: bool

Activate Configuration

Automation details

Command ID: config.activate

Parameters:

row: a row's name, or its id from config.table — sets its parameter values and suppressions

Preview Configuration

Automation details

Command ID: config.preview

Parameters:

row: a row's name, or its id from config.table — validates a rebuild without changing the design or history

Configuration Rule

Parameter	Type	Required	Description
rule	{id,name,enabled,condition,effect}	No
rules	[rule…]	No	added or replaced together, then the rows checked once

Automation details

Command ID: config.rule

Parameters:

rule?: {id,name,enabled,condition,effect}; rules?: [rule…] (added or replaced together, then the rows checked once); id? + delete?; id? + index? (ordered move)

Configuration Rules

Automation details

Command ID: config.rules

Parameters:

ordered typed rules, rows and active state

Other commands: parts

Standard Parts

Parameter	Type	Required	Description
family		No

Automation details

Command ID: parts.library

Parameters:

family? → families (name, standard, system: metric|inch, sizes, lengths) and, with family, each size's dimensions (mm)

Insert Part

Parameter	Type	Required	Description
family		Yes	socket_head_cap_screw \| button_head_cap_screw \| countersunk_socket_screw \| hex_bolt \| hex_nut \| washer \| set_screw \| dowel_pin \| bearing \| hex_cap_screw_inch \| hex_nut_inch \| washer_sae \| washer_uss
size		Yes	"M6", "608" for bearings, "1/2-13 UNC" for inch screws and nuts, "1/2" for inch washers
length		No	mm, inch parts too; screws, bolts, set screws, pins; default a standard length near 2.5 d
flip	bool	No	default false: turned over, head into the material with at, +z against direction with point
name		No

Automation details

Command ID: parts.insert

Parameters:

family (socket_head_cap_screw | button_head_cap_screw | countersunk_socket_screw | hex_bolt | hex_nut | washer | set_screw | dowel_pin | bearing | hex_cap_screw_inch | hex_nut_inch | washer_sae | washer_uss); size ("M6", "608" for bearings, "1/2-13 UNC" for inch screws and nuts, "1/2" for inch washers); length? (mm, inch parts too; 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, head on the picked face and shank into the hole, whichever way the face points) or on a flat face (seated at that point, head out of the face), or a list of them (one component, placed and seated once per pick) | point?: [x,y,z] with direction?: [x,y,z] (no joint: the part's seating plane, under a head or the bottom of a nut, washer or bearing, the top of a set screw, pin or countersunk head, goes to point, and direction is its +z, from the shank's tip toward the head; default [0,0,1], head up, shank down -z); flip?: bool (default false: turned over, head into the material with at, +z against direction with point); name? → component, occurrence, joint?, directions (each placement's head direction in the world, the one chosen), and with at: occurrences, joints (one per pick, in pick order)

Change Part Size

Parameter	Type	Required	Description
component	id\|name of an inserted part	Yes
size		No

Automation details

Command ID: parts.resize

Parameters:

component: id|name of an inserted part; size?; length? — rebuilds it (joints keep it seated)

Other commands: body

Rename Body

Parameter	Type	Required	Description
body	its name	Yes
bodies	several body names	Yes	each in turn gets the first of name, name (2), name (3)… that no other body has
name	the new name	Yes	features that use the bodies follow

Automation details

Command ID: body.rename

Parameters:

body: its name, or bodies: several body names (each in turn gets the first of name, name (2), name (3)… that no other body has), name: the new name (features that use the bodies follow)

Repair Part

Parameter	Type	Required	Description
body	its name	Yes	a part the modelling kernel refuses, or an open part that should be a solid
gap	expr	No	default 0.2 mm, at most 1 mm: free edges that pair up within it are sewn, each sewn edge carrying its own gap as its tolerance
patch_holes	bool	No	default false: loops of free edges left are patched, in the plane of the faces around them where those are that plane, else tangent to them, and sewn in; otherwise the reply offers the patches
name		No

Automation details

Command ID: body.repair

Parameters:

body: its name (a part the modelling kernel refuses, or an open part that should be a solid); gap?: expr (default 0.2 mm, at most 1 mm: free edges that pair up within it are sewn, each sewn edge carrying its own gap as its tolerance); patch_holes?: bool (default false: loops of free edges left are patched, in the plane of the faces around them where those are that plane, else tangent to them, and sewn in; otherwise the reply offers the patches); name? → the feature, and repair: what changed face by face (rebuilt and refused faces, sewn gaps, holes with their surface.patch), faces and largest edge tolerance before and after, closed, modelling, volume. Refused with why when nothing applies

Print Face

Default keyboard shortcut: Ctrl+B

Parameter	Type	Required	Description
body	its name	Yes

Automation details

Command ID: body.print_face

Parameters:

body: its name; point?: [x, y, z] on a flat face of it, in mm (omit to clear) → {body, face?}: marks the face a slicer export (file.send_to_slicer, file.save_mesh with slicer, file.open_in_easyprint), or an STL or 3MF export with lay_on_print_faces (file.export, file.export_stl, file.export_3mf, file.save_mesh), lays the body on: turned so the face points down at Z = 0, the centre of mass over the origin. One per body, replacing the last; flat faces of solid bodies only. A print face that is gone or no longer flat is reported in the export's warnings, and the body exported as it lies

Other commands: document

Change Design Units

Parameter	Type	Required	Description
units	mm\|cm\|m\|in\|ft	Yes	display and unit-less parameters; values keep their meaning

Automation details

Command ID: document.units

Parameters:

units: mm|cm|m|in|ft (display and unit-less parameters; values keep their meaning)

Design Properties

Automation details

Command ID: document.metadata

Parameters:

→ metadata: the design's metadata object as saved (other tools' keys too); properties: each of SolidCraft's design properties (project, part number, revision…), its text or null (absent, or not text)

Change Design Properties

Automation details

Command ID: document.metadata.set

Parameters:

key and value, or values: {key: value, …} (all or nothing, one undo step). SolidCraft's keys, the ones document.metadata's properties lists, take 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]

Remove Design Property

Parameter	Type	Required	Description
key	[keys]	Yes
keys	[keys]	Yes	any key, also one another tool wrote

Automation details

Command ID: document.metadata.remove

Parameters:

key, or keys: [keys] (any key, also one another tool wrote) → metadata, removed: [keys that were there]

Inspect Design

Parameter	Type	Required	Description
measure	bool	No	include body measurements
sketch_counts	bool	No	each sketch also gives its plane and its number of points and constraints
timeline	true\| "summary"\| false	No	default; each feature as id, name, type, with error, warning, suppressed and rolled_back only when set; left out
bodies	true\| "names"\| false	No	default; only the body names, nothing measured; left out

Automation details

Command ID: document.inspect

Parameters:

measure?: bool (include body measurements); sketch_counts?: bool (each sketch also gives its plane and its number of points and constraints); timeline?: true (default) | "summary" (each feature as id, name, type, with error, warning, suppressed and rolled_back only when set) | false (left out); bodies?: true (default) | "names" (only the body names, nothing measured) | false (left out)

Design Revision

Automation details

Command ID: document.revision

Parameters:

→ document_id (this open design's id: kept while it stays open, another for each design started or opened), revision (moves whenever the design, what is hidden or a component's uncaptured position changes, never on a selection or a view; from one counter for the whole run, so it never repeats). Read-only

Other commands: view

New Named View

Read the window tour.

Parameter	Type	Required	Description
name		No
camera	{target: [x,y,z], yaw, pitch, distance, fov?}	Yes	replaces a view of the same name

Automation details

Command ID: view.save

Parameters:

name?; camera: {target: [x,y,z], yaw, pitch, distance, fov?} (replaces a view of the same name)

Rename Named View

Read the window tour.

Parameter	Type	Required	Description
view	name	Yes
name		Yes

Automation details

Command ID: view.rename

Parameters:

view: name, name

Delete Named View

Read the window tour.

Parameter	Type	Required	Description
view	name	Yes

Automation details

Command ID: view.delete

Parameters:

view: name

List Named Views

Read the window tour.

Automation details

Command ID: view.list

No parameter description is provided by the command registry.

Restore Named View

Read the window tour.

Parameter	Type	Required	Description
view	front\|back\|top\|bottom\|left\|right\|iso\|home\| a named view's name	No	frames the model
camera	{target: [x,y,z], yaw, pitch, distance, fov?, roll?}	No	radians, mm, about the up axis; yaw: heading of the line of sight, 0 along +Y (Front), π/2 along +X (Left), π (Back), −π/2 (Right); pitch: the eye's elevation, within ±π/2, π/2 = Top; roll defaults to 0, turns the picture clockwise, must be finite and is clamped to ±π; the View angles readout shows these in degrees; up is refused: the up axis comes from the design settings

Automation details

Command ID: view.apply

Parameters:

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?, roll?} (radians, mm, about the up axis; yaw: heading of the line of sight, 0 along +Y (Front), π/2 along +X (Left), π (Back), −π/2 (Right); pitch: the eye's elevation, within ±π/2, π/2 = Top; roll defaults to 0, turns the picture clockwise, must be finite and is clamped to ±π; the View angles readout shows these in degrees; up is refused: the up axis comes from the design settings) → camera. The viewport (and the MCP screenshot) moves there. View state: not saved, not an undo step

Viewport Status Details

Read the window tour.

Automation details

Command ID: view.status_details

Parameters:

no parameters → current effect settings/detail capabilities and retained per-seam Continuity diagnostics, with current geometry validity; read-only, no evaluation

Viewport Status Items

Read the window tour.

Automation details

Command ID: view.status_items

Parameters:

no parameters → {items}; persistent viewport effects, oldest slot first, with structured settings and executable clear requests; read-only, no model evaluation

Fit

Default keyboard shortcut: F6

Read the window tour.

Automation details

Command ID: view.fit

Parameters:

no parameters → frame the active canvas or selection; display only

Home View

Read the window tour.

Automation details

Command ID: view.home

Parameters:

no parameters → home orientation framing the active canvas; display only

Read the window tour.

Parameter	Type	Required	Description
tool	orbit\|pan\|zoom\|none	Yes

Automation details

Command ID: view.tool

Parameters:

tool: orbit|pan|zoom|none → tool; latch a camera tool, none releases it

Drag to Zoom

Read the window tour.

Parameter	Type	Required	Description
on	bool	No	omitted: toggle

Automation details

Command ID: view.tool.zoom

Parameters:

on?: bool (omitted: toggle) → on?; latch the Zoom tool for left-button drags. A shortcut assigned in the UI zooms while held

Continuous Orbit

Read the window tour.

Parameter	Type	Required	Description
on	bool	No	omitted: toggle

Automation details

Command ID: view.spin

Parameters:

on?: bool (omitted: toggle) → on?; continuous orbit until the next click or key

Visual Style

Read the window tour.

Parameter	Type	Required	Description
style	shaded_with_edges\|shaded\|wireframe\|shaded_with_hidden_edges	Yes

Automation details

Command ID: view.visual_style

Parameters:

style: shaded_with_edges|shaded|wireframe|shaded_with_hidden_edges → style, index (0..3 in that order)

Grid

Read the window tour.

Parameter	Type	Required	Description
on	bool	No	omitted: toggle

Automation details

Command ID: view.grid

Parameters:

on?: bool (omitted: toggle) → on?; show the viewport grid

Ground Shadow

Read the window tour.

Parameter	Type	Required	Description
on	bool	No	omitted: toggle

Automation details

Command ID: view.ground_shadow

Parameters:

on?: bool (omitted: toggle) → on?; show the ground shadow

Read the window tour.

Parameter	Type	Required	Description
visible	bool	No	omitted: toggle

Automation details

Command ID: view.navigation_bar

Parameters:

visible?: bool (omitted: toggle) → visible?; show the navigation bar (window setting)

Custom View Navigator

Read the window tour.

Parameter	Type	Required
style	axes\|cube\|custom	No
body	body name\|null	No
texture	themed\|modeled	No
arrows	bool	No
home	bool	No

Automation details

Command ID: view.navigator

Parameters:

style?: axes|cube|custom; body?: body name|null; texture?: themed|modeled; arrows?, home?: bool → the navigator as set; the app's view navigator, never saved in the design; never opens a dialog (a toolbar start opens the Custom View Navigator panel)

Ribbon Tabs Only

Read the window tour.

Parameter	Type	Required	Description
on	bool	No	omitted: switch

Automation details

Command ID: view.ribbon_tabs_only

Parameters:

on?: bool (omitted: switch) → on?; fold the ribbon to its tab row, a tab click shows its panels over the view (window setting)

Render Focus View

Read the window tour.

Parameter	Type	Required	Description
on	bool	Yes

Automation details

Command ID: view.render_focus

Parameters:

on: bool → {on}; per-window UI state, never saved in the design; headless validation only

Render Frame Guides

Read the window tour.

Parameter	Type	Required	Description
aspect	16:9\|3:2\|1:1\|4:5\|9:16\|custom	No

Automation details

Command ID: view.render_frame

Parameters:

aspect?: 16:9|3:2|1:1|4:5|9:16|custom; thirds?, safe_area?, centre_mark?: bool. At least one field. Validated transient overlay request, echoed headlessly; never saves guides, changes output size, evaluates geometry or opens a dialog

Render Browser

Read the window tour.

Parameter	Type	Required	Description
open	bool	Yes
by_look	bool	No
search	bool	No
query	string	No	up to 1024 bytes

Automation details

Command ID: view.render_browser

Parameters:

open: bool; or by_look?: bool; search?: bool; query?: string (up to 1024 bytes) → validated transient Browser controls; never edits the design or opens a dialog

Render Inspector

Read the window tour.

Parameter	Type	Required	Description
visible	bool	Yes

Automation details

Command ID: view.render_inspector

Parameters:

visible: bool → {visible}; per-document Inspector visibility; never edits the design or opens a dialog

Pause or Resume Live Render

Read the window tour.

Parameter	Type	Required	Description
paused	bool	Yes

Automation details

Command ID: view.render_live

Parameters:

paused: bool → {paused}; pause or resume this document's live Render preview; headless validation only, never saves settings or changes a final image

Render selection

Read the window tour.

Parameter	Type	Required	Description
kind	nothing\|environment\|lighting\|light\|shot\|output\|wear\|sampling\|effects\|check	Yes
id	bounded nonempty string for light/shot	No

Automation details

Command ID: view.render_select

Parameters:

kind: nothing|environment|lighting|light|shot|output|wear|sampling|effects|check; id?: bounded nonempty string for light/shot → validated transient Browser focus; never edits the design or opens a dialog

Render Stage

Read the window tour.

Parameter	Type	Required	Description
stage	look\|light\|frame\|output	Yes

Automation details

Command ID: view.render_stage

Parameters:

stage: look|light|frame|output → {stage}; per-document UI state, never edits or evaluates the design; headless validation only

Shots Strip

Read the window tour.

Parameter	Type	Required	Description
visible	bool	Yes

Automation details

Command ID: view.shots_strip

Parameters:

visible: bool → {visible}; Render Shots strip UI preference. Headless echo only, no document edits or undo

Move Render Dock

Command group: RENDER › SCENE

Read the window tour.

Parameter	Type	Required	Description
panel	inspector\|browser	Yes
side	left\|right	Yes

Automation details

Command ID: view.render_dock

Parameters:

panel: inspector|browser; side: left|right → {panel, side}; Render dock UI preference; headless echo only, no document edits or undo

Workspace layout

Read the window tour.

Parameter	Type	Required	Description
mode	floating\|compact	Yes

Automation details

Command ID: view.layout

Parameters:

mode: floating|compact → validated workspace layout; display only, never opens a dialog

History layout

Read the window tour.

Parameter	Type	Required	Description
width	1..1000000	No
dock	bottom\|left\|under_browser\|browser	No	browser: the history in the browser, no timeline
collapsed	bool	No

Automation details

Command ID: view.history_layout

Parameters:

width?: 1..1000000; dock?: bottom|left|under_browser|browser (browser: the history in the browser, no timeline); collapsed?: bool → validated layout request; display only, never opens a dialog

Graphics Preset

Read the window tour.

Parameter	Type	Required	Description
preset	performance\|quality	Yes

Automation details

Command ID: view.graphics_preset

Parameters:

preset: performance|quality → preset, enabled, display_quality, supersampling, supersampling_adaptive; Quality: AO, Fine, adaptive 2x SSAA; Performance: no AO, Normal, no SSAA

Ambient Occlusion

Read the window tour.

Parameter	Type	Required	Description
enabled	bool	Yes

Automation details

Command ID: view.ambient_occlusion

Parameters:

enabled: bool → enabled; apply soft contact shading in the GPU viewport

Origin Axes Across the Whole View

Read the window tour.

Parameter	Type	Required	Description
enabled	bool	Yes

Automation details

Command ID: view.origin_axes_across_view

Parameters:

enabled: bool → enabled; extend the origin axes across the view, or keep the short axes when false; display only, never opens a dialog

Perspective view

Read the window tour.

Parameter	Type	Required	Description
enabled	bool	Yes

Automation details

Command ID: view.perspective

Parameters:

enabled: bool → enabled; draw the view in perspective, or orthographic when false; a sketch being edited is always shown orthographic

View Angles

Read the window tour.

Parameter	Type	Required	Description
enabled	bool	Yes

Automation details

Command ID: view.angle_readout

Parameters:

enabled: bool → enabled; show the view's pitch, yaw and roll (degrees, as view.apply's camera in radians) and Ortho or Persp under the orientation gizmo; display only, never opens a dialog

Navigate View

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	Yes
direction	[x,y,z] in the camera's up-axis frame	No
action	left\|right\|up\|down\|clockwise\|counterclockwise\|home\|fit	Yes
degrees	0..180	No	how far left\|right\|up\|down turn; default 90
fit	bool	No	frame the whole model from the new direction as well, as home does; default false
motion	pan\|orbit\|zoom	Yes
delta	[dx,dy]	No	pixels, each ±10000
free_orbit	bool	No	orbit through poles, default false
viewport	[width,height]	No	1..1000000, required for pan or pivot
pivot	[x,y,z]	No
factor	0.05..20	No	required for zoom
anchor	[x,y,z]	No

Automation details

Command ID: view.navigate

Parameters:

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), fit?: bool (frame the whole model from the new direction as well, as home does; default false); or motion: pan|orbit|zoom, delta?: [dx,dy] (pixels, each ±10000), free_orbit?: bool (orbit through poles, default false), 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?

Normal to Selection

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.normal_to

Parameters:

camera?: Camera (default: current session camera or home view) → camera; Look At the first selected planar face or plane, centered on the picked point; repeat while aligned to flip the side; preserves scale and projection

Front View

Default keyboard shortcut: Ctrl+1

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.front

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Back View

Default keyboard shortcut: Ctrl+2

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.back

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Left View

Default keyboard shortcut: Ctrl+3

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.left

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Right View

Default keyboard shortcut: Ctrl+4

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.right

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Top View

Default keyboard shortcut: Ctrl+5

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.top

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Bottom View

Default keyboard shortcut: Ctrl+6

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.bottom

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Isometric View

Default keyboard shortcut: Ctrl+7

Read the window tour.

Parameter	Type	Required	Description
camera	Camera	No	default: current session camera or home view

Automation details

Command ID: view.isometric

Parameters:

camera?: Camera (default: current session camera or home view) → camera; turns to that standard view as the view cube does, keeping target, distance and projection

Next Tab

Default keyboard shortcut: Ctrl+Tab

Read the window tour.

Automation details

Command ID: view.next_tab

Parameters:

no parameters → step: 1; the window shows the design tab to the right of the shown one (after the last, the first); never edits the design or opens a dialog

Previous Tab

Default keyboard shortcut: Ctrl+Shift+Tab

Read the window tour.

Automation details

Command ID: view.previous_tab

Parameters:

no parameters → step: -1; the window shows the design tab to the left of the shown one (before the first, the last); never edits the design or opens a dialog

Other commands: note

Add Note

Parameter	Type	Required	Description
anchor	[x,y,z]	No	the point in model space, mm; without it, where the selection points, or the origin
text	the note	Yes	may span lines
hidden	bool	No	saved but not drawn

Automation details

Command ID: note.add

Parameters:

anchor?: [x,y,z] (the point in model space, mm; without it, where the selection points, or the origin); text: the note (may span lines); hidden?: bool (saved but not drawn) → note: id

Edit Note

Parameter	Type	Required	Description
note	id	Yes
text	the new text	No
anchor	[x,y,z]	No	move the anchor
hidden	bool	No	show or hide

Automation details

Command ID: note.update

Parameters:

note: id; text?: the new text; anchor?: [x,y,z] (move the anchor); hidden?: bool (show or hide) → note: id

Delete Note

Parameter	Type	Required	Description
note	id	Yes

Automation details

Command ID: note.delete

Parameters:

note: id → deleted: id

List Notes

Automation details

Command ID: note.list

Parameters:

→ notes: [{id, anchor: [x,y,z], text, hidden}] in creation order

Other commands: selection

Delete

Parameter	Type	Required
items	[selection items]	No
components	[ids or names]	No
occurrences	[ids or names]	No
canvases	[ids or names]	No
point_clouds	[ids or names]	No
joints	[ids or names]	No
dry_run	bool	No

Automation details

Command ID: selection.delete

Parameters:

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

Get Selection

Parameter	Type	Required	Description
detail	bool	No	default true: resolve each item's geometry

Automation details

Command ID: selection.get

Parameters:

detail?: bool (default true: resolve each item's geometry) → {count, items: [{kind (= type: body|face|edge|vertex|feature|sketch_curve|sketch_point|sketch_midpoint|sketch_constraint|profile|plane|axis|construction_point|occurrence…), the selection's own fields as select.set takes them (body, index, point, id, sketch, path…), and with detail: face: name (persistent face name), name_exact, surface ({type: plane|cylinder|cone|sphere|torus|other, normal/point, origin/axis/radius…}), area_mm2, planar; edge: name (persistent edge name), curve (line|circle|arc|other), length_mm, start, end, center/axis/radius for round edges; body: volume_mm3, feature, visible; any body item: component {id, name} and occurrence_path in an assembly; sketch items: sketch (its id, as select.set takes it), sketch_name, entity (line|circle|arc|point|midpoint|…), position for points and midpoints}]}; read-only, [] when nothing is selected

Other commands: ui

Toggle Assistant

Default keyboard shortcut: Ctrl+Shift+A

Automation details

Command ID: ui.assistant

Parameters:

Show or hide Assistant in the app. Headless calls are refused without changing the design

Search Commands

Default keyboard shortcut: S

Automation details

Command ID: ui.palette

Parameters:

Open command search in the app. Headless calls are refused without changing the design

Show/Hide Selection

Default keyboard shortcut: V

Automation details

Command ID: ui.toggle_visibility

Parameters:

Show or hide what is selected in the app. Headless calls are refused without changing the design; browser.visibility takes explicit items

Other commands: edit

Undo

Default keyboard shortcut: Ctrl+Z

Automation details

Command ID: edit.undo

No parameter description is provided by the command registry.

Redo

Default keyboard shortcut: Ctrl+Y

Automation details

Command ID: edit.redo

No parameter description is provided by the command registry.

Repeat Last Command

Default keyboard shortcut: Shift+R

Automation details

Command ID: edit.repeat

Parameters:

Starts the last tool or dialog started in the app again, with its defaults (a toolbar click, not a replay of its values). Only the app has a tool to start: called here it is refused, and changes nothing

Checkpoint

Automation details

Command ID: edit.checkpoint

Parameters:

→ {checkpoint: id}: remember the design, active sketch and undo history (restore with edit.restore_checkpoint; the last 16 are kept, the oldest dropped first)

Restore Checkpoint

Parameter	Type	Required	Description
checkpoint	id	Yes

Automation details

Command ID: edit.restore_checkpoint

Parameters:

checkpoint: id; forget?: bool (true = drop it without going back). Goes back to it, undo history included. Restoring uses it and every later checkpoint up: take a new one to go back again. Forgetting drops only it

Other commands: timeline

Play History

Command group: INSPECT › HISTORY

Parameter	Type	Required	Description
action	toggle\|play\|stop	No	default toggle

Automation details

Command ID: timeline.play

Parameters:

action?: toggle|play|stop (default toggle) → action: validated display request; the connected UI plays from the marker to the end with a half-second pause per rebuilt step. Headless callers only validate the request; no dialog, document edit or animation clock is created

Rename

Parameter	Type	Required	Description
feature	id\|name	Yes
name		Yes	references to it follow

Automation details

Command ID: timeline.rename

Parameters:

feature: id|name, name (references to it follow)

New Feature Folder

Parameter	Type	Required	Description
name		No
features	[id\|name]	No
joints	[id\|name]	No
groups	[folder ids]	No
parent	folder id	No	features and joints leave any other timeline folder

Automation details

Command ID: timeline.group

Parameters:

name?; features?: [id|name]; joints?: [id|name]; groups?: [folder ids]; parent?: folder id (features and joints leave any other timeline folder)

Remove Feature Folders

Parameter	Type	Required	Description
group	id	Yes
groups	[ids]	Yes	features and joints remain in the timeline

Automation details

Command ID: timeline.ungroup

Parameters:

group: id | groups: [ids] (features and joints remain in the timeline)

Rename Feature Folder

Parameter	Type	Required	Description
group	id	Yes
name		Yes	renames the folder holding features and joints

Automation details

Command ID: timeline.rename_group

Parameters:

group: id, name (renames the folder holding features and joints)

Move Features to Folder

Parameter	Type	Required	Description
features	[id\|name]	No
joints	[id\|name]	No
groups	[ids]	No
group	id	No	omit or null to move to the timeline root

Automation details

Command ID: timeline.move_to_group

Parameters:

features?: [id|name], joints?: [id|name], groups?: [ids], group?: id (omit or null to move to the timeline root)

Move Timeline Items

Parameter	Type	Required	Description
features	[id\|name]	No
groups	[folder ids]	No
group	folder id	No
position	insertion slot	Yes
active	bool	No	true = the moved contents end up before the history marker, false = behind it; other features keep their state

Automation details

Command ID: timeline.move_many

Parameters:

features?: [id|name], groups?: [folder ids], group?: folder id, position: insertion slot, active?: bool (true = the moved contents end up before the history marker, false = behind it; other features keep their state); atomically changes folder membership and moves all selected contents as one block

Move Timeline Marker

Automation details

Command ID: timeline.rollback

Parameters:

position: number of features to keep active, or "end" (omit = end)

Roll History Marker

Automation details

Command ID: timeline.roll_to

Parameters:

position: number of features to keep active, or "end" (omit = end) | feature: id|name (the marker goes right after it)

Reorder Feature

Parameter	Type	Required	Description
feature	id\|name	Yes
position	its new index	Yes
active	bool	No	true = it ends up before the history marker, false = behind it; other features keep their state

Automation details

Command ID: timeline.reorder

Parameters:

feature: id|name, position: its new index, active?: bool (true = it ends up before the history marker, false = behind it; other features keep their state); refused when a feature that worked would fail, unless allow_errors?: bool (default false): then made, and broken: [{feature, error}] lists the features it broke → feature, position: its index now, from: its index before, moved: bool, note?: why nothing moved, or that a position past the end meant the last slot

Reorder Features

Parameter	Type	Required	Description
features	[id\|name]	Yes
position	insertion slot in the current history	Yes
active	bool	No	as timeline.reorder's

Automation details

Command ID: timeline.reorder_many

Parameters:

features: [id|name], position: insertion slot in the current history; selected features keep their relative order; active?: bool (as timeline.reorder's); refused when a feature that worked would fail, unless allow_errors?: bool (default false): then made, and broken: [{feature, error}] lists the features it broke

Edit Feature

Parameter	Type	Required	Description
feature	id\|name	Yes
command	the feature's command id	Yes
params	its parameters	Yes	the feature is rebuilt in place

Automation details

Command ID: timeline.redefine

Parameters:

feature: id|name, command: the feature's command id, params: its parameters (the feature is rebuilt in place) → feature, recomputed, restored, rolled_back: bool (the feature is after the history marker, so the edit is not built yet; `note` then says so), warning?

Feature Dependents

Parameter	Type	Required	Description
feature	id\|name	Yes

Automation details

Command ID: timeline.dependents

Parameters:

feature: id|name → features deleted with it, and features that would fail without it

Suppress Feature

Parameter	Type	Required	Description
feature	id\|name	Yes
features	[id\|name]	Yes
groups	[timeline folder ids]	Yes	every feature and joint in those folders and their nested folders; one undo step
suppressed	bool	No	default toggles: features and joints are all suppressed unless all of them already are, then all are unsuppressed

Automation details

Command ID: timeline.suppress

Parameters:

feature: id|name | features: [id|name] | groups: [timeline folder ids] (every feature and joint in those folders and their nested folders; one undo step), suppressed?: bool (default toggles: features and joints are all suppressed unless all of them already are, then all are unsuppressed) → feature: id (or features: [ids]; groups: [ids] and joints: [ids] when groups are given), suppressed

Edit Feature

Parameter	Type	Required	Description
feature	id\|name	Yes
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); a dotted key names a nested field ({"plane.distance": "8 mm"} = {"plane": {"distance": "8 mm"}}); expressions are text, or a number in mm or degrees}	Yes

Automation details

Command ID: timeline.edit

Parameters:

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); a dotted key names a nested field ({"plane.distance": "8 mm"} = {"plane": {"distance": "8 mm"}}); expressions are text, or a number in mm or degrees} → recomputed: features rebuilt, restored: features whose earlier result for the same inputs was reused

Inspect Feature

Parameter	Type	Required	Description
group	folder id	Yes

Automation details

Command ID: timeline.inspect

Parameters:

group: folder id → group, name, parent, features, joints; or 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

Copy Features

Parameter	Type	Required	Description
features	[ids or names]	Yes	in timeline order on paste

Automation details

Command ID: timeline.copy

Parameters:

features: [ids or names] (in timeline order on paste)

Paste Features

Parameter	Type	Required	Description
translate	[x,y,z]	No	moves the copies' geometry
component	where the copies go	No	default: the active one
component_path	its placement	No	default: the active one, else its only one
from_design	true to paste sketch features from the host's cross-design clipboard snapshot	No

Automation details

Command ID: timeline.paste

Parameters:

translate?: [x,y,z] (moves the copies' geometry); component?: where the copies go (default: the active one), component_path?: its placement (default: the active one, else its only one); the copies go at the marker, each where its original is in the world (copies into their own component keep its coordinates); body transfers are left out; from_design?: true to paste sketch features from the host's cross-design clipboard snapshot

Add Recorded Feature

Parameter	Type	Required	Description
feature	a feature as the design file and timeline.inspect hold it	Yes	{type, name?, id?, …}; the name is kept even when another feature has it, the id is kept and refused when another feature has it, so later steps can refer to them
params	[{name, expression, unit?, comment?}]	No	the model parameters its sketch dimensions use

Automation details

Command ID: timeline.add

Parameters:

feature: a feature as the design file and timeline.inspect hold it ({type, name?, id?, …}; the name is kept even when another feature has it, the id is kept and refused when another feature has it, 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

Export Command Script

Parameter	Type	Required	Description
path	write the script to this file	No

Automation details

Command ID: timeline.export_script

Parameters:

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, print-face assignments); components and assemblies are not supported yet

Other commands: select

Select

Read the window tour.

Parameter	Type	Required	Description
items	[{type: body\|edge\|face\|feature\|sketch_curve\|sketch_point\|profile, …}]	Yes
add	bool	No

Automation details

Command ID: select.set

Parameters:

items: [{type: body|edge|face|feature|sketch_curve|sketch_point|profile, …}], add?: bool; face/edge: body plus point [x,y,z] in world mm or index (both also accepted); a point uses Measure's pick tolerance, an index supplies a point on the item; invalid partial picks leave the selection unchanged

Selection filter

Read the window tour.

Parameter	Type	Required	Description
mode	body\|face\|component	Yes

Automation details

Command ID: select.filter

Parameters:

mode: body|face|component → validated UI pick granularity; headless echo only, no document edits or undo

Clear Selection

Read the window tour.

Automation details

Command ID: select.clear

No parameter description is provided by the command registry.

Select Same Look

Read the window tour.

Parameter	Type	Required	Description
body	world body name	No
face	face index	No

Automation details

Command ID: select.same_look

Parameters:

body?: world body name, face?: face index; defaults to the current body/face selection → selects objects using the resolved appearance

Other commands: parameters

List Parameters

Parameter	Type	Required	Description
favorites	bool	No	only favourites
filter	all\|user\|sketch\|feature\|favorites	No

Automation details

Command ID: parameters.list

Parameters:

favorites?: bool (only favourites), filter?: all|user|sketch|feature|favorites → parameters (name, expression, unit, value (mm/deg in every reply), display_value (in its own unit), source, feature/input, comment, favorite, uses, used_by, error) and cycles

Add User Parameter

Parameter	Type	Required	Description
name		Yes
expression		Yes
unit	as parameters.change	No	text: a text parameter, its expression the text
comment		No
favorite	bool	No

Automation details

Command ID: parameters.add

Parameters:

name, expression, unit?: as parameters.change (text: a text parameter, its expression the text), comment?, favorite?: bool

Rename Parameter

Parameter	Type	Required	Description
name		Yes
new_name		Yes	expressions, feature inputs and dimensions that use it follow

Automation details

Command ID: parameters.rename

Parameters:

name, new_name (expressions, feature inputs and dimensions that use it follow)

Delete Parameter

Parameter	Type	Required	Description
name		Yes	refused while something uses it; the error lists the users

Automation details

Command ID: parameters.delete

Parameters:

name (refused while something uses it; the error lists the users)

Favorite Parameter

Parameter	Type	Required	Description
name	bool	Yes
favorite	bool	No	default true

Automation details

Command ID: parameters.favorite

Parameters:

name, favorite?: bool (default true)

Move Parameter

Parameter	Type	Required
name	another user parameter	Yes
before	another user parameter	Yes
after	another user parameter	Yes

Automation details

Command ID: parameters.move

Parameters:

name, before | after: another user parameter; the user parameter is listed just before or after it

Comment Parameter

Parameter	Type	Required	Description
name		Yes
comment		Yes

Automation details

Command ID: parameters.comment

Parameters:

name, comment

Parameter Users

Parameter	Type	Required	Description
name		Yes

Automation details

Command ID: parameters.users

Parameters:

name → users (parameters, feature inputs, dimensions) and the features it drives

Parameter Graph

Automation details

Command ID: parameters.graph

Parameters:

→ nodes, edges [user, used] (users include Feature:<name>), cycles, errors

Export Parameters

Parameter	Type	Required	Description
format	csv\|json	No	default csv, or from the path
path	write to a file	No

Automation details

Command ID: parameters.export

Parameters:

format?: csv|json (default csv, or from the path), path?: write to a file → text

Import Parameters

Parameter	Type	Required	Description
text	CSV	Yes	header with name, expression, unit?, comment?

Automation details

Command ID: parameters.import

Parameters:

text: CSV (header with name, expression, unit?, comment?) or JSON [{name, expression, unit?, comment?}] | path; all or nothing

Complete Expression

Parameter	Type	Required	Description
prefix	the text before the cursor	No

Automation details

Command ID: parameters.complete

Parameters:

prefix?: the text before the cursor → word, suggestions [{text, kind: parameter|function|unit|constant, detail}]

Other commands: expr

Evaluate Expression