Solid features

Features live on the timeline and rebuild incrementally from the first one that changed. Each one can be edited (double-click), suppressed, renamed, reordered (if nothing it depends on moves after it), rolled back to, and deleted. Deleting asks first when other features depend on it.

Extrude automatically selects Join for additions when the active component already has a solid, including sideways elbow connections and screw bosses that meet only part of a face. Extruding into existing material selects Cut. In an empty component it selects New Body; choose New Body explicitly to keep an addition separate. Changing the default does not alter operations already saved in a design.

A taper slopes the sides of any profile, sketch text included: lines, arcs and spline or conic curves move in or out together, and a flat tip shorter than the taper closes to a point. On spline and conic sides the slope is approximate: the moved outline is a curve of the same kind within 2 % of the taper’s offset (or 10 µm) of the true one, a curve that turns too much for that being cut into pieces first; where a curve bends tighter than the offset, the offset folds and is smoothed over. A taper steeper than the profile’s details (a stroke, a curve or a gap narrower than it) is refused with that reason; a smaller taper or distance builds.

Thin Extrude (thin: true on solid.extrude, the Thin Extrude box in its dialog) builds a wall of constant thickness along sketch curves instead of filling profiles: open chains (a single wall) and closed loops (a ring), lines, arcs, circles, ellipses and splines. In the dialog, a picked profile stands for the curves around it (its outline and its holes). The wall lies on the curves’ centre, inside, outside, or on both sides with two thicknesses (side: center, inside, outside, two_sides with thickness2). A closed loop’s inside is the area it encloses; an open chain’s is the side it bends toward (the inside of a U), and a straight line’s is the left of its first curve as drawn. Curves that meet end to end are one chain whose corners are mitred; walls that cross or meet (a ring and a cross, a honeycomb) become one piece. Every extent, operation and target of an extrude applies, and a taper for walls of straight lines or of whole circles. A wall thicker than the radius of a curve it follows on the inside is refused. Spline walls follow the exact offset within 0.0001 mm.

Editing an extrusion retains its signed distances, From/To Object inputs, taper expressions and explicit body targets. Revolve edits retain world, sketch and explicit-line axes, both angle expressions and To Object targets. An unchanged All profiles selection continues to include profiles added later. Cancel restores the complete timeline; a successful edit is one undo step, including downstream parameter changes. Editing a placed component previews the edited feature before its downstream history. Cylindrical Emboss profile guides follow the sketch’s chosen occurrence frame.

Newly selected adaptive profiles store complete outer and hole source identities when the entire boundary can be qualified. Changing an ellipse or periodic offset after extrusion can then change its spline span count while keeping the same selected material region. A partial, intersected or ambiguous boundary cannot satisfy that whole-source reference; changing the hole identities also makes it lost. Older curve-span selections retain their exact stored multisets. If an older feature has already lost its profile after subdivision changed, edit the feature and reselect the intended current region to capture the new identity.

New symmetric solid extrusions treat the entered distance as the total thickness and split it evenly around the start plane: 10 mm spans -5 to +5 mm on an XY sketch. Switching from One Side to Symmetric keeps the entered total thickness. Through All still reaches targets in both directions, and Two Sides retains its independent distances. Symmetric extrusions saved before this change keep their original per-side distances when reopened or edited. Selecting another direction in the feature editor uses the current total-distance convention.

New symmetric revolves split the entered angle evenly around the sketch profile, regardless of which way the selected axis points. Two Sides measures the second angle backward and the first angle forward along the sketch-normal sweep direction. Profiles on opposite sides of an axis each use their own sweep direction. Designs saved before format 11 keep their original angular placement when opened, edited or copied; creating another revolve uses the new behavior. To Object follows that same direction for each selected profile, including curved target faces. Pick a target away from the axis so its angular position is defined.

For cylindrical Emboss, select a supported exterior cylinder face and a tangent sketch profile. Deboss cuts radially into the wall. Orthogonal line profiles, including holes and concave outlines, wrap with exact radial walls; the profile must stay clear of seams and ends. Complete cylinders and coaxial sleeves are supported. Capture pending component positions before applying. The feature stores the selected target and author occurrence paths, so edits and reopening retain the chosen instances. Other curved surfaces and free-form profiles remain unsupported. A new Emboss without an explicit face infers a unique eligible supported cylinder; select the face when the target is ambiguous. Older saved features without a face retain their planar placement.

A Hole with Single placement drills where you pick a planar face. A pick on or near a point of a shown sketch that lies on that face, such as a circle’s centre, places the hole exactly at that point, as Multiple placement picks it; Select Other (press and hold) also offers the face where you clicked. The corners of text outlines don’t count, nor do projected points while the sketch hides projected geometry. The hole keeps that place on the face; to have holes follow later edits of the sketch, place them with Multiple.

Fillets and chamfers handle straight edges between planar faces, whole smooth loops, runs of neighbouring edges with mitred or spherical corners, and closed chains of curved edges (a rolling ball). See the roadmap’s known limitations for the rest.

Curvature (G2) in the Fillet dialog’s Radius Type blends straight edges between two planar faces with an exact quintic section. The tangent plane and curvature match each side face: curvature goes to zero at both contact rails, unlike a circular G1 fillet. Each end must meet one planar face perpendicular to the edge. Curved edges/faces, sloped or multi-face ends, and intersecting corner blends are not supported; they return an error, not a G1 fallback. Equivalent Radius sets the same contact setback as a circular fillet (for a right angle, setback equals the entered value); it is not a constant curvature radius. Reduce/Taper to Fit are unavailable for this type.

Scripts and MCP use the same command, for example on a 20 mm box:

{"command": "solid.fillet", "params": {"edges": [[20, 0, 10]], "radius": 2, "type": "curvature"}}

type: "g2" is an alias. Existing fillets still default to circular, constant-radius G1 blends.

Feature references to faces and edges are stored by name, so an upstream edit that moves geometry keeps them on the right face (see Persistent naming). When a reference can’t be found, the feature warns instead of silently picking another face.

Plane Along Path accepts one sketch curve (including a drawn 3D wire) or model edge. Pick the path in the viewport and enter Position (0 to 1): 0 starts the path, 1 ends it, and 0.5 places the plane halfway along its length. The plane is perpendicular to the path’s local segment. Preview does not change the design; OK creates one editable timeline feature. The plane follows later path edits. Curved paths use their sampled polyline; absolute distance, reference-object placement and multi-curve chains are not yet available in this dialog.

Comparing two bodies

Compare Bodies (inspect.compare) lays two versions of one part over each other, such as a part and the same part exported by another program, and finds the places where only one of them has material. It works from the two surfaces, not from a boolean of the bodies, so it also compares bodies that share almost every face, the case a boolean (Combine, Interference) handles worst.

{"command": "inspect.compare", "params": {"a": "Bracket", "b": "Bracket (2)", "tolerance": 0.01, "color": true}}

Without a and b it compares the two selected bodies, or the design’s only two. Both bodies are measured (volume, area, centre of mass and box, and difference: b − a of each). Each surface is sampled at the corners of its triangles and at points at most spacing (0.5 mm) apart on larger faces, and every sample measures its distance to the other surface: deviation gives the largest and the mean distance each way. Samples further than tolerance (0.01 mm) form the regions: only_in_a where a has material and b has none, only_in_b the other way round. Each region gives its volume, the deviating surface area, the largest deviation and where it is, its centre and box, and the faces of each body it lies on (faces_a, faces_b, numbered as model.faces lists them), largest volume first. The volume is integrated along a grid of parallel lines through the region (resolution gives their spacing), so a thin sliver is measured as well as a block. identical is true when no region is found, and verdict says it in one line. warnings lists what makes the result less certain: a body whose surface does not enclose the volume it measures (open, or with faces that failed to import), and lines left out of a region’s volume because they crossed a gap. With color, the faces that hold a region turn red where only a has material and green where only b has, on both bodies: the faces mostly beyond the tolerance (a small change on a large face leaves the face alone), or, for a region with none, the face with the largest share. That is one undo step; without color the command changes nothing.

The bodies are meshed within a quarter of the tolerance. The kernel meshes no finer than a millionth of a body’s size, so keep the tolerance at least twice that (0.02 mm for a part 10 m across). Large bodies are sampled more coarsely, at about max_points (eight million) points each; sampling.spacing_mm says what was used, and a larger max_points (up to 50 million) samples them finer, at the cost of time.

Editing a feature from a script

For solid.pattern.circular, axis accepts X, Y, Z, or {origin, dir}. An explicit origin must contain three finite numeric coordinates in millimetres ([x, y, z] or {x, y, z}); omitting it uses the world origin. Expressions and construction-axis references are not supported. Invalid origins are rejected rather than silently replaced with zero.

timeline.inspect {feature} returns a feature’s definition: the fields timeline.edit changes, with their current values. timeline.edit {feature, set} merges set into that definition (objects are merged field by field, anything else replaces the value), rebuilds the feature and reports recomputed and restored. The feature’s type cannot change, and sketch geometry is edited with the sketch commands. Expressions are text ("30", "30 mm", "width / 2", "45 deg"); a bare number is a length in the design’s units, or degrees for an angle.

{"command": "timeline.inspect", "params": {"feature": "Slab"}}
→ {"type": "ExtrudeFeature",
   "definition": {"sketch": 1, "profiles": {"type": "all"}, "operation": "new_body",
                  "extent": {"distance": "10", "direction": "positive"}},
   "inputs": [{"label": "Distance", "param": "d1", "expression": "10", "unit": "mm"}], …}
{"command": "timeline.edit", "params": {"feature": "Slab", "set": {"extent": {"distance": "12"}}}}

inputs lists the feature’s named inputs. parameters.change {name: "d1", expression} sets one of those directly. Optional fields that are not set do not appear in the definition; they can still be added through set. The fields of the common features:

For any other feature, timeline.inspect shows the fields.

Where a command takes a face as a point (face.delete, solid.shell, solid.draft, solid.offset_face, solid.split_face, the faces of solid.replace_face, and the face of sheet.convert), a script can give the face’s name instead, as model.faces lists it: {"command": "face.delete", "params": {"faces": ["F2:side#1", "F2:side#2"], "body": "Plate"}}. model.faces also lists a point on each face that picks it (the centroid of a face with a hole in it is in the hole, that of a half cylinder inside the cylinder) and, for a cylindrical face, its cylinder: origin and axis of its axis, and radius. A name that is more than one face (the pieces of a split face, or one face of several bodies) is refused; body says which body to look on.

Press Delete on anything selected (bodies, faces, sketches, features, planes, components, canvases). It runs as one undoable step and lists the features that would go with it or fail.

Face Extrude, face Revolve, and Press Pull retain linked generated profiles. When a modified planar face has no construction certificate, these internal profiles use the legacy named-face attachment and projection behavior so upstream edits still update the plane and outline. This compatibility path is private to those modeling tools: newly attached user sketches require a certified face or an explicitly fixed plane. Legacy internal attachments can follow the nearest matching face after topology changes; inspect their result after major upstream edits. Activate the intended occurrence before generating a face profile from a repeated component; capture a separately moved source position before creating a legacy profile across components.

Negative Press Pull across supported aligned prismatic faces retains round through-holes, including after a joined extrusion and in a rotated component occurrence. The cut partitions the current material into axial sections, preserving the hole through undo, redo, and reopen. Walls that cannot be qualified as a parallel extrusion still use the general Boolean path and may report an unsupported coincident-surface operation atomically.