NOWN-DEV
d0a4443939
New command inspect.compare {a, b, tolerance?}: measures of both and their differences, two-way surface deviation from a bounding-volume tree, regions beyond the tolerance clustered by side (only_in_a / only_in_b) with integrated volumes and faces, a verdict, optional face colouring as one undo step, and warnings for open meshes. Geometry in solidcraft-geom (compare.rs), command in the engine. Closes #1363.
222 lines
16 KiB
Markdown
222 lines
16 KiB
Markdown
# Solid features
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Features live on the **timeline** and rebuild incrementally from the first one that changed.
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Each one can be edited (double-click), suppressed, renamed, reordered (if nothing it depends on
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moves after it), rolled back to, and deleted. Deleting asks first when other features depend on
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it.
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| Panel | Features |
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| Create | extrude (one side, two sides, symmetric, taper, start offset, to a distance or through all; new body, join, cut, intersect; thin walls along curves), revolve, sweep, loft, box, cylinder, sphere, torus, coil, pipe, rib, web, emboss, hole (simple, counterbore, countersink, tapped; on faces or at sketch points), thread, rectangular/circular/path patterns, mirror |
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| Modify | press pull, fillet, chamfer, shell, draft, scale, combine, split body, offset face, replace face, move/copy, align, remove |
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| Construct | offset plane, plane at angle, plane along path |
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| Inspect | measure, section analysis, interference, compare bodies, curvature comb and map, zebra, draft, minimum radius, isocurves, centre of mass |
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Extrude automatically selects **Join** for additions when the active component already has a
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solid, including sideways elbow connections and screw bosses that meet only part of a face.
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Extruding into existing material selects **Cut**. In an empty component it selects **New Body**;
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choose **New Body** explicitly to keep an addition separate. Changing the default does not alter
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operations already saved in a design.
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A taper slopes the sides of any profile, sketch text included: lines, arcs and spline or conic
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curves move in or out together, and a flat tip shorter than the taper closes to a point. On
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spline and conic sides the slope is approximate: the moved outline is a curve of the same kind
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within 2 % of the taper's offset (or 10 µm) of the true one, a curve that turns too much for
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that being cut into pieces first; where a curve bends tighter than the offset, the offset folds
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and is smoothed over. A taper steeper than the profile's details (a stroke, a curve or a gap
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narrower than it) is refused with that reason; a smaller taper or distance builds.
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**Thin Extrude** (`thin: true` on `solid.extrude`, the Thin Extrude box in its dialog) builds a
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wall of constant thickness along sketch curves instead of filling profiles: open chains (a single
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wall) and closed loops (a ring), lines, arcs, circles, ellipses and splines. In the dialog, a
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picked profile stands for the curves around it (its outline and its holes). The wall lies on the curves' centre, inside,
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outside, or on both sides with two thicknesses (`side`: `center`, `inside`, `outside`,
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`two_sides` with `thickness2`). A closed loop's inside is the area it encloses; an open chain's
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is the side it bends toward (the inside of a U), and a straight line's is the left of its first
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curve as drawn. Curves that meet end to end are one chain whose corners are mitred; walls that
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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
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for walls of straight lines or of whole circles. A wall thicker than the
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radius of a curve it follows on the inside is refused. Spline walls follow the exact offset
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within 0.0001 mm.
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Editing an extrusion retains its signed distances, From/To Object inputs, taper expressions
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and explicit body targets. Revolve edits retain world, sketch and explicit-line axes, both
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angle expressions and To Object targets. An unchanged **All profiles** selection continues
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to include profiles added later. Cancel restores the complete timeline; a successful edit is
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one undo step, including downstream parameter changes. Editing a placed component previews the
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edited feature before its downstream history. Cylindrical Emboss profile guides follow the
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sketch's chosen occurrence frame.
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Newly selected adaptive profiles store complete outer and hole source identities when the
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entire boundary can be qualified. Changing an ellipse or periodic offset after extrusion can
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then change its spline span count while keeping the same selected material region. A partial,
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intersected or ambiguous boundary cannot satisfy that whole-source reference; changing the
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hole identities also makes it lost. Older curve-span selections retain their exact stored
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multisets. If an older feature has already lost its profile after subdivision changed, edit
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the feature and reselect the intended current region to capture the new identity.
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New symmetric solid extrusions treat the entered distance as the total thickness and split it evenly
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around the start plane: 10 mm spans -5 to +5 mm on an XY sketch. Switching from One Side to
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Symmetric keeps the entered total thickness. Through All still reaches targets in both
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directions, and Two Sides retains its independent distances. Symmetric extrusions saved before
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this change keep their original per-side distances when reopened or edited. Selecting another direction
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in the feature editor uses the current total-distance convention.
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New symmetric revolves split the entered angle evenly around the sketch profile, regardless
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of which way the selected axis points. Two Sides measures the second angle backward and the
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first angle forward along the sketch-normal sweep direction. Profiles on opposite sides of
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an axis each use their own sweep direction. Designs saved before format 11 keep their original
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angular placement when opened, edited or copied; creating another revolve uses the new behavior.
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To Object follows that same direction for each selected profile, including curved target faces.
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Pick a target away from the axis so its angular position is defined.
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For cylindrical **Emboss**, select a supported exterior cylinder face and a tangent sketch
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profile. **Deboss** cuts radially into the wall. Orthogonal line profiles, including holes and
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concave outlines, wrap with exact radial walls; the profile must stay clear of seams and ends.
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Complete cylinders and coaxial sleeves are supported. Capture pending component positions
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before applying. The feature stores the selected target and author occurrence paths, so edits
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and reopening retain the chosen instances. Other curved surfaces and free-form profiles remain
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unsupported. A new Emboss without an explicit face infers a unique eligible supported cylinder;
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select the face when the target is ambiguous. Older saved features without a face retain their
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planar placement.
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A **Hole** with **Single** placement drills where you pick a planar face. A pick on or near a
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point of a shown sketch that lies on that face, such as a circle's centre, places the hole
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exactly at that point, as **Multiple** placement picks it; **Select Other** (press and hold) also
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offers the face where you clicked. The corners of text outlines don't count, nor do projected
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points while the sketch hides projected geometry. The hole keeps that place on the face; to have
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holes follow later edits of the sketch, place them with **Multiple**.
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Fillets and chamfers handle straight edges between planar faces, whole smooth loops, runs of
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neighbouring edges with mitred or spherical corners, and closed chains of curved edges (a rolling
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ball). See the roadmap's known limitations for the rest.
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**Curvature (G2)** in the Fillet dialog's **Radius Type** blends straight edges between two
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planar faces with an exact quintic section. The tangent plane and curvature match each side
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face: curvature goes to zero at both contact rails, unlike a circular G1 fillet. Each end
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must meet one planar face perpendicular to the edge. Curved edges/faces, sloped or multi-face
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ends, and intersecting corner blends are not supported; they return an error, not a G1 fallback.
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**Equivalent Radius** sets the same contact setback as a circular fillet (for a right angle,
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setback equals the entered value); it is not a constant curvature radius. Reduce/Taper to Fit
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are unavailable for this type.
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Scripts and MCP use the same command, for example on a 20 mm box:
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```json
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{"command": "solid.fillet", "params": {"edges": [[20, 0, 10]], "radius": 2, "type": "curvature"}}
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```
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`type: "g2"` is an alias. Existing fillets still default to circular, constant-radius G1 blends.
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Feature references to faces and edges are stored by name, so an upstream edit that moves geometry
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keeps them on the right face (see [Persistent naming](../dev/naming.md)). When a reference can't
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be found, the feature warns instead of silently picking another face.
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**Plane Along Path** accepts one sketch curve (including a drawn 3D wire) or model edge.
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Pick the path in the viewport and enter **Position (0 to 1)**: 0 starts the path, 1 ends it,
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and 0.5 places the plane halfway along its length. The plane is perpendicular to the path's
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local segment. Preview does not change the design; OK creates one editable timeline feature.
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The plane follows later path edits. Curved paths use their sampled polyline; absolute distance,
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reference-object placement and multi-curve chains are not yet available in this dialog.
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## Comparing two bodies
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**Compare Bodies** (`inspect.compare`) lays two versions of one part over each other, such as a
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part and the same part exported by another program, and finds the places where only one of them
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has material. It works from the two surfaces, not from a boolean of the bodies, so it also
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compares bodies that share almost every face, the case a boolean (Combine, Interference) handles
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worst.
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```json
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{"command": "inspect.compare", "params": {"a": "Bracket", "b": "Bracket (2)", "tolerance": 0.01, "color": true}}
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```
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Without `a` and `b` it compares the two selected bodies, or the design's only two. Both bodies
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are measured (volume, area, centre of mass and box, and `difference`: b − a of each). Each
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surface is sampled at the corners of its triangles and at points at most `spacing` (0.5 mm)
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apart on larger faces, and every sample measures its distance to the other surface: `deviation`
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gives the largest and the mean distance each way. Samples further than `tolerance` (0.01 mm) form
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the **regions**: `only_in_a` where `a` has material and `b` has none, `only_in_b` the other way
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round. Each region gives its volume, the deviating surface area, the largest deviation and where
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it is, its centre and box, and the faces of each body it lies on (`faces_a`, `faces_b`, numbered
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as `model.faces` lists them), largest volume first. The volume is integrated along a grid of
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parallel lines through the region (`resolution` gives their spacing), so a thin sliver is
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measured as well as a block. `identical` is true when no region is found, and `verdict` says it in
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one line. `warnings` lists what makes the result less certain: a body whose surface does not
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enclose the volume it measures (open, or with faces that failed to import), and lines left out of
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a region's volume because they crossed a gap. With `color`, the faces that hold a region turn
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red where only `a` has material and green where only `b` has, on both bodies: the faces mostly
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beyond the tolerance (a small change on a large face leaves the face alone), or, for a region
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with none, the face with the largest share.
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That is one undo step; without `color` the command changes nothing.
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The bodies are meshed within a quarter of the tolerance. The kernel meshes no finer than a
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millionth of a body's size, so keep the tolerance at least twice that (0.02 mm for a part 10 m
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across). Large bodies are sampled more coarsely, at about `max_points` (eight million) points
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each; `sampling.spacing_mm` says what was used, and a larger `max_points` (up to 50 million)
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samples them finer, at the cost of time.
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## Editing a feature from a script
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For `solid.pattern.circular`, `axis` accepts `X`, `Y`, `Z`, or `{origin, dir}`.
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An explicit origin must contain three finite numeric coordinates in millimetres
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(`[x, y, z]` or `{x, y, z}`); omitting it uses the world origin. Expressions and
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construction-axis references are not supported. Invalid origins are rejected rather than
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silently replaced with zero.
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`timeline.inspect {feature}` returns a feature's `definition`: the fields `timeline.edit` changes,
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with their current values. `timeline.edit {feature, set}` merges `set` into that definition
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(objects are merged field by field, anything else replaces the value), rebuilds the feature and
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reports `recomputed` and `restored`. The feature's type cannot change, and sketch geometry is
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edited with the sketch commands. Expressions are text (`"30"`, `"30 mm"`, `"width / 2"`,
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`"45 deg"`); a bare number is a length in the design's units, or degrees for an angle.
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```json
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{"command": "timeline.inspect", "params": {"feature": "Slab"}}
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→ {"type": "ExtrudeFeature",
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"definition": {"sketch": 1, "profiles": {"type": "all"}, "operation": "new_body",
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"extent": {"distance": "10", "direction": "positive"}},
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"inputs": [{"label": "Distance", "param": "d1", "expression": "10", "unit": "mm"}], …}
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{"command": "timeline.edit", "params": {"feature": "Slab", "set": {"extent": {"distance": "12"}}}}
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```
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`inputs` lists the feature's named inputs. `parameters.change {name: "d1", expression}` sets one
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of those directly. Optional fields that are not set do not appear in the definition; they can
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still be added through `set`. The fields of the common features:
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| Feature | Fields |
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| Extrude | `extent`: {`distance`, `direction`: positive\|negative\|symmetric, `distance2`, `start_offset`, `through_all`, `taper`, `to`, `to_offset`, `from`}; `operation`: new_body\|join\|cut\|intersect; `targets`; `profiles`; `sketch`; `thin`: {`curves`, `thickness`, `side`: center\|inside\|outside\|two_sides, `thickness2`} |
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| Revolve | `angle`, `angle2`, `symmetric`, `axis`, `to`, `operation`, `targets`, `profiles`, `sketch` |
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| Fillet | `radius`, `edges` (a point on each edge), `body`, `style` |
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| Chamfer | `distance`, `distance2` or `angle`, `flip`, `edges`, `body` |
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| Box | `length`, `width`, `height`, `corner`, `operation` |
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| Cylinder | `radius`, `height`, `base`, `axis`, `operation` |
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| Hole | `diameter`, `depth`, `position`, `direction`, `hole` (simple, drilled, counterbore, countersink), `thread`, `to` |
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| Shell | `thickness`, `faces`, `direction`, `body`, `tangent_chain` |
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| Draft | `angle`, `faces`, `neutral`, `pull`, `body` |
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| Offset face | `distance`, `faces`, `body` |
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| Pattern | `pattern` (its kind and counts/spacing), `features`, `bodies` |
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| Mirror | `plane`, `features`, `bodies`, `combine` |
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For any other feature, `timeline.inspect` shows the fields.
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Where a command takes a face as a point (`face.delete`, `solid.shell`, `solid.draft`,
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`solid.offset_face`, `solid.split_face`, the `faces` of `solid.replace_face`, and the `face` of
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`sheet.convert`), a script can give the face's name instead, as `model.faces` lists it:
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`{"command": "face.delete", "params": {"faces": ["F2:side#1", "F2:side#2"], "body": "Plate"}}`.
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`model.faces` also lists a `point` on each face that picks it (the centroid of a face with a hole
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in it is in the hole, that of a half cylinder inside the cylinder) and, for a cylindrical face,
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its `cylinder`: `origin` and `axis` of its axis, and `radius`. A name that is more than one face
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(the pieces of a split face, or one face of several bodies) is refused; `body` says which body to
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look on.
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Press **Delete** on anything selected (bodies, faces, sketches, features, planes, components,
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canvases). It runs as one undoable step and lists the features that would go with it or fail.
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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.
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Negative Press Pull across supported aligned prismatic faces retains round through-holes,
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including after a joined extrusion and in a rotated component occurrence. The cut partitions
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the current material into axial sections, preserving the hole through undo, redo, and reopen.
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Walls that cannot be qualified as a parallel extrusion still use the general Boolean path
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and may report an unsupported coincident-surface operation atomically.
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