Tommaso Bianchi
2b02a8e3dd
Review request on PR #15238: "Place CAD-related files (e.g. CadDocument/ GeometryEngine) into a separate folder." src/libslic3r/CAD/ the kernel — CadDocument, GeometryEngine, the four Sketch* units, SketchSolver, ThreadStandards src/slic3r/GUI/CAD/ the tab — DesignPanel, DesignCanvas, DesignSketchTool, SketchInlineEditor, McpControl, generated DesignOffer Pure relocation: no line of logic changes. Two include rewrites follow from it — files that moved re-spell their own neighbours against src/ (already on the include path), and files that did not move pick up the new folder. docs and docs/ux/mockups/gen_offer_table.py follow the same paths. Verified: libslic3r, libslic3r_gui and libslic3r_tests all build, CAD suite green at 2518 assertions in 194 test cases, and the sibling fork builds identically — 17 shared sources still byte-identical, 8 diverging by their expected counts.
8.9 KiB
SnapOrca-CAD vs Onshape — capability gap analysis
Generated 2026-07-22 by enumerating the source, not from recollection:
CadFeatureType and add_* in src/libslic3r/CAD/CadDocument.hpp, Tool in
src/slic3r/GUI/CAD/DesignPanel.hpp, Mode in src/slic3r/GUI/CAD/DesignSketchTool.hpp,
SketchConstraintType + SketchEntity::Type in src/libslic3r/CAD/SketchEngine.hpp,
and the JSON-RPC dispatch in src/slic3r/GUI/CAD/McpControl.cpp.
Scope note. Onshape is a cloud PLM platform; SnapOrca is a Design tab inside a slicer. A large share of Onshape's surface (release management, branching, real-time collaboration, FEA, rendering, PDM) is out of scope by construction and is listed separately at the bottom rather than counted as a "missing tool".
1. What SnapOrca already has
2D sketcher — near parity with Onshape
This is the strongest area. Very little is missing.
| Category | SnapOrca |
|---|---|
| Entities | Line, Polyline, Arc (3-point / tangent / center), Circle (center / 2-point / 3-point), Point, Ellipse, Elliptical arc, B-spline |
| Shapes | Rectangle (corner / center / oblique / rounded), Slot, Arc-slot, Polygon |
| Edit ops | Fillet, Chamfer, Offset, Mirror, Trim, Extend |
| Transforms | Move, Rotate, Scale, Linear array, Polar array |
| Constraints (19) | Fix, Coincident, Horizontal, Vertical, Distance, LockX, LockY, EqualLength, Parallel, Perpendicular, Concentric, Tangent, Midpoint, Symmetric, Angle, Radius, Diameter, PointOnLine, PointOnObject |
| Dimensions | Length, Diameter, Radius, Angle, Distance, Distance-to-line |
Solver: vendored SolveSpace (libslvs, GPL-3.0) — the same solver lineage as a
commercial-grade sketcher.
Part features
| Present | Notes |
|---|---|
| Extrude | + up-to-face / up-to-point, taper, flip |
| Revolve | angle-arc gizmo |
| Sweep | along a path |
| Loft | multi-profile |
| Fillet / Chamfer | edge-level |
| Draft | face taper |
| Shell | wall thickness + open face |
| Hole / Thread | face-aware placement |
| Pattern | linear + circular |
| Boolean | New / Add / Cut / Intersect, with face-mating |
| Cut | plane-based, signed offset |
| Datum plane | offset / 2-face / 2-edge derived |
| Import | STEP (B-rep) + mesh→B-rep (native mesh2step port) |
| Export | STEP (native B-rep, not tessellated) |
| Multi-body | + per-body colour |
| Section view | with flip |
| Undo/redo | full feature-tree recompute |
| 3MF persistence | parametric recipe survives save/load |
Automation
9 MCP JSON-RPC methods: describe_tools, describe_scene, query_topology,
measure, slice_body, import_step, import_mesh, validate_against, plus
build actions extrude, revolve, fillet, chamfer, hole, boolean, pattern.
Onshape's equivalent is its REST API + FeatureScript.
2. Missing tools — ranked by impact
Tier 1 — structural absences (whole subsystems)
1. Assemblies and mates. Entirely absent. No assembly document, no mate
connectors, no fastened / revolute / slider / cylindrical / planar / ball / pin-slot
mates, no assembly patterns, no interference detection, no exploded views.
bool_target_face / bool_tool_face do face-to-face mating for a boolean, which
is geometric alignment, not a kinematic joint.
Impact: multi-part products cannot be positioned or validated as a mechanism.
Note: an MCP-side align_instance_to_face / create_*_mate vocabulary already
exists on the Onshape bridge in this workspace, so the target semantics are known.
2. Drawings / 2D documentation. Absent. No drawing sheets, dimensioned views, section/detail views, GD&T, title blocks, or BOM. Impact: nothing manufacturable-by-a-third-party leaves the tool. For 3D printing this matters less than for machining, which is the honest reason it is Tier 1 by CAD convention but arguably Tier 3 for this product.
3. Variables, equations, configurations. Absent — no add_variable, no
expression evaluation, no configuration table. Every dimension is a literal double.
Impact: this is the biggest parametric gap. "Make this bracket for an M4 vs M5
bolt" requires re-editing every dependent feature by hand. Onshape's Variable
Studio + configurations are a core differentiator, and this is the cheapest Tier 1
item to close for the size of the payoff.
4. Surface modelling. Absent. No surface extrude/revolve/loft/sweep, no fill,
knit, trim/extend surface, offset surface, or thicken. SnapOrca is solid-only.
Impact: organic/complex shapes and repair of imported junk geometry are impossible.
OCCT already provides all of it (TKOffset, TKBRep), so the kernel is not the
blocker — only UI and feature plumbing.
5. Sheet metal. Absent. No flange, bend, tab, relief, or flat-pattern unfold. Impact: arguably out of scope for an FDM slicer; listed for completeness.
Tier 2 — individual features with clear demand
| Missing | Why it matters | Cheap? |
|---|---|---|
| Mirror body (part-level) | Sketch mirror exists; mirroring a solid about a plane does not. Extremely common. | Yes — OCCT gp_Trsf mirror + fuse |
| Helix / spiral curve | No helix ⇒ no springs, no custom threads, no spiral vase geometry. Sweep exists but has no helical path to sweep along. | Yes |
| Move / rotate body as a real feature | m_body_xform exists but is display-only (memory #1655) — it never enters the B-rep. Export/boolean see the original position. |
Medium |
| Split body | Cut removes material; splitting one body into two independently-usable bodies is absent. Very relevant for print-in-parts. | Medium |
| Thicken | Solid from a surface/face offset. | Needs surfaces |
| Rib | Standard structural feature. | Medium |
| Delete face / move face / replace face | Direct/dumb-solid editing — the main tool for fixing imported STEP. Given SnapOrca imports STEP and meshes, its absence is felt. | Medium |
| Datum axis, coordinate system | Only datum planes exist. Axes are needed for revolve/pattern references. | Yes |
| Mass properties | GeometryEngine computes a volume internally, but there is no volume/mass/COM/inertia readout. For print cost/time estimation this is nearly free to expose. |
Yes — trivial |
| Measure tool in the GUI | measure exists over MCP but there is no interactive measure in the UI. |
Yes |
| Hole standards library | Hole exists, but no counterbore/countersink/tapped standards (ISO/ANSI) with callouts. | Medium |
| Project / convert edges into a sketch | Cannot reference existing solid edges as sketch geometry ("Use" in SolidWorks). A significant sketcher gap given everything else is present. | Medium |
| Construction geometry | Could not confirm a construction/reference-line flag on sketch entities. | Yes if absent |
| Curve tools | Projected curve, bridging curve, composite curve, 3D fit spline. | Medium |
| Pattern on curve / pattern faces | Pattern is linear + circular of whole bodies only; no curve-driven pattern, no feature/face pattern. | Medium |
| Wrap / emboss | Text or sketch wrapped onto a curved face. | Hard |
| Enclose | Solid from bounded void regions. | Medium |
Tier 3 — platform capabilities (out of scope by construction)
Version control with branching/merging, release management, real-time multi-user collaboration, cloud PDM, FeatureScript custom-feature authoring, simulation/FEA, photorealistic rendering, app store/integrations. These are Onshape-the-platform, not Onshape-the-modeller. Not defects in SnapOrca.
3. Recommended priority
If the goal is "credible parametric CAD inside a slicer", the ordering that buys the most capability per unit of work:
- Variables + expressions — unlocks genuine parametric reuse; no new kernel work.
- Mass properties + GUI measure — nearly free, immediately useful for printing.
- Mirror body, datum axis, helix — small, self-contained, high-frequency features.
- Promote move/rotate body from display-only to a real B-rep feature — closes a correctness gap, not just a missing tool (exports currently disagree with the view).
- Split body — high value for print-in-parts workflows.
- Project edges into sketch — the sketcher's most conspicuous hole.
- Surface modelling — large, but OCCT already ships the algorithms.
- Assemblies — largest effort; only worth it if SnapOrca targets multi-part products.
Deliberately last: drawings and sheet metal — high cost, low relevance to an FDM-oriented tool.
4. Honest summary
SnapOrca's sketcher is at or near Onshape parity, and its solid feature set covers the mainstream modelling path (sketch → extrude/revolve/sweep/loft → dress-up → boolean/pattern). What is absent is breadth: assemblies, surfaces, sheet metal, drawings, and — most importantly for a tool calling itself parametric — variables and configurations.
The single most defensible criticism is #3: without variables, the feature tree is parametric in structure but not in value, so the promise of "change one number and the model updates" is only half delivered.