Sketch

Status: Implemented

Sketch stores 2D geometry in feature-persistent data and visualises it on a selected plane or face. The sketch mode opens a 2D sketcher environment where you can draft profiles that become the basis for Extrude, Revolve, Loft, or Sweep features.

Overview

Sketch Mode opens the 2D sketcher on a selected plane or face. Geometry is constrained within a local coordinate system, letting you dimension lines, arcs, and splines precisely. When you finish, the sketch remains parametric and updates downstream features as you edit it later.

Workflow

1. Choose a plane or datum, then activate Sketch Mode from the feature history
2. Draw with line, rectangle, circle, arc, spline, and text tools
3. Apply constraints and dimensions to lock intent before returning to Modeling Mode
4. Use the sketch as input for other features like Extrude, Revolve, Sweep, or Loft

Inputs

• sketchPlane – face or datum plane that defines the sketch basis. The plane orientation updates automatically when the reference moves.
• Edit Sketch – opens the in-app sketcher (viewer.startSketchMode) so you can add points, curves, and constraints.
• curveResolution – tessellation setting used when generating circular geometry for downstream features.

Behaviour

• The feature builds a local coordinate frame from the selected plane, saves it in persistent data, and reuses it on every regenerate so the sketch tracks its reference.
• Sketch geometry is kept as JSON, solved through the ConstraintEngine, and rendered as a SKETCH group containing faces and edges that other features (Extrude, Revolve, Sweep) can consume.
• External references are projected into sketch space at regenerate time and expression-backed dimensions are evaluated before solving.

Constraints

Sketch constraints show up as glyphs that use Unicode icons so you can tell them apart at a glance. The solver supports the following set:

Symbol	Constraint	What it does
⏚	Ground	Locks a point in place. Used for the origin and any projected references so they cannot be dragged.
━	Horizontal	Forces two selected points to share the same y value.
│	Vertical	Forces two selected points to share the same x value.
≡	Coincident	Merges two points so they occupy the same coordinates; downstream coincident groups stay merged.
⟺	Distance	Adds a numeric dimension. On lines it fixes the segment length, on arcs/circles it becomes a radius or diameter dimension.
⇌	Equal Distance	Makes two segments (or two radii) match length. Works for line pairs or circular features that need equal radii.
∥	Parallel	Keeps two lines travelling in the same direction, reusing existing horizontal/vertical locks when possible.
⟂	Perpendicular / Tangent	For line pairs it enforces a 90° angle. When applied between a line and a circle/arc it constrains the line to stay tangent by keeping the radius perpendicular at the contact point.
∠	Angle	Stores an explicit angle between two segments. The initial value is captured from the current sketch state.
⏛	Point on Line	Projects a point onto the line defined by the first two selections, useful for keeping construction points collinear.
⋯	Midpoint	Centers the third point midway between the first two and retains equal distances as you edit the sketch.

Grouped constraints that touch the same points share a single anchor and render their glyphs side by side so complex regions stay legible.

Context Toolbar

A floating context toolbar follows the sketch viewport and updates itself based on the active selection. It offers only the constraints and actions that apply to the selected entities, making it quick to add intent without digging through menus.

• Adaptive constraints – Select two line segments and the toolbar lights up Parallel ∥, Perpendicular ⟂, Angle ∠, and Equal Distance ⇌. Pick a line and an arc and it switches to the tangent option. Single, double, or triple point selections surface the matching point-based constraints (H ━, V │, Coincident ≡, Distance ⟺, Colinear ⏛, etc.).
• Radial dimensions – Selecting a single circle or arc reveals Radius and Diameter dimension buttons so you can drop the right measurement without changing tools.
• Construction toggle – Any time geometry is highlighted the toolbar shows a toggle that flips the selection between regular sketch curves and construction geometry. Construction curves remain in the sketch for constraints but are ignored when profiles are consumed by downstream features.
• Utility actions – When you have an active selection the toolbar also surfaces quick delete actions so you can clean up without context switching.

Linking External Geometry

Sketch Mode can link to edges that live outside the current sketch so profiles stay tied to upstream solids:

1. Switch to the sketch and pick Link external edge on the top toolbar.
2. Click scene edges or face boundaries; each pick projects both endpoints into sketch UV space and adds them as fixed points.
3. The viewer lists every linked edge; selecting a row reselects its projected points, and Unlink removes the pair and their auto-created ground constraints.

The sketch feature stores external links as externalRefs in persistent data. On every regenerate it looks up the referenced edge by id or name, reprojects the endpoints into the sketch plane, and reapplies ⏚ constraints so the references remain locked. If the source geometry moves, the sketch updates automatically, keeping downstream features live without requiring you to redraw or manually re-reference the outline.