Sketching and constraints

A sketch lies on a plane: an origin plane, a construction plane or a planar face. Start one with Create Sketch (sketch.create) and click a plane, or pick a face first. Right-clicking a plane, in the view or on its browser row, offers Create Sketch on that plane too. Finish Sketch returns to the model.

In scripts, XY, XZ, YZ and their Top, Front, Right aliases name origin planes. These names are reserved: a construction plane cannot be created with or renamed to one (case-insensitive). If an older design already has a construction plane with such a name, a string argument naming it is ambiguous and is rejected; use the other alias (XY for Top) for the origin plane, the construction feature’s numeric ID to select it, or an explicit {origin: [x,y,z], normal: [x,y,z]} plane. Existing saved references retain their meaning; opening a design does not reinterpret old sketches.

Curves adapt to the current zoom and display scale. Picking and highlighting use the same visible boundary, including small circles at Fit and sketches in rotated components. Profile shading follows those curves while preserving holes. Zooming changes the display without changing sketch geometry, dimensions, or undo history. On short windows or enlarged displays, the Sketch Palette’s options scroll while its constraint status and Finish Sketch button remain visible.

Geometry

Point is available directly on the default Sketch CREATE toolbar. Click it, then click in the sketch to place a point. Existing toolbar customizations are kept; use Reset Toolbar from the toolbar’s context menu to restore the default buttons.

Lines and polylines (L), rectangles (two-point R, three-point, centre), circles (centre C, two-point, three-point, tangent), arcs (three-point, centre, tangent), polygons, slots, ellipses, fit-point and control-point splines, conics, points and text. Construction (X) turns curves into reference geometry that doesn’t form profiles. Modify tools include trim (T), extend, break, fillet, chamfer, offset (O), mirror, patterns, move/copy and scale.

The Sketch Palette’s Construction Geometries option hides construction curves while you work. A hidden construction curve cannot be picked by a click or by a box. Nothing invisible is selectable. The option belongs to one sketch and is saved with the design. Centerlines are a line type of their own and keep showing. Projected geometry that carries the construction line type, such as the trace of a plane, answers to Projected Geometries instead. The option changes display only. Construction curves were already outside every profile.

Polygon tools show their edge outline while positioning the second point, so the orientation can be checked before placement. Inscribed and circumscribed polygons retain their support circle and update the outline when the inline Sides value changes.

Text is set in the built-in font (Liberation Sans) unless it is given another: sketch.text and sketch.edit_text take a font, the family or full name of an installed font (“DejaVu Sans”) or the path of a .ttf / .otf file, and the Edit Text dialog has a Font field for it. An unknown font is an error, and the font is kept with the text in the design, so the text stays editable in it. SOLIDCRAFT_FONT_DIRS adds folders to the ones searched for installed fonts. A text’s height, its angle and each coordinate of its at can be expressions of the design’s parameters, given as strings ("height": "plate_height / 10", "at": ["plate_width / 2", 5]): the text keeps the expression and follows the parameters when they change, and saves it with the design. A number takes the place of an expression, and so does moving the text or dragging its handles (what moves becomes a number; turning a text leaves its height as it was). A string that names no parameter is the number it comes to. The same two commands refuse a text that is not a string, an at that is not two numbers or expressions, a height or angle that is neither (or a height that is not positive) and an expression that cannot be worked out with a message, instead of drawing the text with a default; left out, they keep their defaults.

Right-click a letter’s filled interior or outline and choose Edit Text. You can also start Edit Text first and click the letter. All outlines belonging to that text are highlighted while the dialog is open. A profile bounded by multiple text sources or other geometry cannot identify one text: use Select Other to choose its outline instead. Change the text, font, baseline X/Y, height or angle, then confirm with OK; Cancel keeps the original text. Position and height use the document’s units. The four fields take expressions: one that names a parameter (plate_width / 2) stays an expression, is shown as typed when the dialog is opened again, and keeps the text following the parameter.

A text can follow a curve of its sketch (its Path). That curve becomes construction: the letters stand on it and their descenders cross it, so as a normal curve it would cut them into pieces, and picking the text would pick those pieces. Taking the text off the curve leaves it construction; Normal/Construction turns it back.

Drag a text outline to move all its letters together. Let go to finish in one undo step, or press Esc during the drag to restore the original text. The text stays editable. For an exact displacement, select an outline and choose Move/Copy from its context menu. Enter Distance X, Distance Y and an optional Angle about the text’s baseline; lengths accept document units or explicit units such as 1 in. Enable Create Copy to leave the original in place and create a separately editable text. Cancel leaves the design unchanged. Projected geometry remains protected from ordinary dragging.

Project (P) and Intersect bring model edges into the sketch as linked geometry that follows later changes. Sketching on a face projects its edges automatically. A projected edge stays the edge that was picked, wherever a later change moves it; when that edge no longer exists, the projection keeps its last shape and the sketch says it was lost. For Project, select visible source curves or points from another sketch, model edges, faces, vertices or bodies, or axes and planes, then press P. The entire supported selection is projected in one undo step. A rejected projection keeps the selection for correction; an empty or mixed selection starts the ordinary picking tool. External sketch selections retain their source sketch, even when the active sketch uses the same point or curve names.

A sketch on a construction plane built from the model (through a sketch line, through three points, midway between two faces…) projects, intersects, includes and holds text like a sketch on any other plane, and its links follow when a parameter moves that plane.

Run from a script or the control channel, every command that adds sketch geometry returns the ids of what it added (created: {points, curves, constraints, dimensions}). Ids are stable and never reused within a sketch, even after a delete, so a script can dimension or constrain the new geometry right away.

Extend finds intersections with exact ellipses, rational conics and spline spans. It keeps the original line or circular support and extends only beyond the selected endpoint; conflicting constraints or an ambiguous overlap leave the sketch unchanged.

Closed convex chains of tangent lines and circular arcs support inward offsets that consume a rounded corner. When the offset passes the corner radius, the neighbouring straight supports meet at a sharp corner. The surviving lines and endpoint IDs stay stable; the retired arcs return under their original IDs if a later edit restores their radius. Whole-boundary profile selections follow this transition through save and reopen, so an extruded lip can remain associative. Existing eligible closed analytic offsets upgrade without changing their saved geometry or IDs.

This transition requires a closed convex boundary with tangent junctions and a certified nonempty region. An extinguished arc referenced individually by a constraint or another offset cannot retire. Creating another offset from an already sharp retired boundary also requires breaking its association first. Open, nonconvex and mixed free-form chains keep their existing behavior. Break Offset Association freezes the current boundary, including private arc centres and construction flags, for independent editing.

Offsets of smooth ellipses, conics and splines follow their source after dimension changes, dragging and reopening a design. Their stored cubic spline has a whole-span normal-distance error bound of 0.002 mm. Singular tangents, curvature cusps, possible self-intersections and excessive subdivisions are refused. Offset these curves individually: mixed chain junctions currently require separate geometry. sketch.offset.break releases an offset for independent editing, and undo restores its association. Older independently sampled offsets remain independent. Smooth open and newly created smooth closed offsets can be offset again, including bounded refinement after a source edit. New closed outputs use a periodic cubic fit with continuous tangent and curvature at the seam. Break Offset Association preserves that interpolation, and its closing point remains joined when dragged. Deleting an output also removes its unused private fit points; deleting a source with a retained dependent is refused.

For explicit closed fit splines, sketch.spline.fit_point accepts periodic: true and at least three distinct cyclic samples. It closes the loop automatically. Existing calls and older saved closed splines retain natural interpolation; older associative closed offsets also retain their saved natural fit. A legacy seam without a unique normal still refuses another offset. Periodic intent is stored on each curve and survives save, reopen and Break. While drawing a fit spline, click its starting point after three distinct samples to close it smoothly. Right-click finishes an ordinary natural fit. Offset accepts both ellipse handles and dense fitted curves; the second click sets the side and distance from the curve.

While drawing in a planar sketch, Construction (X) changes the line type without ending the tool or losing picked points and inline values. The preview and hover feedback keep construction dashes and centerline dash-dot patterns visible. With curves selected, Construction changes those curves as before.

Enable 3D Sketch in the Sketch Palette to draw lines, fit splines and points off the plane. While placing these points, you can snap to points on other visible sketches. For a bridge line, start Line and click an endpoint on each source sketch; each endpoint uses its source plane, even when that plane differs from the active sketch. These snaps capture positions; they do not create associative links to the source points. New 3D geometry follows its sketch’s component placement, including the selected occurrence and pending position changes. Click a drawn fit point to show its move triad; its arrows move along world X, Y and Z. Scripts also supply world coordinates to sketch.line3d, sketch.spline3d, sketch.point3d and sketch.move3d. Activate the desired occurrence before editing an explicit sketch belonging to a component with multiple placements.

Older drawn or detached 3D wires keep their saved world positions. Included and surface-linked wires with an explicit component marker keep that meaning after the link is broken. Old files whose links became lost after an incorrectly scoped cross-component refresh may require a fresh link once the source is available; their stored point values are preserved on opening.

Constraints and dimensions

Horizontal/Vertical accepts a click on a line or clicks on two distinct sketch points, including the origin, endpoints and circle centres. For two points, it chooses horizontal or vertical alignment from their current positions. Esc cancels a pending first point.

The solver is SolidCraft’s own (damped Gauss–Newton with degree-of-freedom analysis). Constraints: coincident, horizontal/vertical, parallel, perpendicular, tangent, equal, concentric, collinear, midpoint, symmetry, fix, curvature (G2) and polygon. Sketch Dimension (D) adds linear, aligned, horizontal, vertical, radius, diameter and angle dimensions. Each is a parameter (d1, d2, …), so it can hold an expression.

Press D, click what you want to measure and type the value: as soon as the click settles the dimension (one line, circle or arc, or the second point or line of a distance or angle), its value box takes the keyboard with the measured value selected, so typing replaces it. Numbers, units (1 in), expressions (2*width) and parameter names all work; letters go into the box, not to tool shortcuts. While you type, the dimension text follows the cursor, and Enter places it there (or in its default place if you haven’t moved the cursor) as one undo step. Esc cancels the dimension.

You can still place the text first. Before you type, a click on empty sketch space puts the text there and keeps the value box focused; a click on another point or line makes the dimension a distance or angle instead; Tab leaves the picks waiting for a click to place the text.

Between two points, or on a line, that don’t line up with an axis, where you place the dimension picks what it measures: across from them, the distance between them; above or below them, the horizontal distance; beside them, the vertical distance.

A dimension the sketch can’t take, because the geometry is already fixed by other constraints and dimensions, is added as a driven (reference) dimension instead: it is shown in parentheses, measures the sketch, and has no value to edit.

For Coincident, pick two points, a point and a curve (in either order), or two distinct straight lines. Two lines join their closest pair of endpoints; the first picked line stays in place when the existing constraints allow it. Pick endpoints explicitly when you want to connect a different pair.

Horizontal/Vertical also applies immediately to one selected line or two distinct selected points. Shift-click to add the second point before choosing the constraint.

For Parallel, Perpendicular, Equal, Tangent, Concentric and Collinear, select exactly two sketch curves (Shift-click to add the second) and choose the constraint to apply it immediately. You can also start the constraint first and then pick its curves. An incomplete or mixed selection leaves the tool ready for ordinary picking.

Coincident accepts an exact selection of two points or a point and a curve. Midpoint accepts one point and one line, in either selection order. Symmetry accepts two distinct points and one symmetry line, regardless of where the line occurs in the selection. Successful constraints clear the selection; rejected constraints preserve it.

Under-constrained geometry is blue and fully constrained geometry turns dark, and the status shows the remaining degrees of freedom. A constraint or dimension that would over-constrain the sketch is refused rather than applied. Drag a point to move it; the solver keeps every constraint while you drag.

Profiles

Closed loops become profiles automatically, including regions split by crossing lines and islands inside outlines. Extrude, revolve, sweep and loft pick profiles.

A feature remembers a picked profile by the curves around it, not by where it was clicked: "profiles": [{"curves": ["l1", "l2", "a1", "l3"]}] (or [{"curves": ["c1"]}] for a circle) picks the region whose outer loop is made of exactly those curves, or the pieces of them that other curves cut off. It is found again on every recompute, so the feature keeps the same region when a parameter moves the geometry. Islands inside the region are its holes. When no region, or more than one (both halves of a circle cut by a line), is bounded by exactly those curves, the feature reports an error rather than taking another region. Profiles picked by index or by point ([{"point": [x, y]}]) are stored the same way when the feature is made.

Measurement units

Change the current design through Document Settings > Units in the browser. The units preference applies to new designs. Existing sketch annotations, live drawing lengths and Measure follow the current design units without resizing geometry. Inches display at least three decimal places and retain a meaningful fourth digit; a higher display precision can be selected in Preferences. Bare length values typed in the dimension tool use the current design units. Explicit units such as 25.4 mm remain valid in an inch design. Angular dimensions keep their angular units. Deliberately typed four-place inch literals retain trailing zeros. Component/canvas distance controls and inspection, parts-library and flat-pattern measurements follow design units too; parameter expressions and metric standard names retain their explicit authored units.

Measure shows the currently selected distance (centre, minimum or maximum) and separate X, Y and Z distances on the canvas. The component dimensions follow the world axes and remain visible until the Measure dialog closes. To hide these extra lines and labels, turn off Preferences > Graphics > Show X/Y/Z distances. The choice is saved between runs.

Reviewing mirror, pattern, and offset results

Mirror, rectangular/circular Pattern, and Offset show the active selection step in their shared tool window. Click an input to change it; click a selected object again or Ctrl/Cmd-click it to remove it. Each input has its own Clear button. Source inputs show a count, and single references identify the chosen mirror line, direction, or centre. Box selection also works while the window is open. Sketch modify tools take geometry from the sketch being edited.

Proposed sketch geometry appears green before confirmation. Change the inputs or values to update the preview, then press OK. Cancel discards the preview. A circular pattern centre can be an existing point or a position clicked in empty sketch space.

Sketch patterns keep each instance related to the seed geometry: moving the seed updates the copies, and a copy cannot deform independently. Circle and ellipse radii follow the seed too. Choose a circle’s centre point to keep a circular pattern centred on that circle. A centre placed in empty space becomes a sketch point that can be dimensioned or made coincident. Double-click the pattern badge (at the circular centre or beside the rectangular seed), or right-click a seed or copy and choose Edit Sketch Pattern, to change quantity, spacing, direction or total angle. Confirmed edits preserve surviving instance ids; Cancel discards the preview. Pattern settings survive save/reopen and undo/redo. Deleting a seed, copy or pattern relation breaks that association and leaves the remaining geometry independent. Patterns saved by older versions remain independent copies; recreate them to add associations.

Offset distances are editable driving dimensions: double-click a dimension or change its model parameter to resize the offset without moving its source curves. The selected side, distance, and association survive save/reopen and undo/redo. Symmetric offsets share one driving distance; Two Sides has an independent distance for each side. Disconnected selected curves or chains are all offset. Breaking an association retains its current geometry and removes that association’s driver. Older offsets retain their saved fixed distances.