Documentation
Sketches and constraints
A sketch is a 2D drawing on a plane or a flat face, and most solids start from one. Draw with the sketch tools: what you snap to becomes a constraint, and what you type becomes a dimension. A sketch is fully constrained when its curves turn from blue to white.
How do I start a sketch?
Press N or click New sketch, then click a plane: one of the origin planes, a flat face of a solid, or a construction plane. The camera turns to face it in an orthographic view. The sketch’s origin is the part’s origin projected onto that plane, the way the big CAD programs place it, so a dimension to the sketch origin is a dimension to the part origin. Click Finish sketch when you are done.
Which drawing tools are there?
- Line L: click point after point. Drag from the last end, or press A, for a tangent arc, then carry on with lines.
- Rectangle R: two corners, three points (it can be slanted) or centre and corner.
- Circle C: centre and diameter, two points, three points, tangent to two lines, or tangent to three.
- Arc: three points, centre and ends, or tangent to the curve it starts from.
- Polygon, Ellipse and Slot (five kinds, straight and curved).
- Spline B: through fit points, or by control points (degree 3 or 5). Conic K and the equation curve for exact shapes.
- Text, in a single-stroke CAD font or an outline font (the built-in Liberation Sans or a font on your computer), which you can extrude.
- X turns a curve into construction geometry, which guides the sketch without bounding a profile. A centerline does bound profiles and is picked as the axis when you revolve.
Each tool remembers the variant you used last, and every variant is also a command of its own in the S toolbox.
How do I type exact sizes while drawing?
Start typing. A box beside the cursor takes the length, angle, width or diameter; Tab moves to the next box. A typed value is locked: the preview follows it straight away, and the next click places the shape with that size. Typed values become driving dimensions. A circle takes its diameter by default; write R6 to give a radius.
How do snaps become constraints?
While you draw, the cursor snaps to end points, midpoints, centres and quadrant points, then to intersections, then to horizontal, vertical, parallel, perpendicular and tangent directions, then to points on a curve and to the grid. Each snap is kept as a constraint: an end point becomes coincident, a point on a curve stays on it, a midpoint stays the middle, a direction stays horizontal, parallel or tangent. A line drawn from circle to circle along both tangents comes out fully constrained.
Hold Ctrl to put a point exactly at the cursor without snapping or adding constraints. Hover over a point for a moment to track it: its horizontal and vertical lines then guide the cursor.
Which constraints and dimensions are there?
Geometric constraints: coincident, point on curve, horizontal, vertical, parallel, perpendicular, equal, tangent, concentric, midpoint, collinear, symmetric, fixed, curvature (G2) and regular polygon. Dimensions: length, distance between points, horizontal and vertical distance, radius, diameter, point to line, angle, arc angle, and distances to a circle’s tangent point (useful for wall thickness between holes).
Select one or two objects and the properties panel offers the constraints that fit them. The object you picked first stays put and the second one moves to meet it.
How do I add a dimension?
Press D, click one or two objects, move the cursor to choose between a horizontal, vertical or aligned dimension, click to place it and type the value. A circle clicked with another object is measured from its centre; a circle alone gets its diameter and an arc its radius, and the right-click menu switches between them. Double-click a dimension to change it, and drag it to move it. Every dimension gets a name such as d3, which expressions can use (see Parameters).
What happens when a constraint conflicts?
It is refused, and the constraints it would fight flash red, so you can see which ones to remove. A dimension on something the sketch already fixes is added as a driven dimension instead: shown in brackets, it reports the size and changes with the geometry, and the right-click menu turns it into a driving dimension when that would not over-constrain the sketch.
How do I see what is still free?
Under-constrained curves are drawn blue and fully constrained ones white. The status bar shows how many degrees of freedom are left. Select a curve or point and the properties panel lists what about it is still free, for example “radius not set”. Drag a blue curve to see which way it can move.
How do I edit a sketch?
- Trim T: click the piece to remove, or drag across several. Constraints carry over to what is left, so a fully constrained sketch stays fully constrained.
- Extend N, Break, and Offset O (one side, two sides or symmetric, one dimension for the whole chain).
- Fillet G and Chamfer: corners are rounded or cut while the dimensions you gave the corner keep their meaning.
- Mirror, Rectangular pattern, Circular pattern W, Move/Copy M and Scale. A mirror is kept symmetric and pattern copies follow their original; a moved copy is independent.
- Project P: bring edges of solids or curves of other sketches into this one. Projected geometry is purple and follows its source when the model changes.
- Ctrl+C and Ctrl+V copy sketch geometry, with the constraints between the copied objects, into this sketch or another.
Can I measure inside a sketch?
Yes: press I. Click a point, line, circle or arc for its position, length, angle or radius, and a second one for the distance or angle between them. Measuring adds no constraints.
Can I start from an existing drawing?
Yes. Insert DXF and Insert SVG read a drawing into a sketch, and Insert canvas puts a picture on a plane to trace over. See Import.