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Sketching

A sketch is a 2D profile drawn on a reference plane or on a flat face of an existing body. It is the starting point of almost everything in the Design tab: profiles become solids through Modeling Tools, and they stay editable afterwards.

Starting a Sketch

  1. Click the face or reference plane you want to draw on.
  2. Press Shift + S, or pick Sketch from the offer menu. The sketch opens on the face you clicked, on the first click.
  3. Pick a tool — a single letter, the toolbar, or the offer menu — and draw.

Each tool says in the status line what it wants next, for example Circle — click center, then radius.

The Sketch Environment

Three things change when a sketch opens, so the mode is unmistakable:

  • A banner across the top of the viewport names the sketch and reminds you that N looks normal to the plane and that the sketch is left from the toolbar.
  • The printer bed is muted, because a plate grid and a sketch grid look alike and reading one as the other is how a profile gets drawn against the wrong reference. Press Ctrl + Shift + B to bring the bed back.
  • Single letters drive the sketch tools for as long as the sketch is open. See Design Keyboard Shortcuts.

Press N at any time to look straight at the sketch plane, keeping the current zoom.

Entities

Entity Variants
Line Single line, polyline
Rectangle Corner, center, oblique, rounded
Circle Center and radius, 2-point, 3-point
Arc Center-point, 3-point, tangent
Ellipse Ellipse, elliptical arc
Polygon Inscribed, circumscribed
Slot Straight, arc
Spline B-spline through control points
Point A single point
Text Text on the sketch plane

Press Q to draw the next entity as construction geometry, or to convert a selected entity between construction and real geometry. Construction lines guide the sketch and are ignored when the profile becomes a solid.

Editing

Tool Key What it does
Trim T Cut a segment back to its nearest intersections
Extend X Run a line or arc out to what it would meet
Offset O Copy an entity at a distance
Mirror M Pick an axis, then the entities to reflect
Fillet F Round the corner between two lines
Chamfer H Bevel the corner between two lines
Dimension D Dimension two points or one entity
Value V Type the defining number of the selection — a line's length, an arc's radius, a circle's diameter, or the angle between two entities

Entities can also be moved, rotated, scaled, and repeated in a linear or polar array from the toolbar.

Constraints and Dimensions

Press K to finish the live tool and enter constraining. The available geometric constraints are coincident, collinear, horizontal, vertical, parallel, perpendicular, tangent, concentric, midpoint, equal length, equal radius, symmetric and fix. The dimensional constraints are distance, horizontal and vertical distance, angle, radius and diameter.

The solver reports the remaining degrees of freedom while you work and tells you when the sketch is fully constrained, or when a new constraint conflicts with one already there.

Tip

Constrain the shape before dimensioning it. A profile that is square because it was constrained horizontal and vertical stays square when a dimension changes; one that is square only because it was drawn carefully does not.

Finishing a Sketch

  • Confirm in the floating action bar, or press Enter, to finish the sketch and keep it.
  • Cancel in the action bar discards the sketch, and asks first when there is geometry to lose.
  • Esc never destroys work. It closes an open value field, or drops the entity being drawn, or drops the armed tool back to Select, or clears the selection — one step at a time, in that order. A sketch that holds geometry is only left through Confirm or Cancel.
  • Ctrl + Z inside a sketch removes the last entity drawn. Del or Backspace deletes the selected entities.
  • A sketch whose entities form no closed wire fails with a message rather than producing a default shape. Auto-close sketch loops (Preferences → General → Features) decides how forgiving that check is: on, endpoints within 0.001 mm are welded into one joint; off, only exactly coincident endpoints join, so a loop with a hairline gap is reported as open.

Reopening a Sketch

Sketches stay editable. Select one in the feature tree to reopen it with its dimensions live; change a value and every feature built on it rebuilds. Double clicking a sketch stroke in the viewport edits that entity directly.