Creating a Sketch
Use Create sketch to start the 2D drawing that every solid in Kapy grows from. Press S with nothing selected and pick a plane, or select a planar face first and press S to sketch straight onto it. Choose that support carefully: it decides what the sketch is attached to, and therefore what happens to your part when something upstream changes.
Pick a support
Press S (or Create sketch) and the editor waits for you to say where. There are three answers.
A world plane: XY, YZ or XZ. The three that exist before you build anything. Nothing can move them, so a sketch on one is the most stable thing in the document. Start here for the first sketch of a part, and for anything that should stay put no matter how the model is edited.
A face of a body. Click a planar face and the sketch lives on it. The geometry you are working from is right there, which is convenient, but that face exists because of the features before it. Change one of those and the face may move, tilt or disappear, taking the sketch with it.
A reference plane. Geometry you built yourself: offset from a face, at an angle to one, through three points, halfway between two others. It sits in the middle ground, anchored to the model but to something you control rather than to whatever the last boolean happened to produce. Click it in the viewport like any other support — a datum plane wins wherever it stands in front of the solid — and the editor drops you straight into the new sketch, exactly as it does on a face.
Bounded to the face
A sketch on a model face can be bounded: anything you draw outside the face's outline is clipped away automatically, and the clip re-runs whenever the face changes shape. Ask for it when you want it, because every sketch is born unbounded. Draw a grid of holes over the whole area and the ones that fall off the edge simply do not exist.
A sketch on a world plane or a reference plane is never bounded. Those planes are infinite, so there is no outline to clip to.
Drawing, then leaving
Inside a sketch the toolbar is replaced wholesale: shapes, curves, inserts, and constraints once something is selected. Use Lines, Rectangles and Polygons and Circles, Arcs and Curved Primitives as the reference for the tools themselves.
The viewport changes with it. A note at the bottom right says whether the sketch is pinned down, over-constrained, or how many degrees of freedom are still loose, so you know where you stand without opening a window. Two arrows take the corner the ViewCube usually occupies, turning the view a quarter at a time, since a sketch is locked face-on and the cube has nothing to do there. Closed areas carry a faint tint. Fit to view frames the drawing and every visible body flattened onto the plane, and the Bodies window stays reachable, listing the bodies that existed before this sketch — the ones whose visibility matters while you draw under a face. If you would rather draw on a bare surface, the Customize window's Sketch section turns the grid and the axes off.
Finish sketch is how you leave. Escape does not. Mid-draw it cancels the shape in progress, and with nothing in progress it leaves the sketch alone, so a stray keypress cannot cost you drawn work. The single exception is a sketch you just created and have not drawn in yet. Escape backs out of that one, which is the "wrong plane" gesture.
Coming back to it
A sketch is a feature like any other: it sits in the timeline, and clicking its chip opens it again. Everything built from it rebuilds when you change it.
The Sketches window lists every sketch in the document. From there, rename one, hide it, or change its colour. Each sketch gets its own colour from a palette, so a document with six of them does not turn into a thicket of identical blue lines. None of that touches the geometry.
Next, draw in it. Lines, Rectangles and Polygons starts with the straight-edge tools.
See also
- Lines, Rectangles and Polygons: the straight-edge tools
- Circles, Arcs and Curved Primitives: the curved ones
- Regions and Profiles: what a finished sketch gives a feature