geop-ops-sketch

This page is a reference to the crate; sketches are taught from Lecture 23.

Sketches as an operation (see geop-core-editor). AddSketch places a sketch, drawn with geop-core-sketch, on a plane of the part (SketchPlane): a planar face, a datum plane — the planes of the origin among them — or another sketch’s plane. The plane is resolved when the step runs, so a sketch on a face stays where the face was, whatever later steps do to it.

The sketch is a target of the part, sketch(name), a PlacedSketch — the sketch and the plane it lies on — which is what later steps build on. The target, SketchPlane and the references into a sketch are geop-ops-model’s, so an operation that reads a sketch needs no sketch operation.

Reference geometry

What a sketch is given rather than drawn is reference geometry: fixed points and curves (see geop-core-sketch) that the solver never moves and constraints are measured against.

• The sketch’s own origin and axes. Every sketch has its origin as a point and its x and y axes as construction lines through it, so a point can be made coincident with the origin and a line parallel to an axis like with anything else drawn.
• Projections. A vertex, an edge or a face of the part, or a curve of another sketch, projected into the plane along its normal. A projection refers to what it projects by name, never by position: every time the sketch is built it is brought up to date with the part, so a sketch dimensioned against a projected edge follows the edge when an earlier step moves it. The sketch’s ids for what it projected are keyed by the names of the vertices and edges they come from, and stay the same.

Projecting reads what an edge is from its NURBS curve: a straight one is a line, a circular one in a plane parallel to the sketch an arc or a circle — to be constrained like one — one seen edge-on the line it collapses to (an arc’s extent found on its circle, not on its control polygon, which reaches further), and anything else the spline it projects to exactly (projection along the normal is affine: it moves the control points and keeps weights and knots). An edge seen end-on is only a point.

Reference geometry is always construction geometry, drawn dotted: drawn geometry snaps to it and is constrained against it, but it never bounds a region itself.

Dimensions as formulas

A dimension’s value can be a formula of the part’s parameters (see geop-ops-model) — width / 2, screw.clearance — kept with the step and evaluated every time it is built, the sketch solved anew when that, or what it projects, changed. Angles are in degrees.

Editing a sketch

A new sketch has no plane and starts by picking one — a reference field like any other, so picking another one later moves the drawing onto it — and once it has one it is drawn on it, the viewer facing it head on. Selecting and dragging are the editor’s, as in every operation; drawing is AddSketch’s own: it takes the clicks while a tool is in hand, the keys, and where its points and curves are dragged to (PartOperation::canvas, see geop-core-editor). Every tool is a button of its own, shown as an icon.

• Drawing tools — line, corner, center and 3-point rectangle, center and 3-point circle, 3-point, center-point and tangent arc, polygon, slot, spline, point — and fillet. Each builds its curves and the constraints that keep it what was drawn: a rectangle’s sides square, a polygon’s sides equal on a construction circle, a slot’s ends tangent with their centers as points. The same construction previews the shape to the pointer and builds it on the click. Construction mode (or the curves selected) makes construction geometry.
• Text (W) — a string, its capitals’ height and its angle set in the dialog, shown at the pointer and placed by a click at the start of its baseline: the outlines of its glyphs, each closed contour a loop of the profile, so a word extrudes into a lump or a pocket per letter. Its anchor is a point like any other, to constrain and drag; selected, the text is edited in the same fields. It takes no constraint itself, is not snapped onto, and is never cut by trim, only removed whole (see geop-core-sketch).
• Lines and arcs in one motion. Drawing a chain of lines and moving the pointer back onto the chain’s end switches the next segment to an arc tangent to the last one; after the arc the chain goes on with lines, the first of them tangent to the arc too — and horizontal or vertical as well if drawn so, the arc giving way to both.
• Snapping is by constraint, never by moving geometry. A point placed on an existing point — the origin among them — is that point; one placed where two lines, arcs or circles cross — the sketch’s axes counted as infinite lines — is constrained onto both; one placed on a line’s or arc’s middle is its Midpoint; one placed on a curve is constrained onto it (PointOnCurve); a line drawn within 2° of horizontal or vertical gets that constraint. Dragging a point onto a point, a crossing or a middle snaps the same way, and constrains it there when let go. Where the pointer snaps is shown; holding shift turns snapping off.
• Constraints, one tool each. Coincident, horizontal, vertical, parallel, perpendicular, tangent, collinear, equal, concentric, midpoint, symmetric, fix, and the dimensions distance, horizontal and vertical distance, radius, diameter and angle. Each lists the kinds of operands it takes; with nothing selected every one can be taken up, and a selection greys out those it can never become. Pressed with a selection that is all it needs, a constraint is added at once, measured from the geometry as it is, so adding it moves nothing; otherwise the tool is taken up and picks what is clicked next until it has all it needs. A dimension is added by the click that says where its value goes — previewed at the pointer until then — and drawn there with its extension and dimension lines (an angle with an arc about where its lines meet). It then asks for its value in place; double-clicking the value asks again, and dragging it moves it out of the way. Where it goes is kept as an offset from what it measures, so it moves with the geometry. Constraints are listed, their values or formulas edited there too.
• Dragging a point, a line or a spline moves its points as far as the constraints let them (Sketch::solve_with_drag); dragging a circle sets its radius, an arc its sweep. Reference geometry is not dragged.

Undo and redo go edit by edit while a sketch is edited — a drag is one edit — and back to the program’s own once it is put away.

Every change is solved before it is returned, and one line of the dialog says how that went: degrees of freedom left, or how many constraints conflict, and how many closed regions the sketch has.