geop-ops-extrude-revolve

This page is a reference to the crate; these operations are taught in Lecture 26 to Lecture 28.

Extrude, revolve, sweep and loft operations. They resolve what their arguments refer to — the sketch’s areas as profiles (geop_ops_model::sketch::shape_profiles), the axis, the path — and sweep them with geop-lib-sweep, which describes the sweeps and how what they build is named. With the testing feature, testing draws the sketches and pushes the extrusions other crates’ program tests start from, and testing::bodies the boxes, cylinders and spheres the stress sweeps of geop-ops-fillet and geop-ops-shell blend and shell. Both features write sketches, so the sketch operations are optional dependencies of theirs: the crate itself depends on no other operation.

Its examples — box_with_drill_hole, bracket, cross_drilled_shaft, handle_with_hole, luggage_tag, revolved_cone_on_box, parametric_plate, pipe, name_plate (a word embossed on a plate), and edge_part and square_thread, drawn in the editor and kept as the .geop text it saved (src/drawn/) — are registered with its operations when the feature examples is on; each is tested to round-trip and to build incrementally (example_tests.rs). The programs from bug reports, rebuilt in Rust, are regression_tests.rs.

The operations

Sweep sweeps one sketch’s area along another sketch’s one chain or loop of curves, starting at the end (or joint) of the path nearest the profile; Loft lofts through several sketches’ single loops, in order. Both keep a new body or take a Combine, and as a face build faces standing on their own.

Extrude and Revolve are the operations a program uses (see geop-core-editor): they sweep a sketch of the part into a solid, and name everything after the sketch’s elements. A sketch’s areas — each an outer loop and its holes — are swept together, each a lump of the solid with caps of its own: the first area’s are start and end, every other’s start and end followed by the least name of its outline’s curves, extrude(E,end,K,c5#2). That is how a text is embossed or engraved, a lump or a pocket per letter. Up to the next face takes one area only, each area going as far as a face of its own; blind and through all take any.

How far they go is an Extents: the first side a length — an angle, for a revolve — UpToNext or ThroughAll, along the plane’s normal or, if reversed, against it; symmetric, the same the other way (half a length each way); or else an optional second side on its own terms. Up to next and through all go as far as the target solid. Through all is just a length reaching past all of it, so sides without up to next build one sweep between their ends. A side going up to the next face is built on its own from the sketch’s plane, long enough to reach past the target — for a revolve, short of a full turn, which needs the target clear of the axis — and combined with boolean_up_to_next (see geop-lib-booleans): a join grows up to the target, a cut or an intersection takes the first stretch of the target the profile passes through, and a new body — which goes up to the next face of any solid of the part — is that piece alone, the solids left as they are. If the target stops only part of the profile and the rest goes on past, the side goes exactly as far as the profile first meets the target (the nearest corner of where the two overlap) — or, for a cut or an intersection meeting nothing up to there, on to where it next meets it. The second side built so is named within side2.

As a face, they sweep the sketch’s curves — its area’s outline, or one open chain of curves enclosing nothing — into faces standing on their own, part of no solid: what Split cuts a solid with. A face going up to the next face of a solid picked for it is trimmed where it meets it (trim_up_to_next), leaving the solid as it is.

Editing one, the sketch is picked in the viewport and the extrude’s lengths are handles. A revolve’s axis is any line in the sketch’s plane — a line of the sketch, a datum axis, a frame’s axis, a straight edge: the area, holes and all, lies on one side of it, and touches it only at points of the sketch on it: where the constraints put them, or where the solved sketch cannot tell them from the axis. A new revolve has no axis: the field waits for a click. Dragging or typing the first length across the sketch plane turns a join into a cut and back; on either side, how to combine stays what was chosen — an extrude may cut upwards into a solid above its sketch. Both take a Combine from geop-ops-model: keep the result as a NewBody, or immediately unite, intersect or subtract it with a target solid — which is why this crate depends on the booleans, not the other way round.