Lathe G-code

The same as the material in card 3 (Feeds and speeds): pick it here or there, and the recommended speeds and feeds follow it.

Length is from the chuck to the end face of the blank (X0); it is shown as a dimension on the preview. With a drawn blank every tool path starts from its shape: the turning only cuts where it has metal, and the boring starts from its hole (no drill needed).

After T1 is fitted the program stops at safe; start takes T1 to the bar stop (X first, then in along Y), where it stops again. Push the bar out against the tool, tighten the chuck and press start: the tool backs straight off the bar end along X to safe X, then out to safe Y, and stops there again so you can run the spindle up; start then begins the cutting. The bar end is then in front of X0 by about the bar stop X (where T1's nose meets it), and the facing passes take that off in equal steps, each from outside the bar in to the centre, the last to X0. These passes come first in the passes table (their feeds and stops can be changed there).

The drill is not driven: the work turns, so it only ever drills on the centre line. Set up each drill you have once, with its own offsets: where its tip sits from T1's zero point when it is in the drill chuck in the tool post (X usually minus, Y about +14). Tick Use on the drills for this hole: with more than one, the smaller ones go first (pilots), each to the same depth, and each is a tool change (M0 at safe to fit it). Feed and peck left empty are the ones recommended for the material in card 3, at the drill's own spindle speed, which the M0 that fits it gives; pecks are halved once the hole is deeper than 3 × Ø. Each drill goes to the hole depth unless it has a depth of its own: left empty, a drill bigger than a step in the drawing's bore stops where its point meets the step (the greyed figure), and you can type any depth. Coming right out after each peck lets the brush get to the drill: it comes out to the distance given and waits there for the pause (G4), so the flutes can be brushed clean and loaded with oil before it goes back in. Each drill goes to safe with its own tip at Safe X and Y, so it is always in front of the face. The program always stops at safe with an M0 to fit each drill, and again to refit the turning tool, as at every tool change.

The parting tool is fixed to the saddle behind the work. Its datum is the corner of the cutting edge on the face nearest the chuck; the offset is from the front tool's zero point to that corner. Each cut is one plunge of the blade: the finished size is from X0 to the blade's other face (so its datum face is at the finished size + width); leave it empty for the end of the part. Ø0 parts off, a bigger Ø makes a groove. Extend past centre line takes a part-off that far beyond the centre (e.g. 0.5) so it doesn't leave a pip; grooves are not affected. Cuts are made in order from the face, pecking in and backing off by the back-off distance between pecks.