How to use

1 Draw the part

• Draw half the profile as a side view, centre line along X.
• Put 0,0 at the centre of the tip: where the face meets the centre line. If the face is drawn past X0 (0,0 somewhere else along the part), the app moves it back to X0 and says so; check the result in the preview.
• Draw the outside edge from the face to the chuck end. Y is the radius.
• Lines, arcs, polylines and splines are fine. A centre line and back face can be drawn too.
• A part with a hole (bore): draw it as a half section: the outside as usual and the bore as a second line from the face toward the chuck, ending at the bottom of the bore (down to the centre line for a blind bore, or through to the back face). The face line runs from the bore up to the outside. The app reads the highest line as the outside and the lowest as the bore.
• Save as DXF or DWG, in mm.

2 Load it

Drop the file on card 1 (or browse…). You'll see the length, the smallest and largest diameter and any warnings. Once a part is loaded the drop box folds away (the details stay in view); click Show the file drop box or drag another file over card 1 to open it again. Open with the example part to see how it works.

3 Blank and tool

The card folds away under Show the blank and tools (…), which still gives the blank, T1, T2…, the drill and the rear tool if used; it stays as you left it (and opens by itself when T1 has no offset in the library).

• Enter the blank length (from the chuck to its end face, X0: shown as a dimension above the preview) and diameter, or press Fit to part.
• Pick the blank's material. It is the same setting as the material in card 3 (Feeds and speeds): pick it in either place and the recommended speeds and feeds follow it.
• Pre-drilled / pre-shaped blank (tick box under the blank): load the blank's own DXF or DWG, drawn like a part (half of it, 0,0 at the centre of its end face, Y = radius, with its hole if it is pre-drilled). Its end face goes at X0 and the length box becomes Chuck to end face of the blank. Every tool path starts from that shape: the turning only cuts where the blank has metal and the boring starts from its hole, so no drill is needed (with Drill ticked too, the bigger hole counts). The diameter comes from the drawing. Where a roughing pass would feed through air (the blank already smaller there), it is split and comes down onto the next stock instead.
• Pick the tool. The picture shows the insert and its programmed point (red dot, where the cross hairs cross: left of the nose on right-hand tools, the middle on neutral ones, the right on left-hand ones). A 55° D insert follows steep recesses better than an 80° C insert.
• Set the nose radius of the insert you've fitted. It is T1's nose radius in the tool offset library (the same box, kept in step), so the holder keeps it when it is used again, as T1 or T2…
• Tool zeroed on: nose quadrants (default: length from the 9 o'clock point of the nose, diameter from the 12 o'clock point; on the neutral SCMCN and SDNCN holders length is from 12 o'clock too) or nose radius centre. With the quadrants the path sits on the drawing along diameters and faces and is offset round chamfers, arcs and corners. Zero the tool to match (section 7).
• Left-hand tools (SCLCL, SDJCL, marked LH) feed toward the face (out past the face they lift off once the nose is the approach clearance past it); zero their length on the 3 o'clock point. With a right-hand tool finishing, a left-hand tool ticked as a further finishing tool then finishes what the right-hand one couldn't reach (Finish the rest passes). Groove 3.05: zero on the chuck-side corner; when it is one of the tools, after the turning it plunges, pecking (Groove peck depth in card 4), into the red areas the turning tools couldn't reach.
• Loading the bar (T1 as a bar stop) (optional): tick Load the bar against T1 at the start, then face it to X0 and give the bar stop X and Y (G-code, where T1's point goes), the number of facing passes that bring the face to X0, and whether to go to safe and stop (M0) once the face is at X0 (unticked: the program carries straight on). The program then: fits T1 at safe (M0); stops again at safe (READY TO LOAD THE BAR); start takes T1 to the bar stop, out along X first, then in along Y; it stops there (LOAD THE BAR UP TO THE TOOL): 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 (BAR LOADED - RUN UP SPINDLE): run the spindle up and press start. The bar end now sticks out past X0 by about the bar stop X (where T1's nose meets it; the line under the fields says where), and the facing passes take it off in equal steps, each from just outside the bar in to the centre (the nose centre onto the centre line, so no pip), then straight off the face along X. The last is a finishing pass to X0. They are the first passes in the passes table (Facing), with the roughing feed (finishing feed for the last), which you can change there; a drill set for before the turning drills after them. The preview shows the bar end in front of X0 until it is faced. Errors if the bar would miss the tool (Y outside the blank), if the bar end would end up behind X0, or if safe X isn't in front of it.
• Additional tools (optional; folded away under Show the additional tools (…), which names the tools in use, and stays as you left it): Add tool adds T2, T3…: the insert (as for T1, clicking the box opens a list with a thumbnail of each tool's tip; its tip is drawn next to it) and where its zero point sits from T1's zero point (X + toward the face, Y + toward the back). The passes table then has a Tool column to pick the tool for each pass (or tick passes and use Set tool on ticked); each pass is planned with its own tool's shape, and the tool is changed at the safe position with an M0. If the finishing tool reaches further than the roughing tool (e.g. into a hollow), it roughs those places itself first, so the finishing cut stays light. Which tools finish is set with the Finishing tick boxes (below). Each tool change stops at safe with an M0 to fit the tool, then a second M0 (CONFIRM T2 IS FITTED) so it is never taken for a clear-swarf stop. The safe position is relative to each tool and its offset, and a tool change goes to the safer of the two tools' safe positions, so the new tool is never nearer the work.
• Finishing tools: tick Finishing tool under T1 and/or Finishing against T2, T3… The tools not ticked rough, leaving the finishing allowance. The first ticked tool (in T1, T2… order) makes the finishing pass; any further ticked tools then finish whatever it couldn't reach. With sections this happens in each section before the next is roughed (so T1 roughs S1, T2 finishes it, back to T1 for S2…), and each section's finishing goes back for anything an earlier section couldn't reach while the bar beyond it was still there, or, with Finish each section before the next unticked, once from the face end to the chuck after all the roughing. T1 not ticked and no other tool ticked (e.g. a T2 added before the Finishing column, whose box comes up unticked): the other tools finish anyway, not T1; only with no other turning tool does T1 finish, with a warning. Tools not ticked only rough, leaving the allowance everywhere: they never finish. A new tool starts ticked. A tool picked by hand in the Tool column of the passes table overrides the tick boxes for that pass; changing a Finishing tick box lets go of any tools picked by hand for the finishing passes. With T1 not ticked and a finishing cut depth of 0, T1 would rough right down to size, so a warning says so. Whenever T1 isn't ticked but still makes a finishing pass, a warning gives the pass number and why (picked by hand, or no other turning tool).
• All the tools at their offsets (under Additional tools, shown with more than one tool, not folded away): a picture with T1 and every other tool drawn on top of each other, each where it sits when fitted, its zero point (dot, labelled T1, T2…) at its offset from T1's (the cross hairs), one colour each. A check that the offsets look right: a tool far from where you'd expect it has a wrong offset (or a sign the wrong way). A tool with no offset in the library isn't drawn, and the caption says so.
• Tool offset library (folded away: click Show the library to open it; it stays as you left it, and opens by itself when T1 has no offset): every tool in the drop-down, with a thumbnail of its tip (red dot = zero point), its nose radius (empty = as drawn, shown faint; for the round inserts, SRAPR and SRAPR at 90°, the insert radius, so another insert size can be set: the holder is drawn scaled with it) and its offset from T1 (X + toward the face, Y + toward the back). Each tool's offset is stored once, so a tool keeps it whenever it is used as T2, T3… (typing an offset against T2 fills in the library too). To zero the controller on a different tool, do the test pieces with it and pick it as T1: every other tool's offset, and the drill's and the rear tool's, is worked out again from it. If the new T1 has no offset in the library yet, the others can't be worked out: pick the old T1, enter the new one's offset, then pick it again, or use Start again with T1 as the zero. Leave a box empty for a tool that hasn't been measured. With more than one holder of the same type, pick the type under the table and Add to the library: it is listed as #2, #3… with its own offset, in the T1 and T2… drop-downs too. ✕ deletes any tool (and its offset) from the library and the drop-downs, except T1 and the additional tools in use; Add to the library with its type brings it back, unmeasured.
• Drill (optional): the drill is not driven (the work turns), so it only drills on the centre line. Tick Drill a hole on the centre line. The table holds every drill you have, each set up once with its own diameter and offsets: where its tip sits from T1's zero point when it is in the drill chuck in the tool post (X + toward the face, Y + toward the back; X usually minus, Y about +14). Add a drill adds one; ✕ removes it. Tick Use on the drills for this hole: with more than one, the smaller ones go first (pilot drills), each to the same depth, each a tool change at safe (M0 to fit it, DRILL 1 OF 2 …, and a second M0 to confirm). Feed and Peck left empty are the ones recommended for the material in card 3 (shown greyed in the box, and in the line under the table): each drill at its own spindle speed, which its M0 gives (SPINDLE 800 RPM): set it then. Pecks are halved once the hole is deeper than 3 × Ø. Type a feed or peck to use your own. Then the depth from the face (to the tip, or to the full diameter), whether to come right out after each peck (to clear chips and oil it) or back off only, Come out to (how far in front of the face the tip comes out, default 3 mm, room for the brush) and Pause out of the hole (seconds, default 2; 0 = none): after each peck the drill waits there (G4) so you can brush the flutes clean and load them with oil before it goes back in. And whether to drill before (default) or after the turning. Each drill goes to safe relative to itself: its tip at Safe X and Safe Y, so it is always in front of the face, and the changes to and from it use the safer of its and the tool before's safe positions. It stays at safe X while it moves onto the centre line, then comes in along X; afterwards it backs straight out to safe X before moving in Y. Back to the turning tool, the M0 gives the turning speed again. The hole shows in the preview as it is drilled, each drill's in turn. The depth comes from the drawing: importing a drawing with a bore fills in the depth (to the full diameter): to the bottom of a blind bore, so the boring bar has a hole all the way down (the drill point goes a little further, into the bottom: the line under the box says how much), or 1 mm past the end of the part when the bore goes right through. Change it if you want; Use the drawing's depth puts it back. Each drill can have its own depth (the Depth column). Left empty it goes to the hole depth, except a drill bigger than a step in the drawing's bore: it stops where its point meets the step (the greyed figure), so the step is left for the boring bar to finish. A drill wider than the bore at the face says so. Type a depth to use your own.
• Dish in the end face (face recess): draw it like a bore, the inner line from the face to the centre. Add SRAPR 1616 H10 at 90° in Additional tools (the round insert with its shank turned toward the face), with its offset in the library: zero X on the insert's end (chuck side), Y on the insert centre. With no hole to bore from it cuts the dish: roughing down a cut depth at a time, plunging near the rim and feeding in to the centre, then a finishing pass from the rim to the centre. It only moves in Y in front of the face and goes in and out along X. A warning says if the insert and holder can't reach the bottom. The face can be drawn just inside X0 (a rounded rim). Without the SRAPR at 90°, T1 cuts the recess across the face like a facing cut (its nose centre going to the centre line) only if its outline can follow all of it, i.e. a very shallow recess. Otherwise a warning says how much T1 would leave and where, and the recess is not cut: ordinary turning tools can't get down a dish with steep sides (the cabinet knob's dish needs the SRAPR at 90°).
• Boring (with a bore in the drawing): tick Drill and add a boring bar (S12M-SCLCR09 with CCMT 09T304, or S12M / S10K / S08K / S07K-SCLCR06 with CCMT 06 02 04, or S12M-SDUCR07 with DCMT 07 02 04 (its 55° insert follows steeper tapers in the bore); the first one in the list bores; their pictures show a stub of the bar) as T2, T3… in Additional tools, with its offset in the library like any tool (length zeroed on the 9 o'clock point of the nose, diameter on the bore wall). The drill makes the hole, then the bar opens it out to the drawing: roughing outward from the hole one cut depth at a time, leaving the finishing allowance, then a finishing pass along the bore, its steps and the bottom, with the nose radius allowed for. The bar only moves in Y in front of the face, goes in and out of the hole along X, and backs off toward the centre line after each cut. The hole is drilled and bored first, while the part is still full size and stiffest, then T1 is fitted again for the outside turning; the rear tool comes last. With a bore, Drill after the turning is ignored (with a warning). The drill must reach the bottom of the bore at full diameter, or the program is refused. Warnings say if the hole is smaller than the bar's smallest bore or the bar would rub. The passes show as Bore rough / Bore finish. T1 can't be the boring bar.
• Rear parting-off / grooving tool (optional): tick Use the rear tool and give the offset from the front tool's zero point to the parting tool's datum (the corner of its cutting edge on the face nearest the chuck): X + toward the face, Y + toward the back. Also the blade width, feed and peck distance, and Extend past centre line: how far a part-off goes beyond the centre (mm on the radius, e.g. 0.5) so it leaves no pip (0 = to the centre; grooves are not affected). Each row of the table is one plunge: the finished size (X0 to the blade's other face; empty = the end of the part) and the finish Ø (0 = part off, more = a groove). Cuts are made in order from the face after the turning, each pecking in from just above the turned surface. With Stop (M0) at safe before the rear tool cuts ticked (the default) it waits at safe first. A part-off inside the finished part is allowed, with a warning. With a part-off at the end of the part, the last diameter is turned on through the blade's width, so the turning tool's nose radius is parted away rather than left on the part.

4 Feeds and speeds

Card 3 recommends a spindle speed, feeds and cut depths from the usual published tables for carbide inserts (HSS for the drill), at the gentle end for a manual lathe. There's no flood coolant (cutting oil is brushed on with the swarf brush), so the metals run slower than the flood-coolant tables; acetal and brass cut dry. Its summary gives the material, speed and feeds when folded.

• Material: acetal, aluminium HE30, mild steel, silver steel, stainless steel 304 or 316, titanium, copper or brass. A note under the table gives tips for it (lubricant, insert type).
• Cut slider: from a lighter cut (shallower, slower feed, better finish) to a more aggressive one (deeper, faster).
• Lowest / highest spindle speed: your lathe's range. The recommended speed is the roughing speed on the full blank, kept inside it; if the top speed holds it back, the feeds follow the slower speed.
• Spindle speed you'll set: leave it empty to use the recommended speed, or type the speed you'll dial in and the feeds (mm/min) are worked out from it. Use the recommended speed empties it again.
• The table gives feed per rev and feed in mm/min for roughing, finishing and plunging/grooving, with the first and last roughing depths and the finishing allowance, plus advice for the drill and the rear tool when they are on (set those in card 2). The smallest nose radius of the tools in use sets the feeds (the finishing feed is what that radius can finish smoothly), the smallest insert the deepest cut, and work sticking out more than 3 × its average diameter gets lighter roughing.
• These look right: put them in card 4: ticked, the depths and feeds go into the Cutting card (and the passes) and follow any change you make here, and the spindle speed is written as a comment at the top of the G-code ((SPINDLE 1660 RPM MILD STEEL …)); the machine never gets an S word. Change a depth or feed in card 4 yourself and the box unticks, so your figure stands.

5 Cutting and setup

The Cutting card folds away under Show the cutting settings (…), which still gives the cut depths, feeds and sections; the Program setup card likewise under Show the program setup (…) (safe position, name, file type), with any errors still shown below it. Each stays as you left it.

• First cut depth and Last cut depth before finishing (on the radius): the roughing cuts get lighter in a straight line from the first to the last, so the part is cut more gently as it gets thinner (no cut deeper than asked; leave the last empty for equal cuts). Finishing cut depth: what's left for the finish pass.
• Feeds in mm/min (each pass can be changed later). Back-off: how far the tool comes straight out after a cut.
• Sections (optional): distances from X0 in mm, e.g. 15, 30. The part is roughed and finished from X0 to X-15 first, then to X-30, then the rest, so the bar stays at full size near the chuck while the far end is cut. Each section ends at safe with an M0 to clear swarf (untick Safe + M0 in the passes table if not wanted). The planes show as dashed purple lines marked S1, S2… in the preview.
• Finish each section before the next (ticked by default): each section gets its own finishing cut before the next one is roughed. If a different tool finishes, that means a tool change in each section, which is fine. Unticked: the sections are only roughed, face end first, and then one finishing cut runs from the face end to the chuck in one go (Finish profile, face to chuck in the passes table).
• Finish the face end first (ticked by default): the app also splits the part at the top of every shoulder, where the diameter gets bigger toward the chuck. Each diameter is roughed and finished before the next one is started, with the bar behind it still full size. These splits have no M0. A shoulder within 2 mm of the face or the split before (e.g. an edge chamfer) is not split off, and a plane you type within 1 mm of a shoulder is used instead. It means more passes; untick it to rough the whole length first.
• Safe X / Safe Y: used at the start, for every stop and at the end. Y is negative and must be outside the blank.

6 Check the preview

The preview starts open; Hide the preview folds it away (its warnings stay in view, and Print still prints it). It stays as you left it.

• The blank in the chuck, with the finished part shaded and the tool paths on the front (lower) side.
• A part longer than the blank goes into the chuck: it is only turned up to the approach clearance from the chuck face, and no tool goes into the chuck (a warning says so).
• A label in the top-left corner of the preview says which tool is in use at the playback position (T1, T2… with the insert and nose radius, the drill with its Ø, or the rear tool with its width).
• If the program can't be made yet (a missing offset, a drill deeper than the blank, …), the preview says why, in red over the view, instead of staying blank.
• On the left, Tools used lists every tool the program uses by number (T1, T2…, Drill, Rear) with a picture of the tip, the insert and nose radius (or the drill Ø / blade width).
• Print (top right of the preview) prints just the preview: file name and date, the tools used on the left, the view as it is zoomed now, the legend and the figures, on a white page even in dark mode.
• Grooves and part-offs are cut into the model as the playback reaches them. Only the tool in the tool post is drawn (T1, T2… or the drill: it holds one at a time); the rear parting tool, fixed on the saddle, is always drawn, faint when not cutting; a table under the preview sums up each tool's offset from T1 and the speed to set the spindle to for it (check it with the tachometer): drills that run at their own speed show it there. roughing · finishing, drawn where the nose radius touches the part (tick Finishing: G-code point to see the imaginary tip the G-code moves) · rapids (dashed) · M0 stop.
• Red shading: the tool can't reach there (a groove, or a recess too steep for the insert). Pick another tool, or leave it for grooving.
• ▶ plays it, ⏪ ⏩ jump between passes, the speed button cycles 1× 2× 5× 10× ½×. Scroll to zoom in on the point under the mouse, drag to pan, double-click to fit.

7 Passes

The table (and the buttons for ticked rows) folds away under Show the passes (…), which still gives the number of passes and stops; it stays as you left it.

• Change the feed of any pass.
• Tick Safe + M0 to stop after that pass: the tool goes to safe and waits so you can clear the swarf. Press cycle start to carry on.
• Tick several rows to set their feed or stops together. Click a row to jump the preview to it.

8 G-code and the machine

The program text folds away under Show the G-code (… lines); Copy and Download stay in view. It stays as you left it.

1. Copy or Download the program. Loading a file fills File name (card 5) with the file name plus _LP (lathe path), e.g. Test4_LP, so the download is Test4_LP.nc. Change the name there if you want another (it only names the file, not the G-code header); the next file you load resets it. The first M0 asks you to fit and touch off the tool.
2. Face the end by hand: that face is X0 (the program has no facing pass).
3. Zero the tool to match Tool zeroed on (the first M0 repeats it). Nose quadrants: run a test piece; zero length on the face from the 9 o'clock point of the nose (12 o'clock for SCMCN and SDNCN) (X0) and diameter from the 12 o'clock point (Y = minus half the measured diameter, e.g. Ø21.40 → Y-10.700). Nose radius centre: set X to +R on the face (e.g. X0.400) and Y to minus half the diameter minus R (Ø21.40, R0.4 → Y-11.100).
4. Dry-run clear of the work first, and watch the first pass.