Boring a blind hole on a CNC lathe: tooling, chips, cutting data and G-code
· ~7 min read
Boring a through hole is the easy case: chips fall out the far end, the bar exits on the other side, and you can see the depth. A blind hole is harder: the chips have nowhere to go, the bar works at a long overhang, and it has to stop exactly at depth. Let’s go step by step: preparation, tooling, chips, the bottom, cutting data, and how to get a ready program for a LinuxCNC lathe.
Contents
- Preparation: drilling before boring
- Boring bar and overhang
- Chips: the main problem in a blind hole
- The bottom and the bottom corner
- Cutting data and the finishing pass
- G-code: a real boring example
- Boring in Turn G-code
- Common mistakes
Preparation: drilling before boring
Boring starts with a drilled hole. Things to keep in mind:
- Drill diameter. The hole must be larger than the minimum bore the boring bar fits into, and leave stock for boring. Less stock means fewer passes, but you are closer to the drill’s irregularities. In practice people leave anywhere from 0.5 mm to a few millimetres per side.
- The drill point. A standard 118° drill leaves a cone at the bottom about 0.3 × D of the drill deep. For a 16 mm drill that is about 5 mm. If the bottom must be flat at a given depth, drill a little short and face the bottom with the boring bar, or allow for the cone in the drawing.
- Deep holes are drilled with chip breaking (pecking), or the drill packs up. LinuxCNC has the G83 and G73 cycles for that.
Boring bar and overhang
Overhang is what decides boring quality more than anything else. The further the bar sticks out of the holder relative to its diameter, the more it chatters. Rough guidelines:
| Bar | Approximate overhang limit |
|---|---|
| Steel | about 3-4 × bar diameter |
| Carbide | about 5-6 × bar diameter |
| Damped (anti-vibration) | up to 10 × diameter and more |
Hence the rule: use the thickest bar that fits the hole, and stick it out only as far as the depth needs, plus a little clearance.
Lead angle. For a blind hole with a flat bottom you need a bar with a 93-95° approach angle: it can reach the bottom and face it. A 75° bar leaves a step at the bottom.
Center height. The insert tip must be exactly on the spindle centerline. In boring it matters even more: if the tip is below center, the clearance face rubs the wall of a small bore.
Chips: the main problem in a blind hole
In a through hole chips leave on their own. In a blind hole they gather at the bottom, wrap around the bar, scratch the finished wall and can break the insert. What helps:
- An insert with a chipbreaker for your material and depth of cut: chips should break into short curls, not long strings.
- Coolant or compressed air aimed at the bottom. Ideally, a bar with through-coolant.
- Retracting after every pass. The bar reaches the bottom, backs away from the wall towards the axis and leaves the hole at rapid. The chips come out with it instead of piling up.
- Stopping to clean deep holes: sometimes it is easier to pause the program and blow the chips out than to ruin the wall.
The bottom and the bottom corner
- Corner radius. The insert nose radius (for example 0.4 or 0.8 mm) leaves the same radius in the corner between wall and bottom. If a part with a sharp edge goes into the hole, it needs a chamfer larger than that radius.
- Exact depth. The end Z of the pass sets the bore depth. Make sure the tool’s Z reference in the tool table matches the insert tip, or the bar will hit the bottom or stop short.
- A flat bottom is made with a separate facing pass using a 93-95° bar: from the wall to the center or the other way, at a light feed.
Cutting data and the finishing pass
- Speed and depth of cut are usually lower than for OD turning of the same material: the bar is longer and less rigid. Start from the insert catalogue and back off if you hear chatter.
- Spindle speed: G97 mode. The diameter changes little in boring, so G96 gains almost nothing (see G96 vs G97).
- Finishing allowance small, 0.1-0.3 mm per side: less bar deflection, more accurate size.
- A spring pass, a repeat pass at the same X, removes what the bar left behind due to deflection. Useful at long overhangs.
- Measuring: bore gauge or plug gauge. Bore the first part slightly undersize, measure, then correct.
G-code: a real boring example
An excerpt from a real Turn G-code program, no hand edits (comments translated to English): a Ø22 mm blank with a Ø10 mm hole is bored to Ø20 mm, 20 mm deep, Ø8 mm bar, 0.5 mm depth per pass per side, 0.2 mm allowance. Radius mode G8.
G21 G18 G90 G8 G40 G80 G94
G54
G97 S300 M3
G0 Z3.0000
G0 X0.0000
G0 X0.0000
(Roughing pass 1 of 10)
(Centre X1.5000; edge in X R5.5000 / Ø11.0000; part Z 0.0000 -> -20.0000; tool Z 0.0000 -> -20.0000)
G0 Z0.0000
G1 X1.5000 F40.0000
G1 Z-20.0000 F80.0000
G0 X0.0000
...
(Finish pass 1 of 1)
(Centre X6.0000; edge in X R10.0000 / Ø20.0000; part Z 0.0000 -> -20.0000; tool Z 0.0000 -> -20.0000)
G0 Z0.0000
G1 X6.0000 F40.0000
G1 Z-20.0000 F80.0000
G0 X0.0000
G0 Z25.0000
G0 X25.0000
M5
M30
How to read it:
- X in the program is the bar centre, and the cutting edge is further from the axis by the bar radius (4 mm). So X6 in the finishing pass puts the edge at R10, which is Ø20. The header comments of the program say the same.
- Every pass: approach the face, plunge in X, cut along Z to depth, retract to the axis (X0) and exit. That retract is exactly what a blind hole needs, so the bar does not drag on the wall on the way out and takes the chips with it.
- The full program with all passes is on the Boring cycle page.
Boring in Turn G-code
The Boring cycle in Turn G-code has been cut-tested on the author’s lathe. You do not write the program by hand, you fill in a form:
- the bore diameter after drilling and the final diameter;
- the bar diameter: the program takes it into account when it calculates X;
- the start and end Z: the end sets the depth of the blind hole;
- depth per pass, finishing allowance, plunge and turning feeds, separate finishing RPM.
The built-in 2D simulator shows every pass before the file reaches the machine: you can see whether the bar hits the bottom and whether the hole is big enough for the bar.
Common mistakes
- A thin bar at a long overhang. Chatter, a wavy wall, a tapered bore. Use the thickest bar that fits.
- Chips not cleared. Scratches on the wall, a broken insert. You need a chipbreaker, coolant or air, and a retract after every pass.
- A wrong Z reference. The bar hits the bottom and breaks the insert.
- Tip below center. The clearance face rubs the wall of a small bore.
- Drilling too deep. The drill cone goes past the bore depth and the bottom is not flat.
- Not retracting to the axis. If the bar leaves the hole along the line it cut, it leaves a mark on the finished wall.
The full G- and M-code table is in the LinuxCNC G-code and M-code reference for lathes. Try it yourself: download Turn G-code - 15 days free, no key needed.
