CNC Lathe Programming Examples: A Working Set for Novices

• 1
  What these examples teach
• 2
  Example 1: Shaft with Shoulders, G71 and G70
• 3
  Example 2: External Thread, G76 Two-Block Format
• 4
  Example 3: Groove and Undercut with G75
• 5
  Example 4: Bored Hub with a Through Hole
• 6
  Example 5: Thin-Wall Sleeve, Light Cuts Only
• 7
  Which Cycle Fits Which Feature

The first of these CNC lathe programming examples is a stepped shaft in 6061-T6, Ø40 mm bar, three diameters and a chamfer at the front. Clamp on 25 mm of stock in a three-jaw chuck, face the front, and set Z0 at the finished face. This single decision fixes every other coordinate in the program.

Rough with G71 using 1.5 mm depth of cut per pass and 0.3 mm finish allowance on X and Z. A 0.8 mm corner radius insert handles the shoulders without chatter at 600–900 rpm in aluminum. Leave 0.2–0.5 mm radial stock for G70.

Finish with G70 and a 0.4 mm nose radius insert at 1,200–1,800 rpm, feed 0.08–0.12 mm/rev. For Ø40 mm aluminum, cutting speed of 200–350 m/min gives a clean surface around Ra 0.8–1.6 μm.

Check the shoulder runout on the first part with a dial indicator. If it drifts past 0.02 mm, the jaws are bell-mouthed or the bar was not seated. Fix the clamping before touching the offsets.

• 1
  StockØ40 mm 6061-T6 bar, 120 mm long
• 2
  ToolsCNMG roughing insert, DNMG finishing insert
• 3
  TargetØ30 / Ø25 / Ø20 mm, ±0.05 mm general

Thread turning trips up novices more than any other lathe operation. Take an M20 × 2.5 external thread in 1045 steel. Thread height for a 60° metric form is 0.6134 × pitch, so 1.53 mm of radial infeed. Split that across the first pass and the remaining passes.

In the two-block G76 format, the first block sets the number of spring passes, the chamfer amount, the thread angle and the minimum depth of cut. The second block carries the major diameter, the thread height, the first pass depth and the pitch. Keep the included angle at 60° for a standard metric form.

Load a full-form insert matched to a 2.5 mm pitch. A partial-profile insert works too, but you then have to control the crest diameter yourself.

Run the first thread at reduced speed and check with a ring gauge or thread micrometer. Pitch diameter, not the crest, decides whether the part passes. Adjust the X wear offset by the measured difference and rerun.

• 1
  Thread height0.6134 × pitch for 60° metric form
• 2
  First pass0.5–0.8 mm radial for steel
• 3
  Speed300–500 rpm in 1045 to limit flank load

A relief groove behind a shoulder looks simple and breaks tools anyway. On a Ø50 mm part with a 4 mm wide, 3 mm deep groove in 304 stainless, use a grooving insert narrower than the groove and step over with G75, or plunge once if the insert width matches.

Peck in 0.5–0.8 mm increments. Full-depth plunging in stainless work-hardens the floor and snaps the insert on the second pass. Coolant aimed at the cutting edge, not the part, keeps chips moving.

Feed rate for grooving sits lower than turning: 0.04–0.08 mm/rev. Feed too fast and the insert deflects, leaving a tapered floor that fails a depth check.

Deburr the groove edges in the program with a small chamfer pass. Hand deburring a groove 3 mm deep is slow, and a raised edge on a mating face causes assembly problems later.

• 1
  Step over≤ 70% of insert width
• 2
  Peck depth0.5–0.8 mm in stainless
• 3
  Speed120–200 m/min for 304

Now a hub with a Ø30 mm through bore, 40 mm deep, in 6061. Drill 28 mm first on the lathe, then bore to size with a boring bar. Drilling removes most of the material; boring fixes position and diameter.

Rough the bore in two passes at 0.5 mm radial depth and finish at 0.15–0.25 mm radial depth. A boring bar deflects more than an external tool, so keep the overhang under 4 × bar diameter.

Bore diameter tolerance of +0.02 / 0 mm suits most bearing seats. Measure with a bore gauge at three depths to catch taper from bar deflection.

If the bore comes out tapered, the bar is too long or the feed too high. Shorten the overhang, drop the feed, and rerun the finishing pass.

• 1
  DrillØ28 mm, 118° point, through
• 2
  Overhang≤ 4 × boring bar diameter
• 3
  Finish0.15–0.25 mm radial, 0.08 mm/rev

A sleeve with a 2 mm wall in 6061 or 316L is the case where good programs still fail. Cutting forces push the wall outward, and the finished part springs back oval. Light passes and support are the only real answers.

Rough with 0.5 mm depth of cut and leave 0.5 mm for finishing. Use a sharp, positive-rake insert. Dull edges raise radial force and ovality.

Finish in two passes at 0.15 mm radial depth and 0.06–0.10 mm/rev. Do not aim for one heavy finishing pass to save cycle time.

Check ovality with a micrometer at 0° and 90°. If it exceeds 0.03 mm, reduce depth of cut and add a spring pass at the same setting.

For walls under 1.5 mm, consider a soft-jaw or expanding mandrel setup instead of a three-jaw chuck. Clamping force, not the toolpath, is usually the limiting factor.

• 1
  Roughing0.5 mm depth, 0.15 mm/rev
• 2
  Finishing0.15 mm radial, 0.06–0.10 mm/rev
• 3
  ClampingSoft jaws or expanding mandrel below 1.5 mm wall