Roughing on a lathe is repetitive by nature: take a cut, step over, take another, until the part is nearly to size. The Fanuc-style roughing cycles fold that whole sequence into one call. You describe the finished profile once, and the control plans every pass. G71 and G72 are the two main cycles, and they differ in exactly one idea: which axis the passes run along.
What does G71 do?
G71 is the stock removal in turning cycle. It strips the blank with repeated cuts parallel to the Z axis, stepping down in X after each pass, as the G71 rough turning references show. That motion suits the bread-and-butter lathe job described in any lathe overview: a shaft, a spindle, a long external profile, or a bore, where most of the metal comes off along the length of the part.
The modern two-line format packs the cycle into a handful of words:
G71 U2. R1. (2 mm depth per pass, 1 mm retract)
G71 P10 Q20 U0.4 W0.1 F0.25
N10 G00 X30. (profile start: X move only)
...profile blocks...
N20 G01 Z-60. (profile end)The second line points at the profile (P10 to Q20) and leaves 0.4 mm in X and 0.1 mm in Z for finishing.
What does G72 do differently?
G72 is the stock removal in facing cycle: identical idea, rotated 90 degrees. Its passes run parallel to the X axis, stepping along Z between cuts, per the stock-removal cycle guides. That fits a short, large-diameter part, a flange, a disc, a part whose profile mostly drops across the face, where facing strokes clear stock far faster than long turning passes would.
One detail separates the two in the program besides the code itself: the first profile block. In a G71 profile, the block at P approaches in X only; in a G72 profile it approaches in Z only. The approach axis announces the pass direction, and mixing them up is a common first-week alarm.
Which cycle should you pick?
Decide by where the stock is, then let the geometry confirm it:
G71 (turning) | G72 (facing) | |
|---|---|---|
| Passes run | Parallel to Z | Parallel to X |
| Steps between passes | In X | In Z |
| Best for | Shafts, long profiles, bores | Short large-diameter parts, flanges |
Profile start block at P | X move only | Z move only |
| Verdict | Default for most turned parts | Pick when the face carries the stock |
A concrete example: a 200 mm shaft turned from 50 mm bar is a G71 job, because nearly every gram of chips leaves along the length. A 120 mm diameter brake-disc blank only 20 mm thick flips the logic: the profile lives across the face, so G72 clears it with fewer, longer strokes.
How do the cycles finish the part?
Neither cycle cuts the final surface. Both leave the U and W allowances on the profile, and G70, the finishing cycle, replays the same P to Q blocks at finish feed and speed to bring the part to size. A third sibling, G73, repeats the profile in stepped offsets for blanks that already match the shape, like castings. The whole family works the same way the mill drilling cycles G81 and G83 do: one definition, automatic repetition, and a cancel or finish step at the end.
Because these are lathe cycles, the usual lathe setup discipline applies around them, including the spindle-speed clamp covered in G50 max spindle speed when constant surface speed is active for the finishing pass.
Bottom line
G71 roughs with passes along Z and suits shafts and long profiles; G72 roughs with passes along X and suits short, wide parts where the face carries the stock. Both read one P to Q profile, leave U and W allowances, and hand the surface to G70. Learn the pass-direction difference and the profile’s approach-axis rule, and the rest is filling in numbers. Locking those pairings in is what recall practice on the G-code practice hub does, and the broader lathe-versus-mill code map lives in how to remember lathe M-codes vs mill M-codes.
Sources
Frequently asked questions
What is the difference between G71 and G72 on a lathe?
The direction of the roughing passes. G71 cuts parallel to Z for shafts and long profiles; G72 cuts parallel to X for short, large-diameter facing work. Both repeat automatically until only the finishing allowance remains.
How do G71 and G72 know what shape to cut?
From the profile defined between the block numbers referenced by P and Q. The control plans the passes itself, leaves the U and W allowances, and G70 replays the profile as the finish pass.
When should you use G73 instead?
When the blank already matches the rough shape, such as a casting or forging. G73 repeats the profile in stepped offsets instead of slicing from solid, saving air cuts.
What is the best way to practice lathe cycles like G71 and G72?
Drill the cycle codes with active recall. A free app like G-Code Sprint quizzes G71, G72, and the other everyday codes and repeats whichever ones you miss.
G-Code Sprint is a study and practice tool only. Always follow your instructor, employer, machine manual, and shop safety procedures.