Rough Machining Cycle of Lathe G71 G72: Symptoms, Causes, Fixes

• 1
  G71 and G72 alarm symptoms, causes and fixes
• 2
  Why the rough machining cycle of lathe G71 G72 refuses a profile
• 3
  When the cycle of lathe G71 G72 is the wrong choice
• 4
  Stock allowance, depth of cut, and the numbers behind the alarm
• 5
  Building a clean profile between P and Q
• 6
  How to clear the alarm and finish the part

G71 and G72 are stock removal cycles. The controller reads the finished profile you describe between the P and Q block numbers, then cuts it in parallel passes from the outside in. For that to work, the controller has to know which side of the profile is still raw material. On a simple turned shaft, every X value either rises or falls as Z moves. There is only one answer, so the cycle runs.

Add a groove, an undercut, or a step behind a shoulder and the X value changes direction. Now two points on the profile share the same Z value, and the controller cannot decide which one is the boundary of the stock. The alarm text varies by builder, but it always means the same thing: the profile is not monotonic in the cutting direction.

The fix is never to delete the alarm. You either change how the cycle is called, split the profile into two cycles, or use a cycle that allows non-monotonic motion. Which one you pick depends on the shape, the tool, and how much stock you are removing.

One more thing worth checking before you edit anything. A surprising share of these alarms come from a mistyped arc direction, a G02 where a G03 belongs, which creates a tiny reversal the eye cannot see on the drawing. Run a dry cycle with the tool clear and watch the position display.

• 1
  MonotonicX moves one way only across the profile. Standard G71 or G72 handles it.
• 2
  Non-monotonicX reverses at least once. You need type II or a split profile.
• 3
  Diameter valuesU and W are usually diameters on a lathe, so a 1 mm radial cut is U 2.0.

G71 removes stock along Z, so it suits shafts, bushings, and any part where the profile grows or shrinks from one end to the other. G72 removes stock along X, so it suits face work and short parts where the diameter changes faster than the length. Picking the wrong one is not fatal, but it doubles cycle time and loads the tool on the wrong flank.

Neither cycle likes deep narrow grooves. If the groove is wider than the insert and deeper than about twice the nose radius, cut it with a separate grooving cycle after roughing. Trying to fold it into the G71 profile is the single most common reason shops keep hitting the monotonic alarm on parts that look simple on paper.

Type II G71, sometimes written G71 with a negative U, allows a concave profile. It still needs a clear entry and exit, and it does not accept a profile that doubles back on itself in Z. If your part has a back-facing shoulder, split the operation.

For thin-wall parts, both cycles can distort the bore. Take lighter passes and leave more stock for the finish pass so the last cut removes a consistent chip load.

• 1
  Shafts and bushingsG71 along Z with a monotonic profile.
• 2
  Face and plate workG72 along X, short Z depth.
• 3
  Grooves and undercutsRough with G71, then a dedicated groove cycle.
• 4
  Concave profilesType II G71 or split into two monotonic segments.

U in the G71 or G72 call block is the finish allowance left on the diameter. U 0.4 mm leaves 0.2 mm of radial stock, which is enough for a clean finish pass on most steels. On aluminium, U 0.3 mm is usually plenty. Leaving 1 mm or more means the finish pass has to remove a heavy chip, and the insert will not hold the tolerance.

The first depth of cut is set by the cycle parameters, often labelled as the roughing depth or the first pass. Keep it at or below 60 percent of the insert nose width. On a 3 mm wide insert, that is about 1.8 mm per side. Deeper than that and the tool deflects, the profile drifts, and the cycle can trip a torque alarm before it reaches the groove.

W is the Z finish allowance. For a part with a shoulder, leave 0.1 to 0.2 mm so the finish pass can clean the face without rubbing. Too little and the tool skims; too much and you lose the benefit of the roughing cycle.

Feed and speed come from the insert maker, not from the cycle. But remember that a canned cycle runs at constant feed across the whole profile, so the surface speed changes with diameter. On a part that spans a wide diameter range, a constant surface speed mode gives a more even finish and less tool wear.

• 1
  U allowance0.3-0.5 mm on diameter for steel, less for aluminium.
• 2
  First pass depthUp to 60 percent of nose width, not more.
• 3
  W allowance0.1-0.2 mm on the face and shoulder.

The P and Q block numbers are line numbers, and they must sit on the first and last blocks of the profile you want to cut. If Q points at a block that also contains a tool change or a rapid move, the controller tries to include that motion in the profile and the geometry no longer makes sense. Number the profile blocks, keep them contiguous, and end Q on the last profile move.

Every block inside the P to Q range should contain a real cutting move. Comments, spindle commands, and coolant calls inside that range confuse some controllers. Put them outside.

The profile must start and end at a point the tool can actually reach. A common mistake is to close the profile with a move back to the start point, which creates a closed loop and a reversal the cycle cannot rough. Finish the profile where the part ends.

If the part needs a chamfer or radius at the end, include it in the profile, not in a separate block after Q. The finish pass G70 reads the same blocks, so anything outside the range is ignored.

• 1
  Contiguous blocksNo gaps, no tool changes inside P to Q.
• 2
  Open profileDo not close the loop back to the start point.
• 3
  Chamfers and radiiKeep them inside the profile range.