Every lathe program contains a small lie: it positions a tool point that does not exist. The insert’s actual corner is a radius, a few tenths of a millimeter of curve, and the program’s theoretical sharp point sits where the radius’s tangents would meet. On straight diameters and square faces the lie is free, the contact point sits consistently on one tangent and everything measures right. The first taper or arc presents the bill: the contact point migrates around the radius as the cut angle changes, and the profile comes out wrong by up to the full nose radius. TNR compensation is the control correcting for the lie, and it needs three pieces of information to do it.
How big the lie actually is
Sizing the error keeps the topic honest: standard turning inserts carry nose radii from about 0.2 to 1.6 mm, with 0.4 and 0.8 the everyday workhorses, and the uncompensated profile error on an angled feature runs a meaningful fraction of that radius, growing with the angle. On a 45-degree chamfer with a 0.8 insert, the miss is measured in tenths of a millimeter, far outside most tolerance blocks, while a 2-degree taper with a 0.2 insert hides inside loose tolerances for years. That spread is why the problem presents as intermittent: it was always there, scaled by angle and radius, and the parts that revealed it were simply the first ones where the product of the two exceeded the print.
The three inputs comp needs
| Input | Where it lives | What it tells the control |
|---|---|---|
| G41 or G42 | The program, at profile entry | Which side of the path to offset toward |
| The nose radius | The tool offset table | How big the correction is |
| The orientation number | The tool offset table | Which way the insert’s nose points |
The side question follows milling’s rule, look along the travel direction, G41 offsets left, G42 right, with the lathe twist that turret position and cut direction combine: common outside turning toward the chuck on a rear-turret machine takes G42, boring typically flips to G41, and the milling-side intuition transfers once that twist is absorbed. The orientation number is the lathe-specific input: a digit from the standard 0-9 chart describing how the nose points relative to the axes, 3 for typical outside turning, 2 for typical boring, documented per the tool-table conventions, and entered per tool when the turret is set up. Wrong orientation makes the correction itself point wrong, comp confidently worsening the profile, which is why the number comes from the chart and the insert’s actual mounting, never from memory.
Where the uncompensated error actually shows
The error’s geography explains every mystery measurement: zero on straight diameters and faces (the tangent-contact cancellation), growing with angle on tapers and chamfers, maximal pain on arcs and full radii, where the contact point sweeps the whole nose. The signature is a part whose diameters measure perfect while its tapers run shallow and its radii measure off, the profile pulled toward wherever the theoretical point sat. Shops meet it as the seventeen-year mystery: decades of straight work uncompensated and fine, then the first profiled part from the same proven habits measures wrong, and the habits get blamed before the geometry does.
The lead-in discipline, inherited intact
Comp cannot engage instantaneously on the profile, the offset has to establish over a move, so the engagement and cancel rules arrive from milling unchanged: G41/G42 turn on during a lead-in move clear of the part, stay on through the profile, and cancel with G40 on a lead-out move after it, never mid-profile, never on the first cutting move. A mid-program restart inside a compensated profile inherits the same hazard milling restarts carry: re-entering with comp’s state half-built is how gouges happen, and the tool-change boundaries where comp is freshly established remain the gold-standard re-entry points.
Cycles complicate pleasantly: the G71-family roughing cycles handle comp per their own documented rules, some applying it through the profile description, and the per-control manual owns those specifics the way it owns every cycle detail.
The working summary
Comp on for any profile with angles or curves; G42 for common OD work toward the chuck, G41 for its mirrors, decided by the side rule; radius and orientation in the table from the insert’s reality; lead in, profile, lead out, cancel. The vocabulary is four codes and two table entries, recall material like the rest of the lathe family, drilled free in the 60-second rounds on the G-code practice page, and the payoff is the quiet kind: tapers that measure like the print, arcs that gauge clean, and one less seventeen-year mystery waiting in the shop’s future.
Sources
Frequently asked questions
What does tool nose radius compensation do on a lathe?
It corrects the gap between the theoretical sharp point programs position and the radius inserts cut with: harmless on straight work, the gap cuts tapers and arcs wrong by up to the nose radius. With G41/G42 active and the table carrying radius and orientation, the control offsets the path so the edge follows the profile.
When do I need G41 versus G42 on a lathe?
By the side rule, looking along the travel: G41 left, G42 right. Common outside turning toward the chuck on rear-turret machines takes G42; boring typically flips it.
What is the tool orientation number in the offset table?
A digit from the standard 0-9 chart describing which way the insert’s nose points, 3 for typical OD turning, 2 for typical boring. Wrong orientation makes comp correct in the wrong direction, so it comes from the chart and the mounting.
Do I need TNR comp on every lathe program?
On every profile with tapers, chamfers, or radii, practically yes. Straight-diameter work escapes by cancellation, which is why simple programs run fine uncompensated until the first profiled part measures wrong.