CNC programming and alarms
How does tool nose radius compensation work on a Fanuc-style lathe?
Fanuc-style CNC lathe controls: G41, G42 and G40, tip numbers, and manual offsets for tapers and chamfers.
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
Tool nose radius compensation (TNRC) makes a Fanuc-style lathe control move the insert's nose center one radius away from the programmed profile, so tapers, chamfers and arcs come out to the drawing. Turn it on with G42 (tool right of the path) or G41 (tool left), cancel it with G40, and set the nose radius R and tip number T on the offset page. Without TNRC, an OD taper at angle A comes out oversize by p = R x (sin A + cos A - 1), which the calculator below corrects by hand.
Source: FANUC lathe (T series) operator's manuals, tool nose radius compensation (G40, G41, G42); Machinery's Handbook (CNC programming, tool nose radius compensation); offset geometry derived on this page
Manual compensation for a taper or chamfer (OD tool, tip 3)
Z shift toward the chuck (dZ)
in
dZ = R x (1 - tan(A / 2)) = 0.03125 x (1 - tan(45 / 2)) = 0.0183 in
0.465 mm.
X shift on diameter, smaller (dX)
in
dX = 2 x R x (1 - tan(45 - A / 2)) = 2 x 0.03125 x (1 - tan(45 - 45 / 2)) = 0.0366 in
0.930 mm. Error without compensation, square to the taper: p = R x (sin(A) + cos(A) - 1) = 0.03125 x (sin(45) + cos(45) - 1) = 0.0129 in. Corrected points: start X0.8634 Z0, end X1.0000 Z-0.0683.
The calculator covers an OD taper or chamfer that grows in diameter toward the chuck, cut with a tip 3 tool, X in diameter. For an ID chamfer at a bore entrance with a tip 2 boring bar, the amounts are the same and the X shift goes to a larger diameter.
G41, G42 and G40 on a Fanuc lathe
| Code | What it does | Typical use, rear-turret lathe cutting toward the chuck |
|---|---|---|
| G40 | Cancels compensation | On the move away from the part, and at the start of every program |
| G41 | Tool on the left of the path, looking along the direction of travel | ID boring |
| G42 | Tool on the right of the path, looking along the direction of travel | OD turning |
- Set the nose radius in the R column and the tip number in the T column of the tool offset page, on the same offset number the program calls.
- Tip 3 is the usual OD turning tool and tip 2 the usual boring bar. The tip number tells the control which corner of the nose the X and Z offsets were touched off to. Tip 0 or 9 means the programmed point is the nose center. The diagram for tips 1 to 8 is in your control's manual; it changes with front and rear turret machines.
- Turn compensation on during a linear move (G00 or G01) at least one nose radius long, before the tool touches the part. Never start or cancel it on an arc.
- Cancel with G40 on a linear move away from the part.
N10 G00 X0.8 Z0.1
N20 G42 G01 X0.9 Z0. F0.005 (COMP ON, LEAD-IN MOVE)
N30 X1.0 Z-0.05 (0.050 X 45 DEG CHAMFER, DRAWING NUMBERS)
N40 Z-1.0
N50 G40 G00 X1.2 (COMP OFF, MOVING AWAY)With G42 active you program the drawing: X0.9 Z0 to X1.0 Z-0.05 on diameter, in inches. F0.005 is a placeholder feed of 0.005 IPR (inches per revolution). Without TNRC, the same chamfer takes the corrected points from the calculator: X0.8634 Z0 to X1.0 Z-0.0683.
Why tapers and arcs cut wrong without compensation
You touch off X and Z to the imaginary tip: the corner where the X and Z edges of the nose would meet if the insert were sharp. On a straight Z move or a face, the nose touches the part on those same lines, so the size comes out right. On a taper or an arc, the nose touches somewhere between them, and the imaginary tip is out in the air. The result is extra material on an OD taper or chamfer (oversize) and a profile error on arcs that is zero where the arc runs parallel to Z or X and largest at 45 degrees, 0.4142 x R.
Derivation of the manual offsets
- Put the nose center at C. With tip 3, the imaginary tip T sits R toward the chuck (minus Z) and R toward the centerline (minus X) from C: T = C - (R, R), with X as a radius.
- The taper makes angle A with the Z axis and grows in diameter toward the chuck. The unit normal pointing out of the metal is n = (sin A, cos A) in (Z, X).
- The nose touches the taper where that normal passes through C. The tangent point is C - R x n, which is R x (1 - sin A) along Z and R x (1 - cos A) along X from the imaginary tip. For 45 degrees that is 0.2929 x R on each axis.
- Program T on the taper line and C sits at T + (R, R). Its distance from the line is R x (sin A + cos A). Subtract the nose radius: the cut stands off the line by p = R x (sin A + cos A - 1). That is the material left on.
- Move the programmed line into the metal by p. A shift along Z alone moves the line square to itself by dZ x sin A, so dZ = p / sin A = R x (1 - tan(A / 2)). A shift along X alone does it by (radius) x cos A, so the radial shift is p / cos A = R x (1 - tan(45 - A / 2)), and dX on diameter is twice that.
Manual compensation, OD taper, tip 3
dZ = R x (1 - tan(A / 2)); dX = 2 x R x (1 - tan(45 - A / 2))
| Symbol | Meaning | Unit |
|---|---|---|
| dZ | Move the taper end toward the chuck by this amount | in or mm |
| dX | Move the taper start on the face to a smaller diameter by this amount (diameter value) | in or mm |
| p | Material left on without compensation, square to the taper: R x (sin A + cos A - 1) | in or mm |
| R | Insert nose radius | in or mm |
| A | Taper angle from the Z axis, in degrees; tan(45 - A / 2) is also in degrees | deg |
Checks
| Angle A (deg) | p | dZ | dX (radius) | Meaning |
|---|---|---|---|---|
| 0 | R x (0 + 1 - 1) = 0 | not used | R x (1 - tan 45) = 0 | Straight Z move: no correction |
| 45 | R x (0.7071 + 0.7071 - 1) = 0.4142 x R | R x (1 - tan 22.5) = 0.5858 x R | R x (1 - tan 22.5) = 0.5858 x R | 45 degree chamfer: same shift on both axes |
| 90 | R x (1 + 0 - 1) = 0 | R x (1 - tan 45) = 0 | not used | Face: no correction |
Worked example: 0.050 in x 45 degree chamfer, 1/32 in nose radius
Chamfer 0.050 in x 45 degrees on a 1.000 in diameter, face at Z0, R = 1/32 in = 0.03125 in, OD tool, tip 3, no TNRC.
- Drawing points: start X0.900 Z0 on the face, end X1.000 Z-0.050 on the diameter.
- Material left without compensation: p = 0.03125 x (0.7071 + 0.7071 - 1) = 0.0129 in.
- Z shift: dZ = 0.03125 x (1 - tan 22.5) = 0.03125 x 0.5858 = 0.0183 in.
- X shift on diameter: dX = 2 x 0.03125 x 0.5858 = 0.0366 in.
- Start point: X = 0.900 - 0.0366 = 0.8634 in, Z0.
- End point: Z = -0.050 - 0.0183 = -0.0683 in, X1.000.
Result: program G01 X0.8634 Z0, then X1.0 Z-0.0683. That is a starting point; check the chamfer size on the part.
Worked example: 30 degree taper, 0.8 mm nose radius
Taper at 30 degrees from the Z axis, R = 0.8 mm, OD tool, tip 3, no TNRC.
- Material left without compensation: p = 0.8 x (0.5 + 0.8660 - 1) = 0.293 mm.
- Z shift: dZ = 0.8 x (1 - tan 15) = 0.8 x 0.7321 = 0.586 mm.
- X shift on diameter: dX = 2 x 0.8 x (1 - tan 30) = 2 x 0.8 x 0.4226 = 0.676 mm.
- Check: p / sin 30 = 0.2928 / 0.5 = 0.586 mm = dZ.
Result: move the taper end 0.586 mm toward the chuck and the taper start 0.676 mm smaller on diameter (0.0231 in and 0.0266 in).
Common mistakes
- R left at 0 or T left at 0 on the offset page. The control then compensates nothing, or compensates about the wrong corner.
- G41 and G42 swapped. The tool goes to the wrong side of the path and cuts into the part.
- Compensation turned on in the same block as the first cut, or on an arc. Give it a linear lead-in of at least one nose radius.
- Programming the corrected points and turning on G42 as well. Use one or the other, never both.
- Using this page's offsets for a back taper (diameter shrinking toward the chuck) with a tip 3 tool. The geometry is different; use TNRC or CAM output.
FAQ
How much does a 45 degree chamfer cut off without nose radius compensation?
The nose leaves p = R x (sin 45 + cos 45 - 1) = 0.4142 x R of material, measured square to the chamfer. With a 1/32 in (0.03125 in) nose radius that is 0.0129 in. To correct it by hand, move the chamfer 0.5858 x R = 0.0183 in along each axis.
Do you need tool nose radius compensation for straight turning and facing?
No. At A = 0 degrees (a straight Z move) and A = 90 degrees (a face), p = 0. The nose touches at the same X and Z lines as the imaginary tip, so the part comes out to size.
Is it G41 or G42 for OD turning on a lathe?
On a typical rear-turret (slant bed) lathe cutting toward the chuck, G42 for OD turning and G41 for ID boring. G41 puts the tool on the left of the path, G42 on the right, looking along the direction of travel. Confirm with the manual for your control.
What tip number does an OD turning tool use on a Fanuc lathe?
Tip 3 for a typical OD turning tool cutting toward the chuck, and tip 2 for a typical boring bar. Tip 0 or 9 means the programmed point is the nose center. Enter the tip in the T column and the nose radius in the R column of the tool offset page.
How long does the lead-in move need to be?
At least the nose radius, and it must be a linear move (G00 or G01), not an arc. Cancel with G40 on a linear move away from the part.
Last updated