← AskMachinist · Guides · Calculator · 🔎 Search

Tool Nose Radius Compensation Basics

Guide · Updated October 28, 2026

A turning insert has a rounded nose, but most lathe programs are written for an imaginary sharp point where the X and Z touch-off lines meet. That point and the real cutting edge agree only on straight diameters and flat faces. On tapers, chamfers and arcs the radius leaves material or cuts too deep. Tool nose radius compensation (TNRC) on Fanuc-style controls uses G41 and G42 with a nose radius (R) and tip direction (T) in the offset page to correct the path. This guide covers the logic; always follow your control's manual for exact rules.

Need an exact reference size?

Build any gage block stack with the free Gage Block Calculator. Free, no login.

Step by step

Enter the radius: Put the insert nose radius in the R column of the geometry offset, for example 0.0313 in for a 1/32 in nose.
Enter the tip code: Put the imaginary tip direction in the T column, for example 3 for a typical OD turning tool.
Pick the side: G42 for OD turning toward the chuck, G41 for ID boring toward the chuck (tool right or left of the path as seen moving along it).
Start on a lead-in: Activate G41 or G42 on a linear move longer than the nose radius, clear of the part.
Profile: Program the finished part shape; the control offsets the path.
Cancel: G40 on a linear move away from the part.

Why it matters

On a straight diameter, the nose touches at its lowest X point, which lines up with the imaginary tip, so the size is right. On a face, it touches at its Z-most point, also right. On a 45° chamfer, the nose touches at a point halfway around the radius, so a path written for the imaginary tip leaves material.

Error on a 45° chamfer

Without compensation, the cut lands (√2 − 1) × r = 0.414 r inside the true chamfer, measured normal to it, which is 0.586 r along X or Z. For a 1/32 in (0.0313) nose, that is 0.0129 in normal, or 0.0183 in along each axis. For a 0.8 mm nose, 0.33 mm normal. Chamfers and tapers come out visibly short and arcs off size.

Tip direction codes

T0 or T9: tool center used as the reference point
T1 to T8: imaginary tip quadrant around the nose
T3: typical OD turning tool on a rear-turret, X-plus-up lathe
T2: typical ID boring bar on the same lathe
T8 and T6: tool pointing straight at X or Z, such as a grooving or button tool

Codes depend on control and machine orientation. Check the diagram in your control manual; a wrong T code shifts the whole profile.

Theoretical finish from nose radius and feed

0.004 ipr, 1/64 in (0.0156) nose: peak-to-valley 0.000128 in (128 µin)
0.006 ipr, 1/32 in nose: 0.000144 in (144 µin)
0.008 ipr, 1/32 in nose: 0.000256 in (256 µin)
0.010 ipr, 3/64 in (0.0469) nose: 0.000267 in (267 µin)
0.2 mm/rev, 0.8 mm nose: 6.25 µm

Peak-to-valley = f² ÷ (8 r). Ra is roughly one quarter of that. Bigger nose and lower feed give a better finish but more chatter risk and more radial force.

Worked example: turning a 30° taper

For a straight taper at angle θ from the Z axis, the uncompensated cut leaves r × (cos θ + sin θ − 1) normal to the surface. At θ = 30° with a 0.0313 in nose: 0.0313 × (0.866 + 0.500 − 1) = 0.0115 in normal, which is 0.0115 ÷ cos 30° = 0.0132 in in radius, or about 0.026 in oversize on diameter along the taper. With G42, R0.0313 and T3 the control removes that error; check both ends with a mic.

Common problems

Activating comp on an arc, a lead-in shorter than the radius, wrong T code, forgetting to update R when changing from a 1/64 to a 1/32 insert, and wearing the X offset to fix a taper that is really a TNRC error.

FAQ

What is G42 on a lathe?

Tool nose radius compensation with the tool on the right of the path, typical for OD turning.

What is G41 on a lathe?

Compensation with the tool on the left, typical for boring.

Where do I enter the nose radius?

In the R column of the tool geometry offset.

What is tip direction 3?

The common imaginary tip quadrant for an OD turning tool.

Do I need TNRC for straight turning?

No; it matters on tapers, chamfers and arcs.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your drawing, tool maker's data and your quality system.