Tool Nose Radius Compensation
on Turning Centers
Facing and Straight Turning
• When facing or straight turning, the tool nose radius has
no effect on the part other than leaving a radius on inside
This tangent point
Theoretical sharp point This tangent point
is what we program. finishes diameters.
When turning tapers or radii, the tool nose radius leaves
excess material as shown here:
Excess Material Here
1. Manually program the exact tangent points. This is
time consuming since it requires trig calculations or
accurate CAD drawings to locate the tangent points.
2. Use tool nose radius compensation. The tool nose
radius is entered into the machine controller, and the
program turns on compensation for finish cuts only,
and then turns it off. The machine calculates the
tangent points so we can continue programming as if
the cutter has a sharp point.
Tool Nose Radius G Codes
G Code Application
Cancel tool nose radius
Compensate for tool nose
G41 radius to the LEFT of the
Compensate for tool nose
G42 radius to the RIGHT of the
G41 & G42
G41 – the cutter is to the left of the G42 – the cutter is to the right of the
work when looking in the direction of work when looking in the direction of
the cut. the cut.
Radius Compensation On
To turn compensation on, the machine must move at least the distance of the
nose radius in X and Z. For easy calculations, back away from the start point 0.1
in Z and 0.2 in X. Remember X is diameter based, so 0.2 in X is actually 0.1
Turn Nose Radious Compensation
on in This Move. Compensation Point, 0.1 Away
From Start Point in Z, 0.2 in X.
Start Point of Finish Pass
with Compenation On,
0.1 Away in Z.
Radius Compensation Off
To turn compensation off, we feed the cutter
completely off the work and then make a move
larger than the nose radius while calling G40.
Note: Do not reverse the Z direction with nose
radius compensation on! The machine may get
confused, and then later cuts may be off by some Feed Moves Clear
multiple of the nose radius. Always call G40 of the Part.
BEFORE reversing the Z direction!
Feed Move to Turn
Nose Radius Compensation Off.
A G42 Example
We will program ONLY the
finish pass on this part
using G42 right tool nose
radius compensation. We
are given 800fpm cutting
speed and 0.006ipr feed. R0.375
Ø2.500 Ø1.500 Ø1.750
The Finish Pass
Program Codes Action
% Program Start
G20 G40 G99
T0303 Load the V insert tool.
G50 S4000 Cap the RPM.
G96 S800 M3 Set the cutting speed to 800fpm, forward direction.
G0 Z2.2 Rapid to the G42 start point in Z.
X1.0 M8 Rapid to the G42 start point in X, coolant on.
G42 G1 X0.8 Z2.1 F0.006 Move to turn nose radius compensation on, beginning of chamfer.
X1.5 Z1.75 Machine the chamfer.
Z1.0 Machine the straight 1.0” diameter.
X1.75 Z0.625 Machine the taper.
G2 X2.5 Z0.25 I0.375 Machine the radius.
Z-0.15 Feed clear in Z leaving room for the 0.125” parting tool.
X2.875 Feed clear in X.
G40 X3.075 Z-0.25 Move to turn off nose radius compensation.
M9 Program End
The Final Pass
Select this link to
start the animation.