# black and white Tool Nose Radius Compensation

Document Sample

```					   CNC Applications
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
corners.

This tangent point
finishes faces.

Theoretical sharp point                  This tangent point
is what we program.                    finishes diameters.
The Problem
excess material as shown here:

Excess Material Here
The Solution
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.

G Code             Application
G40       compensation.
Compensate for tool nose
G41       radius to the LEFT of the
programmed path.
Compensate for tool nose
G42       radius to the RIGHT of the
programmed path.
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.
Turning Nose
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

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.
Turning Nose
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
A G42 Example

We will program ONLY the
finish pass on this part
using G42 right tool nose
are given 800fpm cutting
speed and 0.006ipr feed.                            R0.375
0.25x45°

Ø2.500                           Ø1.500     Ø1.750

0.250
0.625
1.000
2.000
The Finish Pass
Program Codes             Action
%                         Program Start
O999
G20 G40 G99
G28 U0
G28 W0
T0303                     Load the V insert tool.
G54
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
M5
G28 U0
G28 W0
M30
%
The Final Pass