Cutter Compensation
Mill & Lathe
TECH 4476
Tool Diameter: Ø0.750
Example
Example
(END HEADER)
G0 X-3.0 Y-0.625 Z1.0
G1 Z0.0 F10.0
X4.375
Y-4.375
X0.625
Y2.0
Z1.0
Now what happens if we use a different tool? Or we use a sharpened end mill?
Cutter Comp
Look ahead (concept)
G40 - Cutter comp cancel (Cancels G41&G42)
G41 - Comp Left
G42 - Comp Right
G43 - Tool Length Compensation
G49 - Cancels G43
Using G41
...
T08 (Tool Number)
G43 H08 (Length comp on, offset)
...
(END HEADER)
G0 X-2.0 Y-1.0 Z1.0
G1 Z0.0 F10.0
X-1.0 G41 D8 (COMP ON)
X4.0
Y-4.0
X1.0
Y1.0
Y2.0 G40 (COMP OFF)
Start
D8
NOT 0.750
Using G41
...
T08 (Tool Number)
G43 H08 (Length comp on, offset)
...
(END HEADER)
G0 X-2.0 Y-1.0 Z1.0
G1 Z0.0 F10.0
X-1.0 G41 D8 (COMP ON)
X4.0
Y-4.0
X1.0
Y1.0
Y2.0 G40 (COMP OFF)
Start
G41 or G42
Look Ahead
Number of look-ahead moves is limited.
Don’t use non-cutting moves in between motions where look ahead would be necessary.
G41 & G42
Takes a D address. If the D value is negative, compensation will be reversed.
Depending on the machine settings, D address can hold a radius or diameter value.
D is assigned in the offset register (screen)
Turning Cutter Comp On and Off
Should not happen while cutting.
Start position is uncompensated, end position is compensated.
Length of comp on move must long enough (usually at least a radius).
If the comp is turned on or off in a line with no X or Y move, it will not take effect until the next line with X/Y moves.
D0 has the effect of canceling comp.
Different Paths for Compensation around Corners
3 Methods for Z
First, the fastest and the worst:
What happens if you want to change tools?
3 Methods for Z
Second, a little better. Allows multiple tools
Now, you can use more tools!
But… What if you want to use another fixture?
We’ll talk about the right way later.
Lathe Offsets - X Dia
Lathe Offsets - Z Axis
Simple case...only one workpiece origin, but can be used for multiple tools.
Lathe Offsets - Z Axis
G54
T101
Tool
Nose
Radius
Imaginary Tool Tip
Straight Cuts
Compensation for the tool tip is not needed for straight cuts.
The imaginary tip follows the part exactly.
Angled & Curved Cuts
Now the part is cut incorrectly.
The imaginary tool tip is not on the actual surface of the part.
Need Tool Nose Compensation
Depends on how the tool is pointed.
Tool Nose Vectors/Tip Directions
Offsets Screen
Using Tool Nose Compensation
Program the actual part outline.
Add approach and depart moves.
Uses G41 and G42 as with mill.
G40 Cancels
Comp in canned cycles
Is sometimes ignored in canned cycles.
Automatic Tool Setting