Originally Posted by
Superman
Cutter comp is usually standard on CNC machines
How do you know it is disabled ?
How are you programming it ?
G41 or G42 is used with a D(offset #) and must be implemented on a line move ( some machines can start/finish comp on an arc movement...)
programming example
G1 Z-1. F123.
G41 D1 X123.456 Y123.456 F123.
G3 X Y
...
G1 G40 X123.456 Y123.456
G0 Z1.
The value placed in the D# is dependant on what method you define the path ( the following methods should NOT be mixed together )
- in control - the path is where you want the edge of the cutter to run against ( normally the cutter radius is put into the D offset register ) ( a value smaller than the tool radius makes the cutter run closer to the part, larger value make the cutter stay further away)
- wear - the programmed path is already offset form the part by the tool radius, D# is set to zero if the cutter is the same as programmed, a -ive value makes the cutter run closer to the part, +ive value leaves more material )
normally, # is the tool number and is kept common for the length & radius callout......... ( some machines require a tool diameter to be input )
Some older Fanucs only have a Wear/Geometry offsets page...so...
...IMO.. the tool length register number should be kept the same as the tool number, and the D# stored (say 30 registers higher, depends on how many tools in your tool carousel )... reason is the Geom & Wear offsets are added together