Fagor 8055 M - Cancellation of Tool Radius Compensation

Programming manual
CNC 8055
CNC 8055i
TOOL COMPENSATION
8.
·M· & ·EN· MODELS
SOFT: V02.2X
·137·
Tool radius compensation (G40, G41, G42)
8.1.3 Cancellation of tool radius compensation
Tool radius compensation is canceled by using function G40.
It should be remembered that canceling radius compensation (G40) can only be done in a block
in which a straight-line movement is programmed (G00 or G01).
If G40 is programmed while functions G02 or G03 are active, the CNC displays the corresponding
error message.
The following pages show different cases of canceling tool radius compensation, in which the
programmed path is represented by a solid line and the compensated path with a dotted line.
End of the compensation without programmed movement:
After cancelling the compensation, it could happen that the plane axes do not get involved in the
first motion block either because they have not been programmed or because the same point as
the tool position has been programmed or because a null incremental move has been programmed.
In this case, the compensation is canceled in the current tool position; depending on the last
movement executed in the plane, the tool moves to the end point without compensating the
programmed path.
· · ·
G90
G03 X-20 Y-20 I0 J-20
G91 G40 Y0
G01 X-20
· · ·
(X0 Y0)
Y
X
· · ·
G90
G01 X-30
G01 G40 X-30
G01 X25 Y-25
· · ·
(X0 Y0)
Y
X