Programming instructions

NC Programming 17VRS Tool Corrections
5-33
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Change in Direction of Compensation
A change in direction of compensation functions as if it were the removal
and then re-establishment of tool path compensation.
[Ps0]
[Ps1]
R
R
[Pe0]
[Pe1]
Programmed
Linear Move
Traversed
Linear Move
R tool radius
[Pe0] programmed end point of the first contour
[Pe1] corrected end point of the first contour
[Ps0] programmed starting point of the second contour
[Ps1] corrected starting point of the second contour
Fig. 5-27: Change in direction of compensation
The change in direction of tool path compensation requires an additional
move in the working plane which is performed only in conjunction with a
programmed linear movement.
CAUTION
If an attempt is made to perform the tool path compen-
sation by means of a circular movement, an error mes-
sage will be issued:
“G41/G42 activated with circular interpola-
tion”
and the NC-program will terminate.
The conditions described in the Chapters „Establishing Tool Path
Compensation at the Contour Beginning“, page 5-29 and „Removing Tool
Path Compensation at the End of the Contour“, page 5-31 regarding the
possibility of violating the starting point and end point of the contour also
apply here.
5.5 Activating and Canceling Tool Path Compensation
Canceling Tool Path Compensation 'G40'
The function G40 is used to cancel an already active tool path compensa-
tion. With tool path compensation canceled the center point of the tool
travels on the programmed path.
If an active tool path compensation (G41 or G42) is canceled by a G41,
the next anticipated move is a linear move on the process plane. The axis
values of both main axis must be programmed in the NC-block so that the
tool path compensation can be removed.
•
G40 is the power-on state; it is modally active. G40 is canceled by G41
or G42.
•
G40 is automatically set after the controller has been powered on,
after an NC-program is loaded and after a BST, M02, M30, RET or
Control-Reset.