HEIDENHAIN TNC 640 User Manual page 264

6
Contouring with radius compensation: G42 and G41
G42: The tool moves to the right of the programmed contour
G41: The tool moves to the left of the programmed contour
The tool center moves along the contour at a distance equal to the
radius. Right or left are to be understood as based on the direction
of tool movement along the workpiece contour.
Between two NC blocks with different radius
compensations G42 and G41 you must program at least
one traversing block in the working plane without radius
compensation (that is, with G40).
The control does not put radius compensation into effect
until the end of the block in which it is first programmed.
When radius compensation is activated with RR/RLG42/
G41 or canceled with G40 the control always positions
the tool perpendicular to the programmed starting or
end position. Position the tool at a sufficient distance
from the first or last contour point to prevent the
possibility of damaging the contour.
Entering radius compensation
Radius compensation is entered in a
coordinates of the target point and confirm your entry with the ENT
key.
Select tool movement to the left of the
programmed contour: Press the G41 soft key, or
Select tool movement to the right of the contour:
Press the G42 soft key, or
Select tool movement without radius
compensation or cancel radius compensation:
Select function G40
Terminate the block: Press the END key
264
G01 block. Enter the
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017
Tools | Tool compensation