HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 200)

Programming: Tools
5.3 Tool compensation
5
200
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
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. See
figures.
Between two program 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 TNC does not put radius compensation into
effect until the end of the block in which it is first
programmed.
In the first block in which radius compensation is
activated with
G42/G41 or canceled with G40 the
TNC 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
G01
block. Enter the
coordinates of the target point and confirm your entry with ENT
Select tool movement to the left of the
programmed contour: Select function G41, or
Select tool movement to the right of the contour:
Select function G42, or
Select tool movement without radius
compensation or cancel radius compensation:
Select function G40
Terminate the block: Press the END key