HEIDENHAIN iTNC 530 (340 422) ISO programming - Manual (Page 152)

152 5 Programming: Tools
5.3 T
o
o
l Compen
satio
n Contouring with radius compensation: G41 and G42
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
at right.
Entering radius compensation
Radius compensation is entered in a G01 block:
To select tool movement to the left of the contour,
select function G41, or
To select tool movement to the right of the contour,
select function G42, or
To select tool movement without radius
compensation or to cancel radius compensation,
select function G40.
To terminate the block, press the END key.
G42 The tool moves to the right of the programmed contour
G41 The tool moves to the left of the programmed contour
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).
Radius compensation does not take effect until the end of
the block in which it is first programmed.
You can also activate the radius compensation for
secondary axes in the working plane. Program the
secondary axes as well in each following block, since
otherwise the TNC will execute the radius compensation
in the principal axis again.
Whenever radius compensation is activated with G42/G41
or canceled with G40, the TNC 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.
X
Y
G41
X
Y
G42