HEIDENHAIN TNC 620 Programming Station, User Manual

Page: 222 / 695

Tools
5.3 Tool compensation
5
222
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
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 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 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