HEIDENHAIN TNC 620 Programming Station, User Manual

Page: 255 / 695

Path contours

Cartesian coordinates
6.4
6
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
255
Rounded corners G25
The
G25
function rounds off contour corners.
The tool moves on an arc that is tangentially connected to both the
preceding and subsequent contour elements.
The rounding arc must be machinable with the called tool.
Rounding radius
: Enter the radius, and if
necessary:
Feed F
(effective only in the
G25
block)
Example NC blocks
N50 G01 X+10 Y+40 G41 F300 M3*
N60 G01 X+40 Y+25*
N70 G25 R5 F100*
N80 G01 X+10 Y+5*
In the preceding and subsequent contour elements,
both coordinates must lie in the plane of the
rounding arc. If you machine the contour without
tool-radius compensation, you must program both
coordinates in the plane.
The corner point is cut off by the rounding arc and is
not part of the contour.
A feed rate programmed in the
G25
block is effective
only in that
G25
block. After the
G25
block, the
previous feed rate becomes effective again.
You can also use an
G25
block for a tangential
contour approach.