FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
B–62764EN/01
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
245
Three–dimensional coordinate conversion can be applied to a desired
combination of three axes selected out of the basic three axes (X, Y, Z) and
their parallel axes. The three–dimensional coordinate system subjected
to three–dimensional coordinate conversion is determined by axis
addresses specified in the G68 block. If Xp, Yp, or Zp is not specified,
X, Y, or Z of the basic three axes is assumed. However, if the basic three
axes are not specified in parameter 1022, P/S alarm No. 048 occurs.
In a single G68 block, both a basic axis and a parallel axis cannot be
specified. If this is attempted, P/S alarm No.047 occurs.
(Example)
When U–axis, V–axis, and W–axis are parallel to the X–axis, Y–axis, and
Z–axis respectively
G68 X_ I_ J_ K_ R_ ; XYZ coordinate system
G68 U_V_ Z_ I_ J_ K_ R_ ; UVZ coordinate system
G68 W_ I_ J_ K_ R_ ; XYW coordinate system
Three–dimensional coordinate conversion can be executed twice. The
center of rotation of the second conversion must be specified with the axis
addresses specified for the first conversion. If the axis addresses of the
second conversion are different from the axis addresses of the first
conversion, the different axis addresses are ignored. An attempt to
execute three–dimensional coordinate conversion three or more times
causes P/S alarm No.5043.
A positive angular displacement R indicates a clockwise rotation along
the axis of rotation. Specify angular displacement R in 0.001 degrees
within the range of –360000 to 360000.
The following G codes can be specified in the three–dimensional
coordinate conversion mode:
G00 Positioning
G01 Linear interpolation
G02 Circular interpolation (clockwise)
G03 Circular interpolation (counterclockwise)
G04 Dwell
G10 Data setting
G17 Plane selection (XY)
G18 Plane selection (ZX)
G19 Plane selection (YZ)
G28 Reference position return
G29 Return from the reference position
G30 Return to the second, third, or fourth reference position
G40 Canceling cutter compensation
G41 Cutter compensation to the left
G42 Cutter compensation to the right
G43 Increasing tool length compensation
G44 Decreasing tool length compensation
G45 Increasing the tool offset
G46 Decreasing the tool offset
G47 Doubling the tool offset
G48 Halving the tool offset
G49 Canceling tool length compensation
G50.1 Canceling programmable mirror image
G51.1 Programmable mirror image
D Three basic axes and
their parallel axes
D Specifying the second
conversion
D Angular displacement R
D G codes that can be
specified

Leave a Reply

Your email address will not be published. Required fields are marked *