Hurco winmax, Programming Manual

Page: 130 / 254

4 - 16 ISNC G Codes
704-0115-307
WinMax Lathe NC Programming
G09 - Exact Stop
G09 causes the axes to decelerate to zero velocity at the end of a block. Since G09 is
non-modal, you must program it in every block that requires the tool to come to a
complete stop.
Modal—No
Format
G09 X ____ Y ____ Z ____ (machine decelerates to stop at specified point.)
G10 - Data Setting (Work Offsets, Tool
Offsets, or Tool Geometry)
G10 used in conjunction with specific parameters provides the following data setting
functions:
Default—No
Modal—Yes
Cancels G11 - Data Setting Cancel (default)
Work Offsets
G10 L2 is used for setting work coordinate systems. One of six work coordinate systems
can be changed as shown below where P is used to select the external work zero point
offset value (P = 0), or one of the work coordinate systems (P = 1 to 6), and X, Y, Z is the
work zero point offset value of each axis.
For Work Offsets, absolute values (X, Y, Z) replace work offset values. Incremental values
(U, V, W) are added to the current work offset values.
Format—Work Offset
G10 L2 P0 or P1-6 X ____ Y ____ Z ____
G10 L2 P1-6 U ____ V ____ W ____
G09 is not used in conjunction with G00 - Rapid Traverse (default),
G01 - Linear Interpolation or G02/G03 - Clockwise/Counterclockwise
Arc commands.
G10 commands can not be performed by graphics at the same time
the program is running.