Hurco winmax, Programming Manual, Page: 148 / 254

4 - 34 ISNC G Codes
704-0115-307
WinMax Lathe NC Programming
G53 - Machine Coordinates
This one-shot usage code causes the part program to ignore the following offsets for one
block so you can program the axes to a position that you define using machine
coordinates:
• active work coordinate offsets (G50 - Set Part Setup or Set Max RPM, G92 -
Work Coordinate Offsets / Spindle Max Speed / Multiple Thread Cutting
Cycle)
• active tool offset
• active fixture offset
Default—No
Modal—Yes
Cancels:
• G54-G59 - Work Coordinates (G54 default)
• G54.1 - G54.93 - Aux Work Coordinates
• G92 - Work Coordinate Offsets / Spindle Max Speed / Multiple Thread Cutting
Cycle
Before you program G53 in a block, the program must meet the following conditions:
• G40 - Cutter Radius Compensation Off (default) must be active.
• G90 - Absolute Programming (default) must be active if using X instead of U.
• Either G00 - Rapid Traverse (default) or G01 - Linear Interpolation mode
must be active.
Format
G53 X(u) ____ Y(v) ____ Z(w) ____
Example
N10 G90 G00 Z0 X0 (Absolute Mode)
N30 G53 Z2 X1 (Move to X1 Z2)
• X indicates Absolute X and (u) indicates Incremental X.
• Y indicates Absolute Y and (v) indicates Incremental Y.
• Z indicates Absolute Z and (w) indicates Incremental Z.
When the N30 block is finished, the machine will return to the G90 -
Absolute Programming (default) mode.