M-Series Operator’s Manual 4/9/15
G29 - Return from Reference Point
G29 moves all axes to the intermediate point stored in a preceding G28 or G30 command. It may be used to return
to the work piece. If a position is specified, the machine will move to that position (in local coordinates) after
reaching the intermediate point. G29 may only be specified after G28 or G30, though there may be intervening
moves.
Examples:
G29 ; move all axes back from reference point to intermediate
; point
G29 X1 Y2 ; move all axes to intermediate point, then move to X1 Y2
* NOTE: As with G0 positioning moves, the Z-axis will move separately. If Z is moving up, Z will move first, then
the other axes. If Z is moving down (the usual case for G29), the other axes will move first, then Z will move.
G30 - Return to Secondary Reference Point
G30 functions exactly like G28, except that by default it uses the second reference point from the Work Coordinate
System Configuration table, and the P parameter may be used to request either reference point.
Examples:
G30 G91 Z0 ; move Z axis directly to second reference point
G30 P1 ; move all axes to first reference point
NOTE: G30 P1 is equivalent to G28.
G40, G41, G42 -Cutter Compensation
G41 and G42 in conjunction with the selected tool diameter (D code) apply cutter compensation to the programmed
tool path.
G41 offsets the cutter tool one half of the tool diameter selected with a D code, to the left of the work piece, relative
to the direction of travel.
G42 offsets the cutter tool one half of the tool diameter selected with a D code, to the right of the work piece,
relative to the direction of travel.
G40 cancels G41 and G42.
Example:
G41 D03 ; Tells the machine to compensate left half of the
; diameter of the amount that corresponds to D03 in the
; Tool Library
To Next Page
Loading...
