Login to enhance your online experience. Login or Create an Account

G80 - Cancel Modal Motion

Program: G80 to ensure no axis motion will occur, to terminate canned cycles etc. Note that it cancels the current G0, G1, G2 or G3 mode so this must be re-established for the next move that is requited. This particularly affects people adapting a CAM postprocessors from another machine as this behavior varies between different CNC controls.

It is an error if:

  • Axis words are programmed when G80 is active, unless a modal group 0 G-code is programmed which uses axis words.
  • G80 Example

    Last Updated Feb 28, 2011
    - Download G80 Code Example   

    (Sample Program G80EX17:)
    (Workpiece Size: X4, Y3, Z1)
    (Tool: Tool #5, 5/8" HSS Drill)
    (Tool Start Position: X0, Y0, Z1)

    N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block)
    N5 G90 G80 G20 (Canned cycle cancel)
    N10 M06 T5 G43 H5
    N15 M03 S1450
    N20 G00 X1.0 Y1.0
    N25 G81 Z-0.5 R0.125 F10.0
    N30 X2.0
    N35 X3.0
    N40 G80 G00 Z1.0 (Canned cycle cancel)
    N45 X0 Y0
    N50 M05
    N55 M30

  • All Machine Code Reference Examples

    Last Updated Sep 16, 2016
    - Download Machine Code Reference Examples