Article Contents
G89 Cycle Introduction
G89 cycle is used in CNC turning machines for boring holes from the side to the workpiece. It is the same as the G85 cycle as a command format, the only difference is that it is used for boring holes in the X axis direction, not in the Z axis direction.
After the command is used, boring to the other coordinates is continued by positioning the Z axis or C axis. The G89 cycle continues to run until the G80 command arrives.
G89 Cycle Format
| G89 X(U)_ R_ P_ F_ K_ M_ ; |
Parameters
| X_ or U_ : Final drilling depth (X for absolute, U for incremental) |
| R_ : The distance from the initial level to point R level |
| P_ : Dwell time at the bottom of a hole |
| F_ : Cutting feedrate |
| K_ : Number of repeats (When it is needed.) |
| M_ : M code for C-axis clamp (when it is needed.) |
After positioning, rapid traverse is performed to point R. Drilling is performed from point R to point X. After the tool reaches point X, it returns to point R at a feedrate twice the cutting feedrate.
| You may be interested also: |
| “CNC Lathe | G85 Cycle | Front Boring” |
G89 Cycle Examples
G89 CNC Program Example – 1
O1234; Program number
M51 ; Setting C-axis index mode ON
M3 S2000 ; Rotating the drill
G00 Z50.0 X50. C0.0 ; Positioning the drill along the Z- and C-axes
G89 X30.0 R10. P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ; Drilling hole 2
C180.0 M31 ; Drilling hole 3
C270.0 M31 ; Drilling hole 4
G80 M05 ; Canceling the drilling cycle and stopping drill rotation
M50 ; Setting C-axis index mode off
M30; Program end
Note: M31is used for C axis Clamp in this example. Could be change due to machine builder.
Need to More?
Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.
