More G84 Cycle

RS274/NGC G-code Reference

G84 Cycle

The G84 cycle is intended for right-hand tapping with a tap tool. Program

G84 X… Y… Z… A… B… C… R… L…

0. Preliminary motion, as described above.
1. Start speed-feed synchronization.
2. Move the Z-axis only at the current feed rate to the Z position.
3. Stop the spindle.
4. Start the spindle counterclockwise.
5. Retract the Z-axis at the current feed rate to clear Z.
6. If speed-feed synch was not on before the cycle started, stop it.
7. Stop the spindle.
8. Start the spindle clockwise.
The spindle must be turning clockwise before this cycle is used. It is an error if:
• the spindle is not turning clockwise before this cycle is executed.
With this cycle, the programmer must be sure to program the speed and feed in the correct proportion to match the pitch of threads being made. The relationship is that the spindle speed equals the feed rate times the pitch (in threads per length unit). For example, if the pitch is 2 threads per millimeter, the active length units are millimeters, and the feed rate has been set with the command F150, then the speed should be set with the command S300, since 150 x 2 = 300.
If the feed and speed override switches are enabled and not set at 100%, the one set at the lower setting will take effect. The speed and feed rates will still be synchronized.


G84 Cycle