en:software:mdurosettacncsoftwaregcode:canned_cycles

6. Canned Cycles

A canned cycle is a command that gives the machine instructions for a pattern of movements.
It’s meant to automate and simplify repetitive and common tasks, such as drilling holes.

Instead of programming every movement and function individually, a canned cycle controls a set of motions.

In this section you can find a quick reference list followed by a paragraph for every cycle explaining how to use it properly.

G-code Description
G73 Drilling - High Speed Peck Drilling Cycle / Chip Break Drilling Cycle
G80 Cancel Motion Mode / Canned Cycle Cancel
G81 Drilling - Standard Drilling
G82 Drilling - Drilling Cycle, Dwell
G83 Drilling - Peck Drilling Cycle
G85 Boring - Boring Cycle, Feed Out
G86 Boring - Boring Cycle, Spindle Stop, Rapid Move Out
G88 Boring - Boring Cycle, Spindle Stop, Manual Out
G89 Boring - Boring Cycle, Dwell, Feed Out
G98 Canned Cycle – Retract Back To The Initial Z
G99 Canned Cycle – Retract Back To R Plane

G73 High Speed Peck Drilling cycle performs high–speed peck drilling.
It performs intermittent cutting feed to the bottom of a hole while removing chips from the hole.

Programming
G73 X Y Z R Q F <L>

Parameters

Parameter Description
X Y Hole position data
Z Z-depth (feed to Z-depth starting from R plane)
R The distance from the initial level to point R level (Position of the R plane)
Q Depth of cut for each cutting feed (depth of each peck)
F Cutting feedrate
L Number of repeats (if required)

Cycle Operation
The tool dips into the workpiece for the infeed Q, drives back with rapid feed of 0.254mm (d retraction) to break chips, dips in again, until end depth is reached, then retracts with rapid feed.

Example

N10 G99 G73 X10 Y10 Z-8 R2 Q1 F100
N20 X20
N30 X30

G98 G99
When G98 is active, the Z-axis will return to the start position (initial plane) every time it completes a single operation.
When G99 is active, the Z-axis will be returned to the R point (plane) every time the canned cycle completes a single hole. Then the machine will go to the next hole.
Generally, G99 is used for the first drilling operation and G98 is used for the last drilling operation.

To cancel a canned cycle you can use G80 or one of the following G-codes from Group 01:

G-code Description
G0 Straight traverse
G1 Straight feed
G2 Clockwise arc feed
G3 Counterclockwise arc feed
G38.x Probing
G80 Cancel motion mode / Canned Cycle Cancel
  • Last modified: 2020/02/17 12:59
  • by cnc212