Canned Cycles G81 through G89 have been implemented for milling. This section describes how each cycle has been implemented. In addition G80 and G98/G99 are considered here because their primary use is related to canned cycles.

All canned cycles are performed with respect to the XY plane With the current 3 axis interpreter, no A, B, C-axis motion is allowed during canned cycles inverse time feed rate is not allowed cutter radius compensation is not allowed Each of the canned cycles defines a new machine motion mode. As a motion mode, they will stay in effect until replaced by another motion G word or by G80 as described below.

All canned cycles use X, Y, R, and Z values in the NC code. These values are used to determine X, Y, R, and Z positions. The R (usually meaning retract) position is along the Z-axis. Some canned cycles use additional arguments that are listed with the specific cycle.

G80 – Canned Cycle Cancel

Since canned cycles are modal commands, they’ll stay active until you turn them off. G80 is the canned cycle cancel command.

Without it, the canned cycle will repeat at every XY coordinate. When you’re done your operation, turn it off with G80.

G81 – Standard Drilling Cycle

This is the most basic holemaking canned cycle.

The tool positions itself at the top of the hole. The tool feeds to the specified Z position at the programmed feed rate. The tool retracts in rapid mode to either the previous Z position or the R plane.

Here are the values to know:

• X: The X location of the first hole (absolute with G90, incremental with G91)

• Y: The Y location of the first hole (absolute with G90, incremental with G91)

• Z: The depth of the first hole (absolute)

• R: Retract plane (optional – default is the last Z point before G73 is activated)

• F: Feedrate. If nothing is input, then the last used feedrate will be used.

Sample code:

G81 X1.0 Y0.0 Z-1.0 R0.1 F10.0; (begin simple drilling cycle, drill first hole at X1.0, Y0.0 to a depth of Z-1.0, final retract is to Z0.1, at a feedrate at 10.0 inches per minute)

X2.0; (drill another hole with the same parameters at X2.0, Y0.0)

X3.0; (yet another identical hole at X3.0, Y0.0)

G80; (cancel G81. Any XY positions programmed from this point further will not automatically start a boring operation)

Syntax

G81 X... Y... Z... R... K... F...

Once G81 drilling cycle is defined, the canned cycle is repeated at every X-Y position in sequential blocks. So G81 drilling cycle must be cancelled with G80.

Usage

N30 G81 X10 Y30 Z-17   R2 F75
N40 Y10
N50 X30
N60 Y30
N70 X90
N80 Y10
N90 G80

In the above example drilling will start with G81 drilling cycle at X10 Y30, so first drill will be at X10 Y30, then second at Y10, third at X30, fourth at Y30, fifth at X90 and the last one at Y10, because next block have G80 code, so drilling cycle will no more be repeated.

Working

Here is briefly described how G81 drilling cycle operates,

1- Rapid traverse to the specified x,y axis position (drilling position).

2- Rapid traverse to the R plane position.

3- Drilling with specified Feed from R-plane position to Z-depth position.

4- Rapid traverse to Initial level or R-plane depends on G98, G99 modes.

G81 drilling cycle working