Hole machining cycles <CYCLE>



<CYCLE> command is used to pass standard drilling cycles G81-G89. Use <CYCLE> command to determine cycle type and process the cycle accordingly. Cycle type is specified by the first parameter, other parameters types and their number depends on the cycle type.

Command:

CYCLE ON(71) | OFF(72) | DRILL(163) | FACE(81) | DEEP(153) |

BRKCHP(288) | TAP(168) | BORE5(209) | BORE6(210) | BORE7(211) |

BORE8(212) | BORE9(213)

Parameters:

Usually SprutCAM generates drilling technology similiar to the following:

...

GOTO.abs X, Y, Z ! Position the tool at the first hole.

CYCLE DRILL(163) ! Perform the drilling calling cycle of appropriate type.

GOTO.abs X, Y, Z ! Move the tool to the next hole.

CYCLE DRILL(163) ! Perform the drilling calling cycle of appropriate type.

...

GOTO.abs X, Y, Z ! Move the tool to the last hole.

CYCLE DRILL(163) ! Perform drilling by calling cycle of appropriate type.

CYCLE OFF(72) ! Turn cycle off.

...

The first drilling cycle command should form the NC-block containing a cycle definition (like G81) and cycle parameters.For example:

G81 X_Y_Z_R_F_

Following commands processing should form block containining only the changed registers. For example:

X_Y_Z_

X_Y_Z_

...

X_Y_Z_

The <CYCLE OFF(72)> command should form the code of cancelling cycle. For example:

G80

When developing ISO postprocessors using masks ISO.G operator can be used. The value of ISO.G is set automatically according to the following table:

See also:

Technology commands description

G81 drilling cycle &lt;CYCLE DRILL(163)&gt;

G82 drilling cycle &lt;CYCLE FACE(81)&gt;

G84 drilling cycle &lt;CYCLE TAP(168)&gt;

G85 drilling cycle &lt;CYCLE BORE5(209)&gt;

G86 drilling cycle &lt;CYCLE BORE6(210)&gt;

G87 drilling cycle &lt;CYCLE BORE7(211)&gt;

G88 drilling cycle &lt;CYCLE BORE8(212)&gt;

G89 drilling cycle &lt;CYCLE BORE9(213)&gt;

Deep drilling with chip removing &lt;CYCLE DEEP(153)&gt;

Deep drilling with chip breaking &lt;CYCLE BRKCHP(288)&gt;