Fanuc Peck Drilling Macro
Move the tool beforehand along the X- and Z-axes to the position where a drilling cycle starts. Specify Z or W for the depth of a hole, K for the depth of a cut, and F for the cutting feedrate to drill the hole.
Following Custom Macro works on Fanuc cnc controls like FANUC Series 30i/31i/32i-MODEL A
Programming
G65 P9100 Z K F
OR
G65 P9100 W K F
| Parameter | Description |
|---|---|
| Z | Hole depth (absolute programming) |
| W | Hole depth (incremental programming) |
| K | Cutting amount per cycle |
| F | Cutting feedrate |
Custom Macro
Main Program
G50 X100.0 Z200.0 ; G00 X0 Z102.0 S1000 M03 ; G65 P9100 Z50.0 K20.0 F0.3 ; G00 X100.0 Z200.0 M05 ; M30
Macro program
O9100; #1=0; (Clear the data for the depth of the current hole.) #2=0; (Clear the data for the depth of the preceding hole.) IF [#23 NE #0] GOTO 1; (If incremental programming, specifies the jump to N1.) IF [#26 EQ #0] GOTO 8; (If neither Z nor W is specified, an error occurs.) #23=#5002-#26; (Calculates the depth of a hole.) N1 #1=#1+#6; (Calculates the depth of the current hole.) IF [#1 LE #23] GOTO 2; (Determines whether the hole to be cut is too deep?) #1=#23; (Clamps at the depth of the current hole.) N2 G00 W-#2; (Moves the tool to the depth of the preceding hole at the cutting feedrate.) G01 W- [#1-#2] F#9; (Drills the hole.) G00 W#1; (Moves the tool to the drilling start point.) IF [#1 GE #23] GOTO 9; (Checks whether drilling is completed.) #2=#1; (Stores the depth of the current hole.) N9 M99 N8 #3000=1; (NOT Z OR U COMMAND Issues an alarm.)
