HOW TO: USE THE G84 CODE FOR ROUGH TURNING CONDITIONS

The following commands allow the cutting conditions to be changed from the desired point(s) during a rough turning cycle. If no change in cutting conditions is necessary, there is no need to use them.

Changes can only be specified three times  – A, B, C. The commands following the three specified entries must be designated after “N……G85 N……”.

Since the number of characters in one line will be very large if these commands are specified in the same line, they are written in different lines preceded by “$”, which indicates that the commands in these lines belong to the same block.

EXAMPLE #1 –

  • N0001 G00 X20 Z20
  • N0002 G50 S4500
  • NAT01
  • N0100 G97 S278 M41 M03 M08
  • N0101 G00 X11 Z0.1 T010101
  • N0102 G96 S800

EXAMPLE #2 –

(ROUGH TURNING CYCLE WITH CHANGE OF CONDITIONS)

N0103 G85 NAT01 D0.3 F0.01 U0.05 W0.005 G84 XA=8.0 DA=.2 FA=.012 XB=6.0 DB=.15 FB=.015

$ XC=4.0 DC=.1

  • NAT01 G81
  • N0105 G00 X3
  • N0106 G01 Z0 G42
  • N0107 Z-4
  • N0108 X11
  • N0109 G40
  • N0110 G80
  • N0111 G97 S278 M05 M09
  • N0112 G00 X20 Z20 T0100
  • N0113 M02

XA=8.0 change of cutting conditions is designated at 8.0” for depth of cut and feedrate

DA=.2 depth of cut in rough turning cycle after turning the 8.0” diameter

FA=.012 feedrate in rough turning cycle after turning 8.0”

XB=6.0 change of cutting conditions is designated at 6.0” for depth of cut and feedrate

DB=.15 depth of cut in rough turning cycle after turning the 6.0” diameter

FB=.015 feedrate in rough turning cycle after turning 8.0”

XC=4.0 change of cutting conditions is designated at 4.0” for depth of cut and feedrate

DC=.1 depth of cut in rough turning cycle after turning the 8.0” diameter

Written by: Trey Starnes – Hartwig Application Engineer