Modify post to post G02 and G03 modal

[camtd]

How would like my post to list a G02 and a G03 with each line? This is the code now.

N170 G1 Z2.36 F200.
N180 G41 D4 X2.178 Y-.7128 F14.06 (CUTTER COMP)
N190 G3 X1.9494 Y-.8075 I-.0669 J-.1616
N200 G2 X1.7493 Y-1.1799 I-1.9494 J.8075
N210 X1.5508 Y-1.2088 I-.1126 J.0767
N220 X1.2088 Y-1.5508 I-1.5508 J1.2088
N230 X1.1799 Y-1.7493 I-.1056 J-.0859
N240 X.4026 Y-2.0712 I-1.1799 J1.7493
N250 X.2418 Y-1.9513 I-.0257 J.1334
N260 X-.2418 I-.2418 J1.9513
N270 X-.4026 Y-2.0712 I-.1351 J.0135

This is where I think it needs to be changed

pcirout1 #Output to NC of circular interpolation
pcan1, pbld, pn, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,
pxout, pyout, pzout, paout, pcout, parc, feed, strcantext, scoolant, pcccomment, pe

Thank You

[mori.seiki.user]

Do you know where in mastercam post, to eliminate these N numbers at the start of every single block? It would be good to turn this function off.

[Superman]

This is where I think it needs to be changed

pcirout1 #Output to NC of circular interpolation
pcan1, pbld, pn, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,
pxout, pyout, pzout, paout, pcout, parc, feed, strcantext, scoolant, pcccomment, pe

You are in the correct area, there may be another pcirout ??
use a * in front of the string the force that item into the NC file
-----find sgcode, change to *sgcode

Do you know where in mastercam post, to eliminate these N numbers at the start of every single block? It would be good to turn this function off.

-It's not in the post for the X series

--> Open the Machine Definition File,
--> then open the Control file for that machine,
--> go to the NC File tab & uncheck the "Use sequence numbers",
--> accept the changes while backing out of the files

This is the same area that you go to to alter the actual numbering pattern defaults. ie the default start at N100 and increment by 100, you may want to start at N1 & increase by 1.

[mori.seiki.user]

You are correct with eliminating the N sequence numbers, but to get into where you're talking about, first select SETTINGS in top menu and MACHINE DEFINITION MANAGER.Then find EDIT CONTROL DEFINITION icon at top, then select NC OUTPUT at left. In this page un-select OUTPUT SEQUENCE NUMBERS box. It takes some looking without knowing each step.