Need help programming (arcs) 20 year old Cinci VMC

Hey guys - having a bit of trouble here with a Cincinnati Lancer VMC - Acramatic 2100 control. I don't do a ton of programming on these with the conversational that's on them, but this morning I had a request for an engraving program. This is about the 4th time I've had this struggle and I haven't yet figured it out. Code below...control catches error on N108. When I ran into this problem last time I thought for sure it had something to do with cutter comp - then tried reprogramming with control, computer, value in diameter, no value in diameter and couldn't figure anything out. This is just a straight no comp program, and I can't figure why it won't go. I believe we can increase the endpoint tolerance, but I'm hoping someone with more experience programming these machines can steer me in the right direction.

:
( MSG, TOOL - 1 | 1/32 FLAT ENDMILL | TOOL DIA. - .03125 )
:100 T1 M6 D0
N102 G0 G90 X4.4587 Y-.3214 D1 S4000 M13
N104 Z.1
N106 G1 Z-.015 F2.
N108 G2 X4.5824 Y-.25 I.1237 J-.0715 F8.
N110 G1 X4.5935
N112 G2 X4.7362 Y-.3864 I0. J-.1429
N114 X4.6993 Y-.476 I-.1427 J.0064
N116 X4.5709 Y-.5719 I-.7722 J.9005
N118 G3 X4.448 Y-.75 I.116 J-.2115
N120 G1 X4.7469
N122 G0 Z.1

Holding out hope this isn't one of those "Hey, look right here under your nose, DUMBASS." type problems.

Your I and J values make no sense. The following code has your original arc endpoints with modified I and J points that I came up with in CAD. Probably not the same as your font, but the curves are all tangent. Good luck.

Burt

:100 T1 M6 D0
N102 G0 G90 X4.4587 Y-.3214 D1 S4000 M13
N104 Z.1
N106 G1 Z-.015 F2.
N108 G2 X4.5824 Y-.25 I4.5824 J-0.39285 F8.
N110 G1 X4.5935
N112 G2 X4.7362 Y-.3864 I4.5935 J-0.39285
N114 X4.6993 Y-.476 I4.62154 J-0.39158
N116 X4.5709 Y-.5719 I4.19683 J0.06953
N118 G3 X4.448 Y-.75 I4.6993 J-0.79073
N120 G1 X4.7469
N122 G0 Z.1

IIRC, the Cincinatti's I, J and K are all absolute. They are not relative to the start point of the arc, like fanuc-ese; the center of the arc in relation to the work origin. Another oddity is the use of P instead of R for arc callouts.

Thanks guys.

The start to center format runs just fine on the Fryer, Haas. Anyways...

I've changed the arc output on the control def to go absolute. Unfortunately the machine is tied up now so I won't know for a few days.

on the 2100 arc centers are programmable either in absolute( usa control manufacturer standard) or incremental( rest of the world). There will be a system configuration page called nc programming.... in that tab is arcs/ circles,,, you will have a choice of g90/g91 switchable, always absolute or always incremental.

WILLEO6709 said:

on the 2100 arc centers are programmable either in absolute (usa control manufacturer standard) or incremental (rest of the world) ...

Click to expand...

USA invented nc/cnc. It's sad that now the original conventions have been deprecated in favor of the Fanuc so-called "standard."

Fanuc sucks

Thanks for the good info you guys. The switch to arc output to absolute gave me a good program to run on the Cinci.