Cinci Arrow with Acramatic 2100e control

[Mitch Rivers]

Hey Folks
Just installed this used machine in our shop.
Using matercam x, contouring a circle. Machinine leads into circle then leads out ignoring the circle geometry. What is going on? Any help? Thanks in advance.
Mitch

[scudzuki]

Hey maybe posting the code that is not producing the toolpath you want would be helpful, ya think?

Joe

[Mitch Rivers]

Mastercam Circle mill path using 1/2" tool, cutting a 1" circle. .1 depth.
:T1 M6
N130 G0 G90 X0. Y0. S3056 M3
N140 Z2.
N150 Z.25
N160 G1 Z.1 F6.42
N170 G3 Y.25 P.125 F24.45
N180 I0. J0.
N190 Y0. P.125
N200 G1 Z.25 F6.42
N210 G0 Z2.
N220 M5
N230 M26
N240 M02

[Mitch Rivers]

I was hoping a parameter in the machine was not set to accept full arc. This happened on a haas vf2 I ran.

[mallardfizz]

cant see anything wrong in prog. please check to see that the circular mode isn't set to incremental.
press MORE
SYSTEM CONFIGURATION
NC PROGRAMMING
CIRCULAR
you have 3 options incremental , absolute or switchable.
incremental is the same as Fanuc - absolute is the Cincinnati standard or switchable is set by g90/g91 in the prog.
since you have g90 in your prog then i can only imagine the circular mode is set to incremental.
have a look and let me know the result
regards
mallardfizz
ps what's M26

[Mitch Rivers]

I changed that to absolute a few days ago but it did not help. Thanks for the reply anyway.
I use the m26 code to send Z to the home position.
Mitch

[Mitch Rivers]

The only other option on that page is the endpoint tolerance. Mine is set at
.01. Does that sound likely.
Thanks, Mitch

[mallardfizz]

hello again no if the move you are trying to do does not finish within the endpoint tolerance you would have the 'endpoint not on circle ' alert ( or words to that effect ).
i would you suggest you try modifying your programme to include all information.ie g3 x0 y.25 i0 j0 followed by g3 x0 y0 p.125. i cant give a reason why yet. i haven't programmed in anger for a while and need to consult my manual - working from memory at the moment.
you can also use the g98.1 to move the axis round. for example g98.1 x0 y0 z20 would move the table to its 'home' position with the carrier 20" above the table in machine co-ordinates. it ignores any offsets and is a one line move only.
the result of trying what i suggest would be more evidence to resolve your problem.
regards
mallardfizz
you can also e-mail me at mallard@fizz58.freeserve.co.uk

[mrivers]

Thanks for all the efforts. Sorry for taking awhile to get back here.
The problem was the mastercam post.
I had to change the arc to break at quadrants and the problem was solved. Just not enough info for the machine the other way i guess...
Thanks again....