haas I,J,K error

[gibbs machine corp]

We have three HAAS machines, 2001 VF3, 1999 VF4, and a 2000 VF6. I am using a post downloaded from the my Mastercam dealer's web site. Whenever we cut letters, (generated in Mastercam) we get an I,J,K error alarm on the machines. We can take the same program and run it on our Milltronics machines and it runs great. Haas says it the post (of course). If I change all the arcs to splines it will usually run but not always. If I am 2D profile cutting something, I have to use ramp and I cannot use an arc of any kind for entry and exit. There are days when nothing seems to want to work and waste a lot of time messing with this. Does anyone else have the same problem or have a remedy?

[Fralex_francois]

if you switch IJK for R?

[Camdude®]

try setting breakarcs to 1 in the post.

[gcode]

Go to Screen Config /NC Settings and

check " Number of decimal places for NCI"

It should not be smaller than 6

also check

Tolerance /"Sysytem Tolerance"

It should be .00005 or smaller

 

also

open your post

and check

"helix arc"= should be set at 1

and

arccheck =1

and

ltol=.002

 

[edit]

and set breakarcs to 1 (per camdude)

 

You might also try downloading the latest MPMASTER

post from this website and give it a try.

[jimspac]

I use Fanuc post for the Haas VFs and Toolroom Mills with very little editing and excellent results for most milling and lettering especially. I did not like the Haas posts that much, but that's my experience thus far.

[Nominal]

Without knowing what your alarm is specifically...

You can set the post for the most conservative code for arcs, which is something like...

break arcs on quadrant

issue G02 or G03 on every line even if its redundant.

issue I,J,or,K on every line that has an arc even if they are redundant.

issue I,J,or,K even if they are zero

don't output G41's or G40's on arcs. (more of a function of your lead in/out ).

You can change all of those things at once and maybe you won't get any alarms, but you wont know exactly what caused it without a little more study. Usually the dumber/cheaper/older controls can't take many shortcuts. Good luck.

[BernieT]

We have 3 Haas machines and use a slightly modified Fanuc post. Never have to edit the code. Try the Fanuc post off the CD and/or what gcode said.

 

I would not recommend setting 'break arcs on quadrant', that used to cause me many problems on an old Bandit control especially on lettering and is not necessary on the Haas control.

 

I agree with jimspac, the Haas post off the CD did not work well. (at least back in version 7 or so)

[gcode]

With a bow to the kind people who run this forum,

I've got to say the MPMASTER post available

for free from this forum has always run perfectly for me on Haas VMC's.

[MACHINEMASTERG]

+1 on the mpmaster post pretty much edit free code for our haas