Post processing

[lgonzales3EL6Z]

I have a DMG Mori CMX V1100 and the generic posts that Fusion has in its library don't work on my mill. " the alarm says T-Code is not specified. and also " out of position for ATC "  it doesn't know where my tool-change position is...

[j.labdik]

I've got one of those machines on my floor. Shoot me your file, post, and current code and I'll test it on my machine. 

[lgonzales3EL6Z]

HERE IS A FACING PROGRAM I JUST WROTE..

[lgonzales3EL6Z]

THANK YOU FOR YOUR HELP

[j.labdik]

Okay... so first glance shows something weird. Have you single block stepped through the program on your machine? I'm just now seeing this message since I didn't get an email about it. Sorry to leave you hanging... 

Without being in front of my machine, I'm betting your alarm kicks in at this line: 

N80 G17 G02 Y-15.0362 J1.3371

Your G02 and G03 lines are not using an X value, which is odd, to say the least. There are a few ways to quickly get around this... Try enabling "force arcs" in the NC program dialog and make sure "use IJK" is not selected. This should force the program to use R instead of J. If you can... share with me that file and the post you're using. I'd like to see if there's something enabled in the defaults. Alternatively, here's my post. This should work for you. But by all means, test it in the air, and use caution. I've got no idea what your machine control is set up like. 

[DarthBane55]

Do not change to R values instead of I-J-K.  I don't really want to contradict what was said before, but I-J-K is simply a better way to go.  Sometimes R causes issues and each arc has to be broken into segments otherwise the machine could turn the wrong way.  I-J-K is safer and more reliable.

The values missing (X and I) are normal in this case.  If you backplot the toolpath that was given, each X value is the same at the start and the end, so they don't repeat.  The code is perfectly fine as is.

My guess is that the line "N195 G30 G91 Y0." is the problem.

G30 is a secondary reference point that is defined with some parameters.  If you did not define that point in the parameters of your machine, it will alarm out, with unknown point, which is pretty much what you described.

I would swap the G30 for G28 and see how that goes.

Reference: https://www.mmsonline.com/articles/understanding-g27-g28-g29-and-g30

[j.labdik]

Not a bad point, but every single program I run on my CMX 1100v uses that closing code, and it's never had an issue.

The CMX is a pile of flaming dog crap in all honesty. For some reason the control hates IJK.. don't ask me why. my CMX is 3 years old and has had 3 new y-axis ball screws. The CMX was DMG's response to the VF2, so they cut corners every single place they could, even though it's a $180k machine. For some reason, the control doesn't seem to be an exclusion to that. Look ahead is really limited, and the machine stumbles with complex code even with smoothing being adjusted accordingly.  In my experience of running this dumpster fire for the last 3 years, R values yield a better surface finish and tighter tolerance than IJK. Again... it's a pile of trash so this isn't exactly the norm.

@lgonzales3EL6Z Can you single block through the code and tell me where your alarms come from? I'm now really invested in this since I loathe the CMX lineup. Our NLX on the other hand is a stout little machine. 

[seth.madore]

Interested to hear your candid opinion of the CLX line. I was somewhat saddened when they retired the DuraVertical line, as I own one of the last 6 "5100" series ever made. The darn thing is over 6 years old, and it runs like the day I bought it. Day in and out, never an issue, would definitely buy again

[DarthBane55]

Sorry, my answer was more to @lgonzales3EL6Z , initial poster (my reply shows it was to @j.labdik, my mistake!

The G30 works for you because you have set its position in the parameters, but maybe OP did not, and has the alarm.  It does not know the tool change position he said, and the only place there is something that could be related is the G30 line I think, but then again, it's just a wild guess (going to G30Y0 if G30 is not set will alarm out).

For the R vs I-J-K, alright, it probably depends on the machine then!  Yours is set, so perfect!  He has the same machine as yours I think, so I hope he can take your advice on this to make his run smoother!

But the issue of tool change position for OP is not related to that though.  The code he listed was good valid code, which is the only reason why I think the G30 is probably not set in his machine.  

But, all that said, the more option OP gets to solve his problem, the better!  I hope he finds the solution in any of the answers!

[j.labdik]

All of the CMX machines I've run use an m code alias for handling M6. It uses G28 G91 Z0 in a protected 9000 program. They were all setup by DMG like that as well, so I wonder if @lgonzales3EL6Z has that macro program in place. 

@lgonzales3EL6Z  if you run a tool change in MDI, and watch the program screen, can you see a program appear showing a 9000 level program being used for tool changes? If not that could be part of your issue. I ran your supplied code in my machine just now and it did some weird movements for the G02 & G03 moves (not unusual for my particular machine) but it didn't have any alarms. 

[kturtonLMJPT]

Do you have a post processor for the 5100? I am lookin for one for fusion. Thanks!

[seth.madore]

---

@kturtonLMJPT wrote:
Do you have a post processor for the 5100? I am lookin for one for fusion. Thanks!

---

I'm just using the library Fanuc post processor with only light modifications. That one should work straight away for you and you can edit it as you see fit (if you prefer).