Super Long Programs - Fanuc 0M

[ArdentIndustries]

Hey all, 

 I have an older Makino RMC55 with a Fanuc 0M control on it. After some difficulty with communication between the machine and my computer, which I finally have figured out, I am realizing my programs are very long for what I am doing. 

 Take for instance, a 3" diameter counter bore that is .150" DOC....which comes out to around 1500 lines of code. The machine doesnt like "N" numbers above 10,000, so I have to limit them to less than that. Also, with the lack of memory, I am often deleting programs in order to add a new one. Often times, I cut back on the step downs, step over, not using helical plunging, etc. just to get the program short enough. 

 Talking to a couple people it seems there should be a macro or something enabled when I output the post in order to shorten these programs up? I have messed with a few options but none seem to shorten the program any. Is there something that will enable some sort of macro or something to make this much shorter? Something that defines a center point then simply clears material out to a certain radius? The current programs are line after line after line of X/Y coordinates. 

 Any help would be appreciated! Thanks in advance!

Kyle

[LibertyMachine]

There are a couple macros floating out on the internet that make circle macros similar to the Matsurra G13 canned cycle, although not as elegant.

1500 lines of code seems excessive. Could you share your file?

File > Export > Save to local folder. Return to thread and attach the .f3d file

I've shared your pain of small memory. My first machine (1982 Matsurra MC-500) had a whopping 17k. I could do quite a bit with it, but engraving and surface machining was out of the question 

[ArdentIndustries]

I will post a sample program when I get home later this evening. I
appreciate the response!

Im not even sure how much memory this machine has, but when starting I had
a heck of a time getting programs loaded. I had a few issues but one simple
one was that I was simply out of memory so it would alarm.

Thanks again!

[ArdentIndustries]

Attached should be this file, if I did it correctly. I am using a generic Fanuc post, that has been modified for a manual tool change operation. I usually am only able to post one process at a time, as the programs are too big otherwise. 

Thanks for any help!

[ArdentIndustries]

In going back to the "generic fanuc" post, it appears the same program is only 132 lines. Unfortunately, as soon as I try to send this program to the machine, I get an 087 alarm...which I think is why I went to the post I was using. (Found that post on this forum somewhere if I remember right)

 Now, I need to figure out the difference in the 2 posts...why the generic creates a smaller program, and what about the generic the Makino doesnt like to load. Also need to figure out how to get the generic to create a program stop at each tool so I can manually do a tool change (I think I found instructions on this process before, and altered the one I have been using myself based on that thread). 

 Any pointers? Thanks!

[Steinwerks]

Googling "Fanuc 087 alarm" got me this thread on Practical Machinist: http://www.practicalmachinist.com/vb/cnc-machining/fanuc-087-alarm-118987/

[ArdentIndustries]

Yeah, ive spent hours and hours deciphering alarms in regards to
communicating with my computer.

There must be something with the generic post that the 0M doesn't like. I
think another member had this issue also and that thread is where I got the
post that seemed to be working.

[Steinwerks]

But the 087 is a buffer overflow according to that thread, which means the data rate is too high for the control to deal with while saving to memory, so the key there was to slow the transfer rate to 4800 baud. What program are you using to send the NC file?

[ArdentIndustries]

It must have something to do with that post though because the other post
has been fine. Literally 2 minutes before switching to the generic, i
loaded a program just fine.
Dan @ PCDNC has been great in helping me through all the alarms I have
fought with.

Wonder if the shorter program contains a macro or something that is to help
keep the program short, but maybe this control won't accept it??

[Steinwerks]

Post the same file with both post processors and share them here is the only suggestion I have in that regard, that way they can be compared.

[ArdentIndustries]

Attached should be 4 files. First two are actual code for the same process, using the 2 different posts. The second 2 files are the post files themselves. 

Any help?

Thanks!

[ArdentIndustries]

Here are the post files. 

[LibertyMachine]

Smoothing and vertical arcs are going to be your friend in reducing the file sizes:

[ArdentIndustries]

Thanks Seth! I am anxious to get home and try this on the "MTC" post I have been using, since the generic Fanuc does not seem to work with my machine. 

To clarify, does smoothing simply utilize radii, instead of many many X,Y coordinates? That is the G02, G03, etc. that you mentioned were present in the smaller program?

Thanks again!

[LibertyMachine]

Yes, I should have mentioned that in my video. Duly noted for next time..

The "Smoothing" will fit arcs in where it can, depending on the tolerance and the Smoothing value. I found that for my machine and preferences, the .0005" and .001" values produce the smoothest results. YMMV

That said; if you are still struggling for disk space, Adaptive toolpaths might be out of the question. My old Matsurra (with 17k) could handle 2D Pocketing, contour, thread milling, drilling. Anything Adaptive or 3D was out of the question (for the most part)

On another note; I'd really like to find out why the generic post is not working with your machine. That said; it's best practice to make the post "Your own". Once you find a post that works, save it to your computer or the cloud. That way any changes made later on down the line (from Autodesk) won't have an effect on you

[randyT9V9C]

Kyle,

I run a 15m which has similar limitations to your 0m. You are correct about the line numbering limitation, by default, if you increment by 5 or 10 it doesn't take long to hit 10k lines. I simply turn off line numbers for most stuff. I suppose you could increment by 1 rather than 5.

As others have mentioned turning on smoothing will convert the arcs from segments to arcs/helical arcs. I really wish Fusion had a global setting for arcs vs segments. I suspect your running up the length on the helical starts. The generic post does helical.

For programs that are larger than your memory, which is very easy these days with adaptive and 3D paths, you could post each operation separately, essentially breaking your program into manageable chunks.

I DNC most of my larger programs which really nullifies most of my line numbering need until something goes ugly. I have a Calmotion USB-CNC unit on the Fanuc 15m and it handles very large programs nicely. Any PC with DNC software will work similarly.

One thing to remember, the Fanuc has the baud rate set in two locations, one for external communications, and another for internal communications. They both must match. One is in the control settings and the other is in the PC/NC settings. Of course this must match your DNC PC also. Like Neil mentioned a 087 implies a serial buffer overrun so something is likely sending faster than something else can read it. I have my 15M running at 9600 baud but I ran at 2400 baud forever until I realized the setting was in two places. Now I'm happy even at 9600 baud.

I have a fairly proven Fanuc 15m post based on the generic Fanuc post. I had to tweaks a bunch of stuff but it's has been a while. Your welcome to give my current post a whirl. I know I fiddled with rigid tapping and a few others items. http://home.lewiscounty.com/~forhire/posts/fanuc15m.cps

[ArdentIndustries]

Thanks so much Seth! I hate when its one simple mouse click...but 9 times out of 10, thats what it is. Thanks for taking the time to help me and make the video. I just posted 2 of the same programs, one with smoothing, one without, and it works great. This is using the manual tool change post I have been using in the past. I can actually load a program that consists of more than 1 tool finally! 🙂 

 Randy, thanks for the input. I will feel like I have a TB of space...for the time being anyways...with having these shorter programs. I have used the DNC drip feed a time or two, but it seems real finicky. Sometimes it works great, sometimes not. After the first run of the program it gets easier, but that first one is nerve racking when it takes off and you dont have any code to look at or anything. Just hope its good and have your hand near the E stop. Lol. 

 Making dinner right now, but will run to the shop afterward and test out the new program setup. Thanks again!

[ArdentIndustries]

Well it did seem to work. I had a different MTC post on my laptop which still didnt like the shorter code. I sent the post from my desktop to my laptop and it works well. 

 Two small issues. This post calls a Tool # out on one line, with nothing else. For some reason the machine stops here. It doesnt know what to do with only a T#. I added "M00" on the same line and it ran perfect. The post creates the M00 on the line following the T#, but I need it on the same line. Anyone with a suggestion on how/what to modify to make this happen? 

 021 Alarm came up because of using helical moves. Anyone know the parameter to check to see if the machine even has this option? I went to the "zig zag" entry method, and it ran the program just fine. 

 Thanks again for all the help!

[randyT9V9C]

I remember checking this on my control. I don't recall off my head but I did find a thread that may help. It say's bit 3 of 910 which sounds familiar. See post #7.

Famuc O-M Contol: Parameter 910 bit 3 (xxxx1xxx) should be a one to enable Helical Interpolation.*

http://www.practicalmachinist.com/vb/cnc-machining/helical-interpolation-fanuc-o-m-control-124545/

[Gmar111]

Is there a way to make thread milling code shorter? In attached sample I'm doing one pass but the code is longer then I would like it to be. I like to be able to understand toolpath (maybe NPT is not easiest think to analyze). For UN threads breaking circle in 2 or 4 arcs makes it easy to understand. Anyway to shorten the code for NPT?

Thanks in advance.