Goto commands in DNC programs

[Bob W.]

I tried to use a goto command in a program running from my data server (Makino A51 - Fanuc 31i) and it alarmed the machine saying that wasn't allowed. Is there another way to accomplish that functionality while running from DNC? Here is what I was trying to do:

 

/ Goto 10000

probing routine

N10000

 

Basically using block skip to either skip or allow a probing routine.

 

Thanks,

Bob

[Ben Wood]

You could put the block skip in front of every line of the probing routine.

[Guest MTB Technical Services]

Bob,

 

If it is a single program file on the Data Server, you can try using an M99 P with the P address being the sequence number.

 

I use this all the time when operating from CNC Memory but I've never tried it with a Data Server.

[Thad]

I can't say with 100% certainty, but I would guess that it's not possible. When drip feeding programs, the machine only knows the code that is currently in its buffer and once it has been executed, it doesn't remember the old code either...so it's lost as well.

 

Thad

[Guest MTB Technical Services]

I can't say with 100% certainty, but I would guess that it's not possible. When drip feeding programs, the machine only knows the code that is currently in its buffer and once it has been executed, it doesn't remember the old code either...so it's lost as well.

 

Thad

 

You might be right.

 

However, this is a 31i-A5 with the Fanuc Data Server so I'm not certain the buffering is the same as DNC off a memory card or RS-232.

Also, as long as you jumping forward and the data is buffered, it shouldn't throw an alarm.

 

James Meyette should be able to tell us.

[mkd]

how about two versions of the program? K.I.S.S.

how about putting the probe routine into memory and calling a subroutine? i've never actually tried this.

 

James Meyette should be able to tell us.

+1 he is THE man.

[mkd]

You could put the block skip in front of every line of the probing routine.

edit software can do this in a snap. just highlight text.........

[Bob W.]

Another application I had in mind for this is:

 

N10000

#500=1.500

nc routine, bore 1.5" circle (circle mill)

/ probing routine (probe bore)

/ if bore diameter is less than #500, adjust tool wear

/ if bore diameter is less than #500 goto 10000

...

 

So basically looping back to remachine a feature based on probing results. In the first example in this thread I could put the block skip ahead of each line of code but I was hoping for something cleaner.

[Joe788]

Bob, is this program massive with a ton of tools all using tens of thousands of lines of code each? Or is it just one or two tools that need the data server? When we have the 50-60MB 3D files, I call only the long 3D portions from the hard drive as a sub, and the rest of the program is in regular machine memory. Much easier to deal with probing, restarting, macros, etc.

 

We don't do it often enough to make it worth automating the program management, but I would think it'd be a somewhat straightforward post mod for somebody who knows what they're doing. Maybe have a Misc Integer that tells the post to save that operation as a separate file name and generate a sub call.

[Bob W.]

They are pretty small programs generally (100k-1mb) but they are all archived on the data server under customer folders because they are repeat production jobs. I'd like to keep everything as automated as possible to minimize setup complexity and chances for mistakes. All I really have in CNC memory are the probing routines, a few macros, and a few M198 master programs. Everything else resides on the data server permanently. My PS95 doesn't have a data server so it is mostly running DNC from a compact flash card.

 

If these routines could be done it would speed up the first cycle/ first article big time because tolerance issues could be cleared up in process in the first cycle without the operator needing to adjust tool wear values then re-run the applicable parts of the program to get a good part. It would also help a great deal on parts with extremely tight tolerances.

[Bob W.]

I guess worst case is I could copy the programs into CNC memory when these jobs come along, then clear them out once they are complete. I don't have enough cnc memory to store all of my programs.

[Joe788]

Bob, have you looked into any of the program management systems out there, like Refresh Your Memory, Cimco DNC, etc? They help make the file management and sending/receiving from machines pretty foolproof. I was in a shop once like 10 years ago, and their system would actually fetch the program from the server just by inputting the part number into a macro program at the machine. Totally remote. It was pretty neat.

[Tim Johnson]

Like Joe what I've always done with the Fanuc 18i and continued with the 31i is to put all macro data in CNC memory and put toolpath subs only in the Data Server. I've read somewhere that you can run macro B off the 31i server but my post is already set up so there has been no reason for me to try.