[dingo0722]

I was running a program buffered into my VF2. When the program hit line 100,000 the machine gave me an unknown number error. I have seen this before with other machines not being able to recognize the additional numeral. When I called my cam software company about modifying the post to accept this, they said they have never run into this issue with Hass machines and that they should be able to handle lines of code well into the Nxxxxxx range. Is this true and is there a setting I can adjust to accept additional lines of code or do I need to have the post modified to automatically re-sequence from 1 to 99999 back to 1...

[Andre' B]

Are you using N numbers?
And have you tried turning them off?

[dingo0722]

I am using N lines of code. I will see how to turn them off in the Cam program

[dingo0722]

Will a Hass accept code without a Numerical number starting the line

eg. N100, N101 N102

[pit202]

yes, is it so hard to try ? 10 sec. in front of the machine and wait few hours for an answer ?

[dingo0722]

yes, is it so hard to try ? 10 sec. in front of the machine and wait few hours for an answer ?

Thanks for the value added comment. I guess asking a question here while simultaniously working on it on my side is unacceptable to you

[Geof]

Will a Hass accept code without a Numerical number starting the line

eg. N100, N101 N102

There are three situations when Haas needs a line number;

Calling a subroutine; M97 P1000 looks for a line N1000 so you have to number the first line of the subroutine.

Jumping down the program using M99; M99 P100 looks for line N100 somewhere in the program.

Roughing and finishing canned cycles on a lathe, G73, G72, G71, G70 all need a start and finish line that must be numbered. G71 P100 Q110 looks for the line N100 and reads to N110 for the roughing sequence. The intermediate lines do not need to be numbered and (I think) and there can be more or fewer lines than the difference in the line numbers.

[dingo0722]

what I did first was to remove the sequencing from a program I just ran. After that was confirmed to work I modified the post. I also did away with sub routines in my posting. hopefully I wont have any issues down the line.

[Matt@RFR]

To answer your original question, there is no limit to how many lines of code you can run. I just pulled up a fairly random program that I've already run, and it has 646,699 lines of code WITH N numbers! That's 19.2MB and ran flawlessly off a USB thumb drive. Ditching the N numbers brings it down to 14.3MB, cut that shouldn't have anything to do with your question.

Also, look where Pit202 is from, then realize English is a second language for him before getting defensive.

[HelicopterJohn]

Hi Matt,

Thanks for the info on the USB drive file size.

Is there any restrictions or rules as far as running programs directly from the USB thumb drive? I think???? I heard something about sub programs and being able to restart the program if it is being run from a USB thumb drive.

I have never done this and just want some clarification from experts.

Thanks again for any additional information you or others could supply.

My programs tend to be on the small side so I typically copy them from the USB thumb drive to the memory and then run them. This could save me a step in the process.

[Geof]

Your question about subroutines and Restart was answered here on CNCzone a few years back. Neither are possible when drip feeding either from an external computer via RS232 or from a USB thumb drive. The explanation give was that because the entire program is not held in the machine's memory it cannot scan down to find a subroutine because it is not there. Similarly it cannot scan through a program for a Restart because the program is not there.

[Matt@RFR]

To be clear, local subs work just fine off a USB, but external subs won't work at all. And no, program restart doesn't work either when running of the USB, but restarting at a toolchange does. Gotta be careful with that one though because the control just uses any modal commands that were active when the machine last ran unless you have a comprehensive safety block right before or after the tool change. (Mine is before the M6 block, and I restart on the safety block, NOT the tool change block)

Everything else works...Macros, probing, M30 and M99 counters, tool life, etc. when running off the USB.

Also, you cannot edit a program unless it is on the hard drive, but the only size restriction for the program is the USB size. Mine is a 2GB stick, and I highly doubt I'll ever run a program that big.

[HelicopterJohn]

Hi Geof & Matt,

Thanks for refreshing my memory and the additional USB use information.

You guys are always a BIG help.

John

[Ydna]

Does the haas control allow 5, 6, 7, digits of N numbers? The two CAM programs we have tend to reset the N number count once it hits 9,999 and reverts back to zero. I still post the line numbers though since there have been times in the past where we had to adjust feedrate for a little group of lines that were found on-the-fly.

[Matt@RFR]

I don't know about 7 digits (that's a LOT of code!), but in the example I posted earlier with 646,699 lines, that program ran with every line having an N number. I don't see any reason 7 digits would be any different.

[KenFoulks]

Yes, in the latest SW version you can have an N with 7 digits after it.