Robodrill outputs all progs from directory

[Newbeeee™]

Hi all,

Funac Robodrill E model with 31iA5 control.

This is a new one to us, the other machine doesn't do it.

Select a program to output via DNC, type O1234 execute, and all other programs are exported together with the one I wanted.

The other machine doesn't do this - it only outputs the one that we want.

Anyone know of a parameter change please?

TIA - Cheers

[Guest CNC Apps Guy 1]

Go through the MGI side...

 

EDIT mode, GRAPH hardkey, O LIST softkey, M-CARD softkey, OUTPUT softkey, highlight the program you want to be output, press OUTPUT and there you go.

 

 

Or, for you old school FANUC guys on the 31i's, EDIT mode, PROG hardkey, FOLDER softkey, right arrow softkey to punch, cursor to program you want to punch, press F-GET softkey, press P-SET softkey, EXEC.

 

 

HTH

[Newbeeee™]

Thanks James, I'll give that a go.

It's never been a 'problem' before as we only ever have the one program in the control at once so never noticed this.

But where we moved the machines and had no dnc for a while, there's a few progs in the control temporarily while we were getting the dnc set.

[Guest CNC Apps Guy 1]

You DNC'ing from the card or RS-232?

[Newbeeee™]

Was the card for a while (fget fset etc) all ok.

Now back to RS232.

On the Oi machines, typing just the prog number (ie O1234) > execute would export just that prog.

Perhaps the robo doesn't then by doing it this way? Perhaps it only does it the way you said above? I thought it did the same as the Oi but as I said, it's a long time since we had more than one prog in the control and I've been to sleep a few times since

Thanks

[Guest CNC Apps Guy 1]

0/16/18 = same

 

30/31/32 = not the same as above.

 

The 30 series controls intruduced folders to the fray and changed some other things.

 

RS-232.... eeeeeeeeeeeeeeeeeeeeeewwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwww!

 

 

[Newbeeee™]

0/16/18 = same

 

30/31/32 = not the same as above.

 

The 30 series controls intruduced folders to the fray and changed some other things.

 

RS-232.... eeeeeeeeeeeeeeeeeeeeeewwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwwww!

James - Yeh I know RS232 is a little, well, sloooooowww but the Oi's only have a small memory. All our progs that have any tools with dynamic paths tend to have the long toolpath on the flash card (M198) to keep the main prog down in size so we can keep that in the memory and beable to jump in and out of tools as and when.

BTW - What is the benefit of folders, apart from being able to keep lots of different progs into lots of different customer directories? And from an aerospace standpoint, do many people use this?

I always thought one prog in the control at a time is the best way, especially with multi machines in case the prog gets modded. Otherwise 5 machines and 5 variations of the 'same' prog etc?

Just wondering how people use this feature.

Cheers

[Guest CNC Apps Guy 1]

What is the benefit of folders, apart from being able to keep lots of different progs into lots of different customer directories?

That's one use. Another even more practical use is MACRO/O9xxxx storage. In the 30 series controls you have MTB1, MTB2, SYSTEM, and USER folders. Under the USER folder you have LIBRARY. Typically I will put MACRO programs related to machine functions (M6, etc...) in the SYSTEM folder. Probing, Laser/Tool MEasurement/Breakage Detection, and user friendliness MACRO programs in there. It's a nice way to keep those programs out of general view.

 

And from an aerospace standpoint, do many people use this?

I would say if they are old school users generally they dont. They like to keep things the same. If they are new school then it's probably closer to 50-50. If they have Dataservers then the usage goes up probably abother 20%-ish.

 

I always thought one prog in the control at a time is the best way, especially with multi machines in case the prog gets modded. Otherwise 5 machines and 5 variations of the 'same' prog etc?

Just wondering how people use this feature.

Cheers

That really depends on the customer. I've got an increasing customer base that DOES NOT edit programs at the control so that really does not come into play.

 

The most common feature I see 30 series customers using is program names instead of O numbers. You can have a 30 character program name. Part Number, Rev and Operation generally will fit. Helps with ISO rev tracking.

 

HTH

[Newbeeee™]

Thanks James - Interesting.

[huskermcdoogle]

 

The most common feature I see 30 series customers using is program names instead of O numbers. You can have a 30 character program name. Part Number, Rev and Operation generally will fit. Helps with ISO rev tracking.

 

 

 

James, I to you. This just made my day. I have accepted a new job, one machine at the moment with a 31i, foundations in for 5 more... This makes life soo soo much easier when constantly switching part numbers. Having used names instead of numbers (especially for offset subs) in a previous job with Mazaks I am o so excited to be able to do this with a Fanuc.

 

Husker

[Guest CNC Apps Guy 1]

Gald to be of help HUsker. Here's the format you'll need to follow;

 

%

<TEST-MAIN.TXT>(SUB CALL BY PROGRAM NAME TEST)

N1 M98<TEST-T1.TXT>

M1

N2 M98<TEST-T3.TXT>

M1

N3 M98<TEST-T3.TXT>

M1

N4 M98<TEST-T4.TXT>

M1

N5 M98<TEST-T5.TXT>

M1

N6 M98<TEST-T6.TXT>

M30

 

<TEST-T1.TXT>(TEST 1 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

 

<TEST-T2.TXT>(TEST 2 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

 

<TEST-T3.TXT>(TEST 3 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

 

<TEST-T4.TXT>(TEST 4 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

 

<TEST-T5.TXT>(TEST 5 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

 

<TEST-T6.TXT>(TEST 6 FILE)

N1G4X1.

N2G4X1.

N3G4X1.

N4G4X1.

N5G4X1.

M99

%