ALARMS 250 and 251

[Geof]

Have you ever come across alarm 250 PROG DATA ERROR or 251 PROG DATA STRUCT ERROR; both with the explanation; "Possible corrupted program. Save all programs to disk, Delete all, then Reload"?

I have a few times on different machines and it seems to be hitting keys too fast in EDIT mode; especially when doing copy/pastes or re-numbering lines. Most times the Save/Delete/Reload instructions work, or they did on my older machines. But that first time when your finger is hovering over the ERASE key with a couple of hundred programs in the machine that you neglected to back up is tough...until you calm down and realise you can go and look at the disk you just copied them onto and make sure they are there.

But this week has gone beyond reason; on Monday my Simulator gave these alarms so I dropped it of to be purged and the control software reloaded. Today my TL2 has done the same. In both cases the machine would not let me copy to disk, or delete all; which would have been okay because I have everything backed up now.

Haas Apps are you looking? This is a glitch that should have been corrected a long time ago....please......pretty please(?).

[Haas_Apps]

Yes, I am looking. Please contact the Haas factory so we can resolve this. Please be ready to describe, in detail, how to duplicate the issue and I am sure we can resolve this.

[drewcuzz594]

HI i'm very new to live tooling machines, we have purchased a new Haas sl20 machine I've managed to figure out most things but I can not figure out how to peck drill using live tooling on the x axis any help would be appreciated.
Thanks
andy

[Geof]

Well I guess it was kinda my fault but not entirely. I found out how to do it deliberately.

In the Haas Editor you can select a block of text using the F2, Scroll Down (or Up), then F2 again; that highlights the text.

Then you open the menus using F1 and select what you want to do, copy, renumber, delete, etc.

For drilling and tapping bolt hole patterns on one offs I normally enter all the coordinates for the first tool, usually a spot drill, then to save time just highlight that section of code, copy it twice and then change the tool numbers in the copies and change the G82 to G83 or G84 and edit the feeds and depths.

Sometimes I renumber the blocks while they are still highlighted from the copy operation.

It seems if I try to do too many operations on a highlighted portion of code then I can corrupt everything; to avoid this I need to use UNDO to de-select then re-select with the F2/F2 sequence again.

And one of my guys found on an older machine that you can do the multiple copy using WRITE and the third time you hit WRITE you get the Alarms. We have had these alarms on our older machines and have always been able to recover using the Download/Delete/Reload sequence.

Maybe someday I will check if it also depends on the number of lines selected? Maybe it is a case of some temporary memory buffer used for these editing operations getting too full? That would possibly explain why it did not happen everytime I did the multiple copy operation.

[Donkey Hotey]

Originally Posted by Geof For drilling and tapping bolt hole patterns on one offs I normally enter all the coordinates for the first tool, usually a spot drill, then to save time just highlight that section of code, copy it twice and then change the tool numbers in the copies and change the G82 to G83 or G84 and edit the feeds and depths.

Okay, total hijack of the thread here.

Geof: I used to think that it was necessary to copy & paste the codes like you're doing for drill, tap, c-cink, etc. But while reading one of the Haas manuals one night, they suggested using a sub-routine. I'm absolutely sure you know about sub routines but this is the part I had backward: I thought of writing a sub-program for the drill-tap cycle, then calling it a dozen times. That was incorrect.

The canned cycles are modal--they keep doing whatever you instructed them to do, at as many coordinates as you specify until you 'end canned cycle'. The Haas example did it backward from my initial thinking. They do a main program of drill one hole, tap one hole. But in between, they jump to a sub-program before canceling the cycle.

The example was a simple program of:
1 Spot Drill
Go do sub-program
Cancel Canned Cycle
1 Peck Drill
Go do sub-program
Cancel Canned Cycle
1 Tap Cycle
Go do sub-program
Cancel Canned Cycle
End program

The sub program is nothing but XYZ locations for the holes. So it would grab the drill, poke a hole, go do the same modal peck-cycle at every block location specified in the sub-program, then return. Then it would grab the tap, do one hole, then go do it everywhere else in the sub-program, etc.

What dawned on me was that I could write a simple hole tapping routine (with the pointer to the sub-program) and keep it as a utility program (along with the commonly used tools). Then by writing just the sub-program with nothing but XYZ locations for tapped holes, I could call that main program and it would obediently prep all of the holes with no fuss.

Of course, you may already know this...in which case: never mind (just tryin' to give back).

[Geof]

Mr Hotey, or should I call you Donkey? That does not really sound very respectful. You are forgiven the hijack.

Actually I do both depending on my mood; simply copy/paste as I described or put the coordinates in a subprogram which is called by each tool.

For a lot of simple programs I have what you have; simple routines that just need the coordinates entered; I call them template programs. Once you are comfortable with the control it is a simple matter to whip up a small drill/tap sequence.

One program I have 'Facing X axis' which is handy when I need to quickly face a plate of some variable size. It uses two work zeroes and an L count and for different sizes all that has to be changed is the L value.

One work zero (G54) is placed slightly more than the cutter radius outside the right rear corner of the plate and the other (G55) outside the left rear corner (these are just eyeballed), and the tool offset is placed at the level of the finished surface. The facing moves are:

etc
etc
G54 G00 X0. Y0. Z1.
Z0. (This is outside the plate area)
G91 G00 Y-.7 M97 P1000 L(whatever) (The Y value is a bit smaller than the cutter dia.)
G90 G00 Z1.
etc
etc
M30
(-----)
N1000 G90 G55 G01 X0. F(whatever)
G91 Y-.7
G90 G54 X0.
M99

The L count is the width in the depth of the plate in Y divided b y 2 x the Y increment; for a plate 6" deep this would be 6/2x0.7=4.28 so it is L5