Drill Cycles Forever

[MetalMarvels]

I have a slightly weird problem at my day job. Using Mastercam 8.1.1 and MPFADAL2.pst, if I create a drill cycle as the 1st operation, the FADAL 4020 continuously runs the canned drill cycle over and over and over. It never gets to the next line that cancels the drill cycle. If I post another operation in front of the drill cycle, the drill cycle operates perfectly (and only once!). The FADAL is runing in Format 2.

 

The posted code is:

 

N1 G00 G17 G20 G40 G49 G80 G90

N3 T1 M06

N5 G00 G90 S6000 M03 G54 X.32 Y-.2

N7 G43 H1 Z.025 M08

N9 G99 G81 Z-.03 R.025 F6.

N11 G80 M09

N13 M05

N15 G91 G28 Z0.

N17 M01

 

If I post an operation in advance of the drill cycle (in this case a contour) I get the following which works properly:

 

N1 G00 G17 G20 G40 G49 G80 G90

.

. Code for a contour

.

N151 M05

N153 G91 G28 Z0.

N155 M01

N157 T1 M6

N159 G00 G90 S6000 M03 G54 X.32 Y-.2

N161 G43 H1 Z.025 M08

N163 G99 G81 Z-.03 R.025 F6.

N165 G80 M09

N167 M01

 

My question is - am I looking at a post/programming problem or a FADAL control problem????? I can consistently repeat the problem. If I create the same condition at home and use my personal copy of MC9 SP1 and my customized post the only real difference is that I get:

 

G81 G98 Z-.03 R.025 F.

 

instead of line N163. BUT it works........

 

Any help would be appreciated.

[Keith Graydon]

I've seen effect a long time ago.

Check for a correct "O" word and that the file doesnt have a lot of comments in the header.

 

HTH

-KLG

[n_tydingco]

IMHO -- It may be a control problem that can be remedied with a post adjustment.

 

Try posting your XY coordinates on the line with your drill cycle callout and see if that helps.

[chris m]

Maybe I misunderstand the problem here but I think it would be easy enough to rule out either the CNC or the post processor by hand-writing a one-tool program in the exact block-for-block format that the Fadal programming manual describes and run that in the machine. If it works properly, then the CNC machine would [i think] be ruled out as the problem.

 

If you can get the post to generate the same format, it should work, shouldn't it? Am I oversimplying? I don't know...

 

Another thing: if your initial point and R point are the same; why use G99? Probably unrelated, but G99 can really bite you in the xxxx if you make a quick change to your program and don't notice it...

 

[ 09-04-2002, 02:12 PM: Message edited by: chris m ]

[MetalMarvels]

Keith, the program does have 12 lines of commentary after the "O" word, but removing the comments has no effect on the problem. Putting any other non-canned type cycle in advance of the canned cycle makes the problem go away.

 

n_tydingco, I will give that a try....

 

Chris, that is a good point on the G99. On my system at home, I post a G98 rather than the G99 and the order is G81 G98 rather than the G99 G81 that I get at work. However, I had previously dug out my FADAL 3016L books at home and thoroughly modified my home post to output the Gcode as shown in the manuals for my 3016L. I also modified my home post to output all of the proper preparatory codes for the FADAL Format 2 and to output the codes in the order shown in the manual.

 

Unfortunately at work, I am only a dumb engineer who couldn't possibly know anything about post processors.... Management doesn't want me messing with the post, hence the need for an outside agent (which may end up being our distributor) to fix the problem. One bright point is that the machine tool distributor and the Mastercam reseller are one and the same.

 

Mostly, I am just interested in trying to understand the problem (if for no other reason than to NOT repeat it on my own equipment).

 

Cheers,

[n_tydingco]

Good point Chris. I'm waiting to read Gary's response and solution.

[chris m]

Is it possible for you [not Mastercam] to just write a quickie program using your editor (CIMCO or whatever you use) and send it to the machine to see if it works? My interest is really awakened by these problems because some day it will happen to me and I will say "I remember hearing about this before..."

 

C

[MetalMarvels]

Chris, I will be doing as you suggest - hand coding a series of test cases to see what the variables appear to be. I will let you know the results.

 

Also, I managed to get folks to agree to finally migrate to MC9 SP1 (we have owned it at work for months now.....).

 

Yeeeeehhhhaaaaaaa

[Jack Mitchell]

Gary,

 

Please consider these programs.

 

O0099

N005 G00 G17 G90 G95 G98

N010 G54 (Example**Mitchell**09/04/02)

N015 M06 T01 (#3 C-Drill T01/H01)

N020 G43 H01 X.32 Y-.2 Z2.0 S6000 M03 M08

N025 G99 G81 X.32 Y-.2 Z-.03 R.1 F.001

N030 X1.32

N031 X2.32

N035 G80 G49 Z2.0 M09

N040 G91 G28 XYZ

N045 M02

%

 

O0099

N005 G00 G17 G90 G94 G98

N010 G54 (Example**Mitchell**09/04/02)

N015 M06 T01 (#3 C-Drill T01/H01)

N020 G43 H01 X.32 Y-.2 Z2.0 S6000 M03 M08

N025 G98 G81 X.32 Y-.2 Z-.03 R.1 F6.0

N030 X1.32

N031 X2.32

N035 G80 G49 Z2.0 M09

N040 G91 G28 XYZ

N045 M02

%

 

Either program should render the same result on your machine tool or mine.

The most common error in programming is the “O” instead of “0”

The fore & aft comment brackets are also essential – otherwise the control will attempt to execute the various number and letters contained within.

 

Please key these up and try them both out and shift your G54 over a couple of inches.

This example is a learning experience for good programming practice.

 

Regards, Jack

[chris m]

quote:

---

N020 G43 H01 X.32 Y-.2 Z2.0 S6000 M03 M08

N025 G99 G81 X.32 Y-.2 Z-.03 R.1 F.001

---

quote:

---

N020 G43 H01 X.32 Y-.2 Z2.0 S6000 M03 M08

N025 G98 G81 X.32 Y-.2 Z-.03 R.1 F6.0

---

Jack,

 

I hate to break balls [well, actually, no I don't; but in this case I do] but the first program is going to traverse between holes at .100" and the second is going to traverse at 2.000" so they won't be quite

 

quote:

---

...the same result on your machine tool or mine...

---

or did I misunderstand what you meant?

 

Also...

 

quote:

---

The most common error in programming is the “0” instead of “O”

---

while this certainly happens, wouldn't you normally get an "illegal G code" error instead of the machine just ignoring the block?

 

[ 09-05-2002, 07:07 AM: Message edited by: chris m ]

[perfecseal mankato]

I may have a simple solution to this problem.

try putting the R-plane in at the G80 line,

Or the initial tool height.

We used to have this problem all of the time.

This did correct the problem.

Of course this would mean you would want to edit the post processor, or manually edit this move in on every drill cycle.

[MetalMarvels]

In the FADAL controls on the 2000 vintage 3016L and the 1996 vintage 4020, using a "0" rather than an "O" in the "O-word" results in an error every time when downloading the program to the machine. It doesn't tell you what it didn't like - it just errors out on the "TA,1" download.

[MetalMarvels]

Jack, I just noted in the preparatory block the use of a G95 (per revolution feed) - apparently this option is not available in the 4020 or 3016L FADAL controls.... I can definitely use the G94 (per minute feed) but this is already the default for the control and a G94 is not normally coded. The exception is when a G93 (inverse time) is used, then a G94 MUST follow on the next line. Apparently FADAL didn't think a G95 was necessary!

[chris m]

Gary

 

quote:

---

Apparently FADAL didn't think a G95 was necessary!

---

That would be because Fadals are best used as boat anchors or elevator counterweights

 

It may also be a software option that you didn't buy [it is on a couple of my older machines]

 

I don't know if Jack meant a zero in the O word (which would cause a DNC error) or an O in the G80 block (which I think would cause an illegal G code error) but I don't think either thing would cause your problem; did you try what we talked about?

 

C

[Thad]

quote:

---

Apparently FADAL didn't think a G95 was necessary!

---

Possibly because "feed per rev" is typically associated with turning operations???

 

To the best of my knowledge, it's not an additional option that you would need to purchase. I don't believe the Fadal control is set up like that. Either it's a code that the control understands, or it isn't.

 

Thad

[MetalMarvels]

Chris,

OUCH

quote:

---

That would be because Fadals are best used as boat anchors or elevator counterweights

---

While I would really love to have it, I couldn't afford a high-end mill to put in my garage and the FADAL does a very nice job for what I use it for. Bearing in mind that I am not doing work that requires a .0001 or better tolerance all day long. I have done the same work with a coping saw and files, but I certainly can't recommend it......and the FADAL IS paying for itself and getting the job done (while I am not even there). What more could you ask from an elevator counterweight?

[n_tydingco]

OTS -- We could be opening up a can of worms talking about what machines are best suited for maritime duty. We have our fair share of problems with the Fadals in our shop (and in previous shops I have been associated with), however, I've also seen and heard horror stories about other brands of machine tools.

 

So anyway Gary, is the problem resolved? What was the root cause?

[chris m]

You've got a 4020 in your garage?!!?!?

 

COOL!!!

 

I wish I had that kind of space at my house; the only thing I have in the garage that I could make any $ with is my lawnmower.

 

Did you get it to work?

 

C

[MetalMarvels]

Guys,

 

I have 5 different code scenarios in the stack, but SOMEONE wanted to do real work... I just can't understand why REAL work should get in the way of the search for knowledge. I hope to get control of the machine this afternoon to run the test cases. So far there is no clear-cut cause of the "endless drill cycle". I will keep all informed of the results..........

 

 

[ 09-05-2002, 01:34 PM: Message edited by: MetalMarvels ]

[Jim Whipple]

posted 09-05-2002 12:37

You've got a 4020 in your garage?!!?!?

 

COOL!!!

 

I wish I had that kind of space at my house; the only thing I have in the garage that I could make any $ with is my lawnmower.

 

I've got a 550 Matsuura and a LB15 Okuma in mine

What's everyone else got hiding in there?

Jim

 

[ 09-05-2002, 01:25 PM: Message edited by: Jim Whipple ]

[MetalMarvels]

Chris,

 

Actually I have the 3016L in the garage - the 4020 would not quite fit. The z-height would require that I cut a 2x3 hole in the floor of my daughter's room. For some strange reason she strongly objected to the head of my mill z-ing up thru her floor. Just no reasoning with teenagers!

 

[Keith Graydon]

My garage is kinda full-up. See Below.

|

|

|

|

|

|

|

|

|

|

|

|

My great Uncle has a Fabulous basement Shop. He Retired from the tool room At Browne & Sharp.

|

|

|

|

[gstephens]

I think the problem is probably either:

1. the X and Y need to be in the G8? line.

or

2. the R needs the R0=+0.025 format.

 

I think both of those are in the post we've got running at the Fadal plant.

[MetalMarvels]

OK, latest results......

 

I tried all of the suggestions and they all work just fine (when you only post 1 or 2 drill cycles). In addition, I could not repeat the problem today. Yesterday I could do it at will, today....NOT. I went back to the ORIGINAL posted code: a centerdrill, drill, tap ... problem reappears and centerdrill endlessly repeats(whew - I wasn't imagining it). Took the same file and only posted the 1st 2 tools... problem gone (WHAT???). Post all three .. problem back. I can reproduce the issue again at will.

 

I have now tried various mixtures of drill cycles - the only time it "breaks" is with 3 canned drill cycles in a row with no other toolpaths preceding the drill cycles (stick a contour 1st and it all works).

 

When running the "broken" code it never processes the 1st drill cycle cancel (G80) and loops thru the 1st drill cycle forever. This ONLY happens when at least 3 canned drill cycles are posted sequentially and NO other op preceeds the drill cycles.

 

I am now proceeding thru the suggested fixes in a controlled fashion to determine what will "fix" the "broken" code. I think that I am starting to get a handle on this and I will keep you posted.

 

[ 09-05-2002, 02:49 PM: Message edited by: MetalMarvels ]

[MetalMarvels]

FINALLY GOT IT!!!!!!!!!

 

When the code comments (all the header junk) are posted, they do not have "N-words" assigned to them out of the post processor. When the code (with unnumbered comments) is transmitted to the FADAL, the controller adds N-words to the unnumbered comments (for example N1 thru N13) THEN the program starts AGAIN at N1 (as posted). With three or more canned cycles as the program, the 4020 control appears to interpret the 2nd (N1....Nx) numbered set of codes as a subroutine that it repeats..... If I pre-number the comments sequentially with the following code it all works. If I delete the un-numbered comments before tranmitting it or delete them after the control assigned new N1...Nx to them, it all works.

 

This only occurs with the 1996 vintage FADAL 4020, my 2000 vintage 3016L ignores the comments (except to display them) and does not attempt to assign N-words to them.

 

All in all, a truly bizarre thing. The permanent fix is that I will be forcing the assignment of N-words to the comment lines in the post processor.

 

Weird, No????

 

As an aside, I have noted that with the FADAL controller, if you have duplicate N-words (too many lines for the available number of N-words) and then start in mid-program AFTER the roll-over of N-words, it will not work properly (you end up at the 1st instance of the N-word rather than where you wanted to be). This has caused me to add memory to the FADAL and change the N-word step size to "2" and the length to 5 places.

 

Thanks for all the help and suggestions.