Newb looking for program help with Mazatrol.

Hello everyone.

So a couple months ago I started working in the machine shop at my job. I was initially another button pusher until one of the mill guys got fired. So now I am to be his replacement eventually, however i know very little about machining and G&M code programming. They have 3 Mazak mills and up until now I have been using the Mazatrol interface to do parts. Recently I wanted to try to write code in the EIA/ISO format. My first practice program I'm trying to do is a figure eight followed by a sideways "S" movement. My problem is when I go to run the program I get the alarm "806 illegal address _, 0, 0. When I try to watch the graphic tool path on the screen I get the alarm "465 EIA shape data not found". I assume it is a syntactical error on my part but I don't know what it is. I would ask my Lead but unfortunately he doesn't have the time right now. Im on a Mazak VCN 510C-II with a Mazatrol Matrix Nexus.

Here is the code:
N1 G20 G90 G17 G94
N2 T01 M06
N3 G00 X-10 Y-5 Z-5 S1500 M03 M08
N4 G91 G02 I0 J2 F.5
N5 G03 I0 J-2
N6 G02 X-5 I-2.5 J0
N7 G03 X-5 I-2.5 J0
N8 G28 Z0 Y0 X0
N9 M30

I tried with and without % and beginning and end of prog. Also tried with the "O" prog number. I appreciate all constructive criticism, even if its unrelated to the errors I'm receiving. Thanks

The EIA/ISO code on Mazaks can have different requirements than the Fanuc code which we tend to consider industry standard, so pay close attention to the programming manuals from Mazak. If your shop has lost them, they are probably available in some corner of the internet. Your machine will be picky about a bunch of M and G codes at the beginning of each program and after tool changes. It's a good idea to find full program examples from the manuals and find out the meaning of each M/G code so you can understand why it's needed. Mazatrol code simplifies 99% of this and sort of hides these things in the background.

One thing I'm not sure about Mazak is that you have moves like X-10 and Y-5 instead of X-10. and Y-5. A Fanuc would interpret X-10 as X-0.001 and Y-5 as Y-0.0005, but X-10. would actually mean X-10.0, so programmers have to be extra careful to always include the punctuation. Meanwhile, a Siemens 840D control I used in EIA/ISO mode didn't care whether it was X-10 or X-10. - it would always read it as X-10.0

It's also moving on three axes at once in N03, can it do so without problem? I don't know if I ever tried this, usually moved max two axes at once, but I'm more of a lathe guy anyway.

Move M08 from N3 to N4. Mazatrol does not like multiple M codes per line.

Here's the first section of a program that runs perfectly. Copy the safety line and use for yourself. I didn't see a work offset in your program either so that may also be the problem. Also, ALWAYS punctuate numbers, not doing so can turn really sour! I don't use an O##### or % top bottom.

N100 G20
N110 G0 G17 G40 G49 G80 G90
(VISE 1)
( 2X PLUNGE .250 HOLES THRU )
N290 T5 M6
N300 G0 G90 G54 X5.927 Y-4.929 S10000 M3
N310 Z1. M8
N320 Z.6
N330 G99 G81 Z-.05 R.6 F20.
N340 X7.103 Y-4.554
N350 G80
N360 Z.6
N400 M01

It was the punctuation error at the end of my coordinates like you guys suggested. Thank you guys, I appreciate the help.

Plastic extrusion machine : The whole production line is a intelligent control system. The cutting machine adopt automatic chipless cutting to ensure the smooth cut surface. ISO9001 certificate.

abdelghani said:

Spammers Bite Here: The whole product is a intelligent spam control system. The machine adopts automatic seamless banning to ensure the spammers never come back.

Click to expand...

That's just what we need! Thank you so much!

N3 2 M codes on the same line, usually not allowed. Also rapid to Z-5 might be noisy and hard on the cutter.

N4 on, all incremental arc moves, not illegal but normally the way you would program the part...

I want to participate on your forum is that it bothers you

abdelghani said:

I want to participate on your forum is that it bothers you

Click to expand...

It doesn't just bother me. There are a few others here too........

Hijacking is what you guys do best. Well, ya dun it again.

When I was learning on the Mazak lathes, I found the mazak machine alarm books to be of big help. They are not very good to say the least, but better than nothing and therefore big help when you don't much to lean on.