to jump from G-code to Mazatrol

toolmakerjim · Jul 26, 2006

looking at a new job and they have Mazaks ive run Mazaks but only using G-code.

heres the question.

how hard is it to pick up the Mazatrol format or would i be better off staying with the G-code.

TIA...jim

Bobw · Jul 26, 2006

Its a piece of cake, 2-axis lathe, you'll beat your head against the nearest brick wall wondering why you ever bothered with g-code on a lathe, particuarly in a job shop environment.

If you have half a brain, and a knowledge of any kind of programming, which I know you do, you'll have it up and running in no time. It does take a bit of time to learn what it wants for some things (grooves, Id face is a pain), but basically a few hours to figure out your first program if its moderately simple.

On the mill, a little tougher, a little more limited in tool paths, but its great for the simple parts.

If there is somebody there to give you a crash course, and answer the tougher questions when they come up, piece of cake.

My only advice is 95% of the time, you don't have to lie to it, especially on the lathe, you lie a little more on the mill. You'll learn real quick were you have to lie to it, and if you're lieing to it too much, then there is something amiss, some little thing that you are missing, didn't pick up or aren't taking advantage of.

Good luck.

fizzissist · Jul 26, 2006

Mazatrol was first described to me as "Mazalarm".
You'll see what I mean soon enough.

It's really rather nice to program in once you figure out the secret handshakes and learn how to lie to it.

I had a hard time believing that guys would just take a print and stand at the machine, programming. Now that's what I do. The control will do a lot of the calculations for you, and it's pretty 'conversational'.

You can still use G-codes within the mazak format too with the manual program command.

If you've already run 'em, picking up the new format should be easy!

toolmakerjim · Jul 27, 2006

actually there isnt anyone there to help me.
the operators just ran programs that the guy im replacing wrote.
i have 23 yrs writing G-Code on various machines so that im not worried about so essiantaly i'll be training those guys in my own way...jim

psychomill · Jul 27, 2006

Go in head first Jim....

For lathes, Mazatrol is easy, simple, fast, etc.

For mills or milling on lathes,... I prefer G-code. Mazatrol will still get the jobs done. And for most live tooling work or "simple" mill work on lathes, Mazatrol is fine. It's when you get into the complex/arbitrary shapes, thin wall, surfacing and other 3D work where I don't care for mazatrol. Not enough control and the cycles do some weird things even when trying to control it through TPC or "cheating" the pattern.

fizzissist · Jul 27, 2006

If you already know how to set up tools, jaws, Z, and everything BUT the programming in Mazatrol, you're still way up on the learning curve.

Do you have the programming and parameter manuals for the machines? If so, we should be able to walk you through the basics.

In any case, you can at least start out programming G, then play with the mazatrol when you've got some free time...and no one's looking..

toolmakerjim · Jul 27, 2006

thats what i thought i'd do i made the bosses aware that i was not a mazatrol guy and they do have all the manuals.
the guy im replacing ive known for 20 yrs and he is willing to help but i know there is a lot of varied talent here.
im going to put in some time on my own to shorten the learning curve if possible.
there probably wont be too many complex parts on this job mostly repair and bolt patterns on the mill and some simple lathe parts radii and OD grooving but mostly onesy twosey's. nothing over 25 to 50 parts.
plus i have to learn their work flow procedure i just ordered a computer to log work and times not a performance log just a time estimate log for my own benefit.
thanks for the help and keep any suggestions coming...jim

MachineMan77 · Jul 28, 2006

learning curve????

toolmakerjim · Jul 28, 2006

sure you always have to learn something new, unless your intutive or a woman...jim

fizzissist · Jul 28, 2006

One thing about the Mazaks is the built-in time analysis....Go into "DIAGNOS" then go to "Running Control"...there's other statistics available too for actual run time, etc...

One problem you might encounter is the way Mazatrol handles grooving....I don't like the way it starts a groove from the headstock out...I like to start out and move in, so I have to do multiple grooves to rough (type "0"), then do a single wide light pass (type "2" to finish. If someone knows a better way...I'd be happy to learn!!

Onsey-twosey is our specialty..so I can relate. Biggest time sink here is workholding and tooling change-overs. Still on the low side of the learning curve myself, but if I can learn it, ANYONE can. (I could even teach Solar!)

toolmakerjim · Jul 28, 2006

thanks fizzissist;

can i set the time analysis to down load to a computer assigning job # or any other info tools-speeds-feeds?

i dont like lathe work too much anyway and will more than likely address that side to G-Code at least iniatially. i to like to start at the face and work towards the chuck.

are the normal canned cycles roughing with finish allowances - finish -threading with pull out ramping turned off etc. on board already?

when i get to the new job i'm sure that i will be slamming ya'll with questions for a few days at least...jim

fizzissist · Jul 28, 2006

I'm sure the file is downloadable.....but readable on a PC? Is there a Mazak software guru lurking??

All the cycles (for all practical purposes...almost all) have a rough SFM setting, a finish SFM, rough feed, rough depth of cut, and a button to select the finish you want. X and Z finish allowances are at the head of the program and set for all 'unit's. ...You can fool it if you need to by offsetting the individual roughing tools..

Never run a Mazak mill....but for lathe work, I think the Mazatrol runs circles around general G-code. AND, you can use the TPC (tool path control) or MNP (manual program) to stick in a little G of your choosing when you need some special operation.

Threading is very easy...once you figure out the way it thinks. Ramping is automatic, and parameters for it are user-available.

You'll find that the parameter book is WAY handy...like changing the boring bar retract amount for little boring bars, the increasing it for larger bars...but ya have to remember to change it back!!

D. Rey · Jul 28, 2006

I'm not a Mazak guru but I have one. You can't view Mazak files on a PC without software that can read Mazak CMT code. Camlink, Mazacam are the only two I'm aware of.

psychomill · Jul 28, 2006

You can't view Mazak files on a PC without software that can read Mazak CMT code.

Correct.... but, you can output a Mazatrol program through the Tape I/O and read any Mazatrol program on a regular editor. It outputs in whats called a 3-digit format.

fizzissist · Jul 28, 2006

psycho....
...which leads to the obvious question.....Can you edit it on a regular editor and feed it back to the machine???

psychomill · Jul 28, 2006

psychomill · Jul 28, 2006

OK, OK.... I won't leave you hanging with an answer like that... That's a Pi manuever..

If you look in the back of the Mazatrol programming book, there's a section called 3-digit G-format. This is the EIA code for Mazatrol. Now, it takes a while to get a hang of it, but you can edit and write programs from this format. I've never written complete programs this way but I've done plenty of editing including program adjustments, adding passes, adding cuts, changing tool data, moving around program cycles, modify priorities, adjust offsets,.... basically just about anything you do with regular G-code.

The book goes over this stuff briefly but you at least you get most of the syntax and format. The easiest way to learn it is to download a bunch of Mazatrol programs and go through it. Kind of the same way you would to follow/learn macro programs or learn how to write post processors. After awhile, you understand and recognize the the format and you can edit it just like you would standard G-code.

I will say though.... It's way easier to do this in its native format using Griffo or Mazacam or something. I only do it because I had the "itch" to figure it out years ago and now I can.

fizzissist · Jul 28, 2006

Oh goody!!! Something new to explore!! Thanks!!!

I've been reluctant to have the Mazak communicate with other computers....due to my puritannical moral standards, knowing that it runs under Windows95, and I'm scared to death it'll catch a dose of the clap....not that my computers have anything...but...

Since I wrote the programs, know what they do and why, it'll be easy to figure out! (he says optimistically)

>For Jim, ...you're gonna love how easy it is to write up a quick program to bore or turn jaws in situ. I've got 3 different programs saved expressly for that purpose, and 1 generic turn/face program for parts. Quick and easy to change some simple features, stick the program numbers on the "End" unit, and away you go!

toolmakerjim · Jul 28, 2006

im still here reading thanks guys...jim

Integrexman · Jul 28, 2006

If your mazak has a newer control Fusion 640 and has Win2k not Win95. For about $10-$15 you can buy online a pdf printer driver. It will let you print to a file in pdf format. Install it on your machines then at the top of the program (or any screen) use your mouse and goto file-print and select the printer driver you installed. It will create a pdf file you can move out of the machine to pc and view it just like it is in the control.

to jump from G-code to Mazatrol

Titanium

Diamond

Cast Iron

Titanium

Titanium

Cast Iron

Titanium

Plastic

Titanium

Cast Iron

Titanium

Cast Iron

Titanium

Titanium

Cast Iron

Titanium

Titanium

Cast Iron

Titanium

Aluminum

Similar threads